Morii-Seiiki ZL-153, ZL-153MC, ZL-153S, ZL-153SMC, ZL-203 PROGRAMING Manual

...

PROGRAMMING MANUAL

Applicable Model

ZL-153, 153MC ZL-153S, 153SMC ZL-203, 203MC ZL-203S, 203SMC ZL-253, 253MC ZL-253S, 253SMC ZT1000Y ZT2500MC, ZT2500Y AZL2400

Applicable NC Unit

MSG-501

Before starting operation, main tenance, 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-NLTTMSG501-A2E

 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.

whole or in part, is not permitted without the written consent of Mori Seiki.

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

Machine Information

Description of machine: CNC lathe

Model name:

Machine serial No.:

Manufacturing date:

Representative:

Business hours: 8:30 - 17:30

FOR SAFE OPERATION SIGNAL WORD DEFINITION 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

K: EXAMPLE PROGRAMS APPENDIX INDEX

FOR SAFE OPERATI O N

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 CNC 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 the instruction manual, ladder diagrams and parameter tables are also supplied with the machine to help with electrical maintenance, and there is an electrical circuit diagram in the document compartment inside the control panel. Please make use of this material 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-B8E/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-B8E/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, chec k that there is nobod y 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 w hile the po wer is switched on, it must be carried out by a qualified electrical engineer, taking the proper precautions; there is a danger of electric shock.

SO-NL-B8E/P

-4- FOR SAFE OPERATION

DANGER

WARNING

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.

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 pu tting 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. Always keep the front door closed during machine operation. Leaving the machine running or operating it with the front door 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 or crushed by its moving parts, struck by a workpiece or soft jaws if they fly out of the chuck, 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-B8E/P

FOR SAFE OPERATION -5-

WARNING

6. The machine specifications are set before shipping so that the machine can deliver its full performance. Changing the settings without consultation may lead to accidents involving serious injuries, impaired machine performance, and considerable shortening of the machine service life. 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.

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 relevan t 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-B8E/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-B8E/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 suppor ted by t he 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-B8E/P

-8- FOR SAFE OPERATION

WARNING

CAUTION

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.

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.

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.

SO-NL-B8E/P

FOR SAFE OPERATION -9-

CAUTION

NOTE

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

SO-NL-B8E/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-B8E/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 pr ogram entry. Be aware that the program will be up dated if progr am editing operations are carried out with the operation selection key-switch at the "operation and edit enable" position. If the progra m is executed af ter 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 ser ious i njur ies o r dama ge to the mac hine. Incor rect setti ng could also distort the workpiece.

SO-NL-B8E/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 standar d conditions, whic h are not necessa rily 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 manuf acturer. 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 tu rr et to the ir or iginal posit ions 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 seri ous operator injurie s or damage t he machine. The workpiece could also be machined with the wrong tool, and the cutting tool could be damaged.

SO-NL-B8E/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 pro gram e ntry t hat r equire s 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 workpiec e grip ping 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.

SO-NL-B8E/P

-14- FOR SAFE OPERATION

WARNING

CAUTION

17. 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.

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.

SO-NL-B8E/P

FOR SAFE OPERATION -15-

CAUTION

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 an d cu t tin g t ool may collide or interfere wi t h ea ch ot he r, 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.

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.

SO-NL-B8E/P

-16- FOR SAFE OPERATION

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.

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

SO-NL-B8E/P

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.

FOR SAFE OPERATION -17-

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-B8E/P

-18- FOR SAFE OPERATION

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 highe r 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)

SO-NL-B8E/P

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.

FOR SAFE OPERATION -19-

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 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 cou ld also be interference with the chuck and chuck jaws. This interference will cause damage to the machine.

SO-NL-B8E/P

-20- FOR SAFE OPERATION

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.)

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 automatic operation (cycle 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-B8E/P

FOR SAFE OPERATION -21-

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-B8E/P

-22- FOR SAFE OPERATION

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.

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 limit 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 limit 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-B8E/P

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.

FOR SAFE OPERATION -23-

CAUTION

1. Do not stop the spindle or rotary tool spindle (milling specification) by specifying the M05 command while the cutting tool is in contact with the workpiece. This could cause damage to the cutting tool.

2. Start the spindle or rotary tool spindle by executing either the M03 or M04 command or the M13 or M14 command (milling specification) 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, it 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-B8E/P

-24- FOR SAFE OPERATION

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 com ma nds , and speci fy 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-B8E/P

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.

DANGER

WARNING

CAUTION

COMMAND

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.

The format identified by this symbol gives information for programming.

Indicates an imminently hazardous situation which, if not avoided, will result in death or serious injury.

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

Indicates a potentially hazardous situation which, if not avoided, could result in death or serious injury.

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

Indicates the items that must be taken into consideration.

NOTE

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.

Ex.

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 PROGR AMMING

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. 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.

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.

-1-

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

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.

WARNING

CAUTION

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-23 (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-38 (13).

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.

-1-

CAUTION

NOTE

5. With G and M codes, two types of formats such as F18 format and F15 format are available. The programming method varies between these two formats 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.

Before shipping the machine, the format is set to the F18 format.

