mori seiki SL-150, 150MC, 150Y, SL-150S, 150SMC Programming Manual

...

PROGRAMMING MANUAL

Applicable Model

SL-150, 150MC, 150Y SL-150S, 150SMC, 150SY SL-200, 200MC SL-200S, 200SMC SL-250, 250MC SL-250S, 250SMC SL-303, 303MC, 303Y SL-400, 400MC SL-600, 600MC SL-25E SL-65, 65MC SL-75, 75MC TL-40, 40MC, 40Y VL-25 VL-55, 55MC LL-7, 8 CL1500, 1500T CL2000, 2000T

Applicable NC Unit

MSC-500 MSD-501 MSC-501 MSD-518 MSC-518 MSD-501II MSG-501 MSD-518II

Before starting operation, maintenance, or programming, carefully read the manuals supplied by Mori Seiki, the NC unit manufacturer, and equipment manufacturers so that you fully understand the information they contain.

Keep the manuals carefully so that they will not be lost.

PM-NLTMSC518-I1EN

• The contents of this manual are subject to change without notice due to improvements to the machine or in order to improve the manual. Consequently, please bear in mind that there may be slight discrepancies between the contents of the manual and the actual machine. Changes to the instruction manual are made in revised editions which are distinguished from each other by updating the instruction manual number.

• Should you discover any discrepancies between the contents of the manual and the actual machine, or if any part of the manual is unclear, please contact Mori Seiki and clarify these points before using the machine. Mori Seiki will not be liable for any damages occurring as a direct or indirect consequence of using the machine without clarifying these points.

The product shipped to you (the machine and accessory equipment) has been manufactured in accordance with the laws and standards that prevail in the relevant country or region. Consequently it cannot be exported, sold, or relocated, to a destination in a country with different laws or standards.

The export of this product is subject to an authorization from the government of the exporting country.

Check with the government agency for authorization.

990730

SIGNAL WORD DEFINITION

FOR SAFE OPERATION

FOREWORD

BEFORE READING THIS PROGRAMMING MANUAL

A : BEFORE PROGRAMMING

B : G FUNCTIONS

C : M FUNCTIONS

D : T, S, AND F FUNCTIONS

E : AUTOMATIC TOOL NOSE RADIUS

OFFSET

F : MANUAL TOOL NOSE RADIUS OFFSET

G : CUTTER RADIUS OFFSET

H : MULTIPLE REPETITIVE CYCLES

I : HOLE MACHINING CANNED CYCLE

J : TOOL LIFE MANAGEMENT B

FUNCTION (OPTION)

K : EXAMPLE PROGRAMS

APPENDIX

INDEX

SIGNAL WORD DEFINITION

A variety of symbols are used to indicate different types of warning information and advice.

Learn the meanings of these symbols and carefully read the explanation to ensure safe operation while using this manual.

The warning information is classified into three categories, DANGER, WARNING, and CAUTION.

The following symbols are used to indicate the level of danger.

Indicates a potentially hazardous situation which, if not avoided, may result in minor or moderate injury damages to the machine.

The information described following the caution symbol must be strictly observed.

COMMAND

The format identified by this symbol gives information for programming.

Indicates an imminently hazardous situation will result in death or serious injury.

The information described in the DANGER frame must be strictly observed.

Indicates a potentially hazardous situation could result in death or serious injury.

The information described in the WARNING frame must be strictly observed.

which, if not avoided,

Indicates the items that must be taken into consideration.

Indicates useful guidance relating to operations.

Indicates the page number or manual to be referred to.

The number in ( ) indicates the section number.

Indicates the procedure used for displaying the required screen.

Indicates the example of operations.

FOR SAFE OPERATION

This machine is intended for use by persons who have a basic knowledge of machine tools, including cutting theory, tooling and fixtures. Mori Seiki cannot accept responsibility for accidents that occur as a result of operation or maintenance of the machine by personnel who lack this basic knowledge or sufficient training.

Workpiece materials and shapes vary widely among machine users. Mori Seiki cannot predict the chucking pressure, spindle speed, feedrate, depth of cut, etc., that will be required in each case and it is therefore the user's responsibility to determine the appropriate settings.

Each machine is shipped with a variety of built-in safety devices. However, careless handling of the machine can cause serious accidents. To prevent the occurrence of such accidents, all programmers and other personnel that deal with the machine must carefully read the manuals supplied by Mori Seiki, the NC unit manufacturer, and equipment manufacturers, before attempting to operate, maintain, or program the machine.

Because there are so many "things that cannot be done" and "things that must not be done" when using the machine, it is impossible to cover all of them in the Instruction Manual. Assume that something is impossible unless the manual specifically states that it can be done.

FOR SAFE OPERATION -1-

The following manuals are supplied with your NC lathe:

I. Safety Guidelines prepared by Mori Seiki

II. Instruction Manual prepared by Mori Seiki

• MAINTENANCE MANUAL

• OPERATION MANUAL

• PROGRAMMING MANUAL

III. NC unit Operation and Maintenance Manuals prepared by the NC unit manufacturer

IV. Instruction Manuals prepared by equipment manufacturers

In addition to these manuals, ladder diagrams, parameter tables and electrical circuit diagrams are also supplied with the machine to help with electrical maintenance. The ladder diagrams are provided in the document box, parameter tables and electrical circuit diagrams are stored in the document compartment inside the electrical cabinet. Please make use of these materials when carrying out maintenance work.

Fundamental safety information is presented in the following pages.

All cautions on operation must be strictly observed when operating the machine, carrying out maintenance work, or writing programs. Failure to observe fundamental safety information can cause accidents in which the operator or other personnel working near the machine are seriously injured, or the machine is damaged. All personnel that deal with the machine must carefully read and thoroughly understand the information in the following pages before attempting programming or operating the machine.

SO-NL-B16E/P

-2- FOR SAFE OPERATION

The vocabulary and terms used for machine parts and operations in the warnings, cautions and notes are defined or explained in the manual texts and illustrations.

If you are unsure of the meaning of any word or expression, please refer to the corresponding textual explanation or illustration. If you still cannot understand or are unsure of the meaning, contact Mori Seiki for clarification.

"Operator", as used in these cautions, means not only the operator who operates or supervises a machine tool to perform machining, but also any person, including maintenance personnel who maintain and inspect a machine tool or safety device or safety measures provided with it, and the programmers who create programs used for machining, who are engaged in operations which deal with a machine tool.

Therefore, all persons engaged in these operations must carefully read these cautions and related materials, and thoroughly understand the contents before attempting to operate the machine.

SO-NL-B16E/P

FOR SAFE OPERATION -3-

1 CONSIDERATIONS BEFORE OPERATING THE MACHINE

The cautions that must constantly be born in mind when operating the machine are listed below.

Listed below are important cautions that apply to all machine-related work (machine operation, maintenance, inspection, programming, etc.).

DANGER

1. Never touch a switch, button, or key with wet hands.

If it is not properly grounded or is leaking current, you could receive an electric shock.

2. Before starting machine operation, check that there is nobody inside the protective cover or close to rotating or moving parts of the machine. Never touch or stand near the rotating or moving parts of the machine while it is operating; you could be seriously injured by being entangled in the rotating parts or crushed by the moving parts.

3. Never operate the machine with the protective cover removed or while interlocks or other safety devices are ineffective, since the machine could operate in an unexpected manner, causing accidents involving serious injuries.

Contact Mori Seiki, the NC unit manufacturer or relevant equipment manufacturers immediately if the protective cover or safety devices are damaged.

4. Always lock out the power to the machine before carrying out work inside the machine – such as setup work or cleaning the inside of the machine – and before carrying out inspections, repairs, or maintenance work. In addition, set the main switch to the OFF position and lock it, and place "PERSONNEL INSIDE MACHINE" or "UNDER MAINTENANCE" signs around the machine to stop anyone from switching on the power or operating the machine while the work is in progress. If work inside the machine or inspection or maintenance work is carried out with the power switched on, machine elements could be moved, and the personnel carrying out the work could be seriously injured by being entangled in the rotating parts or crushed by the moving parts of the machine.

5. Always switch off the power before carrying out inspection or maintenance work in the electrical cabinet or on motors and transformers. If work has to be done while the power is switched on, it must be carried out by a qualified electrical engineer, taking the proper precautions; there is a danger of electric shock.

6. Cover power supply cables that are run along the floor with rigid insulated plates to prevent them from being damaged. Damage to the insulation of the power supply cable could cause electric shocks.

SO-NL-B16E/P

-4- FOR SAFE OPERATION

DANGER

WARNING

7. Even after the power is turned off, some devices will remain charged and the temperature of motors, lights inside the machine, etc., will remain high. Make sure that the charge has been discharged or the temperature has fallen before carrying out maintenance work or inspections on these devices. If you touch these devices/units carelessly while they are still charged or while the temperature is still high you could receive an electric shock or be burned.

8. Check that all cables are properly insulated before using the machine. There is considerable danger of electric shock if damaged cables are used.

1. Keep the floor area around the machine tidy and clean; do not leave things lying on it, and clean up spilled water or oil immediately. If you fail to do this, plant personnel may injure themselves by tripping over or slipping on the floor.

2. Before operating the machine, check the area where you will have to stand and walk to make sure you can operate the machine safely. If you do not check your footing beforehand, you could loose your balance while working and injure yourself by putting your hands in a dangerous place while trying to find support, or by falling over.

3. Before using a switch, button, or key, check visually that it is the one you intend to use, and then press or set it decisively. Pressing the wrong switch, button, or key by mistake can cause accidents involving serious injuries or damage to the machine.

4. Keep the doors closed during machine operation. Leaving the machine running or operating it with doors open could cause accidents involving serious injuries or damage to the machine; plant personnel could be seriously injured by being entangled in the rotating parts of the machine, crushed by its moving parts, struck by broken tools, workpieces or jaws flying out of the machine, hit by flying chips, or splashed with coolant.

5. The parameters are set on shipment in accordance with the machine specifications; do not change them without first consulting Mori Seiki. If the parameters are changed without consultation, the machine may operate in an unexpected manner, causing accidents involving serious injuries or damage to the machine.

SO-NL-B16E/P

FOR SAFE OPERATION -5-

WARNING

6. The machine specifications are set before shipping so that the machine can deliver its full performance. If the specifications and/or settings have to be changed or the machine has to be modified to meet new machining requirements or due to changes in the operating conditions, consult Mori Seiki. Changing the settings without consultation may lead to accidents involving serious injuries, impaired machine performance, and considerable shortening of the machine service life.

7. Before operating or programming the machine, or performing maintenance work, carefully read the instruction manuals provided by Mori Seiki, the NC unit manufacturer and the equipment manufacturers so that you fully understand the information they contain. Keep these instruction manuals safely so that you do not lose them. If you do lose an instruction manual, contact Mori Seiki, the NC unit manufacturer, or the relevant equipment manufacturer. If you attempt to operate the machine without having carefully read the instruction manuals first, you will perform dangerous and erroneous operations which may cause accidents involving serious injuries or damage to the machine.

8. Always observe the instructions in the caution labels stuck to the machine. Carefully read the Safety Guidelines supplied with the machine so that you fully understand them. If the writing on the labels becomes illegible, or if the labels are damaged or peel off, contact Mori Seiki. Also contact Mori Seiki if you cannot understand any of the labels. If you operate the machine without observing the instructions on the labels, or without understanding them properly, you will perform dangerous and erroneous operations which may cause accidents involving serious injuries or damage to the machine.

9. Never operate, maintain, or program the machine while under the influence of alcohol or drugs. Your concentration will be impaired, you may loose your balance and fall against dangerous parts of the machine, and you may operate the machine incorrectly, causing accidents involving serious injuries or damage to the machine.

10. Machine operators and authorized personnel working inside the plant and in the vicinity of the machine must put their clothing and hair in order so that there is no danger they will be entangled in the machine. If you have uncontrolled long hair or loose clothing and it gets caught in the machine, you will be seriously injured by being entangled in the rotating parts of the machine or crushed by its moving parts. Always wear safety shoes, eye protectors and a helmet.

SO-NL-B16E/P

-6- FOR SAFE OPERATION

WARNING

11. The machine is equipped with interlock functions such as the door interlock, chuck interlock, tailstock spindle interlock (applies only to machines equipped with a tailstock) and electrical cabinet door interlock to ensure the operator's safety. All the interlock functions must be ON when operating the machine. If you have to operate the machine with the interlocks released, you must recognize that there are many hazards involved and pay particular attention to safety while operating the machine in this condition. After finishing the necessary work, you must switch the interlocks back ON.

If the machine is operated with the interlocks released, it may operate in an unexpected manner, causing accidents involving serious injuries or damage to the machine.

12. The door interlock function serves only to protect the machine operator from accidents that can be prevented by inhibiting manual and automatic operation of the spindle, axis movement, and all other operations in automatic operation when the door is opened and while it is open; it will not afford protection against other hazards.

For example, each machine user will machine a variety of workpiece types and use a variety of workpiece holding fixtures, cutting tools, and cutting conditions; you are still responsible for ensuring safety with regard to the hazards that can arise from these user-specific conditions.

13. If the door interlock function is released, the machine is able to operate with some limitations while the door is open, exposing you to danger. In daily production operation, the door interlock function must be set "valid" and the key operating the switch must be removed from the switch and kept safely.

When shaping soft jaws, measuring the tool offset data, program check, test cutting or carrying out other setup work, it may be necessary to release the door interlock function. If you have to carry out work while the interlock function is released, you must recognize that there are many hazards involved and pay particular attention to safety. While the door interlock function is released, the warning lamp blinks in red and the warning buzzer beeps intermittently. You must recognize that the door interlock function is in the released state when the warning lamp is blinking in red and the warning buzzer is beeping intermittently. After finishing the necessary work, you must switch the interlock function back valid.

SO-NL-B16E/P

FOR SAFE OPERATION -7-

WARNING

14. Before operating the machine, memorize the locations of the emergency stop buttons so that you can press one immediately from any location and at any time while operating the machine. The emergency stop buttons are used to stop all operations in the event of an emergency. If there is an obstacle in front of an emergency stop button it will not be possible to press it immediately when an emergency occurs and this could cause accidents involving serious injuries or damage to the machine.

15. Always switch the tailstock spindle interlock function ON before carrying out center-work operations. If this function is OFF, it will be possible to start automatic operation when the tailstock spindle is extended, even though it may not support the workpiece correctly. If automatic operation is started in this condition, the workpiece will fly out, causing serious injuries or damage to the machine. (Applies only to machines equipped with a tailstock.)

16. Adjust the position of the tailstock body so that the workpiece is securely held by the tailstock spindle center when the tailstock spindle is extended.

After making this adjustment, clamp the tailstock body to the bed. If the tailstock body is not clamped to the bed, or if the position of the tailstock body is incorrectly adjusted, it will be possible to start automatic operation when the tailstock spindle is extended, even if the workpiece is not supported by the tailstock spindle center. If machining is carried out while the workpiece is not supported by the tailstock spindle center, the workpiece will fly out, causing serious injuries or damage to the machine. (Applies only to machines equipped with a tailstock.)

17. To prevent hazardous situations, the plant or equipment supervisor must bar entry to the plant or the vicinity of the machine to anyone with insufficient safety training. Allowing persons without sufficient safety training unhindered into the plant and the vicinity of the machine could cause accidents involving serious injuries.

18. Because of the inertia of the moving parts of the machine, they may not be stopped immediately when the emergency stop button is pressed. Always confirm that all operations have stopped before going near these parts. If you approach the moving parts of the machine without due care you may be entangled in them and seriously injured.

SO-NL-B16E/P

-8- FOR SAFE OPERATION

WARNING

19. Do not leave articles such as tools and rags inside the machine. If the machine is operated with such articles inside it they may become entangled with a tool and thrown out of the machine, and this could cause accidents involving serious injuries or damage to the machine.

20. When the machine is running, operating noise may possibly be produced, depending on the cutting conditions and other factors.

When an operator works near the machine, either change cutting conditions to limit generation of noises or the operator must wear protective gear, meeting the level of generated noise, which will not cause inconvenience for performing intended work. Working under noises might impair operator's health, such as hearing.

21. This is not the explosion-proof specification machine. Dangers such as the ejection of a large workpiece or harmful dust or an explosion caused by the machining of metals such as magnesium are not preventable even if the door is closed. Do not rely on door and protective devices alone. Recognition of the dangers involved in machining procedures is required at all times.

22. This machine is equipped with a read-ahead function for the running program, and retains the read-ahead program commands stored in the NC memory during a temporary stop of automatic operation in order to eliminate latency time when restarting. Therefore, check the program commands or present positions of the axes when stopping the machine temporarily. In cases such as when discontinuing the

CAUTION

machining, press the (RESET) key to clear the program

RESET

commands stored in the NC if necessary. Changing the program start position after a temporary stop in particular may cause accidents after the machining is restarted since the program commands stored in the NC are activated. Pay extra attention to the difference in the specifications in relation to other manufacturers' machines because the read-ahead program data may be cleared at temporary stops on these machines.

