HEIDENHAIN CNC Pilot 4290 User Manual

Download

Pilot

CNC PILOT 4290

Software version 6.4/7.0

English (en) 6/2003

CNC PILOT 4290 V7.0—Keyboard Manual operating mode

Automatic operating mode

Programming modes (DIN PLUS, Simulation, TURN PLUS)

Organization modes (Parameter, Service, Transfer)

Display error status

Call info system

CNC PILOT 4290 V7.0—Keyboard INS (insert)

■ Insert list element

■ Close dialog box, save data

Numerals (0...9)

For entering numbers and selecting soft keys

Minus

For entering an algebraic sign

Decimal point

Enter

To confirm your input

...

ESC (escape)

■ Go back by one menu level

■ Close dialog box, do not save data

“Continue key”

For special functions (e.g. marking)

DEL (delete)

■ Deletes the list element

■ Deletes the selected character or the character

to the left of the cursor

ALT (alter)

■ Edit the list element

Cursor keys

Moves the cursor by one position in the direction of the arrow (one character, one field, one line, etc.)

Page Up, Page Down

■ Go to previous/next screen page

■ Go to previous/next dialog box

■ Switch between input windows

...

CNC PILOT 4290 V6.4—Keyboard Operating modes key

Call the selection of operating modes

CNC PILOT 4290 V6.4—Keyboard Numerals (0...9)

For entering numbers and selecting soft keys

...

Display error status

Call the info system

ESC

■ Go back by one menu level

■ Close dialog box, do not save data

>> (“continue” key)

For special functions (e.g. marking)

DEL

Delete key

ALT (alter)

■ Edit the list element

INS (insert)

■ Insert list element

■ Close dialog box, save data

Minus

For entering an algebraic sign

Decimal point

Enter

To confirm your input

Cursor keys

Moves the cursor by one position in the direction of the arrow (one

character, one field, one line, etc.)

Page Up, Page Down

■ Go to previous/next screen page

■ Go to previous/next dialog box

■ Switch between input windows

...

The Pilot

Contents

... is your concise programming guide for the HEIDENHAIN CNC PILOT 4290 contouring control. For more comprehensive information on programming and operating, refer to the CNC PILOT User's Manual.

Certain symbols are used in the Pilot to denote specific types of information:

Important note!

Warning: Danger for the user or the machine!

Chapter in User's Manual. Here you will find more detailed information on the current topic.

The information in this Pilot applies to the CNC PILOT with the software number 340 340 460-xx (release 6.4) and the CNC PILOT with the software number 368 650-xx (release

7.0).

DIN Programming .............................................................. 6

Overview: G Functions for Contour Description ................ 6

Program Section Codes ..................................................... 8

G Functions for Contour Description ................................. 10

Front, Rear and Lateral Surface Contours.......................... 26

Overview: G Functions for the Machining Part .................. 42

Simple Linear and Circular Movements ............................. 45

Feed Rate, Spindle Speed .................................................. 48

Tool-Tip and Cutter Radius Compensation (TRK) ................ 50

Datum Shifts, Oversizes ................................................... 51

Tools, Compensation ......................................................... 57

Turning, Drilling and Threading Cycles ............................... 59

C-Axis Machining .............................................................. 82

Other G Functions ............................................................. 90

Subprograms ..................................................................... 94

DIN Programming

NC blocks start with the letter “N” followed by a block

number (with up to four digits). Comments are enclosed in parentheses „[...]“. They are

located either at the end of an NC block or in a separate NC block.

Instructions for operation

During editing, the CNC PILOT shows programmed contours in a maximum of two simulation windows. You can select the windows from the DIN PLUS main menu (Menu item ”Graphics—Windows”).

■ The starting point of the contour will be marked with a

”small box”

DIN Programming

■ If the cursor is located on a block from ”blank or finished

part”, the corresponding contour element will be indicated in red in the simulation window (”Contour display”)

• Additions/changes to the contour will only be considered if the ”Graphics” menu item is reactivated.