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 Models NC Unit

ZL series ZL-153, ZL-153MC

MSG-501 ZL-203, ZL-203MC ZL-253, ZL-253MC

ZL-S series ZL-153S, ZL-153SMC

MSG-501 ZL-203S, ZL-203SMC ZL-253S, ZL-253SMC

ZT series ZT1000Y

MSG-501 ZT2500MC, ZT2500Y

AZL2400 AZL2400 MSG-501

-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-2

3 WHAT IS "CREATING A PROGRAM"?. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-3

4 INPUTTING THE PROGRAM TO THE MACHINE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-4

5 FLOW UNTIL THE PRODUCT IS COMPLETED . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-5

5-1 Flow of Operation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-5

5-2 Check Items . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-6

6 TERMS FOR PROGRAMMING . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-12

6-1 Program Number. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-12

6-2 Sequence Number . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-13

6-3 Part Program. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-13

6-4 Address. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-14

6-5 Data. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-14

6-6 Word . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-15

6-7 Block . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-15

6-8 Summary. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-15

7 AXIS CONTROL AND DIRECTION . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-16

7-1 Movement along the Controlled Axes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-16

7-1-1 ZL Series . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-16

7-1-2 ZL-S Series . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-17

7-1-3 AZL2400 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-18

7-1-4 ZT Series . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-19

7-2 Expressing Axis Movement in Programming. . . . . . . . . . . . . . . . . . . . . . . . . . . . A-20

8 SPECIFYING THE DIMENSIONS. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-23

8-1 Absolute Commands. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-23

8-2 Incremental Commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-26

8-3 Summary. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-28

9 SPECIFYING THE CUTTING CONDITIONS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-29

10 FUNCTIONS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-31

11 BASIC PATTERN OF PROGRAM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-32

11-1 Chuck-Work Programming . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-32

11-2 Center-Work Programming . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-33

11-3 Both-Center-Work Programming. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-34

12 CAUTIONS FOR CREATING A PROGRAM. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-35

12-1 Program Number. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-35

12-2 Space between the Words in the Program . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-35

12-3 Signs and Symbols . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-35

12-4 Inputting a Decimal Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-36

12-5 Role of Decimal Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . A-37

13 JIS SPECIFICATION AND REVERSE JIS SPECIFICATION . . . . . . . . . . . . . . . . . . . . A-38

1 WHAT IS A PROGRAM?

O0001;

N1;

G50 S2000;

G00 T0101;

BEFORE PROGRAMMING A-1

What do you think of when you hear the term "program"? Do you think of a program for a sporting event, an

educational exercise, or for operating a computer? Generally speaking, a program is an instructional statement that contains the contents of plan or is written to work in conformity with certain rules.

A program is required to operate an NC machine tool.

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

A good program is essential for the operation of the NC machine tools. Programs are specified by inputting an alphabet and the numerals which succeed it.

A part of program is shown in the left. The explanation given below discusses the items

necessary for writing such programs. Please read this manual carefully for creating programs.

A-2 BEFORE PROGRAMMING

2 WHAT IS REQUIRED OF PROGRAMMERS?

Programmers must have a knowledge of machining. They should write programs based on this knowledge, and also observe the points listed below, to ensure accurate, efficient and safe operation.

Programmers must:

1. Develop a knowledge of the theory of cutting.

2. Acquire a knowledge of workpiece holding tools (chuck, fixtures, tailstock) in order to determine the machining method that ensures safe and accurate operation.

3. Determine the appropriate tools by taking into consideration the shape and material of workpiece, spindle speed, feedrate, and depth of cut, to prevent accidents which might occur during machining.

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.

3 WHAT IS "CREATING A PROGRAM"?

What kind of actions are required to create a program?

1) Checking a drawing to determine the machining required.

The drawing must be checked carefully to know what is required.

2) Examine the section to be machined, and determine the fixtures and tools that need to be used.

Some people create a program immediately , as soon as they see drawing. This kind of impatience can lead to unproductive and very dangerous operation of the machine.

BEFORE PROGRAMMING A-3

Process Description Tool No.

1 2

O.D. rough cutting O.D. finishing

01 02

O0001;

N1;

G50 S2000;

G00 T0101;

3) Determine the machining processes required based on the information and dimensions given in the drawing.

Machining process: O.D. rough cutting in the first process and O.D. finishing in the second process.

4) To create the machining process, first write down the program required as a combination of letters and numerals on paper.

5) After a program has been created, carefully check its contents.

A-4 BEFORE PROGRAMMING

4 INPUTTING THE PROGRAM TO THE MACHINE

After the program is created, input the program into the NC memory using the keyboard on the NC operation panel.

The contents of a program that has been input can be checked on the screen. Execute the program. The machine operates according to the program commands.

There may be cases that a decimal point is not input mistakenly. To avoid such careless mistake, the programmer should 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.

WARNING

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 lead to the workpiece being machined with the wrong tool, or to damage to the cutting tool.

For the methods required to input a program to the NC, or to execute the program, refer to the OPERATION MANUAL separately provided.

BEFORE PROGRAMMING A-5

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

roduction lanning and rogramming

Setup operation

2) Determine the tools to be used

3) Examine the chucking method and the fixtures

4) Create the program

5) Turn on the power supply

"TURNING ON THE POWER" in the OPERATION MANUAL

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)

"TOOLING SYSTEM" in the MAINTENANCE INFORMATION

"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 OPER ATION" in the OPERATION MANUAL "TOOLING SYSTEM" in the MAINTENANCE INFORMATION

"T AI LSTOCK OPERATION", "ADJUSTING THE PRESSURE", and

in the OPERAT ION MANUAL

Thrust"

"Adjusting the Tailstock Spindle

Mass production

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 S YSTEM" in the OPERATION MANUAL

"PREPARATION BEFORE STARTING PRODUCTION" in the OPERATION MANUAL

MASS

"PREPARATION BEFORE STARTING MASS PRODUCTION" in the OPERATION MANUAL

A-6 BEFORE PROGRAMMING

NOTE

1. Operation steps 4) and 7) above should be skipped when a program is created using the conversational programming function.

2. Operation step 6) above should be skipped when the conversational programming function is not used for creating 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.

1. Are tolerances readable on the drawing?

2. Are the symbols used to indicate accuracy understandable?

Reading the

Drawing

3. 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?

Check Items

Check

Column

Order and

Conditions of

Machining

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

4. workpiece blank?

5. Is machining free of inte rfere nc e?

Check

Column

(To the next page)

BEFORE PROGRAMMING A-7

Inputting the

Program

Check Items

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

1. next process taken into consideration?