1. User programs stored in the memory, parameters set before shipping, and the offset data input by the user, can be destroyed or lost due to incorrect operation or other causes. To protect data against destruction and loss, back it up using an external I/O device (option), or other device.

If you fail to make backup files, Mori Seiki cannot accept responsibility for any problem resulting from destroyed programs or lost parameter data and/or offset data.

Keep the parameter table supplied with the machine in a safe place. Note that if the data is destroyed it will take some time to set the parameters again.

2. Never touch chips or the cutting edges of tools with your bare hands since you may be injured.

SO-NL-B16E/P

FOR SAFE OPERATION -9-

CAUTION

3. Take care not to stumble over the footswitch since you may be injured.

4. If it becomes necessary to perform a memory clear operation, contact Mori Seiki first. If a memory clear operation is performed without due care, the entire memory contents may be deleted, making the machine inoperable.

5. The machine operator must have normal sensory perception. If a person who has an abnormality affecting any sense operates the machine, he/she will not be able to accurately confirm the machine status and surrounding conditions by eye/ ear/touch. Sensory confirmation is extremely important when operating the machine and an inability to make such confirmations properly could cause accidents involving serious injuries or damage to the machine.

6. Ensure that the workplace is adequately lit. If there is insufficient light, the operator may trip over something or be unable to perform or check work accurately, and this could cause accidents involving serious injuries or damage to the machine.

7. Remove any obstacles around the machine.

Secure adequate space around the machine for working and adequate passageway, considering both ease of operation and safety. If there are any obstacles or if there is insufficient space or passageway, the operator may trip and fall or be unable to work properly, and this could cause accidents involving serious injuries or damage to the machine.

8. Stack products (workpieces) stably. If they are not stacked stably they may fall and injure the machine operator. Unstable stacking may also damage the products (workpieces), causing defects.

9. Keep the area around the machine clean; remove chips and foreign matter near the machine. If left, chips and foreign matter may cause plant personnel to fall and injure themselves.

10. Use a working bench strong and stable enough to support the weight of the workpieces and tools. If an unstable working bench is used the workpieces and tools could fall off and injure the machine operator.

If a machine alarm or NC alarm occurs, check its meaning by referring to the alarm list in

NOTE

the instruction manual or ladder diagram, and take the appropriate action. If this is ineffective, consult Mori Seiki or the NC unit manufacturer and take action only when you understand clearly what to do.

SO-NL-B16E/P

-10- FOR SAFE OPERATION

2 SAFETY PRACTICES DURING PROGRAMMING

The safety practices that the programmer must observe while programming are presented below. Read them before attempting programming.

Workpiece shapes and materials vary widely among machine users and, since the workpiece holding fixtures, cutting tools, cutting methods, and machining conditions will also vary accordingly, Mori Seiki cannot predict what factors will apply in individual cases. It is the machine user's responsibility to take these factors into account when creating a program. It is also the machine user's responsibility to ensure safety with respect to the hazards that may arise due to these user-dependent factors.

WARNING

1. Specify a spindle speed limit that is lower than the lowest of the individual allowable speed limits for the chuck, fixture, and cylinder. If you do not follow this instruction, the workpiece could fly out of the machine, causing serious injuries or damage to the machine.

2. Clamp workpieces and cutting tools securely. Determine the depth of cut and cutting feedrate for test cutting with safe operation as the first priority; do not give priority to productivity when making these determinations. If you fail to observe this warning, the tool or workpiece could fly out of the machine, causing serious injuries or damage to the machine.

3. Always select the most appropriate cutting tool and holder for the material and shape of the workpiece to be machined and cutting method, and check that the workpiece can be machined without any problems.

If an inappropriate cutting tool or holder is selected, the workpiece could fly out of the chuck during machining, causing serious injuries or damage to the machine. Machining accuracy will also be adversely affected.

4. Before starting spindle rotation, check that the workpiece is securely clamped. Or, if performing center-work, check that the tailstock spindle center securely supports the workpiece. (Applies only to machines equipped with a tailstock.)

SO-NL-B16E/P

If the workpiece is not securely clamped or supported, it will fly out when the spindle is rotated, causing serious injuries or damage to the machine.

5. Do not insert bar stock into the spindle while the spindle is rotating or you will be entangled in the machine. The length of the bar stock must be shorter than the spindle length unless a bar feeder is used. If the bar stock protrudes from the spindle it will increase spindle runout, and could bend, causing accidents involving serious injuries or damage to the machine.

FOR SAFE OPERATION -11-

WARNING

6. For the machine with the flat type operation panel, always place the operation selection key-switch in the "operation enable" or "operation disable" position after completing program entry. Be aware that the program will be updated if program editing operations are carried out with the operation selection key-switch at the "operation and edit enable" position. If the program is executed after being accidentally updated in this way the machine could operate unexpectedly, causing serious injuries or damage to the machine.

7. For the machine with the discrete type operation panel, always place the edit enable key-switch in the "edit disable" position after completing program entry. Be aware that the program will be updated if program editing operations are carried out with the edit enable key-switch at the "edit enable" position. If the program is executed after being accidentally updated in this way the machine could operate unexpectedly, causing serious injuries or damage to the machine.

8. For the machine with the touch panel, always return the WRITE PROTECT switch (PROGRAM) back to ON after completing program entry. Be aware that the program will be updated if program editing operations are carried out with the WRITE PROTECT switch (PROGRAM) set OFF. If the program is executed after being accidentally updated in this way, the machine could operate unexpectedly, causing serious injuries or damage to the machine.

9. Select the appropriate chucking pressure and tailstock spindle thrust force (applies only to machines equipped with a tailstock) for the workpiece shape and material, and the cutting conditions. If you cannot determine the appropriate chucking pressure, contact the chuck manufacturer or cylinder manufacturer. If you cannot determine the appropriate spindle thrust force (applies only to machines equipped with a tailstock), contact Mori Seiki. If the chucking pressure or spindle thrust force (applies only to machines equipped with a tailstock) is not set appropriately in accordance with the shape and material of the workpiece being machined and the cutting conditions, the workpiece could fly out during machining, causing serious injuries or damage to the machine. Incorrect setting could also distort the workpiece.

SO-NL-B16E/P

-12- FOR SAFE OPERATION

WARNING

10. Give full consideration to the type of chuck and cylinder used when setting the chucking pressure. Even if the same hydraulic pressure is applied to the chuck, the chuck gripping force will vary according to the manufacturer and type of chuck and cylinder.

For details on the chuck gripping force, consult the chuck and cylinder manufacturers.

If the chuck gripping force is different from that intended, the workpiece could fly out when the spindle is started, causing serious injuries or damage to the machine.

11. Workpiece materials and shapes vary widely among machine users. Mori Seiki cannot predict the workpiece clamping method, spindle speed, feedrate, depth of cut, and width of cut, etc., that will be required in each case and it is therefore the user's responsibility to determine the appropriate settings.

Note also that the machining conditions determined in automatic programming are the standard conditions, which are not necessarily the most suitable for the user's purposes and may have to be changed in accordance with the workpiece, chuck, etc. The conditions determined in automatic programming are for reference only and the final responsibility for determining the conditions rests with the user. (Conversational NC specification)

If you have difficulty determining these conditions, consult the chuck and cylinder manufacturers and tool manufacturer. Machining under inappropriate machining conditions can cause the workpiece to fly out of the chuck during machining, causing serious injuries or damage to the machine. It will also adversely affect machining accuracy.

12. While the machine is temporarily stopped during machining –for example when checking a program, performing test cutting, or cleaning chips out of the machine – do not feed the axes or index the turret head in manual operation. Or, if it is absolutely necessary to do so, be sure to return the axes and turret to their original positions before restarting the program. If machining is restarted without returning them to their original positions, the turret will move in unexpected directions, causing collisions between the cutting tools, holders, or turret head and the workpiece, chuck, or tailstock (if featured), which could cause serious operator injuries or damage the machine. The workpiece could also be machined with the wrong tool, and the cutting tool could be damaged.

SO-NL-B16E/P

FOR SAFE OPERATION -13-

WARNING

13. If the program is input to the NC memory not by the programmer but by a machine operator, the operator may misread the numerical values and input incorrect values. This could cause accidents involving serious injuries or damage to the machine: the workpiece could fly out of the chuck during machining, and the cutting tool, holder, or turret head, could interfere with the workpiece, chuck, fixture, or tailstock (if featured). It could also cause the workpiece being machined with the wrong tool, or cause damage to the cutting tool.

14. If you forget to enter a decimal point in a program entry that requires one and start the machine without noticing the error, the turret may move to an unexpected position, causing, causing accidents involving serious injuries or damage to the machine. Check that you have entered decimal points where necessary.

15. Do not change the spindle gear range while a cutting load is applied. The workpiece could fly out of the chuck, causing serious injuries or damage to the machine and the cutting tool. In addition, excessive loads will be applied to the machine motors and machine elements, shortening their service lives. (Applies only to machines equipped with a transmission.)

16. Before starting the spindle, carefully check the workpiece gripping conditions and the machining conditions, including the chucking pressure, spindle speed, cutting feedrate, and depth of cut. If you start the spindle without adequate checking, the workpiece could fly out of the chuck, causing serious injuries or damage to the machine.

17. The chuck gripping force may be reduced due to a malfunction of the chuck or cylinder or a centrifugal force during high-speed spindle rotation. If machining is performed without securing a sufficient gripping force, the workpiece may fly out, causing serious injuries or damage to the machine.

If the chuck gripping force is reduced due to deterioration over time or damage from an accident or inadequate maintenance, contact Mori Seiki Service Department.

To prevent the chuck gripping force from lowering, clean and grease the chuck at regular intervals.

If the gripping force is reduced due to the centrifugal force applied to the jaws during high-speed spindle rotation, readjust the cutting conditions such as chucking pressure, cutting feedrate or cutting amount. Refer to the manuals prepared by the chuck manufacturer and the cylinder manufacturer.

SO-NL-B16E/P

-14- FOR SAFE OPERATION

CAUTION

1. Contact Mori Seiki when cutting cast iron, ceramics, or other materials which generate powder-type chips in dry cutting. If chips are not dealt with in an appropriate manner for the workpiece material, they can cause machine faults.

2. Before starting mass production, always check the program and perform test cutting in the single block mode. If you fail to do this the workpiece could collide with the cutting tool during machining, causing damage to the machine. Machining defects could also be caused.

3. When shifting the coordinate system in order to check a center-work program, set the shift direction and shift amount carefully to avoid interference between the turret and tailstock, which could cause damage to the machine. (Applies only to machines equipped with a tailstock.)

4. You will probably use a variety of workpiece shapes and materials, and the chucking method will differ according to the workpiece type. Therefore, when checking a program with the workpiece clamped in the chuck, check for interference carefully, taking the workpiece shape and material, and the chuck gripping force, into account. Depending on these factors, the cutting tool, holder, or turret head might interfere with the workpiece, chuck, fixture, or tailstock (if featured), causing damage to the machine.

5. When the emergency stop button or reset key has been pressed to stop the machine during a threading operation or a hole machining operation, especially a tapping operation, carefully feed the axes after checking the workpiece and cutting tool carefully for damage. If you feed the axes without due care, the workpiece and cutting tool may collide or interfere with each other, and this could cause damage to the machine.

6. Do not discharge coolant while the spindle is not rotating.

In addition, take measures to ensure that coolant does not enter the spindle bearings when it is discharged while the spindle is rotating. If coolant enters the spindle bearings, the spindle will be damaged.

SO-NL-B16E/P

7. Support the workpiece securely before stepping on the chuck clamp/unclamp footswitch to remove it. If you step on the footswitch without taking this precaution the workpiece will fall and this could cause damage to the machine.

8. If abnormal vibration or chattering is generated during machining due to improper combination among jig, cutting tool, workpiece material, etc., change the machining conditions to proper values. If machining is continued forcibly under the machining conditions with improper values, it will bring critical problems for the machine and accuracy such that the bearings is damaged quickly and cutting tool is worn excessively will take place.

9. If data is set for "COMMON" ("EXT" for MSC-

) on the WORK OFFSET screen by specifying G10 or system variable commands, the workpiece zero point is shifted in the same direction in all of the work coordinate systems, G54 - G59. Careless data setting for COMMON of the WORK OFFSET screen causes the tool or the turret to interfere with the chuck resulting in damage to the machine.

3 TO ENSURE HIGH ACCURACY

The accuracy of the finished product cannot be maintained unless the following points are observed when operating the machine. Failure to observe these points can also cause serious injuries and damage to the machine. Study these points carefully before operating the machine.

FOR SAFE OPERATION -15-

WARNING

1. Provide a chucking allowance that is large enough to ensure that the workpiece will not come out of the chuck due to cutting forces or the centrifugal force generated by spindle rotation. Depending on the shape of the workpiece, it may need to be supported by the tailstock (applies only to machines equipped with a tailstock). If the workpiece flies out of the chuck during machining it could cause serious injuries or damage to the machine.

2. Workpiece materials and shapes vary widely among machine users, and Mori Seiki cannot predict the requirements for individual cases. Give full consideration to the workpiece material and shape in order to set the appropriate machining conditions. If inappropriate settings are used, the workpiece and cutting tool could fly out during machining, causing serious injuries or damage to the machine. Inappropriate settings will also adversely affect machining accuracy.

3. When forged or cast workpieces are used, the cutting allowance with respect to the finished dimensions varies greatly. Either write a program which takes the variation into consideration or perform premachining so that a uniform cutting allowance is left on the workpiece. If this caution is not observed, the workpiece could fly out during machining, causing serious injuries or damage to the machine. In addition, an excessive load could be applied to the cutting tool, breaking it.

CAUTION

1. When machining bar stock on a machine equipped with a bar feeder or spindle through-hole, use straight workpieces only. When machining bar stock with a diameter smaller than that of the spindle (or draw bar), always use guide bushes in order to prevent vibration. If you use a bent workpiece or fail to use guide bushes, the machine will vibrate and the workpiece will shake; this could cause damage to the machine. It will also seriously affect machining accuracy.

2. When setting the tooling, refer to the turret interference diagram and axis travel diagram in the maintenance manual (DRAWINGS or PARTS LIST l published separately) so as to avoid interference. In the case of machines with two spindles, also make sure there will be no interference during workpiece transfer. Careless tooling will lead to interference between the tools and the workpiece, chuck, chuck jaws, covers, tailstock (if featured) or headstock 2 (if featured), which could cause damage to the machine.

SO-NL-B16E/P

-16- FOR SAFE OPERATION

NOTE

1. When chucking or supporting a workpiece, take the rigidity of the workpiece into account when determining the chucking or supporting method and chucking pressure or tailstock thrust force (if a tailstock is featured), so as not to distort the workpiece. If the workpiece is distorted the machining accuracy will be adversely affected.

2. If any chips become entangled with the workpiece or cutting tool, machining accuracy will be adversely affected. Select a cutting tool and machining conditions which do not cause entangling of chips.

SO-NL-B16E/P

FOR SAFE OPERATION -17-

4 CAUTIONS RELATING TO SPINDLE SPEED

The cautions that relate to spindle speed are given below. Observe these cautions during programming.

WARNING

1. The spindle speed limit set using G50 must be no higher than the lowest of the individual allowable speed limits for the chuck, fixture, and cylinder. If you set a higher speed the workpiece will fly out of the machine, causing serious injuries or damage to the machine.

2. In the G96 (constant surface speed control) mode, the spindle speed increases as the cutting tool approaches the center of the spindle.

Near the center of the spindle, the spindle speed will reach the allowable maximum speed of the machine. At this speed, the chuck gripping force, cutting force, and centrifugal force cannot be balanced to hold the workpiece securely in the chuck. As a result, the workpiece will fly out of the machine, causing serious injuries or damage to the machine.

The spindle speed limit must always be specified in a part program by using the G50 command in a block preceding the G96 block, in order to clamp the spindle speed at the specified speed.

3. When a G97 speed command is used in a program, specification of the maximum speed with a G50 command will be ignored. Therefore, when specifying the spindle speed with a G97 command, specify a speed no higher than the lowest speed among the allowable speed limits for the chuck, fixture, and cylinder. If you set a higher speed the workpiece will fly out of the machine, causing serious injuries or damage to the machine. (FANUC)

4. The setting of the spindle speed override switch (if there is one) is valid even when a spindle speed limit is set using G50.

If the switch is set to 110% or 120%, for example, the programmed spindle speed will be overridden in accordance with this setting. If this causes the actual spindle speed to exceed the allowable speed of the chuck, fixture, or cylinder, the workpiece will fly out of the chuck during machining, causing serious injuries or damage to the machine.

Therefore, the spindle speed override switch must be set at 100% or lower.

SO-NL-B16E/P

-18- FOR SAFE OPERATION

When the spindle speed control mode is switched from the G96 mode to the G97 mode, if

NOTE

no spindle speed is specified in the G97 block, the spindle speed obtained in the block immediately preceding the G97 block is used as the spindle speed for the G97 mode operation.

Therefore, if no spindle speed is specified in the G97 block, the spindle speed for the G97 mode will depend on the position of the cutting tool in the block preceding the G97 block, and this could adversely affect machining accuracy and shorten the life of the tool.