• Unambiguous NC block numbers are a prerequisite for the contour display!

• For programming variables, see ”CNC PILOT 4290 User's Manual”

• For programming in the Y axis, see ”CNC PILOT 4290 with Y Axis User's Manual”

Program section codes Page Program section codes 8

Definition of blank Page G20-Geo Chuck part, cylinder/tube 10

G21-Geo Cast part 10 Basic elements for contour description Page

G0-Geo Starting point of contour 11 G1-Geo Line segment 11 G2-Geo Arc with incr. center dimensioning 12 G3-Geo Arc with incr. center dimensioning 12 G12-Geo Arc with abs. center dimensioning 12 G13-Geo Arc with abs. center dimensioning 12

Contour form elements Page G22-Geo Recess (standard) 13

G23-Geo Recess/relief turn 14 G24-Geo Thread with undercut 15 G25-Geo Undercut contour 16 G34-Geo Thread (standard) 19 G37-Geo Thread (general) 20 G49-Geo Bore hole at turning center 22

Help commands for contour description Page Overview: Help commands for contour definition 23

G7-Geo Precision stop ON 23 G8-Geo Cycle stop OFF 23 G9-Geo Precision stop blockwise 23 G10-Geo Peak-to-valley height 23 G38-Geo Feed rate reduction 24 G39-Geo Attributes of superimposed elements 24 G52-Geo Blockwise oversize 25 G95-Geo Feed per revolution 25 G149-Geo Additive compensation 25

Superimposed contours Page G308-Geo Beginning of pocket/island 26

G309-Geo End of pocket/island 26 Elements of the end face contour Page

G100-Geo Starting point of face contour 27 G101-Geo Line segment on face 27 G102-Geo Circular arc on face 28 G103-Geo Circular arc on face 28 G300-Geo Bore hole on face 29 G301-Geo Linear slot on face 30 G302-Geo Circular slot on face 30 G303-Geo Circular slot on face 30 G304-Geo Full circle on face 31 G305-Geo Rectangle on face 31 G307-Geo Eccentric polygon on face 32 G401-Geo Linear pattern on face 32 G402-Geo Circular pattern on face 33

Elements of the lateral surface contour Page G110-Geo Starting point of lateral surface contour 34

G111-Geo Line segment on lateral surface 34 G112-Geo Circular arc on lateral surface 35 G113-Geo Circular arc on lateral surface 35 G310-Geo Bore hole on lateral surface 36 G311-Geo Linear slot, lateral surface 37 G312-Geo Circular slot on lateral surface 37 G313-Geo Circular slot on lateral surface 37 G314-Geo Full circle on cylindrical surface 38 G315-Geo Rectangle on lateral surface 38 G317-Geo Eccentric polygon on lateral surface 39 G411-Geo Linear pattern, lateral surface 40 G412-Geo Circular pattern, lateral surface 41

Overviesw: Contour description

Circular arc on lateral surface

Program section codes

When you create a new DIN program, certain program section codes are already entered. Delete or add codes, depending on the task. A DIN program must include the codes ”MACHINING” and ”END.”

Overview of program section codes

PROGRAMMKOPF [ PROGRAM HEAD ] TURRET CLAMPING DEVICE ROHTEIL [ BLANK ] FERTIGTEIL [ FINISHED PART ] FRONT END REAR END

Program section codes

CYLINDER SURFACE AUXILIARY CONTOUR BEARBEITUNG [ MACHINING ] ENDE [ END ] SUBPROGRAM RETURN

PROGRAMMKOPF [ PROGRAM HEAD ]

The PROGRAM HEAD comprises:

■ Organizational information (does not influence

program execution)

■ Setup information (does not influence program

execution)

■ SLIDE: NC program is only executed for the indicated slide – No in-

put: NC program is executed for every slide (input: “$1, $2, ...”)

■ UNIT: unit of measurement ”metric/inches”—No input: the unit set

in control parameter 1 is used

The ”Unit” can be programmed only when a new program is being created (set under PROGRAM HEAD). It is not possible to post-edit this entry.