Is the program bein g wri tten to suit the shape and ma teri al 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?

Check Items

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

2. Are the replaceable tool tips new?

Check

Column

Check

Column

Mounting the

Tools

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?

(To the next page)

A-8 BEFORE PROGRAMMING

Shaping and Mounting the

Soft Jaws

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?

5. 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 c ontact 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

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 sele cti on app ropri ate ?

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?

Check

Column

(To the next page)

BEFORE PROGRAMMING A-9

Dry Run

Operation

Check Items

1. Is the chucking pressure checked and adjusted? If performing center work, is the tailstock spindle thrus t 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?

7. Are 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

Column

(To the next page)

A-10 BEFORE PROGRAMMING

Test Cutting

Check Items

1. Is the chucking pressure checked and adjusted? If performing center work, is the tailstock spindle thrus t 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 the cutting tools and replaceable tips selected properly?

9. Is the workpiece chucking method correct?

10. Is the progress of cutting 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?

Check

Column

Measuring

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

15. Can the machine be stopped immediately when necessary?

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

Column

(To the next page)

BEFORE PROGRAMMING A-11

Mass

Production

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

A-12 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.

Ex.

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

NOTE

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.

Ex.

O0001; N1; Sequence number G50 S2000; G00 T0101;

BEFORE PROGRAMMING A-13

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-14 BEFORE PROGRAMMING

Ex.

O0001; N1; G50 S2000; G00 T0101;

G00 X150.0 Z100.0; M01;

N2; G50 S2000; G00 T0202;

M30;

6-4 Address

An address is expressed using letters of the alphabet.

Part program for the tool No. 1

Part program for the tool No. 2

G00 X150.0 Z100.0;

6-5 Data

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

NOTE

Address

G00 X150.0 Z100.0;

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.

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

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

BEFORE PROGRAMMING A-15

G00 X150.0 Z100.0;

Word

Specify the end of a block with [ ; ].

NOTE

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; Program number N1; Sequence number G50 S2000; 1 block G

00 T 0101;

Address + Data

Word

G00 X150.0 Z100.0;

Part program

Program

M01; N2; Sequence number G50 S2000; G00 T0202;

M30; 1 block

Part program

A-16 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 ZL Series

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

Axis Unit + and - Direction

X Turret 1 + direction: The direction in which the machining diameter

Turret 2

increases.

Z Turret 1 + direction: The direction in which a cutting tool moves

away from the spindle.

thread advances when viewing a cutting tool

(MC type)

Turret 2

Spindle - direction: The rotation direction in which the right-hand

from the spindle.

For the X-axis reversed JIS specification machine, positive and negative directions of the

NOTE

X-axis are reversed from those applied to conventional specification machines.

Turret 1

Spindle (Spindle 1)

Turret 2

7-1-2 ZL-S Series

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

Axis Unit + and - Direction

X Turret 1 + direction: The direction in which the machining diameter

Z Turret 1 + direction: The direction in which a cutting tool moves

Turret 2

BEFORE PROGRAMMING A-17

increases.

away from spindle 1.

(MC type)

Z2 (B) Spindle 2 + direction: The direction in which spindle 2 moves away

For the X-axis reversed JIS specification machine, positive and negative directions of the

NOTE

X-axis are reversed from those applied to conventional specification machines.

Spindle 1 - direction: The rotation direction in which the right-hand

thread advances when viewing a cutting tool from spindle 1.

Spindle 2 + direction: The rotation direction in which the right-hand

thread advances when viewing a cutting tool from spindle 2.

from spindle 1.

Turret 1

Spindle 2

Spindle 1

Turret 2

A-18 BEFORE PROGRAMMING

7-1-3 AZL2400

For AZL2400, the controlled axes and their directions are determined as follows:

Axis Unit + and - Direction

X Turret 1 + direction: The direction in which the machining diameter

Turret 2

Z Turret 1 + direction: The direction in which a cutting tool moves

Turret 2

E Spindle + direction: The direction in which the spindle moves

increases.

away from the spindle.

toward the operator when viewing the machine from the front.

NOTE

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.

2. For E-axis movements, the spindle IN/OUT M codes (M369/M368) are used.

Turret 1

Turret 2

7-1-4 ZT Series

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

Axis Unit + and - Direction

BEFORE PROGRAMMING A-19

X Turret 1 + direction: The direction in which the machining diameter

Turret 2

Z Turret 1 + direction: The direction in which a cutting tool moves

Turret 2

increases.

away from spindle 1.

Spindle 1

(MC type, Y-axis

specification)

B Spindle 2 + direction: The direction in which spindle 2 moves away

(Y -axis

specification)

For the X-axis reversed JIS specification machine, positive and negative directions of the

NOTE

X-axis are reversed from those applied to conventional specification machines.

Spindle 1 - direction: The rotation direction in which the right-hand

thread advances when viewing a cutting tool from spindle 1.

Spindle 2 + direction: The rotation direction in which the right-hand

thread advances when viewing a cutting tool from spindle 2.

from spindle 1.

Turret 1 + direction: The direction in which a cutting tool moves up

when viewing the machine from the front.