When switching the spindle speed control mode to the G97 mode, always specify a spindle speed.

5 CAUTIONS RELATING TO THE RAPID TRAVERSE RATE

The cautions that relate to the rapid traverse rate are given below. Observe these cautions during programming.

WARNING

CAUTION

When setting the G00 mode approach to the workpiece, determine the approach paths carefully, taking the workpiece shape and cutting allowance into consideration. The approach point in the Z-axis direction should be more than "chucking allowance + 10 mm" away from the workpiece end face.

When the spindle is rotating, centrifugal force acts on the chuck jaws, reducing the chuck gripping force. This can cause the workpiece to come out of the chuck.

Unless the approach point is at least "chucking allowance + 10 mm" away from the workpiece end face, the cutting tool could strike the workpiece while moving at the rapid traverse rate if the workpiece does come out of the chuck, or if there is a large amount of material to be removed. This could cause accidents involving serious injuries or damage to the machine.

If X- and Z-axis movements are specified in the same block in the G00 mode, the tool path is not always a straight line from the present position to the programmed end point. Make sure that there are no obstacles in the tool path, remembering that X- and Z-axis movement is at the rapid traverse rate. If the workpiece, fixture or tailstock (if featured) lies in the tool path, it could interfere with the tool, tool holder, or turret head. Depending on the workpiece holding method, there could also be interference with the chuck and chuck jaws. This interference will cause damage to the machine.

SO-NL-B16E/P

6 CAUTIONS RELATING TO CENTER-WORK

The cautions that apply when carrying out center-work or both-center-work are given below.

Observe these cautions during programming. (Applies only to machines equipped with a tailstock.)

FOR SAFE OPERATION -19-

WARNING

CAUTION

In machining programs for both-center-work, specify the M11 command to unclamp the chuck before the M30 command to reset and rewind the

program. If the M11 command is not executed and the (START) switch

is pressed by mistake, automatic operation will start and the operator may be injured.

However, if the M11 command is executed when the center at the spindle side is held by the chuck during programming, the center will fall or shift, which in turn will cause the workpiece to fall, causing damage to the machine. If the center at the spindle side is held by the chuck, do not execute the M11 command. (Applies only to machines equipped with a tailstock.)

In a center-work program, if you program approach movement by specifying the X-axis and Z-axis commands in the same block in the G00 mode, the cutting tool could strike the tailstock.

For center-work, move the Z-axis first and then the X-axis to position the cutting tool at the approach point.

In the cutting tool retraction operation, retract the cutting tool in the X-axis direction first to a point where continuing cutting tool movement does not result in interference with the tailstock. After that, move the Z-axis to the required retraction position. (Applies only to machines equipped with a tailstock.)

SO-NL-B16E/P

-20- FOR SAFE OPERATION

7 CAUTIONS RELATING TO COORDINATE SYSTEM SETTING

The cautions that apply when setting the coordinate system are given below.

Observe these cautions during programming.

WARNING

CAUTION

When the coordinate system is set using G50, the start and end points of the part program must be the same point.

At the end of a part program, the tool wear offset data of the cutting tool used to set the coordinate system must be canceled.

If you do not cancel the tool wear offset data, the X and Y coordinate values will be shifted by the tool wear offset data each time the program is executed. This will shift the start (end) point of the program, which could cause interference between the cutting tool, holder or turret head and the workpiece, chuck, fixture, or tailstock (if featured), causing accidents involving serious injuries or damage to the machine.

1. When setting the coordinate system using the machine coordinate system setting function, any mistake in specifying the X and Z values in the G50 block will cause interference between the cutting tool, tool holder, or turret head, and the workpiece, chuck, fixture, or tailstock (if featured), damage to the machine, or will cause the cutting tool failing to reach the cutting position.

2. When the coordinate system is set using G50, do not input the tool geometry offset data. If you input this data, the workpiece zero point will be shifted by the amount of the tool geometry offset data, which could cause interference between the cutting tool, holder or turret head and the workpiece, chuck, fixture, or tailstock (if featured), causing damage to the machine.

SO-NL-B16E/P

8 CAUTIONS RELATING TO G CODES

The cautions that relate to G codes (also called "preparatory codes") are given below.

Observe these cautions during programming.

FOR SAFE OPERATION -21-

CAUTION

NOTE

1. Never specify "G28 X0 Z0;" to return the axes to the machine zero point, since the axes will first be positioned at the workpiece zero point (X0, Z0) and then moved to the machine zero point, and this may cause the cutting tool to strike the workpiece.

Instead, specify "G28 U0 W0;" to return the axes directly from the present position to the machine zero point.

2. In the G98 mode, the turret moves at the feedrate specified by the F code even when the spindle is not rotating. Make sure that the cutting tool will not strike the workpiece, etc., since this could cause damage to the machine.

3. When using the stored stroke check function, always execute a machine zero return operation after switching the power ON, otherwise the function will not be valid. If the machine is operated in this condition it will not stop even if the cutting tool enters the prohibited area, and this could cause damage to the machine. (stored stroke check specification)

1. When specifying G codes in a block, they must be placed before the addresses (other than G and M) which are executed under the mode they establish. If a G code is specified after addresses for which it establishes the mode of processing, the mode established by it is not valid to these addresses.

2. When executing a dwell using the G04 command, if the cutting tool is kept in contact with the workpiece at a position such as the bottom of a groove for a long time it will shorten the life of the tool nose as well as adversely affecting machining accuracy.

The dwell period should be the time it takes for the spindle to rotate approximately one turn.

SO-NL-B16E/P

-22- FOR SAFE OPERATION

9 CAUTIONS RELATING TO M CODES

The cautions that relate to M codes (also called "miscellaneous codes") are given below. Observe these cautions during programming.

CAUTION

1. Do not stop the spindle or rotary tool (milling specification) by specifying the M05 command while the cutting tool is in contact with the workpiece. If the spindle or rotary tool (milling specification) is stopped while the cutting tool is in contact with the workpiece, the cutting tool could be damaged.

2. Rotate the spindle or rotary tool by executing either M03 or M04 (M13 or M14 for the milling specification) command before the cutting tool comes into contact with the workpiece. If the cutting tool is brought into contact with the workpiece while it is not rotating, the cutting tool could be damaged.

3. Always specify an M05 command to stop spindle rotation before using a pull-out finger or workpiece pusher, etc. If spindle rotation is not stopped the machine could be damaged.

4. Specify the M10 or M11 command in a block without other commands, and specify the G04 command in the next block to allow the chuck to complete the clamp or unclamp operation correctly. Since the time required for the chuck to carry out the clamp or unclamp operation varies depending on the chuck type and chucking pressure, the dwell time should be a little longer than the actual clamp/unclamp time.

If G04 is not specified in the block following the M10 or M11 block, the next block will be executed while the chuck is still opening or closing, and this could cause damage to the machine.

5. When the M73 command is specified, make sure that the turret head or headstock 2 spindle (Applies only to machines equipped with two spindles) is retracted to a position where it will not interfere with the parts catcher when it swings out to the chuck side position. Interference could cause damage to the machine.

6. When the automatic door is closed by specifying the M86 command, make sure that your fingers, etc., do not get caught in the door and that there are no obstacles that will prevent the door from closing. If your fingers are caught in the door you could be injured.

SO-NL-B16E/P

FOR SAFE OPERATION -23-

CAUTION

7. Specify the M25 command (to extend the tailstock spindle) or M26 command (to retract the tailstock spindle) in a block without other commands, and specify the G04 command in the next block to suspend program operation for a period long enough to allow the tailstock spindle to extend and the center to hold the workpiece correctly, or long enough to allow the tailstock spindle to retract into the tailstock correctly.

If G04 is not specified in the block following the M25 or M26 block, the next block will be executed before the workpiece is held by the center properly, or before the tailstock spindle has retracted properly; the tool, holder, or turret head will then interfere with the tailstock spindle or tailstock spindle center, causing damage to the machine.

The period of time specified for suspension of program execution should be longer than the time required to extend or retract the tailstock spindle. (Applies only to machines equipped with a tailstock.)

8. Specify the M73 command (to swing the parts catcher out) or M74 command (to swing the parts catcher in) in a block without other commands, and specify the G04 command in the next block to suspend program operation for a period long enough to allow the parts catcher to complete the swing in/out operation.

If G04 is not specified in the block following the M73 or M74 block, the next block will be executed before the parts catcher has reached the swing in/out end position; the tool, holder, or turret head will then interfere with the parts catcher, causing damage to the machine.

The period of time specified for suspension of program execution should be longer than the time required for the parts catcher to complete the swing IN or swing OUT operation. (Applies only to machines equipped with a parts catcher.)

SO-NL-B16E/P

FOREWORD

Machining workpieces in a CNC lathe requires programs.

This manual describes the items that are required to create programs.

An overview of each chapter is given below.

A: BEFORE PROGRAMMING

This chapter describes the basics for creating a program. It is written for beginners who might be creating a program for the first time.

B: G FUNCTIONS

This chapter describes the G functions. The G codes are also called the preparatory functions. The NC determines the machining method and axis control mode for each block according to the specified G code.

C: M FUNCTIONS

This chapter describes the M functions. The M codes are also called the miscellaneous functions. In addition to serving in auxiliary roles when used with G codes, M codes are used to suspend program execution, discharge or stop coolant, etc.

D: T, S, AND F FUNCTIONS

This chapter describes the T, S, and F functions. The T function rotates the turret to index the required tool and calls the tool offset number. The S function specifies the spindle speed, rotary tool spindle speed or cutting speed. The F function specifies the feedrate of the cutting tool.

E: AUTOMATIC TOOL NOSE RADIUS OFFSET

This chapter describes how the automatic tool nose radius offset function works. Because the cutting edge of the tool does not come to a sharp point, but is slightly rounded, the position of the tool nose actually engaged in cutting differs slightly from the point assumed for program writing. The error caused by this difference is automatically offset by specifying the appropriate G codes (G41, G42).

F: MANUAL TOOL NOSE RADIUS OFFSET

This chapter describes how the value for tool nose offset is determined. Because the tool edge does not come to a sharp point, but is slightly rounded, the position of the tool nose actually engaged in cutting differs slightly from the point assumed for program writing. By manually calculating the offset data and slightly shifting the tool nose, the programmed tool point (imaginary tool nose) can be offset to coincide with the cutting point.

G: CUTTER RADIUS OFFSET

This chapter describes the cutter radius offset function used by the Y-axis specification machines of the SL, SL-S, and TL series. Cutter radius offset means the shift of the tool path by the radius amount to the right or left from the programmed path. This function is mainly used for pocket cutting or contouring with the end mill.

–1–

H: MULTIPLE REPETITIVE CYCLES

This chapter describes the multiple canned cycles. Using a multiple canned cycle, roughing processes that would otherwise require several blocks of commands can be defined by a single block of commands, preceded by a G code that calls a multiple canned cycle. This is followed by blocks that define the finished shape. The tool paths from rough cutting cycles to finishing cycles are generated automatically.

I: HOLE MACHINING CANNED CYCLE

This chapter describes hole machining canned cycle function. It specifies hole machining cycle using commands in one block including a G function, which usually requires several blocks.

J: TOOL LIFE MANAGEMENT B FUNCTION (OPTION)

This chapter describes the tool life management B function. The tool life management B function automatically selects an available tool in a registered tool group if the tool called in the same group has been used to the preset life.

K: EXAMPLE PROGRAMS

This chapter describes the programming procedure using several examples.

APPENDIX

The appendix shows a program for center work with consideration given to safety.

Please read this Programming Manual carefully. The manual is written to help you operate your CNC lathe more effectively.

–2–

BEFORE READING THIS PROGRAMMING MANUAL

To machine a workpiece in a CNC lathe, a program must be created. This manual describes the basic information to be understood before starting programming and several example programs. When reading this manual, always remember the following points.

Also please note that the programs and portions of programs given in this manual are only examples that help readers understand the explanation easier. Therefore, the programs in this manual are not always applicable to actual production. Programming method and numeric values in a program such as machining conditions must be determined meeting actual machine operating environment including the workpiece material and shape.

1 The programmer is requested to read this manual carefully and

observe the cautions it contains when creating programs, so as to ensure the safety of the operator during operation. If the cautions in this manual are ignored when creating a program, the machine may operate in an unexpected manner when the program is run, causing accidents involving serious injuries or damage to the machine.

2 Explanation for programs will include the discussion on

parameters. The parameters are set on shipment in accordance with the machine specifications; do not change them without first consulting Mori Seiki. If the parameters are changed without consultation, the machine may operate in an unexpected manner, causing accidents involving serious injuries or damage to the machine.

1 There are two methods for specifying the coordinate values; an absolute

command and an incremental command. In this manual, the absolute command is usually being described. Unless otherwise stated, the program can also be created using incremental commands. When a specified method using incremental commands is different from one using absolute commands, or if either an absolute or an incremental command cannot be used, some cautionary notes will be described at that point.

Absolute commands and incremental commands are discussed in detail in Chapter A.

For absolute commands and incremental commands, refer to page A–20 (8.).

2 The illustrations used in this manual may vary depending on the machine

model.

3 The contents of this manual apply to machine tools which conform to JIS

standards.

For CNC lathes that have a reversed JIS specification for the X-axis, refer to page A–33 (12.).

–1–

4 The illustrations of cutting tools in this manual may not indicate the correct

setting orientation, since this will differ according to the machine model.

Make sure the correct relationship between the cutting tool mounting position and the workpiece (spindle) rotation direction when writing a program.

5 With G and M codes, standard format and F15 format are available. The

command format differs between standard format and F15 format for some of the G and M codes and such differences are explained in the related items in this manual. Pay attention to the difference when creating a program.

6 Please note that all of the functions and optional devices/equipment

explained in this manual are not always available with the delivered machine.

Retrofitting of such functions and optional devices/equipment is not always possible. For details, contact Mori Seiki.

In this manual, the various models are classified under the generic names indicated in the table below.

Generic Name

SL series SL-150, SL-150MC, SL-150Y

SL-200, SL-200MC SL-250, SL-250MC SL-303, SL-303MC, SL-303Y SL-400, SL-400MC

Models NC Unit

MSC-500 MSC-501 MSG-501 MSD-501

MSD-501II SL-600, SL-600MC SL-25E, SL-65, SL-65MC, SL-75, SL-75MC

SL-S series SL-150S, SL-150SMC, SL-150SY

SL-200S, SL-200SMC

MSC-501

MSD-501II SL-250S, SL-250SMC

VL series VL-25

MSC-500 VL-55, VL-55MC

TL series TL-40, TL-40MC, TL-40Y MSC-518

MSD-518

MSD-518II

LL series LL-7, LL-8 MSC-501

MSD-501II

CL series CL1500, CL1500T

MSC-500 CL2000, CL2000T

–2–

CHAPTER A

BEFORE PROGRAMMING

This chapter describes the basic considerations for creating a program.

A : BEFORE PROGRAMMING

1. What is a Program? A–1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. What is Required of Programmers? A–1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. What is “Creating a Program”? A–2. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. Inputting the Program to the Machine A–2. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5. Flow until the Product is Completed A–3. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 Flow of Operation A–3. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 Check Items A–4. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. Terms for Programming A–8. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 Program Number A–8. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.2 Sequence Number A–9. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3 Part Program A–9. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.4 Address A–10. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5 Data A–10. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.6 Word A–11. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.7 Block A–11. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.8 Summary A–11. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. Axis Control and Direction A–12. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 Movement along the Controlled Axes A–12. . . . . . . . . . . . . . . . . . . . . .

7.1.1 SL, TL Series A–12. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1.2 SL-S Series A–13. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1.3 VL Series A–14. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1.4 LL Series A–15. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1.5 CL Series A–16. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 Expressing Axis Movement in Programming A–17. . . . . . . . . . . . . . . .

8. Specifying the Dimensions A–20. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 Absolute Commands A–20. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2 Incremental Commands A–22. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 Summary A–24. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. Specifying the Cutting Conditions A–25. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10. Basic Pattern of Program A–27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 Chuck-Work Programming A–27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 Center-Work Programming A–28. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.3 Both-Center-Work Programming A–29. . . . . . . . . . . . . . . . . . . . . . . . . . .

11. Cautions for Creating a Program A–30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 Program Number A–30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 Space between the Words in the Program A–30. . . . . . . . . . . . . . . . . .

11.3 Signs and Symbols A–30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4 Inputting a Decimal Point A–31. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5 Role of Decimal Point A–32. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12. JIS Specification and Reverse JIS Specification A–33. . . . . . . . . . . . . . . . . . . .

1. What is a Program?

The “program” here is an instruction for machine operation consisting of letters of the alphabet and numerals in combination.

All operations of the machine, including “spindle rotation”, “tool movement”, or “coolant discharge” can be controlled by a program.

When creating such programs, the information discussed in this manual will be necessary. Please carefully read this manual and thoroughly understand the information before creating a program.

Creating a program is called “programming”.