TURRET x

contains the assignment for the tool carrier x (x: 1..6). If the tool is described in the data bank, enter the T number and the ID number. Alternately, you can define the tool parameters in the NC program.

Tool data input:

Call the tool input: INS key T-number: position in the tool carrier ID (identification number): reference to the tool database– No in-

put: tool data is not included in the tool database.

Simple tool:

■ Only suitable for simple traverse paths and turning cycles (G0...G3,

G12, G13; G81...G88).

■ There is no regeneration of the contour.

■ Cutter radius compensation is carried out.

■ Data are not stored in the tool database (”Simple tools” have no ID).

Continued

Enhanced input: No limitations for use of the tool (data is transferred

to the tool database during program conversion.)

If you do not program TURRET, the tools entered in the turret table will be used.

CLAMPING DEVICE x

Defines the type of clamping device X used on the spindle (x: 1..4). If you do not program CLAMPING DEVICE, the machining simulation

assumes there is no clamping device (see also G65).

Parameters

H: Clamping device number (reference for G65) – Range: 1  H  9 ID: Identification number of clamping device X: Clamping diameter Q: Chucking shape – defines the position of the clamping device ref-

erence point (see G65)

ROHTEIL [ BLANK ]

Program section for the definition of the blank.

FERTIGTEIL [ FINISHED PART ]

Program section for the contour definition of the finished part. Additional program section codes within the finished part definition:

■ FRONT END Z.. : Section ”Front end contour” – ”Z..” defines the po-

sition of the front contour.

■ REAR SIDE Z.. : Section ”Rear side contour” – ”Z..” defines the posi-

tion of the rear side contour.

■ LATERAL SURFACE X.. : section ”Lateral surface

contour” – ”X..”

■ AUXILIARY CONTOUR: indicates further contour

definitions

If you have several independent contour definitions, then repeated use of the program section codes (FRONT END, REAR END, etc.) is permitted.

BEARBEITUNG [ MACHINING ]

Program section for the machining of the workpiece. MACHINING must be included in your program.

ENDE [ END ]

Ends your NC program. The code END must be included in your program (replaces M30).

SUBPROGRAM ”12345678”

If you define a subprogram within your NC program (within the same file), it is identified with SUBPROGRAM, followed by the name of the subprogram (max. 8 characters).

RETURN

Ends your NC subprogram.

Program section codes

Blank material for cylinder/pipe G20-Geo

G20 defines the contour of a cylinder/hollow cylinder.

Parameters

■ Diameter of cylinder/hollow cylinder

■ Diameter of circumference of polygonal blank

Z: Length of blank K: Right edge (distance between workpiece datum and right edge) I: Inside diameter for hollow cylinders

Definition of blank

Cast part G21-Geo

G21 generates the contour of the blank part from the contour of the finished part – plus the ”equidistant allowance P.”

Parameters

P: Equidistant finishing allowance (reference: finished part contour) Q: Bore holes yes/no – default: Q=0

■ Q=0: without bore holes

■ Q=1: with bore holes

Starting point of turning contour G0 Geo

G0 defines the starting point of a turning contour.

Parameters

X, Z: Starting point of the contour (X diameter value)

Line segment in a contour G1-Geo

G1 defines a line segment in a turning contour.

Parameters

X, Z: End point (X diameter value) A: Angle to rotary axis – for angle direction see illustration Q: Select point of intersection – default: 0

■ Q=0: Near intersection

■ Q=1: Far intersection

B: Chamfer/rounding

■ B is undefined: Tangential transition

■ B=0: Nontangential transition

■ B>0: Rounding radius

■ B<0: Chamfer width

E: Special feed-rate factor (0 < E  1) – default: 1

(special feed rate = active feed rate * E)

Basic elements for

contour description

Circular arc in a contour

G2/G3-Geo – incremental, G12/G13-Geo – absolute center coordinates

G2/G3 or G12/G13 defined a circular arc in a contour. The direction of rotation is visible in the help graphic.