Spindle 2

Turret 1

–

Turret 2

A-20 BEFORE PROGRAMMING

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:

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

specification)

Y-axis

(Y-axis specification)

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

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

Headstok

-Z direction

-Z

-X

-Z

+X direction

area

-X direction

area

Workpiece

Workpiece zero point (X0, Z0)

-X area

Turret 1

+Z direction

Headstock

-Z direction

Workpiece

-X direction

-X area area

-Z

area

-Z +X direction

-X +Z

+Z direction

Workpiece zero point (X0, Z0)

area

Tailstock

Turret 2

BEFORE PROGRAMMING A-21

<ZL-S series>

Headstock 1

-Z direction

Headstock 1

-Z direction

+X direction

area

-Z

-X

area area area area

-Z

-X direction

area

Workpiece

Workpiece zero point (X0, Z0)

-X +Z

Turret 1

+Z direction

Turret 1

Workpiece

-Z direction

Workpiece zero point (X0, Z0)

+X direction

area area

-Z

-X

-Z

-X direction

+X +Z

-X +Z

-X direction

-X

area

-Z

area area area area

-Z +X direction

-X

area

Workpiece

+Z direction

Workpiece zero point (X0, Z0)

+X +Z

Turret 2

Workpiece

-Z direction

Workpiece zero point (X0, Z0)

Turret 2

-X direction

-X area area

-Z

-Z +X direction

-X +Z

+X +Z

Headstock 2

+Z direction

Headstock 2

+Z direction

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

NOTE

workpiece from spindle 1. With the ZL-S series, this movement is made along the B-axis.

A-22 BEFORE PROGRAMMING

Headstock 1

-Z direction

Headstock 1

-Z direction

+X direction

area

-Z

-X

area area area area

-Z

-X direction

area

Workpiece

Workpiece zero point (X0, Z0)

-X +Z

Turret 1 Turret 1

+Z direction

Workpiece

-Z direction

Workpiece zero point (X0, Z0)

+X direction

area area

-Z

-X

-Z

-X direction

+X +Z

-X +Z

-X direction

-X

area

-Z

area area area area

-Z +X direction

-X

area

Workpiece

+Z direction

Workpiece zero point (X0, Z0)

+X +Z

Workpiece

-Z direction

Workpiece zero point (X0, Z0)

Turret 2 Turret 2

-X direction

-X area area

-Z

-Z +X direction

-X +Z

+X +Z

Headstock 2

+Z direction

Headstock 2

+Z direction

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

NOTE

workpiece from spindle 1. With the ZT series, this movement is made along the B-axis.

<X-axis and Y-axis>

Used in Y-ax i s speci fic at ion machi ne .

-X

-X direction

-X

-Y

+Y direction

area area

-Y direction

+X +Y

-Y

Workpiece zero point (X0, Y0)

+X direction

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:

X-axis X_ ; Z-axis Z_ ;

BEFORE PROGRAMMING A-23

2. With the ZL-S and ZT 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_ ;".

A-24 BEFORE PROGRAMMING

Specifying the absolute commands (1)

Ex.

To express tool movement from point 1 to point 2 using absolute commands.

-Z

Z direction

-X

-Z

area

(10.0, -5.0)

-5

NOTE

+X direction

X10.0 Z-5.0; . . . . . . . . . . . . . . . . . . . . . . . . . . .

X20.0 Z10.0; . . . . . . . . . . . . . . . . . . . . . . . . . . .

Workpiece zero point (X0, Z0)

-X direction

area

+Z direction

-X

area

(20.0, 10.0)

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

1. The positive (+) sign may be omitted.

X+10.0 X10.0 Z+10.0 Z10.0

2. The values specified as ( , ) in the illustration above indicate the coordinate values (X, Z).

BEFORE PROGRAMMING A-25

Specifying the absolute commands (2)

Ex.

To express tool movement (point 1 2  3 4 5) using absolute commands.

C10

X40.0

(X0, Z0)

X40.0 Z0; . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

X50.0 Z-5.0; . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

(X50.0) Z-50.0; . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

100

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.

T o determine X coordinate of point 1, 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

40 55

50 - (5  2) = 40 Therefore, X coordinate of point 1 is X40.0.

100

4 5

X80.0 and Z-60.0

C10

To determine X coordinate of point 4, 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 4 is X80.0. To determine Z coordinate of point 5, 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 5 is Z-60.0.

A-26 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.

NOTE

1. In a program using incremental commands, the axes are expressed using the following address characters:

X-axis U_ ; Z-axis W_ ;

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)

Ex.

-Z

Z direction

-X

-Z

To express tool movement from point 1 to point 2 using incremental commands.

+X direction

X20.0 Z10.0; . . . . . . . . . . . . . . . .

U-10.0 W-15.0; . . . . . . . . . . . . . .

area

(10.0, -5.0)

-5

NOTE

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.

area

+Z direction

-X

area

(20.0, 10.0)

1. The positive (+) sign may be omitted.

U+10.0  U10.0 W+15.0  W15.0

2. The values specified as ( , ) in the illustration above indicate the coordinate values (X, Z).

BEFORE PROGRAMMING A-27

Specifying the incremental commands (2)

Ex.

To express tool movement (point 1 2 3 4 5) using incremental commands.

4 3

C10

(X0, Z0)

U10.0 W-5.0

X40.0 Z0; . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

U10.0 W-5.0; . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

(U0) W-45.0; . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

U30.0 (W0); . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

100

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 2 (5 mm) is executed from point 1

Chamfer size 5 mm should be converted into diametral value.

is X50.0; chamfering of C5

(X40.0) to point 2.

5 mm  2 = 10 mm

40 55

Therefore, coordinate value of U is U10.0. Z coordinate value of point 2 is Z-5.0; Z-axis moves 5 mm

in the negative direction from point 1 (Z0). Therefore , coordinate value of W is W-5.0.

4 5

U30.0 (W0) and U20.0 W-10.0

C10

100

X coordinate value of point 4 is X80.0; X-axis moves 30

mm in the positive direction from point 3 (X50.0). Therefore, coordinate value of U is U30.0.

Tool movement from point 3 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 5 is X100.0; chamfering of

C10 (10 mm) is executed from point 4 (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. Z coordinate value of point 5 is Z-60.0; Z-axis moves 10

mm in the negative direction from point 4 (Z-50.0). Therefore , coordinate value of W is W-10.0.

A-28 BEFORE PROGRAMMING

8-3 Summary

Differences between absolute programming and incremental programming are summarized below.