2. What is Required of Programmers?

BEFORE PROGRAMMING A–1

Programmers must have a thorough of knowledge about machining operation. They should write programs and observe the points listed below to ensure accurate, efficient

operation with safety. Programmers must:

1 Develop a knowledge of the theory of cutting.

2 Acquire a good knowledge of workpiece holding tools (chuck, fixtures, tailstock).

3 To prevent accidents which might occur during machining, select appropriate tools

taking into consideration the shape and material of workpiece as well as machining conditions, such as spindle speed, feedrate or depth of cut.

4 Understand the machining performance of the machine to be used.

5 Understand the safety devices and interlock functions featured by the machine to be

used.

6 Become familiar with the functions related to programming.

A–2 BEFORE PROGRAMMING

3. What is “Creating a Program”?

When creating a program:

1) Check the part print to determine the machining required.

2) Examine the section to be machined, the fixtures and the tools that need to be used. Creating a program as soon as you see a part print could lead to unproductive and dangerous operation of the machine.

3) Determine the machining processes based on these requirements and the dimensions given on the part print.

4) According to the machining processes required, create a program using letters of the alphabet and numerals.

5) When you have created a program, carefully check its contents.

4. Inputting the Program to the Machine

When the program is created, input the program into the NC memory using the keyboard on the NC operation panel. Check the contents of the program that has been input on the screen. A decimal point may be likely to be omitted. To avoid such a careless mistake, write the numerical data in the manner as indicated below.

1 Z.5 → Z0.5

2 X200. → X200.0

After inputting the program, check the input program carefully on input error and omission of the data in the program.

Write the program clearly and accurately so that anyone can read it. If the operator misreads the program and inputs incorrect data, the workpiece could fly out of the chuck during machining, and the cutting tools, holders or turret head, could collide with the workpiece, chuck, fixture or tailstock (tailstock specification), resulting in serious injuries or damage to the machine.

5. Flow until the Product is Completed

5.1 Flow of Operation

This section describes the flow of operation, including programming. Follow and understand the flow so that the operation can be performed smoothly.

1) Examine the drawing to determine the machining required

BEFORE PROGRAMMING A–3

Production planning and programming

Setup operation

Mass production

2) Determine the tools to be used

“TOOLING SYSTEM” in the MAINTENANCE INFORMATION

3) Examine the chucking method and the fixtures

4) Create the program

5) Turn on the power supply

6) Store the program into memory

7) Check or adjust the chucking pressure

8) Shape soft jaws

“SHAPING SOFT JAWS FOR FINISHING” in the OPERATION MANUAL

9) Mount the tools and workpiece to the machine

10) For the center-work, set the tailstock Check or adjust the tailstock spindle thrust (Tailstock specification)

“TURNING ON THE POWER” in the MAINTENANCE INFORMATION “TURNING ON THE POWER” in the OPERATION MANUAL

“PROGRAM EDITING” in the OPERATION MANUAL Instruction manual supplied by the NC unit manufacturer

“Adjusting the pressure” and “ADJUSTING THE CHUCKING PRESSURE” in the OPERATION MANUAL Instruction manual supplied by the NC unit manufacturer

“MANUAL OPERATION” in the OPERATION MANUAL “TOOLING SYSTEM” in the MAINTENANCE INFORMATION

“TAILSTOCK OPERATION” “CAUTIONS ON CHUCKING A WORKPIECE” “ADJUSTING THE TAILSTOCK SPINDLE THRUST” in the OPERATION MANUAL

11) Measure and input the tool geometry offset value

12) Set the workpiece zero point

“SETTING OF COORDINATE SYSTEM” in the OPERATION MANUAL

13) Check the program by carrying out dry run operation (Correct the program if necessary)

14) Check the machining condition by carrying out test cutting (Correct the program if necessary) (Input the tool wear offset value if necessary)

15) Machine the workpiece in automatic operation

16) Product is completed

“SETTING OF COORDINATE SYSTEM” in the OPERATION MANUAL

“PREPARATION BEFORE STARTING MASS PRODUCTION” in the OPERATION MANUAL

A–4 BEFORE PROGRAMMING

Reading the

Conditi

of Machining

Program

5.2 Check Items

The items to be checked in the course of programming and before starting machine operation are summarized in the following tables. Check these items to ensure smooth operation.

Reading the

Drawing

Order and

ons

Check Items

1. Are tolerances readable on the drawing?

2. Are the symbols used to indicate accuracy understandable?

Are the shape and material of the workpiece blank made clear?

Are the processes before and after the processes to be carried out on the

4. NC lathe made clear?

Can the workpiece be machined to the specified accuracies on the NC

5. lathe?

6. Are the keys for machining understandable?

7. Is the use of the workpiece made clear?

8. Have you read all the dimensions and notes on the drawing?

9. Is the drawing kept clean, with no unnecessary information entered on it?

Check Items

Are the order of machining and machining conditions determined in

1. accordance with the shape and material of the workpiece blank?

Are the chucking method and chucking pressure setting determined

2. correctly?

3. Are the cutting tools and replaceable tips selected correctly?

Are the machining processes appropriate for the shape and material of the

4. workpiece blank?

5. Is machining free of interference?

Check

Column

Check

Column

123

64975

Inputting the

Check Items

When inputting the program for a particular process, is the program for the

1. next process taken into consideration?

Is the program being written to suit the shape and material of the workpiece

2. blank?

3. Is a decimal point entered in all numerical values?

4. Is the sign (+, –) preceding numerical values correct?

5. Are feed modes (rapid traverse and cutting feed) used correctly?

6. Are approach paths and cutting feed identified?

7. Is all input data checked for correctness?

8. Is the program free of errors caused by lack of concentration?

(To the next page)

Check

Column

BEFORE PROGRAMMING A–5

Shaping and

Mounting the

Mountin the Tools

Soft Jaws

Check Items

1. Are tool holders and cutting tools cleaned before mounting?

2. Are the replaceable tool tips new?

3. Are the material and shape of replaceable tool tips appropriate?

4. Are replaceable tool tips mounted securely and correctly?

5. Is the tool overhang appropriate?

6. Is the replaceable tool tip mounting angle correct?

7. Are mounting bolts tightened securely and evenly?

8. Is the tool nose center height correct?

Check Items

1. Are the soft jaws and master jaws cleaned before mounting?

2. Are the soft jaw mounting positions correct?

3. Are the soft jaw mounting bolts tightened securely and evenly?

4. Is the mounting bolt length appropriate?

Is the plug (ring) used for shaping the soft jaws to the correct size?

6. Is the chucking pressure checked and adjusted?

7. Is the DOOR INTERLOCK key-switch placed in the NORMAL position?

8. Is the front door closed?

Are the cutting tools, replaceable tool tip, spindle speed, and feedrate all

9. correct for shaping soft jaws?

10. Is the workpiece contact face area appropriate?

11. Is relief provided at the soft jaw corners?

12. Are run-out on I.D. and end face waviness measured?

Check

Column

Check

Column

Tool Offset

Check Items

Is due consideration given to possible interference during measurement of

1. tool offset data?

Are the spindle speed, feedrate, and depth of cut used for the measuring

2. tool offset data appropriate?

3. Is the DOOR INTERLOCK key-switch placed in the NORMAL position?

4. Is the front door closed?

5. Is the standard tool selection appropriate?

6. Is the measured dimension correct?

7. Is the calculation for offset data correct?

8. Is the offset direction correct?

9. Is the tool offset number correct?

Are the tool geometry offset data, tool wear offset data, and coordinate

10. system used for offset identified correctly?

(To the next page)

Check

Column

A–6 BEFORE PROGRAMMING

Dry Run

Operation

Test Cutting

Operation

TEST

Check Items

1. Is the chucking pressure been checked and adjusted?

If performing center work, is the tailstock spindle thrust checked and

2. adjusted?

Is the DOOR INTERLOCK key-switch placed in the NORMAL position?

4. Is the front door closed?

5. Is the single block function turned on?

6. Are the feedrate and spindle speed appropriate for operation?

7. Are the feed modes (rapid traverse and cutting feed) used correctly?

8. Is the tool retraction direction after cutting correct?

9. Is tool movement smooth in the calculated area?

10. Are the tools free of interference with the workpiece, soft jaws, and chuck?

Is the turret head indexed at a position where there is no interference with

11. the workpiece?

12. Can the machine be stopped immediately when necessary?

Check Items

1. Is the chucking pressure been checked and adjusted?

If performing center work, is the tailstock spindle thrust checked and

2. adjusted?

3. Is the DOOR INTERLOCK key-switch placed in the NORMAL position?

4. Is the front door closed?

5. Is the single block function turned on?

6. Are the feedrate and spindle speed appropriate for operation?

Are the order of machining and machining conditions determined in

7. accordance with the shape and material of the workpiece blank?

8. Are cutting tools and replaceable tool tips selected properly?

9. Is the workpiece chucking method correct?

10. Is the progress of cutting been observed?

11. Are coolant supply volume and direction correct?

Are the cutting tools free of interference with the workpiece, soft jaws and

12. chuck?

13. Are the dimensions measured after the rough cutting process?

14. Are the settings for feed override and rapid traverse override correct?

15. Can the machine be stopped immediately when necessary?

Check

Column

Check

Column

(To the next page)

BEFORE PROGRAMMING A–7

Measuring

Production

Mass

Check Items

1. Is the measuring instrument functioning correctly?

2. Is the choice of measuring instrument correct?

3. Is the measuring order correct?

4. Is the measuring method appropriate?

5. Is the area to be measured indicated clearly?

6. Is the area to be measured free of chips and coolant?

7. Are the dimensions measured after the rough cutting process?

8. Is the workpiece cool when the dimensions are measured?

Check Items

1. Is the DOOR INTERLOCK key-switch placed in the NORMAL position?

2. Is the front door closed?

Are all NC functions such as single block functions used to check the

3. program turned off?

4. Is dimensional variation checked?

5. Are run-out on I.D. and O.D., and end face waviness measured?

Is a target work time established on the basis of the machining time for one

6. workpiece?

7. Is tool nose wear observed?

8. Are the dimensions measured after the rough cutting process?

Check

Column

Check

Column

A–8 BEFORE PROGRAMMING

6. Terms for Programming

This section describes the basic terms that must be understood for creating a program.

6.1 Program Number

Several programs can be stored in the NC memory.

Program numbers are used to keep multiple programs arranged in numerical order. Program numbers appear at the beginning of a program stored in the memory.

A program number is set by inputting numbers four digits or less after the alphabet “O”. Numbers from 1 to 9999 can be used.

O0001; Program number

N1;

G50 S2000;

G00 T0101;

... ...

G00 X150.0 Z100.0;

M01;

N2;

G50 S2000;

G00 T0202;

M30;

If a program number to be input is already in the memory, that number, and therefore that program cannot be input. Change its number to input the program.

The program number can have less than four significant digits. It can be input using less than four digits. For example, even if a program number is input as O1, the screen will automatically display “O0001”.

6.2 Sequence Number

The sequence number is used to search for or call the position that is being executed, or to facilitate finding the position you want to edit in the program easily.

The sequence number is expressed as a number of five digits or less (1 to 99999), following the letter “N”.

Generally, the sequence numbers are assigned to the part programs for individual cutting tools in the ascending order in the order the machining processes are executed.

O0001;

N1; Sequence number

G50 S2000;

G00 T0101;

... ...

BEFORE PROGRAMMING A–9

G00 X150.0 Z100.0;

M01;

N2; Sequence number

G50 S2000;

G00 T0202;

M30;

1 If a sequence number consists of more than five digits, the five digits from the

least significant position are recognized as the sequence number.

2 The sequence number is not necessarily specified. Also, it is not necessary to

input numbers with five significant digits.

If a program is too long and exceeds the memory capacity, put the sequence numbers at the beginning of the program for each process, or do not specify these numbers. This will help save memory capacity.

6.3 Part Program

The part program refers to the program which contains all the information necessary for executing the cutting process to be carried out by a single cutting tool.

Each process (1st process, 2nd process...) for machining a component contains the part programs for as many tools as are necessary to complete each process.

A–10 BEFORE PROGRAMMING

O0001;

N1;

G50 S2000;

G00 T0101;

... ...

G00 X150.0 Z100.0;

M01;

N2;

G50 S2000;

G00 T0202;

M30;

Part program for the tool No. 1

Part program for the tool No. 2

6.4 Address

An address is expressed using letters of the alphabet.

6.5 Data

The numbers (including the sign and decimal point) that follow the address are called the “data”.

In addition, the information (program and other) to be input to the NC for machining the workpiece is also called the data. Determine the type of data from the explanation of the statement.

G00 X150.0 Z100.0;

Address

G00 X150.0 Z100.0;

Data

6.6 Word

A word is the minimum unit for specifying functions. A word consists of an address and the data.

6.7 Block

A block is the minimum command unit necessary to operate a machine (including the NC unit). It is also the minimum unit used to create a part program. A block consists of words.

On the program sheet, each one line corresponds to one block.

O0001; First block. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

N1; Second block. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

BEFORE PROGRAMMING A–11

G00 X150.0 Z100.0;

Word

G50 S2000; Third block. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Specify the end of a block with [ ; ].

6.8 Summary

A program consists of words, a combination of address and data, and of blocks, a combination of words, as shown below.

O0001; N1; G50 S2000; G00 T0101;

Word

...

DataAddress

Program number

Sequence number 1 block

Part program

Program

G00 X150.0 Z100.0; M01; N2; G50 S2000; G00 T0202;

M30;

...

Sequence number

Part program

1 block

A–12 BEFORE PROGRAMMING

7. Axis Control and Direction

This section describes movement along the controlled axes and its relationship with the program.

Knowing the direction of the controlled axes is essential when creating a program.

7.1 Movement along the Controlled Axes

This section deals with the axis definition and how the axis movement is defined in programming.

7.1.1 SL, TL Series

In the SL, TL series, the controlled axes and their directions are determined as follows:

Axis

Unit + and – Direction

+ direction: The direction in which the machining

X Turret

diameter increases. (the direction in which a cutting tool moves away from the spindle center line.)

+ direction: The direction in which a cutting tool moves

Z Turret

away from the spindle. (the direction in which the cutting tool is viewed from the spindle.)

(MC type, Y-axis

specification)

(Y-axis

specification)

Spindle

Turret

– direction: The rotation direction in which the

right-hand thread advances when viewing a cutting tool from the spindle.

+ direction: The direction in which a cutting tool moves

up when viewing the machine from the front.

For the X-axis reversed JIS specification machine, positive and negative directions of the X-axis are reversed from those applied to conventional specification machines.

Turret

Headstock

(chuck)

Tailstock

7.1.2 SL-S Series

(MC type, Y-axis

In the SL-S series, the controlled axes and their directions are determined as follows:

BEFORE PROGRAMMING A–13

Axis

X Turret

Z Turret

specification)

(Y-axis

specification)

B Spindle 2

Unit + and – Direction

+ direction: The direction in which the machining

diameter increases. (the direction in which a cutting tool moves away from the spindle (spindle 1 or spindle

2) center line.)

+ direction: The direction in which a cutting tool moves

away from spindle 1. (the direction in which the cutting tool is viewed from spindle 1.)

– direction: The rotation direction in which the

Spindle 1

right-hand thread advances when viewing a cutting tool from spindle 1.

+ direction: The rotation direction in which the

Spindle 2

right-hand thread advances when viewing a cutting tool from spindle 2.

+ direction: The direction in which a cutting tool moves

Turret

up when viewing the machine from the front.

+ direction: The direction in which spindle 2 moves

away from spindle 1. (the direction in which spindle 2 is viewed from spindle 1.)

For the X-axis reversed JIS specification machine, positive and negative directions of the X-axis are reversed from those applied to conventional specification machines.

Turret

Spindle 2

Spindle 1

A–14 BEFORE PROGRAMMING

7.1.3 VL Series

In the VL series, the controlled axes and their directions are determined as follows:

Axis

Unit + and – Direction

+ direction: The direction in which the machining

X Turret

diameter increases. (the direction in which a cutting tool moves away from the spindle center line.)

+ direction: The direction in which a cutting tool moves

Z Turret

away from the spindle. (the direction in which the cutting tool is viewed from the spindle.)

For the X-axis reversed JIS specification machine, positive and negative directions of the X-axis are reversed from those applied to conventional specification machines.

–X

Turret

–Z

Chuck

7.1.4 LL Series

In the LL series, the controlled axes and their directions are determined as follows:

BEFORE PROGRAMMING A–15

Axis

Unit + and – Direction

+ direction: The direction in which the machining

diameter increases.

Front-side turret

Rear-side turret

Front-side turret

Rear-side turret

+ direction: The direction in which the machining

+ direction: The direction in which a cutting tool

(the direction in which a cutting tool moves away from the center of rotation)

diameter decreases. (the direction in which a cutting tool moves toward the center of rotation)

moves away from the workpiece. (the direction in which the cutting tool is viewed from the spindle.)

A–16 BEFORE PROGRAMMING

7.1.5 CL Series

In the CL series, the controlled axes and their directions are determined as follows:

Axis Unit + and – Direction

X Turret

Z Turret

For the X-axis reversed JIS specification machine, positive and negative directions of the X-axis are reversed from those applied to conventional specification machines.

Turret

+ direction: The direction in which the machining

diameter increases. (the direction in which a cutting tool moves away from the spindle center line.)

+ direction: The direction in which a cutting tool moves

away from the spindle. (the direction in which the cutting tool is viewed from the spindle.)

Spindle

7.2 Expressing Axis Movement in Programming

When writing a program, the numerical values used for specifying axis position and positive/negative sign used for determining axis movement direction vary depending on the position taken as the reference for programming.

The reference position (workpiece zero point) and axis movement direction are determined as follows:

BEFORE PROGRAMMING A–17

<SL, TL series>

Headstock

–Z direction

Workpiece zero point

To write a program, the origin for the program, e.g. the workpiece zero point must be determined.

The workpiece zero point (X0, Z0) is taken as the reference for programming and also for machining.

X-axis The diametral dimensions of a product are expressed using

address X. X0 is taken on the center line of the product.

Z-axis The longitudinal dimensions of a product are expressed using

address Z. Z0 is taken on the end face of the finished product.

C-axis

(MC type, Y-axis

Spindle index angle for executing milling is expressed using address C. C0 is taken at the zero point of the C-axis.

specification)

Y-axis

(Y-axis specification)

The dimensions measured in right angle direction to X-axis and Z-axis are expressed using address Y. Y0 is taken on the spindle center line.

Turret

Headstock

+Z direction

–Z direction

+X –Z

–X –Z

+X direction

area

–X direction

area

Workpiece

Workpiece zero point (X0, Z0)

–X

area

+X –Z

Workpiece

–X –Z

+X direction

area

–X

area

–X direction

Turret

Tailstock

area

+Z direction

Workpiece zero point (X0, Z0)

area

<X-axis and Y-axis>

Used in Y-axis specification machine.

–X

area

–X direction

–X

area

–Y

+Y direction

–Y direction

area

Workpiece zero point (X0, Y0)

area

–Y

+X direction

A–18 BEFORE PROGRAMMING

<SL-S series>

+X direction

+X +Z

Workpiece

Workpiece zero point (X0, Z0)

–X +Z

Headstock 1

–Z direction

+X –Z

–X –Z

area

–X direction

In cutting off operation, spindle 2 moves in the Z-axis direction when it receives a workpiece from spindle 1.

With the SL-S series, this movement is made along the B-axis.

area

+Z direction

area

Turret

–Z direction

Workpiece zero point (X0, B0)

+X direction

area

–Z

Workpiece

–X

area

–Z

–X direction

+X +Z

–X +Z

area

Headstock 2

+Z direction

area

–X direction

–X +Z

–X –Z

area

+Z direction

–Z direction

Turret

area

Workpiede zero point (X0, Z0)

+X direction

Workpiece

area

–Z

Headstock

Headstock

–Z direction

–X –Z

–X direction

area

–X

area

Workpiece

+Z direction

Workpiece zero point (X0, Z0)

BEFORE PROGRAMMING A–19

Rear-side turret

Headstock

–Z direction

+X –Z

area

+X direction

+X +Z

area

Front-side turret

Turret

Headstock

+Z direction

–Z direction

+X –Z

–X –Z

+X direction

area

–X direction

area

Workpiece

Workpiece zero point (X0, Z0)

–X

area

+X –Z

Workpiece

–X –Z

+X direction

area

–X

area

–X direction

Turret

Tailstock

area

+Z direction

Workpiece zero point (X0, Z0)

area

A–20 BEFORE PROGRAMMING

8. Specifying the Dimensions

To specify tool movement from the presently located point to the next point (target point), the following two types of commands can be used.

1) Absolute commands

2) Incremental commands

When writing a program, it is necessary to understand the nature of these two types of dimension specifying commands.

This section deals with the basic and the command specifying method for using the absolute and incremental commands in a program.

8.1 Absolute Commands

Absolute commands define a specific point by the distance from the workpiece zero point (X0, Z0) with a (+) or – sign.

1 In a program using absolute commands, the axes are expressed using the

following address characters:

–Z direction

X-axis³X_ ; Z-axis³Z_ ;

2 With the SL-S series, absolute commands of the B-axis is expressed as “B_ ;”.

3 With the Y-axis specification machine, absolute commands of the Y-axis is

expressed as “Y_ ;”.

4 With the MC type and the Y-axis specification machine, absolute commands of

the C-axis is expressed as “C_ ;”.

Specifying the absolute commands (1)

To express tool movement from point

+X direction

+X –Z

–X –Z

area

(10.0, –5.0)

–5 10

Workpiece zero point (X0, Z0)

–X direction

(20.0, 10.0)

area

–X

area

to point 2 using absolute commands.

X20.0 Z10.0;

. . . . . . . . . . . . . . . .

X10.0 Z–5.0;

+Z direction

. . . . . . . . . . . . . . . .

For the X-axis, since dimensions are all expressed in diametral values, actual X-axis movement distance is a half of the specified value.

BEFORE PROGRAMMING A–21

1 The positive (+) sign may be omitted.

X+10.0³X10.0 Z+10.0³Z10.0

2 The values specified as (f, f) in the illustration above indicate the coordinate

values (X, Z).

Specifying the absolute commands (2)

To express tool movement (point

absolute commands.

C10

(X0, Z0)

X40.0

∅ 50

∅ 100

∅ 50

∅ 40 55

³ point 2 ³ point 3 ³ point 4 ³ point 5) using

X40.0 Z0;

X50.0 Z–5.0;

(X50.0) Z–50.0;

X80.0 (Z–50.0);

X100.0 Z–60.0;

. . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . .

Since the commands in ( ) are the same as in the previous block, they can be omitted.

To determine X coordinate of point

, subtract C5

chamfer size (5 mm) from the workpiece diameter 50 mm.

Chamfer size 5 mm should be converted into diametral value.

5 mm 2 = 10 mm

∅50 – (5 2) = 40

∅ 100

X80.0 and 5 Z–60.0

C10

∅ 50

Therefore, X coordinate of point 1 is X40.0.

To determine X coordinate of point

, subtract

C10 chamfer size (10 mm) from the workpiece diameter 100 mm.

Chamfer size 10 mm should be converted into diametral value.

10 mm 2 = 20 mm

∅100 – (10 2) = 80

Therefore, X coordinate of point

To determine Z coordinate of point

is X80.0.

, add

chamfer size 10 mm to 50 mm. Since the Z dimensions are all measured in the negative direction from the workpiece zero point, the calculation should be,

(–50) + (–10) = –60

Therefore, Z coordinate of point

is Z–60.0.

A–22 BEFORE PROGRAMMING

8.2 Incremental Commands

Incremental commands define relative position on a given coordinate system by specifying the motion distance from the present position. The positive sign indicates that the position to be defined is in the positive direction from the present position.

For the B-axis, an incremental command cannot be used.

1 In a program using incremental commands, the axes are expressed using the

following address characters:

X-axis³U_ ; Z-axis³W_ ;

2 With the Y-axis specification machine, incremental commands of the Y-axis is

expressed as “V_ ;”.

3 With the MC type and the Y-axis specification machine, incremental commands

of the C-axis is expressed as “H_ ;”.

Specifying the incremental commands (1)

–Z direction

To express tool movement from point

+X direction

+X –Z

–X –Z

area

(10.0, –5.0)

–5 10

Workpiece zero point (X0, Z0)

–X direction

For the X-axis (U command), since dimensions are all expressed in diametral values, actual X-axis movement distance is a half the specified value.

1 The positive (+) sign may be omitted.

U+10.0³U10.0 W+15.0³W15.0

2 The values specified as (f, f) in the illustration above indicate the coordinate

values (X, Z).

(20.0, 10.0)

area

–X

area

to point 2 using incremental commands.

X20.0 Z10.0;

. . . . . . . . . . . . . . . .

U–10.0 W–15.0 ;

+Z direction

. . . . . . . . . . . . .

Specifying the incremental commands (2)

BEFORE PROGRAMMING A–23

To express tool movement (point

incremental commands.

C10

(X0, Z0)

U10.0 W–5.0

∅ 50

∅ 100

∅ 50

∅ 40 55

³ point 2 ³ point 3 ³ point 4 ³ point 5) using

X40.0 Z0;

U10.0 W–5.0;

(U0) W–45.0;

U30.0 (W0);

U20.0 W–10.0;

. . . . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . .

. . . . . . . . . . . . . . . . .

. . . . . . . . . . . . . .

Since the commands in ( ) are the same as in the previous block, they can be omitted.

X coordinate value of point

of C5 (5 mm) is executed from point

point

is X50.0; chamfering

(X40.0) to

Chamfer size 5 mm should be converted into diametral value.

5 mm 2 = 10 mm

Therefore, coordinate value of U is U10.0.

∅ 100

U30.0 (W0) and 5 U20.0 W–10.0

C10

∅ 50

Z coordinate value of point

is Z–5.0; Z-axis

moves 5 mm in the negative direction from point

(Z0).

Therefore, coordinate value of W is W–5.0.

X coordinate value of point

is X80.0; X-axis

moves 30 mm in the positive direction from point

(X50.0).

Therefore, coordinate value of U is U30.0.

Tool movement from point

to point 4 is

made only in the X-axis direction. In such a case, Z-axis movement command (W0) may be omitted.

X coordinate value of point

is X100.0;

chamfering of C10 (10 mm) is executed from point

(X80.0) to point 5.

Chamfer size 10 mm should be converted into diametral value.

10 mm 2 = 20 mm

Therefore, coordinate value of U is U20.0.

A–24 BEFORE PROGRAMMING

8.3 Summary

Differences between absolute programming and incremental programming are summarized below.

Address Characters

Meaning of the Sign (+/–)

Meaning of the Numerical Values

Reference Point of Commands

Z coordinate value of point

is Z–60.0; Z-axis

moves 10 mm in the negative direction from point

(Z–50.0).

Therefore, coordinate value of W is W–10.0.

Absolute Programming Incremental Programming

X_ Z_ Y_ C_ ; B_ ; U_ W_ V_ H_ ;

The area where the specified point exists.

Coordinate values

(distance from the workpiece zero point, angle of index from the zero point)

Workpiece zero point (X0, Z0, Y0) Zero point (C0) (B0)

The direction in which the cutting tool advances.

Distance of tool movement, angle of spindle index

Actual positions of tool and spindle

1 Generally, a program is written using absolute commands.

Incremental commands are usually used for tool retraction or chamfering operation.

2 Absolute commands and incremental commands may be specified in the same

block such as “X_ W_ ;”, “U_ Z_ ;”, and “X_ V_ ;”.

3 If absolute and incremental commands representing the same axis (X and U, Z

and W, Y and V, or C and H) are specified in the same block, the address character specified later becomes valid.

Example: X10.0 U–20.0; ³ U–20.0 is valid.

9. Specifying the Cutting Conditions

BEFORE PROGRAMMING A–25

Cutting feedrate

Depth of cut

Spindle speed

1) Spindle speed (min

The spindle speed or cutting speed is specified directly following address S (S function).

COMMAND

G97 S400; Spindle speed 400 min

–1

), cutting speed (surface speed) (m/min)

. . . . . . . . . . . .

The cutting conditions that are set when programming have a great influence on the machining efficiency and accuracy. These conditions must be checked carefully.

The following four cutting conditions are necessary for machining the workpiece.

–1

G96 S200; Cutting speed 200 m/min. . . . . . . . . . . .

2) Cutting feedrate (mm/rev) (mm/min)

Feedrate is specified directly following address F (F function).

COMMAND

G99 F0.1; Feedrate per spindle revolution, 0.1 mm/rev. . . . . . . . . . . . .

G98 F100; Feedrate per minute, 100 mm/min. . . . . . . . . . . .

3) Depth of cut

There is no special function used to specify the depth of cut. Depth of cut is specified using tool movement along the X- or Z-axis.

For multiple repetitive cycles, depth of cut may be specified using an address.

For details of multiple repetitive cycles, refer to Chapter H “MULTIPLE REPETITIVE CYCLES”.

A–26 BEFORE PROGRAMMING

4) Chuck gripping force

The chuck gripping force is reduced when the spindle is rotated since the rotation applies centrifugal force to the chuck jaws. This reduction of the chuck gripping force could cause the workpiece to fly out of the chuck during machining, causing serious injuries or damage to the machine. Therefore, when checking a program, measure the chuck gripping force that will actually be applied when the spindle is rotated at the speed used for machining by using a gripping force meter. If the measured chuck gripping force value is lower than that required to hold the workpiece safely, change machining conditions such as the chucking pressure, spindle speed, feedrate, and depth of cut.

Periodically measure the chuck gripping force with a gripping force meter to make sure that the required gripping force is maintained. If it is not, consult the chuck manufacturer and cylinder manufacturer.

For details on the relationship between the spindle rotation speed and chuck gripping force, refer to the instruction manuals prepared by the chuck manufacturer and cylinder manufacturer.

For details of chuck gripping force, refer to the instruction manuals prepared by the chuck and cylinder manufacturers.

10. Basic Pattern of Program

10.1 Chuck-Work Programming

When creating a part program for each tool (O.D. cutting tool, thread cutting tool etc.), the following basic patterns are used.

O0001; Program number (This is specified only once at the beginning of all programs.)

N1; Sequence number (This is specified at the beginning of a part program.)

G50 S_ ; Specifies the maximum spindle speed for clamping. In the G96

(constant surface speed control) mode, spindle speed is clamped at this speed if a command requiring a higher speed is specified.

G00 T0101 M41(M42, M43, M44);

Specifies the tool number, the tool offset number, and the spindle speed range.

G96 S150 M03(M04); G96 specifies the cutting speed (150 m/min).

or,

G97 S150 M03(M04); G97 specifies the spindle or spindle 1 speed (150 min

direction of rotation. M03: Normal M04: Reverse

(G00) X_ Z20.0 M08; Approach to the workpiece at a rapid traverse

G01 X_ Z_ F_ ; Approach to the workpiece at a cutting feedrate to ensure safety.

...... ...

Start of coolant supply

BEFORE PROGRAMMING A–27

–1

) and the

When specifying rapid approach to the workpiece, study the workpiece shape carefully. For the approach in the Z-axis direction, positioning must be made at a point “chucking amount + 10 mm” away from the end face of the workpiece.

Machining program

G00 U1.0 Z20.0 M09; Escape from the machining area, stop of coolant supply

For I.D. cutting, determine the escape stroke depending on the diameter having been machined. Note that the escape U command must be specified as U–_.

X_ Z_ ; Move to a position where the turret head can be rotated. M01; Optional stop

The part program same as *

Part programs are written for each tool.

M01; Optional stop

The part program same as *

The spindle stop command (M05) is entered in the last part program.

Part programs are written for each tool.

M30; End of program

M41 to M44 commands can be specified only for the machine equipped with a transmission.

A–28 BEFORE PROGRAMMING

10.2 Center-Work Programming

O0001; Program number (This is specified only once at the beginning of all programs.)

N1; Sequence number (This is specified at the beginning of a part program.)

G50 S_ ; Specifies the maximum spindle speed for clamping. In the G96

(constant surface speed control) mode, spindle speed is clamped at this speed if a command requiring a higher speed is specified.

G00 T0101 M41(M42, M43, M44);

Specifies the tool number, the tool offset number, and spindle speed range.

G96 S150 M03(M04); G96 specifies the cutting speed (150 m/min).

or,

G97 S150 M03(M04); G97 specifies the spindle speed (150 min

rotation. M03: Normal

M04: Reverse

Z_ M08; Approach to the workpiece (Z-axis direction)

Start of coolant supply

X_ ; Approach to the workpiece (X-axis direction)

... ......... ......

Machining program

–1

) and the direction of

If the cutting tool might interfere with the center, stop the rapid traverse at a safe point and continue the approach at a cutting feedrate (G01). The feedrate for approach should be a little faster than a cutting feedrate.

G00 X_ M09; Escape along the +X-axis, stop of coolant supply Z_ ; Move to a position where the turret head can be rotated. M01; Optional stop

The part program same as *

Part programs are written for each tool.

M01; Optional stop

The part program same as *

The spindle stop command (M05) is entered in the last part program.

Part programs are written for each tool.

M30; End of program

M41 to M44 commands can be specified only for the machine equipped with a transmission.

10.3 Both-Center-Work Programming

O0001; Program number (This is specified only once at the beginning of all programs.)

N1; Sequence number (This is specified at the beginning of a part program.)

G50 S_ ; Specifies the maximum spindle speed for clamping. In the G96

(constant surface speed control) mode, spindle speed is clamped at this speed if a command requiring a higher speed is specified.

G00 T0101 M41(M42, M43, M44);

Specifies the tool number, the tool offset number, and spindle speed range.

G96 S150 M03(M04); G96 specifies the cutting speed (150 m/min).

or,

G97 S150 M03(M04); G97 specifies the spindle speed (150 min

rotation. M03: Normal

Z_ M08; Approach to the workpiece (Z-axis direction)

X_ ; Approach to the workpiece (X-axis direction)

............ ......