Absolute Programming Incremental Programming

Address Characters

Meaning of the Sign (+/-)

Meaning of the Numerical Values

Reference Point of Commands

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; U-20.0 is valid.

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

BEFORE PROGRAMMING A-29

9 SPECIFYING THE CUTTING CONDITIONS

Feed

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) (/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

G98 F45;. . . . . . Angular feedrate per minute, 45/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 the following cycles, depth of cut may be specified using an address.

NOTE

 Multiple repetitive cycles  Hole machining canned cycles (high-speed deep hole machining cycle and deep

hole drilling cycle) for the MC type and Y-axis specification machines

For details of multiple repetitive cycles and hole machining canned cycles, refer to CHAPTER H, "MULTIPLE REPETITIVE CYCLES" and CHAPTER I, "HOLE MACHINING CANNED CYCLE".

A-30 BEFORE PROGRAMMING

4. Chuck gripping force

WARNING

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 w ith a g ripping 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 FUNCTIONS

A program is created using alphabets which show functions, and numerical values. The G, M, S, F, and T functions represent the main functions.

Details of each function are described in Chapter B and succeeding chapters. The following table gives an overview of functions:

Code Functions

G code

M code

S code Specifies the spindle speed and the cutting speed.

BEFORE PROGRAMMING A-31

Specifies the machining method in each block of a program or movement along an axis. Proceeding from this command, the NC prepares for movement in each block. For this reason, the G function is called a preparatory function.

Example: G00. . . . . . . . Rapid traverse of axes

Is called the miscellaneous function and works as the function to support the functions call ed by the G cod e. It specifies ON/OFF control of machine operations, including program stop, coolant discharge or stop, and spindle rotation or stop etc.

Example: M08 . . . . . . . Coolant discharge

M09 . . . . . . . Coolant stop

F code Specifies the feedrate of the tool. T code Specifies the tool number and the tool length offset number.

A-32 BEFORE PROGRAMMING

11 BASIC PATTERN OF PROGRAM

11-1 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; N1; G50 S_ ;

Program number (This is specified only once at the beginning of all programs.) Sequence number (This is specified at the beginning of a part program.)

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(M 42, M43 , M 44 );

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);

(G00) X_ Z20.0 M08;

G01 X_ Z_ F_ ;

Machining program

G97 specifies the spindle or spindle 1 speed (150 min-1) and the direction of rotation.

M03: Normal M04: Reverse

Approach to the workpiece at a rapid traverse Start of coolant supply

When specifying rapid approac h to the workpiece , study the

NOTE

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.

Approach to the workpiece at a cutting feedrate to ensure safety.

G00 U1.0 Z20.0 M09;

X_ Z_ ; M01;

The part program same as *

M01;

The part program same as *

M30;

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

NOTE

transmission.

Escape from the machining area, stop of coo lan t supp ly

For I.D. cutting, determine the escape stroke depending on

NOTE

the diameter having been machined. Note that the escape

U command must be specified as U-_. Move to a position where the turret head can be rotated. Optional stop

Part programs are written for each tool. Optional stop

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

11-2 Center-Work Programming

BEFORE PROGRAMMING A-33

O0001; N1; G50 S_ ;

Program number (This is specified only once at the beginning of all programs.) Sequence number (This is specified at the beginning of a part program.)

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(M 42, M43 , M 44 );

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);

Z_ M08;

X_ ;

Machining program

G97 specifies the spindle or spindle 1 speed (150 min-1) and the direction of rotation. M03: Normal M04: Reverse

Approach to the workpiece (Z-axis direction) Start of coolant supply Approach to the workpiece (X-axis direction)

If the cutting tool might interfere with the center, stop the

NOTE

rapid traverse at a safe point and conti nue the app roach at a

cutting feedrate (G01). T he feedr ate for app roach s hould be

a little faster than a cutting feedrate.

G00 X_ M09; Z_ ; M01;

The part program same as *

M01;

The part program same as *

M30;

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

NOTE

transmission.

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

Part programs are written for each tool. Optional stop

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

A-34 BEFORE PROGRAMMING

11-3 Both-Center-Work Programming

O0001; N1;

Program number (This is specified only once at the beginning of all programs.) Sequence number (This is specified at the beginning of a part program.)

G50 S_;

G00 T0101 M41(M 42, M43 , M 44 );

G96 S150 M03(M04); or, G97 S150 M03(M04);

Z_ M08;

X_ ;

Machining program

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.

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

G96 specifies the cutting speed (150 m/min).

G97 specifies the spindle or spindle 1 speed (150 min-1) and the direction of rotation. M03: Normal M04: Reverse

Approach to the workpiece (Z-axis direction) Start of coolant supply Approach to the workpiece (X-axis direction)

If the cutting tool might interfere with the center, stop the

NOTE

rapid traverse at a safe point and con tinue the appr oach at a

cutting feedrate (G01). The feedrate for approach should

be a little faster than a cutting feedrate.

G00 X_ M09; Z_ ; M01;

The part program same as *

M01;

The part program same as *

M11;

M30;

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

Part programs are written for each tool. Optional stop

The spindle stop command (M05) is entered in the last part program. Chuck unclamp command; the STATUS indicator [CHCL] goes off.

WARNING

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.

End of program

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

NOTE

transmission.

BEFORE PROGRAMMING A-35

12 CAUTIONS FOR CREATING A PROGRAM

12-1 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.

NOTE

12-2 Space between the Words in the Program

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

O0001; N1; G50 G00

S2000; T0101;

Space

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

12-3 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:

NOTE

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.

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

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.

The following signs and symbols are also used. "," "*" "[ ]" "( )" "#" "@"

A-36 BEFORE PROGRAMMING

12-4 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

WARNING

NOTE

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

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

X1. . . . . . . . X0.001 mm or X0.0001 mm

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

"inch" setting (specified by G20)

X1.0 . . . . . . X1 inch

X1. . . . . . . . X0.0001 inch or X0.00001 inch

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

"inch", "degree" and "second".