Machining program

M04: Reverse

Start of coolant supply

BEFORE PROGRAMMING A–29

–1

) and the direction of

G00 X_ M09; Escape along the +X-axis, stop of coolant supply Z_ ; Move to a position where the turret head can be rotated. M01; Optional stop

The part program same as *

Part programs are written for each tool.

M01; Optional stop

The part program same as *

The spindle stop command (M05) is used in the last part program.

M11; Chuck unclamp command; the STATUS indicator [ CHCL ] goes

off.

Before specifying the M30 command, execute the M11 command. If the M11 command is not executed and the (ST) switch is pressed by mistake, automatic operation will start and the operator may be injured. However, if the workpiece is supported with the center at the spindle side held by the chuck, do not use the M11 command. If the M11 is specified in a program when the center at the spindle side is held by the chuck, the center will fall or shift, which in turn will cause the workpiece to fall, damaging the machine.

M30; End of program

M41 to M44 commands can be specified only for the machine equipped with a transmission.

A–30 BEFORE PROGRAMMING

11. Cautions for Creating a Program

11.1 Program Number

This manual describes all program numbers in a four digit number. However, it is not necessary to write or enter a program number in a four digit number. A program number specified in less than four digit number is recognized and displayed in a four digit number after it is input to the NC. If “O1” is entered, for example, it is recognized and displayed as “O0001”.

An entry of a program number of five or more digits is not permitted.

11.2 Space between the Words in the Program

In this manual, a program is described in the manner as indicated below.

O0001; N1; G50

S2000; . . . . . . . . . . . . . . . . . . .

G00

T0101;

Space

11.3 Signs and Symbols

A program is expressed in a combination of alphabetic letters, positive/negative (+/–) signs, and numbers containing a decimal point. In addition to these, the end of block symbol “;” and the block delete symbol “/” are used.

Block delete function:

If the block delete function is on, the commands beginning with the slash “/” are ignored up to the end of block code “;” in the same block. The program is continuously executed from the block not containing the slash.

In line

, for example, a space is placed between “G50” and “S2000”. When entering a program to the NC, the word-to-word space may not be

inserted.

When a program is input to the NC memory, a space is automatically inserted.

If the block delete function is off, all blocks (even those preceded by a slash) are executed.

The following signs and symbols are also used.

“,” “∗” “

[ ]” “( )” “#” “@”

11.4 Inputting a Decimal Point

For an NC, it is possible to use a decimal point to enter numerical values. A decimal point can be used to express the numerical values that have the unit of “distance”, “angle”, “time”, or “speed”.

The addresses which allow the use of a decimal point are indicated below.

Distance or angle: X, Y, Z, C, U, V, W, H, I, J, K, R, B

Time: U, X

Feedrate: F

If you forget to enter a decimal point in a program entry that requires one and start the machine without noticing the error, the turret may move to an unexpected position, damaging the machine. Check that you have entered decimal points where necessary.

“mm” setting (specified by G21)

X1.0 X1 mm. . . . . .

BEFORE PROGRAMMING A–31

“inch” setting (specified by G20)

X0.001 mm. . . . . . .

(if a decimal point is not entered, it is assumed that the value is specified in the unit of least input increment.)

X1.0 X1 inch. . . . . .

1 There are limits in the usable units depending on addresses. Setting units are

“mm”, “inch”, “degree” and “second”.

X0.0001 inch. . . . . . .

(if a decimal point is not entered, it is assumed that the value is specified in the unit of least input increment.)

X15.0 X15 mm or X15 inches G04 U1.0 Dwell for 1 second F10.0 10 mm/rev, 10 mm/min, 10 inch/rev, or 10 inch/min

2 In the case of a dwell command, a decimal point can be used when address X

is used. However, it is not allowed to use a decimal point if address P is used since address P is also used to specify a sequence number.

1 To call for dwell for 1 hour, specify as

G04 U3600.0 (X3600.0);

(1 hour = 3600 seconds)

2 In a program, or in a block, it is allowed to specify the commands with and

without a decimal point.

X1000 Z23.7; X10.0 Z22359;

A–32 BEFORE PROGRAMMING

11.5 Role of Decimal Point

The following shows how the tool paths are generated if a decimal point is omitted mistakenly.

Use a decimal point carefully

The program to machine the workpiece shape as illustrated below

∅ 100

∅ 90

Rapid traverse

Cutting feed

2 1

If “X90” is entered for “X90.0” in block illustration below.

(G99) G00 X78.0 Z20.0 M08; G01 Z1.0 F2.0; X90.0 Z–5.0 F0.2; Z–60.0; X102.0 Z–66.0; G00 U1.0 Z20.0 M09; X200.0 Z150.0;

...

, the resultant tool paths are generated as in the

3. . . . . . . .

∅ 100

∅ 90

Rapid traverse

Cutting feed

Since the numerical value specified without a decimal point is regarded to have been set in least input increment, “X90” is executed as “X0.09 mm”.

X1.0 = X1 mm

X1 = X0.001 mm

Therefore, use a decimal point when entering numerical values.

BEFORE PROGRAMMING A–33

12. JIS Specification and Reverse JIS Specification

This section explains items to be kept in mind when creating a program in the JIS specification and in the reverse JIS specification.

The following summarizes the items which differ from the programming in the JIS specification when a program is written in the reverse JIS specification.

1) For the X-axis commands, the positive/negative (+/–) sign is reversed.

Addresses for which the sign of the data is reversed: X, U, I

JIS Specification

X100.0 X–100.0

U10.0 U–10.0

I80.0 I–80.0

2) In the circular interpolation, G02 calls for rotation in the counterclockwise (CCW) direction and G03 calls for rotation in the clockwise (CW) direction.

JIS Specification Reverse JIS Specification

G02

G03 CCW

CW CCW

Reverse JIS Specification

A–34 BEFORE PROGRAMMING

3) In the automatic tool nose R offset function (G41, G42), the offset direction is reversed and command position of the imaginary tool nose differs.

Tool position is offset to the left side of the tool paths in reference to the programmed tool moving direction.

G41

Tool moving direction

JIS Specification Reverse JIS Specification

Tool position is offset to the right side of the tool paths in reference to the programmed tool moving

Workpiece

direction.

Tool moving direction

Workpiece

Tool position is offset to the right side of the tool paths in reference to the programmed tool moving direction.

G42

Tool moving direction

Workpiece

JIS Specification Reverse JIS Specification

X+

162

Actual tool nose

Z+

Tool position is offset to the left side of the tool paths in reference to the programmed tool moving direction.

Workpiece

Tool moving direction

X–

483

Actual tool nose

Z+

BEFORE PROGRAMMING A–35

∅ 100

∅ 90

∅ 60

∅ 50

JIS Specification

O0001; G50 S2000; G00 T0101; G96 S180 M03;

G42 X50.0 Z20.0 M08; . . . . . . . . . . . . . .

G01 Z2.0 F1.0; . . . . . . . . . . . . . . . . . . . . .

Z–30.0 F0.2; . . . . . . . . . . . . . . . . . . . . . . .

X60.0 Z–35.0; . . . . . . . . . . . . . . . . . . . . .

X90.0; . . . . . . . . . . . . . . . . . . . . . . . . . . . .

G03 X100.0 Z–40.0 R5.0; . . . . . . . . . . .

G40 G00 U1.0 Z20.0; . . . . . . . . . . . . . . .

X150.0 Z100.0 M09; . . . . . . . . . . . . . . . .

M01;

Rapid traverse

Cutting feed

Reverse JIS Specification

O0001; G50 S2000; G00 T0101; G96 S180 M03;

G41 X–50.0 Z20.0 M08; . . . . . . . . . . . . .

G01 Z2.0 F1.0; . . . . . . . . . . . . . . . . . . . . .

Z–30.0 F0.2; . . . . . . . . . . . . . . . . . . . . . . .

X–60.0 Z–35.0; . . . . . . . . . . . . . . . . . . . .

X–90.0; . . . . . . . . . . . . . . . . . . . . . . . . . . .

G02 X–100.0 Z–40.0 R5.0; . . . . . . . . . .

G40 G00 U–1.0 Z20.0; . . . . . . . . . . . . . .

X–150.0 Z100.0 M09; . . . . . . . . . . . . . . .

M01;

CHAPTER B

G FUNCTIONS

This chapter describes the G functions.

The following G functions are only outlined in this chapter and they are explained in details in Chapters E, G, H, and I, respectively.

– Section 10. “G40, G41, G42 Automatic Tool Nose Radius Offset”: Chapter E

– Section 11. “G40, G41, G42 Cutter Radius Offset”: Chapter G

– Section 15. “G70 - G76 Multiple Repetitive Cycle”: Chapter H

– Section 16. “G80, G83 - G85, G87 - G89 Hole Machining Canned Cycles”: Chapter I

The examples of program given in this chapter all assume tool nose R0.

For the G codes not explained in this chapter, refer to the instruction manual supplied by the NC unit manufacturer.

B : G FUNCTIONS

1. G Code List B–1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. G00 Positioning the Cutting Tool at a Rapid Traverse Rate B–5. . . . . . . . . .

3. G01 Moving the Cutting Tool Along a Straight Path

at a Cutting Feedrate B–10. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. G02, G03 Moving the Cutting Tool Along Arcs

at a Cutting Feedrate B–12. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5. G50 Setting the Spindle Speed Limit B–14. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. G96 Controlling Spindle Speed

to Maintain Surface Speed Constant B–17. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. G97 Controlling Spindle Speed at Constant Speed B–19. . . . . . . . . . . . . . . . .

8. G04 Suspending Program Execution (Dwell) B–22. . . . . . . . . . . . . . . . . . . . . .

9. G98, G99 Setting Feedrate Units B–24. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10. G40, G41, G42 Automatic Tool Nose Radius Offset B–28. . . . . . . . . . . . . . . .

11. G40, G41, G42 Cutter Radius Offset B–30. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12. G32, G92 Thread Cutting

(Continuous Thread Cutting and Thread Cutting Cycle) B–33. . . . . . . . . . . . . .

13. G32 Tapping (On the Center of Spindle) B–49. . . . . . . . . . . . . . . . . . . . . . . . . .

13.1 Cautions on Programming Tapping Using G32 B–50. . . . . . . . . . . . . .

13.1.1 Dwell Command B–50. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.2 Precautions on Using the Tapper B–50. . . . . . . . . . . . . . . . .

13.1.3 To Finish Tapping at Correct Depth in Blind Hole B–51. . .

14. G90, G94 O.D./I.D. Cutting Cycle and Face Cutting Cycle B–53. . . . . . . . . . .

15. G70 - G76 Multiple Repetitive Cycle B–56. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16. G80, G83 - G85, G87 - G89 Hole Machining Canned Cycles B–58. . . . . . . .

17. G22, G23 Setting Barrier to Define the Tool Entry Inhibited Zone B–63. . . . .

18. G28 Returning the Axes to Machine Zero Automatically B–66. . . . . . . . . . . . .

19. G53 Selecting the Machine Coordinate System B–68. . . . . . . . . . . . . . . . . . . .

20. G54 - G59 Setting a Work Coordinate System B–70. . . . . . . . . . . . . . . . . . . . .

21. G38 Workpiece Pushing Check B–73. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22. G07.1 (G107) Cylindrical Interpolation B–76. . . . . . . . . . . . . . . . . . . . . . . . . . . .

23. G12.1 (G112), G13.1 (G113)

Notching (Polar Coordinate Interpolation) B–82. . . . . . . . . . . . . . . . . . . . . . . . . .

24. G479 Tailstock Connect B–85. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

APPENDIX 1 Workpiece Transfer APPENDIX B–1. . . . . . . . . . . . . . . . . . . . . . . .

1.1 Work Coordinate System APPENDIX B–2. . . . . . . . . . . . . . . . . . . . . . .

APPENDIX 2 G65 P9020/G65 P9021 Workpiece Transfer

Macro Program (MSD-501II) APPENDIX B–4. . . . . . . . . . . . . . . .

APPENDIX 3 G65 P9022 Workpiece Ejection

Macro Program (MSD-501II) APPENDIX B–12. . . . . . . . . . . . . . . .

1. G Code List

G codes are also called preparatory functions. The G codes consisting of the address G and a numerical value that follows address G define the machining method and the axis movement mode in a specified block. The NC establishes the control mode in response to the specified G code.

The numerical value following address G defines the commands written in that block. Depending on how the G codes remain valid, they are classified into the following two types:

G FUNCTIONS B–1

Type

Meaning

One-shot G code (G codes in group 00,

The G code is valid only in the specified block.

excluding G10 and G11)

Modal G code (G codes in groups other than group 00)

The G code remains valid until another G code in the same group is specified.

For example, G00 and G01 are both modal codes, that is, they are G codes in the group other than group 00.

G01 X_ Z_ ;

X_ ;

G01 is valid in this range.

Z_ ;

G00 X_ Z_ ;

1 When specifying G codes in a block, they must be placed before the addresses

(other than G and M) which are executed under the mode they establish. If a G code is specified after addresses for which it establishes the mode of processing, the mode established by it is not valid to these addresses.

2 More than one G code, each belonging to a different G code group, may be

specified in the same block.

3 If more than one G code, belonging to the same group, are specified in a block,

the one specified later is valid.

4 If a G code not listed in the G code table or a G code for which the

corresponding option is not selected is specified, an alarm message (No. 010) is displayed on the screen.

5 The NC establishes the G code modes, identified by the symbol, when the

power is turned on or when the

Concerning G54, however, pressing the

(RESET) key is pressed.

RESET

(RESET) key does not establish

RESET

the G code mode of them but the G code selected for each group remains valid.

B–2 G FUNCTIONS

21 06

6 *

: Optional for the Y-axis specification.

: Standard for the MC type and the Y-axis specification.

: Standard for MSD-518 and MSD-501.

: Standard for MSC-518, MSD-518, and MSD-518II.

: Standard for the SL-S series.

: Optional for the MC type and the Y-axis specification.

: Standard for the SL and the SL-S series equipped with MC type and

Y-axis specification (excludes the SL-400, SL-600, SL-65, and SL-75).

: Standard for the Y-axis specification of the SL-S series. Note that the 3rd

zero point is used for the retract position of the X- and Y-axes when moving spindle 2 (B-axis) and cannot be used for other purposes.

: Not available for the MSC-500.

: Standard for the SL-600 series.

: Standard for the MSD-501II of SL-S series.

: Optional for the SL-25E.

: Not available for the VL-25, the LL series and the MSC-500.

: Standard for the Y-axis specification.

: Optional for MSC-500 and MSC-501.

f : Standard

: Option : Not available

Code Group Function Division

G00 Positioning f G01 Linear interpolation f G02

G03

Circular interpolation/helical interpolation, CW (clockwise) f/ * Circular interpolation/helical interpolation, CCW

(counterclockwise)

f/ *

G04 Dwell f

G07.1

(G107)

G10

Cylindrical interpolation

Data setting

G11 Data setting mode cancel

G12.1

(G112)

G13.1

(G113)

Polar coordinate interpolation mode *

Polar coordinate interpolation mode cancel *

G17 XpYp plane Xp: X-axis or its parallel axis f G18 16 ZpXp plane G19 YpZp plane G20 G21

G22

G23

Data input in inch system f Data input in metric system f

Stored stroke check function ON

Stored stroke check function OFF

Yp: Y-axis or its parallel axis Zp: Z-axis or its parallel axis

G FUNCTIONS B–3

20 00

f : Standard

: Option : Not available

Code Group Function Division

G25 G26

Spindle speed variation detection OFF Spindle speed variation detection ON *

G27 Reference point return check f G28 Reference point return f

G30

G30.1 Floating reference point return

G31 Skip function/Multi-step skip function

Second/third, fourth reference point return

G32 Thread cutting f G34

G35

G36 Circular thread cutting, CCW (counterclockwise)

Variable lead thread cutting

Circular thread cutting, CW (clockwise)

G38 00 Workpiece pushing check * G40 Tool nose radius offset cancel/Cutter radius offset cancel f/ * G41 07 Tool nose radius offset, left/Cutter radius offset, left f/ * G42 Tool nose radius offset, right/Cutter radius offset, right f/ * G50 00 Coordinate system setting/Spindle speed limit setting f

G50.2

(G250)

G51.2

(G251)

G52 G53 G54 Work coordinate system 1 selection f* G55 Work coordinate system 2 selection f* G56 G57 G58 Work coordinate system 5 selection f* G59 Work coordinate system 6 selection f* G65 00 Macro call G66 G67

Polygon cutting cancel *

Polygon cutting *

Local coordinate system setting f* Machine coordinate system selection f*

Work coordinate system 3 selection f* Work coordinate system 4 selection f*

Macro modal call Macro modal call cancel

* * *

G70 Finishing cycle f

G71 O.D./I.D. rough cutting cycle/Pocket cutting

G72 Rough facing cycle/Pocket cutting

G73

Closed-loop cutting cycle f

f/f*

G74 Face cut-off cycle, deep hole drilling cycle f G75 O.D./I.D. grooving cycle, cut-off cycle f

G76 Multiple thread cutting cycle/Zigzag infeed mode

f/f*

B–4 G FUNCTIONS

Hole

f : Standard

: Option : Not available

Code Group Function Division

G80 Hole machining canned cycle cancel * G83 Face hole machining cycle * G84 G85 10 G87

Hole

machining

canned cycle

Face tapping cycle * Face boring cycle *

Side hole machining cycle * G88 Side tapping cycle * G89 Side boring cycle *

G90 O.D./I.D. cutting cycle f G92 01 Simple thread cutting cycle f G94 Face cutting cycle f G96 G97 G98 G99

G334

G335

G336 Group command (Tool life management B function)

G337 Skip command (Tool life management B function)

Constant surface speed control f Constant spindle speed command f Feed per minute mode f Feed per revolution mode f Turning on the tool life data registration mode

(Tool life management B function) Turning off the tool life data registration mode

(Tool life management B function)

G338

G339

G340

State flag clear command (Tool life management B function)

Tool life management information reading command (Tool life management B function)

PMC address information reading command

(Tool life management B function) G380 Synchronized tapping cycle cancel * G384 Synchronized tapping cycle *

G479 Tailstock connect (only for the SL, TL and CL series)

G FUNCTIONS B–5

2. G00 Positioning the Cutting Tool at a Rapid Traverse Rate

By specifying the G00 command, all axis movement commands are executed at the rapid traverse rate. In other words, the cutting tool is positioned at the programmed target point at a rapid traverse rate.

The G00 mode is usually used for the following operations:

1) At the start of machining:

To move the cutting tool close to the workpiece.

2) During machining:

To move the cutting tool, retracted from the workpiece, to the next programmed target point.

When moving the cutting tool at a rapid traverse rate during machining, make sure that there are no obstacles in the tool paths.

3) At the end of machining:

To move the cutting tool away from the workpiece.

When setting the G00 mode approach to the workpiece, determine the approach paths carefully, taking the workpiece shape and cutting allowance into consideration. The approach point in the Z-axis direction should be more than “chucking allowance + 10 mm” away from the workpiece end face.

When the spindle is rotating, centrifugal force acts on the chuck jaws, reducing the chuck gripping force. This can cause the workpiece to come out of the chuck.

Unless the approach point is at least “chucking allowance + 10 mm” away from the workpiece end face, the cutting tool could strike the workpiece while moving at the rapid traverse rate if the workpiece does come out of the chuck, or if there is a large amount of material to be removed. This could cause accidents involving serious injuries or damage to the machine.

B–6 G FUNCTIONS

COMMAND

G00 X(U)_ Z(W)_ ;

D G00 Calls positioning at a rapid traverse rate.. . . . . . . . .

D X, Z Specifies the positioning target point at a rapid traverse. . . . . . . . .

rate. The coordinates are specified in absolute values.

D U, W Specifies the positioning target point.. . . . . . . . .

The coordinates are specified in incremental values in reference to the present position.

1 If X- and Z-axis movements are specified in the same block in the G00

mode, the tool path is not always a straight line from the present position to the programmed end point. Make sure that there are no obstacles in the tool path, remembering that X- and Z-axis movement is at the rapid traverse rate. If the workpiece, fixture or tailstock (if featured) lies in the tool path, it could interfere with the tool, tool holder, or turret head. Depending on the workpiece holding method, there could also be interference with the chuck and chuck jaws. This interference will damage the machine.

Page B–9

2 For center-work, move the Z-axis first and then the X-axis to position the

cutting tool at the approach point.

Page B–9

G FUNCTIONS B–7

1 Once the G00 command is specified, it remains valid until another G code in

the same group is specified. G01, G02, and G03 are examples of G codes which belong to the same group.

G codes which remain valid until another G code in the same group is specified are called modal G codes.

For the G code groups, refer to page B–1 (1.).

2 The maximum rapid traverse rate varies among the machine models.

Page D–25 (3.4)

3 The rapid traverse rate is adjustable by using the rapid traverse rate override

switch on the machine operation panel.

4 If the rapid traverse rate override switch is set to “0” during automatic

operation, the programmed rapid traverse is not executed and the operation enters the feed hold mode.

5 In a block where a T code is specified, G00 should be specified.

This G00 command is necessary to determine the cutting tool movement feedrate to execute offset motion.

6 With the SL-400 and SL-600 series machines, if a T code is specified with G00

in the same block, the direction of the axis movement is automatically judged whether it is away from or toward the workpiece from the remaining axis movement distance. If the axis is going to move toward the workpiece, the machine stops with an alarm message (No. 1320) displayed on the screen.

B–8 G FUNCTIONS

Programming using G00

M60 P=2

C1.5

∅ 54

O0001;

N1;

G50 S2000;

G00 T0101;

G96 S200 M03;

X56.0 Z20.0 M08; Positioning at

the cutting tool close to the workpiece

G01 Z0 F1.0; Positioning at 2 at a cutting feedrate, the start. . . . . . . . . . . . . . . . . . . . . .

point of facing

X30.0 F0.15;

G00 X50.0 W1.0; Positioning from

execute O.D. cutting

G01 X54.0 Z–1.0;

Z–5.0;

X56.8;

X59.8 Z–6.5;

Z–23.0 F0.2;

G00 U1.0 Z20.0; Positioning at

from the workpiece at a rapid traverse rate

X200.0 Z150.0 M09; Positioning at

rotated

M01;

Rapid traverse

Cutting feed

at a rapid traverse rate to move. . . . . . . . . . . . . . . . . .

to 4 at a rapid traverse rate to. . . . . . . . . . . . . . . . . .

to move the cutting tool away. . . . . . . . . . . . . . . . . . .

where the turret head can be. . . . . . . . . . . . . . . .

The G00 mode is used to move the cutting tool close to and away from the workpiece.

G00 X(U)_ Z(W)_ ;

If the rapid traverse rates of X-axis and Z-axis are:

X-axis 18000 mm/min

Z-axis 24000 mm/min

G FUNCTIONS B–9

The tool path generated by the simultaneous movement of the two axes in the G00 mode is shown in the illustration.

Z (24000)

Therefore, the tool paths are generated as illustrated below depending on the positional relationship between the start and target points.

Start point

Programmed target point

For center-work, move the Z-axis first and then the X-axis to position the cutting tool at the approach point.

X (18000)

B–10 G FUNCTIONS

3. G01 Moving the Cutting Tool Along a Straight Path at a Cutting Feedrate

By specifying the G01 command, the cutting tool is moved along a straight line to cut a workpiece.

The feedrate is specified with an F code by the distance the cutting tool should be moved while the spindle rotates one turn, or the distance to be moved in a minute.

COMMAND

G01 X(U)_ Z(W)_ F_ ;

D G01 Calls the linear interpolation mode.. . . . . . . . .

D X, Z Specifies the cutting target point.. . . . . . . . .

The coordinates are specified in absolute values.

D U, W Specifies the cutting target point (distance and direction).. . . . . . . . .

The coordinates are specified in incremental values in reference to the present position.

D F Specifies the feedrate in ordinary control. . . . . . . . . . . .

D In the G99 mode, the feedrate is specified in “mm/rev”.

F0.2 0.2 mm/rev. . . . . .

D In the G98 mode, the feedrate is specified in

“mm/min”.

F200 200 mm/min. . . . .

1 Once the G01 command is specified, it remains valid until another G code in

the same group is specified. G00, G02, and G03 are examples of G codes which belong to the same group.

G codes which remain valid until another G code in the same group is specified are called modal G codes.

For the G code groups, refer to page B–1 (1.).

2 The cutting feedrate is adjustable by using the feedrate override switch on the

machine operation panel in the range of 0 to 150%.

3 The feedrate data is “0” until an F code is specified.

If an axis movement command is read before an F code is specified, the machine does not operate. In this case, an alarm message (No. 011) is displayed on the screen.

4 When the power is turned on, the NC is in the G99 (feed per revolution) mode.

Programming using G01

G FUNCTIONS B–11

To move the cutting tool at a cutting feedrate along the paths

³ 6 ³ 7 ³ 8 ³ 9.

M60 P=2

C1.5

∅ 54

O0001; N1; G50 S2000; G00 T0101; G96 S200 M03; X56.0 Z20.0 M08; Positioning at

at a rapid traverse rate to move. . . . . . . . . . . . . . . . . .

the cutting tool close to the workpiece

G01 Z0 F1.0; Positioning at

at a cutting feedrate, the start. . . . . . . . . . . . . . . . . . . . . .

point of facing

X30.0 F0.15; Facing at a feedrate of 0.15 mm/rev. . . . . . . . . . . . . . . . . . . . . .

G00 X50.0 W1.0; Positioning from

to 4 at a rapid traverse. . . . . . . . . . . . . . . . . .

rate, the start point of O.D. machining at a rapid

traverse rate G01 X54.0 Z–1.0; Cutting along path

0.15 mm/rev

Z–5.0; Cutting along path

0.15 mm/rev

X56.8; Cutting along path 6³ 7 at a feedrate of . . . . . . . . . . . . . . . . . . . . . . . . . . . .

0.15 mm/rev

X59.8 Z–6.5; Cutting along path

0.15 mm/rev

Z–23.0 F0.2; Cutting along path

0.2 mm/rev

G00 U1.0 Z20.0; Positioning at

at a rapid traverse rate to move. . . . . . . . . . . . . . . . . . .

the cutting tool away from the workpiece X200.0 Z150.0 M09; Positioning at

where the turret head can be. . . . . . . . . . . . . . . .

rotated M01;

³ 3, and 4 ³

³ 5at a feedrate of . . . . . . . . . . . . . . . . . .

³ 6at a feedrate of . . . . . . . . . . . . . . . . . . . . . . . . . . . .

³ 8at a feedrate of . . . . . . . . . . . . . . . . . . . . . .

³ 9at a feedrate of . . . . . . . . . . . . . . . . . . . . . .

Rapid traverse

Cutting feed

B–12 G FUNCTIONS

4. G02, G03 Moving the Cutting Tool Along Arcs at a Cutting Feedrate

By specifying the G02, G03 command, the cutting tool is moved along an arc to cut a workpiece.

COMMAND

G02(G03) X(U)_ Z(W)_ R_ F_ ; G02(G03) X(U)_ Z(W)_ I_ K_ F_ ;

D G02 Calls the circular interpolation . . . . . . . . .

mode in the clockwise direction.

D G03 Calls the circular interpolation . . . . . . . . .

mode in the counterclockwise direction.

D X, Z Specifies the end point of the arc.. . . . . . . . .

The coordinates are specified in absolute values.

D U, W Specifies the end point of the arc (distance and direction).. . . . . . . . .

The coordinates are specified in incremental values in reference to the present position.

D R Specifies the radius of the arc.. . . . . . . . . . . .

D I Specifies the distance and the direction from the start point. . . . . . . . . . . . .

of the arc to the center of the circle in the X-axis direction. The value should be specified as a radius.

D K Specifies the distance and the direction from the start point. . . . . . . . . . . .

of the arc to the center of the circle in the Z-axis direction.

D F Specifies the feedrate in ordinary control. . . . . . . . . . . .

D In the G99 mode, the feedrate is specified in “mm/rev”.

F0.2 0.2 mm/rev. . . . . .

D In the G98 mode, the feedrate is specified in

“mm/min”.

F200 200 mm/min. . . . .

G02

G03

1 If an R command and a pair of I and K commands are specified in the same

block, the R command is given priority and the I and K commands are ignored.

2 For the arc whose central angle is larger than 180_, an R command cannot be

used.

In this case, use I and K commands to define the arc.

3 When I and K commands are used to specify the distance and direction to the

center of an arc while X and Z commands are omitted or the start and end points lie at the same position, a full circle (360_) is defined. If an R command is used instead of I and K commands, no axis movement results.

G FUNCTIONS B–13

4 To cut a half-circle accurately or to accurately define the center of an arc of

which the center angle is close to 180_, use I and K commands instead of an R command.

If an R command is used, there are cases that the center of a half-circle or an arc of which the center angle is close to 180_ cannot be set accurately due to calculation error.

Programming using G02 or G03

To move the cutting tool at a cutting feedrate along the arc

∅ 32

15°

∅ 44

³ 3.

Rapid traverse

Cutting feed

O0001;

N1;

G50 S2000;

G00 T0101;

G96 S200 M03;

X47.069 Z20.0 M08;

G01 Z1.0 F1.0; Positioning at

to move the cutting tool close to. . . . . . . . . . . . . . . . . . . .

the workpiece

Z0 F0.2; Positioning at

at a feedrate of 0.2 mm/rev. . . . . . . . . . . . . . . . . . . . . . . . . .

G02 X43.205 Z–1.482 R2.0 F0.07; Cutting an arc of 2 mm radius in the clockwise. . .

direction at a feedrate of 0.07 mm/rev

G01 X32.0 Z–22.392; Cutting along path

³ 4 at a feedrate of . . . . . . . . . . . . . . .

0.07 mm/rev

Z–41.0 F0.1; Cutting along path 4 ³ 5 at a feedrate of . . . . . . . . . . . . . . . . . . . . . .

0.1 mm/rev

G00 U–1.0 Z20.0; Positioning at

at a rapid traverse rate to move. . . . . . . . . . . . . . . . . .

the cutting tool away from the workpiece

X200.0 Z150.0 M09; Positioning at

where the turret head can be. . . . . . . . . . . . . . . .

rotated

M01;

B–14 G FUNCTIONS

5. G50 Setting the Spindle Speed Limit

The spindle speed limit for an automatic operation is set with the G50 command.

If the programmed spindle speed is faster than the limit value set in the G50 block, actual spindle speed is clamped at the set limit speed.

1 The spindle speed limit set using G50 must be no higher than

the lowest of the individual allowable speed limits for the chuck, fixture, and cylinder. If you set a higher speed the workpiece will fly out of the machine, causing serious injuries or damage to the machine.

2 In the G96 (constant surface speed control) mode, the spindle

speed increases as the cutting tool approaches the center of the spindle.

The spindle speed limit must always be specified in a part program by using the G50 command in a block preceding the G96 block, in order to clamp the spindle speed at the specified speed.

COMMAND

G FUNCTIONS B–15

G50 S_ ;

D G50 Calls the mode to specify the spindle speed limit for. . . . . . . . .

automatic operation.

–1

D S Specifies spindle speed limit (min

1 The setting of the spindle speed override switch (if there is one)

is valid even when a spindle speed limit is set using G50.

Therefore, the spindle speed override switch must be set at 100% or lower.

).. . . . . . . . . . . .

2 When a G97 speed command is used in a program,

specification of the maximum speed with a G50 command will be ignored. Therefore, when specifying the spindle speed with a G97 command, specify a speed no higher than the lowest speed among the allowable speed limits for the chuck, fixture, and cylinder. If you set a higher speed the workpiece will fly out of the machine, causing serious injuries or damage to the machine.

An alarm message (No. 245) is displayed on the screen if a T command is specified in the G50 block.

B–16 G FUNCTIONS

Programming using G50 (Setting the spindle speed limit)

To move the cutting tool at a cutting feedrate along the path

∅ 54

M60 P=2

C1.5

O0001; N1;

G50 S2000; Setting the spindle speed limit for automatic. . . . . . . . . . . . . . . . . . . . . . .

operation at 2000 min

G00 T0101;

G96 S200 M03; Starting the spindle or spindle 1 in the normal. . . . . . . . . . . . . . . . . . . .

direction; surface speed is 200 m/min The spindle speed is controlled to maintain the surface speed constant at 200 m/min.

X56.0 Z20.0 M08; Positioning at

at a rapid traverse rate to move. . . . . . . . . . . . . . . . . .

the cutting tool close to the workpiece

G01 Z0 F1.0; Positioning at

at a cutting feedrate, the start. . . . . . . . . . . . . . . . . . . . . .

point of facing

X30.0 F0.15; Facing at a feedrate of 0.15 mm/rev. . . . . . . . . . . . . . . . . . . . . .

In order to maintain the surface speed constant, the spindle speed increases as the cutting tool moves closer to the workpiece center to reach the allowable maximum speed of the machine. However, since spindle speed limit is set at

–1

2000 min

in the “G50 S2000”, the spindle speed

does not exceed this limit value.

G00 X50.0 W1.0; G01 X54.0 Z–1.0;

... ... ...

³ 3to execute facing.

Rapid traverse

Cutting feed

–1

Machining program

G00 U1.0 Z20.0; X200.0 Z150.0 M09; M01;

G FUNCTIONS B–17

6. G96 Controlling Spindle Speed to Maintain Surface Speed Constant

The G96 command is used to maintain surface speed constant at the specified value.

The surface speed is also called the cutting speed. It indicates the distance the cutting tool moves along the workpiece surface (periphery) per minute.

When the surface speed is specified with the G96 command, the spindle speed is automatically controlled to maintain the surface speed constant as the cutting diameter varies. This mode is used to maintain the cutting conditions constant.

For example, if the cutting speed (V) is specified at 100 m/min to cut a 30 mm diameter (D) workpiece, the spindle speed (N) is calculated as indicated below.

1000V

N =

π@D

1000 100

N =

Therefore, the spindle rotates at 1061 min

3.14 30

1061 min

Generally, the standard cutting speed is determined according to the material of the workpiece and the cutting tool, the workpiece shape, and the chucking method.