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;

12-5 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

Ex.

The program to machine the workpiece shape as illustrated below

100

2 1

Rapid traverse Cutting feed

BEFORE PROGRAMMING A-37

(G99) G00 X78.0 Z20.0 M08;

G01 Z1.0 F2.0;

X90.0 Z-5.0 F0.2; . . . . . . . . . . . . . . . [3]

Z-60.0; X102.0 Z-66.0; G00 U1.0 Z20.0 M09; X200.0 Z150.0;

If "X90" is entered for "X90.0" in block [3], the resultant tool paths are generated as in the illustration below.

100

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.

WARNING

A-38 BEFORE PROGRAMMING

13 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

Ex.

JIS Specification Reverse 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

CW CCW

CCW CW

BEFORE PROGRAMMING A-39

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.

JIS Specification Reverse JIS Specification

G41 Tool position is offset to the left side of

the tool paths in reference to the programmed tool moving direction.

Workpiece

Tool moving direction

G42 Tool position is offset to the right side

of the tool paths in reference to the programmed tool moving 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.

Tool moving direction

Workpiece

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

Workpiece

Tool moving direction

X+

JIS Specification Reverse JIS Specification

162

Actual tool

nose

Z+

X-

483

Actual tool nose

Z+

A-40 BEFORE PROGRAMMING

Ex.

100

JIS Specification Reverse 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;

234

Rapid traverse Cutting feed

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.

NOTE

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

1-1 ZL, ZL-S, ZT Series, and AZL2400 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-2

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-18

7 G97 CONTROLLING SPINDLE SPEED AT CONSTANT SPEED. . . . . . . . . . . . . . . . B-22

8 G04 SUSPENDING PROGRAM EXECUTION (DWELL). . . . . . . . . . . . . . . . . . . . . . . B-25

9 G98, G99 SETTING FEEDRATE UNITS . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-28

10 G40, G41, G42 AUTOMATIC TOOL NOSE RADIUS OFFSET . . . . . . . . . . . . . . . . . . B-32

11 G40, G41, G42 CUTTER RADIUS OFFSET . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-35

12 G32, G92 THREAD CUTTING

(CONTINUOUS THREAD CUTTING AND THREAD CUTTING CYCLE). . . . . . . . . . . B-37

13 G32 TAPPING (AT THE CENTER OF SPINDLE) . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-54

13-1 Cautions on Programming Tapping Using G32. . . . . . . . . . . . . . . . . . . . . . . . . . B-55

13-1-1 Dwell Command. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-55

13-1-2 Precautions on Using the Tapper. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-56

13-1-3 To Finish Tapping at Correct Depth in Blind Hole . . . . . . . . . . . . . . . . . B-57

14 G90, G94 O.D./I.D. CUTTING CYCLE AND FACE CUTTING CYCLE . . . . . . . . . . . . B-59

15 G70 - G76 MULTIPLE REPETITIVE CYCLE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-62

16 G80, G83 - G85, G87 - G89 HOLE MACHINING CANNED CYCLES . . . . . . . . . . . . . B-65

17 G22, G23 SETTING BARRIER TO DEFINE THE

TOOL ENTRY INHIBITED ZONE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-70

18 G28 RETURNING THE AXES TO MACHINE ZERO AUTOMATICALLY. . . . . . . . . . . B-73

19 G53 SELECTING THE MACHINE COORDINATE SYSTEM. . . . . . . . . . . . . . . . . . . . B-75

20 G38 WORKPIECE PUSHING CHECK. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-77

21 G07.1 (G107) CYLINDRICAL INTERPOLATION. . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-81

22 G12.1 (G112), G13.1 (G113) NOTCHING

(POLAR COORDINATE INTERPOLATION) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-86

23 G479 TAILSTOCK CONNECT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-90

24 G68, G69 BALANCE CUT . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-93

25 G68.1, G69.1 3D COORDINATE CONVERSION . . . . . . . . . . . . . . . . . . . . . . . . . . . . . B-95

APPENDIX 1 WORKPIECE TRANSFER . . . . . . . . . . . . . . . . . . . . . . . . . . . . . APPENDIX B-1

1-1 Work Coordinate System . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . APPENDIX B-2

APPENDIX 2 AUTOMATIC IN-MACHINE TOOL PRESETTER

MACRO PROGRAM (OPTION) . . . . . . . . . . . . . . . . . . . . . . . . . APPENDIX B-8

1G 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:

Type Meaning

G FUNCTIONS B-1

One-shot G code

The G code is valid only in the specified block. (G codes in group 00, excluding G10 and G11)

Modal G code (G codes in groups other

The G code remains valid until another G code in the

same group is specified. than group 00)

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_ ;

NOTE

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 (RESET) key is pressed.

Concerning G54, however, pressing the (RESET) key does not establish the G

RESET

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

B-2 G FUNCTIONS

1-1 ZL, ZL-S, ZT Series, and AZL2400

NOTE

Standard for the MC type and Y-axis specification. However, designation is not possible in the turret 2 program of the ZL series.

Optional for the MC type and Y-axis specification.

Designation is not possible in the turret 2 program.

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

Standard for the ZT series and AZL2400.

Standard for the MC type (excludes the ZT series).

Standard for the ZL-S and ZT series. However, designation is not possible in the turret 1 program.

Standard for the Y-axis specification.