COMMAND

–1

G96 S_ M03(M04);

D G96 Calls the constant surface speed control mode.. . . . . . . . .

D S Specifies the cutting speed (m/min).. . . . . . . . . . . .

D M03(M04) Specifies spindle or spindle 1 rotation in the normal. . . .

(reverse) direction.

In the G96 (constant surface speed control) mode, the spindle speed increases as the cutting tool approaches the center of the spindle.

The spindle speed limit must always be specified in a part program by using the G50 command in a block preceding the G96 block, in order to clamp the spindle speed at the specified speed.

–1

B–18 G FUNCTIONS

Programming using G96

To move the cutting tool at a cutting feedrate along the path 2 ³ 3 to execute facing.

M60 P=2

C1.5

O0001;

N1;

G50 S2000; Setting the spindle speed limit for automatic. . . . . . . . . . . . . . . . . . . . . . .

G00 T0101;

G96 S200 M03; Starting the spindle or spindle 1 in the normal. . . . . . . . . . . . . . . . . . . .

X56.0 Z20.0 M08; Positioning at 1at a rapid traverse rate to move. . . . . . . . . . . . . . . . . .

G01 Z0 F1.0;

X30.0 F0.15; Facing at a feedrate of 0.15 mm/rev. . . . . . . . . . . . . . . . . . . . . .

G00 X50.0 W1.0;

G01 X54.0 Z–1.0;

...

Machining program

∅ 54

operation at 2000 min

–1

Rapid traverse

Cutting feed

direction; surface speed is 200 m/min

The spindle speed is controlled to maintain the surface speed constant at 200 m/min.

the cutting tool close to the workpiece

1000V

N = =

π@D

1000 200

3.14 56

1137 (min–1)

At this position, the spindle or spindle 1 rotates at 1137 min–1 in the normal direction.

1000V

N = =

π@D

1000 200

3.14 30

2123 (min–1)

At this position, the spindle or spindle 1 should

–1

rotate at 2123 min

to provide the surface speed

of 200 m/min. However, since the spindle speed

–1

limit of 2000 min

is set in the “G50 S2000”, the

spindle speed does not exceed this limit value.

G00 U1.0 Z20.0;

X200.0 Z150.0 M09;

M01;

G FUNCTIONS B–19

7. G97 Controlling Spindle Speed at Constant Speed

The G97 command is used to call the mode in which a constant spindle speed is maintained.

During automatic operation, the spindle rotates at the programmed speed.

1000V

N =

π@D

N: Spindle speed (min

V: Cutting speed (m/min)

D: Cutting diameter (mm) π: Circumference constant

The G97 command must be specified for thread cutting operation and turning drilling operation at the center of workpiece end face.

During thread cutting operation, the thread is cut gradually by changing the cutting diameter for each thread cutting path while maintaining the start point of the thread. Therefore, if the spindle speed is not kept constant, the start point shifts in each thread cutting cycle making thread cutting impossible or tipping the tool nose.

–1

)

The G97 mode is also specified for carrying out copy turning on straight bar workpiece.

COMMAND

G97 S_ M03(M04);

D G97 Calls the constant spindle speed command mode.. . . . . . . . .

D S Specifies the spindle speed (min

D M03(M04) Specifies spindle or spindle 1 rotation in the normal. . . .

(reverse) direction.

When a G97 speed command is used in a program, specification of the maximum speed with a G50 command will be ignored. Therefore, when specifying the spindle speed with a G97 command, specify a speed no higher than the lowest speed among the allowable speed limits for the chuck, fixture, and cylinder. If you set a higher speed the workpiece will fly out of the machine, causing serious injuries or damage to the machine.

–1

).. . . . . . . . . . . .

B–20 G FUNCTIONS

When the spindle speed control mode is switched from the G96 mode to the G97 mode, if no spindle speed is specified in the G97 block, the spindle speed obtained in the block immediately preceding the G97 block is used as the spindle speed for the G97 mode operation.

When switching the spindle speed control mode to the G97 mode, always specify a spindle speed.

Programming using G97

To execute O.D. thread cutting

M60 P=2

∅ 57.4

G FUNCTIONS B–21

Rapid traverse

Cutting feed

O0001;

N1;

G00 T0101;

G97 S640 M03; Starting the spindle or spindle 1 at 640 min

normal direction

X70.0 Z20.0 M08;

G01 Z5.0 F1.0 M24; Positioning at

, the start point of the G92 thread. . . . . . . . . . . . . . . .

cutting cycle.

G92 X59.4 Z–24.0 F2.0;

X58.9;

X58.5;

X58.1; Execution of the G92 thread cutting cycle. . . . .

X57.8; (

³ 2 ³ 3 ³ 4 ³ 1 )

X57.56;

X57.36;

X57.26;

G00 X200.0 Z150.0 M09; Positioning at

where the turret head can be. . . . . . . . . . .

rotated

M05;

M30;

–1

in the. . . . . . . . . . . . . . . . . . . .

B–22 G FUNCTIONS

8. G04 Suspending Program Execution (Dwell)

The G04 command is used to suspend program execution during automatic operation for the period specified in the program.

This function is called the dwell function, and is used in operation such as the grooving operation.

If dwell is specified at the bottom of the groove, the tool stops moving. The spindle keeps rotating while the tool stays at the bottom of the groove.

By rotating the spindle one turn while locating the tool at the bottom of the groove, the groove profile accuracy is improved and uncut portion is eliminated. The dwell function is also used for opening and closing the chuck when the machine is equipped with the air blow, the bar feeder or the loader.

When executing a dwell using the G04 command, if the cutting tool is kept in contact with the workpiece at a position such as the bottom of a groove for a long time it will shorten the life of the tool nose as well as adversely affecting machining accuracy.

COMMAND

G04 X_ ; G04 U_ ; G04 P_ ;

D G04 Calls the dwell function.. . . . . . . . .

D X, U Specifies the period in which the program execution is. . . . . . . . .

suspended. The dwell period should be specified in units of seconds with a decimal point.

X1.0 (U1.0) 1 sec. . .

X1 (U1) 0.001 sec. . . . . .

D P Specifies the period in which the program execution is. . . . . . . . . . . .

suspended. The dwell period should be specified in units of 0.001 second without a decimal point.

P1000 1 sec. . . . . . .

1 A decimal point cannot be used when address P is used.

Dwell for 1.5 seconds G04 P1500;. . . . . . . .

Dwell for 2.3 seconds G04 P2300;. . . . . . . .

2 Programmable dwell period is 0.001 to 99999.999 seconds.

3 The dwell function is valid only in the specified block.

4 Dwell period per revolution of the spindle is calculated as follows:

t (sec) =

5 An alarm message (No. 245) is displayed on the screen if a T command is

specified in the G04 block.

60 (sec)

Spindle speed (min–1)

Programming using G04

To cut a 3 mm wide groove.

5 4

∅ 69

C0.5

∅ 56

M60 P=2

G FUNCTIONS B–23

Rapid traverse

Cutting feed

O0001; N1; G50 S1500; Setting the spindle speed limit at 1500 min

automatic operation to ensure safety G00 T0101;

G96 S100 M03; Starting the spindle or spindle 1 in the normal. . . . . . . . . . . . . . . . . . . .

direction at cutting speed of 100 m/min X70.0 Z20.0 M08; Positioning at

to move the cutting tool close to. . . . . . . . . . . . . . . . . .

the workpiece at a rapid traverse rate G01 Z–26.0 F1.0; Positioning at

, the start point of grooving at a. . . . . . . . . . . . . . . . . .

cutting feedrate X68.0 Z–25.0 F0.07; Cutting along path

³ 3 at a feedrate of . . . . . . . . . . . . . . . .

0.07 mm/rev

X56.0 F0.1; Cutting along path

³ 4 at a feedrate of . . . . . . . . . . . . . . . . . . . . . . .

0.1 mm/rev

G04 U0.2; Suspending program execution for 0.2 seconds at. . . . . . . . . . . . . . . . . . . . . . . . .

the bottom of the groove to allow spindle to rotate

one turn

Spindle speed at

1000V

N = = 569 (min–1)

π@D

Period required for the

spindle to rotate one turn

1000 100

3.14 56 60

= 0.11 (sec)

569

–1

for. . . . . . . . . . . . . . . . . . . . . . .

G00 X60.8

...

M01;

To suspend program execution at the groove bottom for more than one turn of the spindle, dwell period is determined to 0.2 seconds.

The following program may be used instead of “G04 U0.2;” G04 X0.2; or G04 P200;

Machining program

B–24 G FUNCTIONS

9. G98, G99 Setting Feedrate Units

Axis feedrate units are determined by specifying the following two G codes:

G98

The G98 command calls the mode in which axis feedrates specified by F codes are interpreted in units of mm per minute. This mode is used when the bar feeder, the pull-out finger, or the rotary tool is used.

G99

The G99 command calls the mode in which the axis feedrates specified by F codes are interpreted in units of mm per revolution.

This mode is used for general turning operations such as O.D. cutting, I.D. cutting, and thread cutting.

In the G98 mode, the turret moves at the feedrate specified by the F code even when the spindle is not rotating. Make sure that the cutting tool will not strike the workpiece, etc., since this could damage the machine.

G98;

G01 Z_ F100.0; The cutting tool moves at a rate of 100 mm/min even . . . .

when the spindle is not rotating.

COMMAND

G98; Specifies the feedrate per minute (mm/min). . . . . .

G99; Specifies the feedrate per revolution (mm/rev). . . . . .

1 The G98 and G99 commands are modal.

Therefore, once the G98 command is specified, it remains valid until the G99 command is specified, or vice versa.

2 When the power is turned on, the G99 mode (feedrate per revolution) is set.

Programming using G99

To execute O.D. cutting in the G99 mode

M60 P=2

C1.5

G FUNCTIONS B–25

O0001;

N1;

(G99;) Since the G99 command is specified, the F codes. . . . . . . . . . . . . . . . . . . . . . . . . . . .

G50 S2000;

G00 T0101;

G96 S200 M03;

X56.0 Z20.0 M08;

G01 Z0 F1.0;

X30.0 F0.15;

G00 X50.0 W1.0;

G01 X54.0 Z–1.0;

Z–5.0;

X56.8;

X59.8 Z–6.5;

Z–23.0 F0.2;

G00 U1.0 Z20.0;

X200.0 Z150.0 M09;

M01;

∅ 54

Rapid traverse

Cutting feed

are interpreted in units of “mm/rev”.

B–26 G FUNCTIONS

Programming using G98

To use the pull-out finger for bar machining operation in the G98 mode

The workpiece is pulled out of the chuck with the pull-out finger mounted in the turret head while the spindle rotation is stopped.

Always specify an M05 command to stop spindle rotation before using a pull-out finger or workpiece pusher, etc. If spindle rotation is not stopped the machine could be damaged.

G98 (feedrate per minute)

G00 (rapid traverse)

O0001; N1;

G00 T0101 M05;

X0 Z20.0 M09; Positioning at

workpiece

G98; Establishing the “mm/min” mode. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

In the following blocks, the F codes are all interpreted in the unit of “mm/min”.

G01 Z–60.0 F500; Positioning at

workpiece (bar stock)

M11; Unclamping of the chuck. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

G04 U2.0; Dwell for 2 seconds to ensure unclamping of the. . . . . . . . . . . . . . . . . . . . . . . . .

chuck

The dwell period should be a little longer than the time required for the chuck to operate (open, close) to ensure safe operation.

Z–10.0; Moving to

stock from the chuck

M10; Clamping of the chuck. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

G04 U2.0; Dwell for 2 seconds to ensure clamping of the. . . . . . . . . . . . . . . . . . . . . . . . .

chuck

Rapid traverse

Cutting feed

at a rapid traverse rate to grip the. . . . . . . . . . . . . . . . . . . . .

at 500 mm/min to grip the. . . . . . . . . . . . . . . . . .

at 500 mm/min to pull out the bar. . . . . . . . . . . . . . . . . . . . . . . . . . .

The dwell period should be a little longer than the time required for the chuck to operate (open, close) to ensure safe operation.

G FUNCTIONS B–27

G00 Z20.0; Positioning at

the bar stock from the pull-out finger

X200.0 Z50.0; Positioning at

rotated

G99; Selecting the G99 (mm/rev) mode. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

In the following blocks, the F codes are all interpreted in the unit of “mm/rev”.

M01

N2;

(G99;)

G00 T0202;

G96 S120 M03;

... ... ...

Machining program

at a rapid traverse rate to release. . . . . . . . . . . . . . . . . . . . . . . .

where the turret head can be. . . . . . . . . . . . . . . . . . . . .

B–28 G FUNCTIONS

10. G40, G41, G42 Automatic Tool Nose Radius Offset

The tool nose does not have a sharp edge but is rounded as illustrated on the left. Therefore, the point of the tool nose used for programming is offset from the actual cutting point. The tool nose radius offset function is used to eliminate

Programmed point

Actual cutting point

R: Tool nose radius

For details on the automatic tool nose radius offset (G40, G41 and G42), refer to Chapter E, “AUTOMATIC TOOL NOSE RADIUS OFFSET”.

dimensional errors caused by this difference.

If taper or arc cutting is programmed without taking into consideration the tool nose radius, overcut or undercut will occur.

The G41 and G42 commands are specified in a program to automatically eliminate this overcut or undercut by offsetting for the tool nose radius.

COMMAND

G01(G00) G41 X_ Z_ F_ ; G01(G00) G42 X_ Z_ F_ ; G01(G00) G40 X_ Z_ I_ K_ F_ ;

D G01(G00) Calls the interpolation mode in which the tool nose radius. . . .

offset function is specified.

G00 Rapid traverse. .

G01 Cutting feed. .

D G41 Calls the tool nose radius offset (left) function.. . . . . . . . .

The tool position is offset to the left in reference to the tool advancing direction.

D G42 Calls the tool nose radius offset (right) function.. . . . . . . . .

The tool position is offset to the right in reference to the tool advancing direction.

D G40 Cancels the tool nose radius offset function.. . . . . . . . .

D X, Z Specifies the coordinate values of the end point.. . . . . . . . .

D I, K The direction of the workpiece shape defined in the. . . . . . . . . .

following block. The I and K commands are specified in incremental values (I: in radius).

D F Specifies the feedrate. . . . . . . . . . . .

G42

Tool advancing direction

Workpiece

G41

mori seiki SL-150, 150MC, 150Y, SL-150S, 150SMC Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

CONTENTS

SIGNAL WORD DEFINITION

FOR SAFE OPERATION

1 CONSIDERATIONS BEFORE OPERATING THE MACHINE

2 SAFETY PRACTICES DURING PROGRAMMING

3 TO ENSURE HIGH ACCURACY

4 CAUTIONS RELATING TO SPINDLE SPEED

5 CAUTIONS RELATING TO THE RAPID TRAVERSE RATE

6 CAUTIONS RELATING TO CENTER-WORK

7 CAUTIONS RELATING TO COORDINATE SYSTEM SETTING

8 CAUTIONS RELATING TO G CODES

9 CAUTIONS RELATING TO M CODES

FOREWORD

BEFORE READING THIS PROGRAMMING MANUAL

CONTENTS

1. What is a Program?

2. What is Required of Programmers?

3. What is “Creating a Program”?

4. Inputting the Program to the Machine

5. Flow until the Product is Completed

5.1 Flow of Operation

5.2 Check Items

6. Terms for Programming

6.1 Program Number

6.2 Sequence Number

6.3 Part Program

6.4 Address

6.5 Data

6.6 Word

6.7 Block

6.8 Summary

7. Axis Control and Direction

7.1 Movement along the Controlled Axes

7.1.1 SL, TL Series

7.1.2 SL-S Series

7.1.3 VL Series

7.1.4 LL Series

7.1.5 CL Series

7.2 Expressing Axis Movement in Programming

8. Specifying the Dimensions

8.1 Absolute Commands

8.2 Incremental Commands

8.3 Summary

9. Specifying the Cutting Conditions

10. Basic Pattern of Program

10.1 Chuck-Work Programming

10.2 Center-Work Programming

10.3 Both-Center-Work Programming

11. Cautions for Creating a Program

11.1 Program Number

11.2 Space between the Words in the Program

11.3 Signs and Symbols

11.4 Inputting a Decimal Point

11.5 Role of Decimal Point

12. JIS Specification and Reverse JIS Specification

CONTENTS

1. G Code List

2. G00 Positioning the Cutting Tool at a Rapid Traverse Rate

3. G01 Moving the Cutting Tool Along a Straight Path at a Cutting Feedrate

4. G02, G03 Moving the Cutting Tool Along Arcs at a Cutting Feedrate

5. G50 Setting the Spindle Speed Limit

6. G96 Controlling Spindle Speed to Maintain Surface Speed Constant

7. G97 Controlling Spindle Speed at Constant Speed

8. G04 Suspending Program Execution (Dwell)

9. G98, G99 Setting Feedrate Units

10. G40, G41, G42 Automatic Tool Nose Radius Offset