: Standard : Option K: Not available

Code Group

G00 G01 Linear interpolation G02 Circular interpolation/helical interpolation, CW (clockwise)

Positioning

Function

G03 Circular interpolation/helical interpolation, CCW (counterclockwise) G04

G07.1

(G107)

Dwell Cylindrical interpolation

G10 Data settin g G11 Data setting mode cancel

G12.1

(G112)

G13.1

(G113)

G17 G18

16 G19 G20 G21 Data input in metric system

G22

Polar coordinate interpolation mode

Polar coordinate interpolation mode cancel XpYp plane Xp: X-axis or i ts parallel axis

ZpXp plane Yp: Y-axis or its parallel axis YpZp plane Zp: Z-axis or its parallel axis Data input in inch system

Stored stroke check function ON

09 G23 Stored stroke check function OFF

G27

Reference point return check G28 Reference point return G30 Second/third, fourth reference point return

G30.1 Floating reference point return

G31

Skip function/Multi-step skip function

Division

G FUNCTIONS B-3

: Standard : Option K: Not available

Code Group

G32

Thread cutting

Function

G34 Variable lead thread cutting G35 Circular thread cutting, CW (clockwise)

G36 Circular thread cutting, CCW (counterclockwise) G38 00 Workpiece pushing check G40 G41 Tool nose radius offset, left/Cutter radius offset, left

Tool nose radius offset cancel/Cutter radius offset cancel

G42 Tool nose radius offset, right/Cutter radius offset, right G50

G50.3 Work coordinate system preset

G50.2

(G250)

G51.2

(G251)

G52 G53 Machine coordinate system selection

G54

Coordinate system setting/Spindle speed limit setting

Polygon cutting cancel

Polygon cutting

Local coordinate system setting

Work coordinate system 1 selection G55 Work coordinate sy ste m 2 sele ct ion G56 Work coordinate sy ste m 3 sele ct ion G57 Work coordinate sy ste m 4 sele ct ion

G58 Work coordinate sy ste m 5 sele ct ion G59 Work coordinate sy ste m 6 sele ct ion G65 00 Macro call G66

Macro modal call

G67 Macro mo dal call cancel G68 G69 Balance cut mode cancel

G68.1 G69.1 3D coordinate conversion cancel

G70

Balance cut mode

3D coordinate conversion

Finishing cycle G71 O.D./I.D. rough cutting cycle/Pocket cutting G72 Rough fa cing cycle/Pocket cutting G73 G74 G75

Closed-loop cutting cycle

Face cut-off cycle, deep hole drilling cycle

O.D./I.D. grooving cycle, cut-off cycle G76 Multiple thread cutting cycle/Zigzag infeed mode

Division

/ /

*5 *5

B-4 G FUNCTIONS

: Standard : Option K: Not available

Code Group

G80

Function

Hole machining canned cycle cancel G83 Face hole machini ng cy cl e G84 Face tapping cycle G85 Face boring cycle

Hole machining can ned cycle

G87 Side hole machining cycle G88 Side tapping cycle G89 Side boring cycle G90 G92 Simple thread cutting cycle

O.D./I.D. cutting cycle

G94 Face cutting cycle G96 G97 Constant spindle speed command G98 G99 Feed per revolution mode

G334

G335

Constant surface speed control

Feed per minute mode

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)

G336 Group command (Tool life management B function) G337 Skip command (Tool life management B function) G338 State flag clear command (Tool life management B function)

G339

G340

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

PMC address information reading command

(Tool life management B function) G380 Rigid tapping cycle cancel G384 Rigid tapping cycle G479

Tailstock connect joint (only for the ZL-153, 203 and 253 series)

Division

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.

CAUTION

3. At the end of machining

WARNING

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

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

CAUTION

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

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

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

The coordinates are specified in absolute values.

 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. 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.)

Page B-9

G FUNCTIONS B-7

NOTE

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-30 (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.

B-8 G FUNCTIONS

Programming using G00

Ex.

M60 P = 2

C1.5

Rapid traverse Cutting feed

O0001; N1; G50 S2000; G00 T0101; G96 S200 M03;

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

cutting tool close to the workpiece

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

of facing X30.0 F0.15;

G00 X50.0 W1.0; . . . . . . . . . . . . . . . . . Positioning from point 3 to 4 at a rapid traverse rate to

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 point 5 to move the cutting tool away from

the workpiece at a rapid traverse rate

X200.0 Z150.0 M09; . . . . . . . . . . . . . . Positioning at point 6 where the turret head can be rotated

M01;

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

G FUNCTIONS B-9

CAUTION

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

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.

X (18000)

Programmed target point

CAUTION

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. 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).

B-10 G FUNCTIONS

3 G01 MOVING THE CUTTING TOOL ALONG A STRAIGHT P ATH

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_ ;

 G01 . . . . . . . . Calls the linear interpolation mode.

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

The coordinates are specified in absolute values.

NOTE

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

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

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

 In the G99 mode, the feedrate is specified in "mm/rev".

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

 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.

G FUNCTIONS B-11

Programming using G01

Ex.

To move the cutting tool at a cutting feedrate along the paths 2  3, and 4  5  6  7  8  9.

M60 P = 2

C1.5

Rapid traverse Cutting feed

O0001; N1; G50 S2000; G00 T0101; G96 S200 M03;

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

cutting tool close to the workpiece

G01 Z0 F1.0; . . . . . . . . . . . . . . . . . . . . Positioning at point 2 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 point 3 to 4 at a rapid traverse rate to

execute O.D. cutting

G01 X54.0 Z-1.0; . . . . . . . . . . . . . . . . . Cutting along path 4  5 at a feedrate of 0.15 mm/rev

Z-5.0; . . . . . . . . . . . . . . . . . . . . . . . . . . Cutting along path 5  6 at a feedrate of 0.15 mm/rev

X56.8; . . . . . . . . . . . . . . . . . . . . . . . . . Cutting along path 6  7 at a feedrate of 0.15 mm/rev

X59.8 Z-6.5; . . . . . . . . . . . . . . . . . . . . . Cutting along path 7  8 at a feedrate of 0.15 mm/rev

Z-23.0 F0.2; . . . . . . . . . . . . . . . . . . . . . Cutting along path 8  9 at a feedrate of 0.2 mm/rev

G00 U1.0 Z20.0; . . . . . . . . . . . . . . . . . Positioning at point 10 at a rapid traverse rate to move the

cutting tool away from the workpiece

X200.0 Z150.0 M09; . . . . . . . . . . . . . . Positioning at point 11 where the turret head can be

rotated M01;

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_ ;

 G02 . . . . . . . . Calls the circular interpolation

mode in the clockwise direction.

 G03 . . . . . . . . Calls the circular interpolation

mode in the counterclockwise direction.

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

The coordinates are specified in absolute values.

 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.

G03

G02

NOTE

 R . . . . . . . . . . Specifies the radius of the arc.

 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.

 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.

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

 In the G99 mode, the feedrate is specified in "mm/rev".

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

 In the G98 mode, the feedrate is specified in "mm/min".

F200 . . . . . . 200 mm/min

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

NOTE

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

Ex.

To move the cutting tool at a cutting feedrate along the arc 2  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 point 1 to move the cutting tool close to the

workpiece

Z0 F0.2; . . . . . . . . . . . . . . . . . . . . . . . . Positioning at point 2 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 5 at a feedrate of 0.1 mm/rev

G00 U-1.0 Z20.0; . . . . . . . . . . . . . . . . . Positioning at point 6 at a rapid traverse rate to move the

cutting tool away from the workpiece

X200.0 Z150.0 M09; . . . . . . . . . . . . . . Positioning at point 7 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.

WARNING

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.

G FUNCTIONS B-15

COMMAND

WARNING

G50 S_ ;

 G50 . . . . . . . . Calls the mode to specify the spindle speed limit for automatic

operation.

-1

 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. 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.

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. (FANUC)

NOTE

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

2. With the ZL, ZL-S and ZT series, although the spindle speed limit setting command (G50) may be specified in either of the program s (turr et 1 program and tur ret 2 program), the one specified only in the program where the spindle start command (M03, M04) has been specified is regarded the valid command. In other words, the M03 or M04 command determines in which program the G50 command is valid. To set the spindle speed limit by specifying the G50 command, specify it in the program where the M03 or M04 command is specified to start the spindle. The spindle speed limit setting is not executed if the G50 command is specified i n the program where the M03 or M04 command has not been specified.

B-16 G FUNCTIONS

Programming using G50 (Setting the spindle speed limit)

Ex.

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

M60 P = 2

C1.5

Rapid traverse Cutting feed

O0001; N1;

G50 S2000; . . . . . . . . . . . . . . . . . . . . . Setting the spindle 1 speed limit for automatic operation at

2000 min

-1

G00 T0101;

G96 S200 M03; . . . . . . . . . . . . . . . . . . Starting 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 point 1 at a rapid traverse rate to move the

cutting tool close to the workpiece

G01 Z0 F1.0; . . . . . . . . . . . . . . . . . . . . Positioning at point 2 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 2000 min

-1

in the "G50 S2000;", the spindle speed does not exceed this limit value.

G00 X50.0 W1.0; G01 X54.0 Z-1.0;

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

G FUNCTIONS B-17

Machining program

B-18 G FUNCTIONS

6 G96 CONTROLLING SPINDLE SPEED TO MAINTAIN SURFACE

SPEED CONSTANT

The G96 comma nd 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 cons tant.

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 = = 1061 min

 • D

Therefore, the spindle rotates at 1061 min-1.

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

1000  100

3.14  30

G96 S_ M03(M04);

-1

G96 S_ M203(M204);

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

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

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

direction.

 M203(M204). . Specifies spindle 2 rotation in the normal (reverse) direction.

The M203 and M204 commands can be used only for the ZL-S and ZT series machines.

NOTE

WARNING

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.

G FUNCTIONS B-19

With the ZL, ZL-S and ZT series, although the constant surface speed control command

NOTE

(G96) may be specified in either of the programs (turret 1 program and turret 2 program), the one specified only in the program where the spindle start command (M03, M04) has been specified is regarded the valid command. In other words, the M03 or M04 command determines in which program the G96 command is valid. To specify the constant surface speed control with the G96 command, specify it in the program where the M03 or M04 command is specified to start the spindle. The constant surface speed control is not executed if the G96 command is specified in the program where the M03 or M04 command has not been specified.

B-20 G FUNCTIONS

Programming using G96

Ex.

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

M60 P = 2

C1.5

Rapid traverse Cutting feed

O0001; N1;

G50 S2000; . . . . . . . . . . . . . . . . . . . . . Setting the spindle 1 speed limit for automatic operation at

2000 min

-1

G00 T0101;

G96 S200 M03; . . . . . . . . . . . . . . . . . . Starting 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 point 1 at a rapid traverse rate to move the

cutting tool close to the workpiece

1000V

N = = 1137 (min

 • D

At this position, spindle 1 rotates at 1137 min

1000  200

3.14  56

-1

)

-1

in the

normal direction.

G01 Z0 F1.0;

Morii-Seiiki ZL-153, ZL-153MC, ZL-153S, ZL-153SMC, ZL-203 PROGRAMING Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

CONTENTS

FOR SAFE OPERATI O N

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

SIGNAL WORD DEFINITION

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 ZL Series

7-1-2 ZL-S Series

7-1-3 AZL2400

7-1-4 ZT 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 FUNCTIONS

11 BASIC PATTERN OF PROGRAM

11-1 Chuck-Work Programming

11-2 Center-Work Programming

11-3 Both-Center-Work Programming

12 CAUTIONS FOR CREATING A PROGRAM

12-1 Program Number

12-2 Space between the Words in the Program

12-3 Signs and Symbols

12-4 Inputting a Decimal Point

12-5 Role of Decimal Point

13 JIS SPECIFICATION AND REVERSE JIS SPECIFICATION

CONTENTS

1G CODE LIST

1-1 ZL, ZL-S, ZT Series, and AZL2400

5 G50 SETTING THE SPINDLE SPEED LIMIT