Parameters

X, Z: End point (X diameter value) R: Radius Q: Selection of intersection – default: 0

■ Q=0: Far intersection

■ Q=1: Near intersection

B: Chamfer/ rounding at end of circular arc

■ B no entry: tangential transition

■ B=0: no tangential transition

■ B>0: Radius of rounding

Basic elements for

contour description

■ B<0: Width of chamfer

E: Special feed-rate factor (0 < E  1) – default: 1

(special feed rate = active feed rate * E)

With G2/G3:

I: Center point incremental (distance from starting point to center

as radius)

K: Center point incremental (distance from starting point to center)

With G12/G13:

I: Absolute center (radius) K: Absolute center

Example: G2-Geo

Example: G12-Geo

Recess (standard) G22-Geo

G22 defines a recess on an axis-parallel reference element (G1). G22 is assigned to the previously programmed reference element.

Parameters

X: Starting point of recess on the end surface (diameter) Z: Starting point of recess on lateral surface I, K: Inside corner

■ I for recess on front face: recess end point (diameter value)

■ K for recess on end face: recess base

■ I for recess on lateral surface: recess base (diameter value)

■ K for recess on lateral surface: recess end point

Ii, Ki: Inside corner – incremental (pay attention to sign !)

■ Ii for recess on end face: recess width

■ Ki for recess on end face: recess depth

■ Ii for recess on lateral surface: recess depth

■ Ki for recess on lateral surface: end point of recess (recess

width)

B: Outside radius/chamfer (at both ends of the recess) – default: 0

■ B>0: Radius of the rounding

■ B<0: Width of the chamfer

R: Inside radius (in both corners of recess) – default: 0

Program either X or Z.

Form elements

for contour description

Recess (general) G23-Geo

G23 defines a recess on a linear reference element (G1). G23 is assigned to the previously programmed reference element. On the lateral surface the recess can be positioned on an inclined reference straight.

Parameters

H: Recess type – default: 0

■ H=0: symmetrical recess

■ H=1: free rotation

X: Center point of recess on end surface (diameter) Z: Center point of recess on lateral surface I: Recess depth and position

■ I>0: recess to right of reference element

■ I<0: recess to left of reference element

K: Recess width (without chamfer/rounding)

Form elements

for contour description

U: Recess diameter (diameter of recess floor) – use only if the

reference element runs parallel to the Z axis.

A: Recess angle – default: 0

■ with H=0: 0°  A < 180° (angle between edges of recess)

■ with H=1: 0° < A  90° (angle between reference straight and

recess edge)

B: Outside radius/corner. Starting point near corner - default: 0

■ B>0: Radius of rounding

■ B<0: Width of chamfer

P: Outside radius/corner. Starting point distant from corner - default: 0

■ P>0: Radius of rounding

■ P<0: Width of chamfer

R: Inside radius (in both corners of recess) – default: 0

Simple recess

The CNC PILOT refers the recess depth to the reference element. The recess base runs parallel to the reference element.

Recess or free rotation

Thread with undercut G24-Geo

G24 defines a linear base element, a linear thread (external or internal thread; metric ISO fine-pitch thread DIN 13 Part 2, Series 1) and a subsequent thread undercut (DIN 76).

Calling the contour macro:

N..G1 X..Z..B.. /Starting point for thread N..G24 F..I..K..Z.. /Contours for thread and undercut N..G1 X.. /Next surface element

Parameters

F: Thread pitch I: Depth of undercut (radius) K: Width of undercut Z: End point of the undercut

• G24 can be used only if the thread is cut in the direction of contour definition.

• The thread is machined with G31.

Form elements

for contour description

Undercut contour G25-Geo

G25 generates the following undercut contours in paraxial contour corners. The meaning of the parameters depends on the type of undercut.

If you program G25

■ after the reference element, the undercut is turned at the end of the

reference element.

■ before the reference element, the undercut is turned at the

beginning of the reference element.

Calling the contour macro (example):

N..G1 Z.. /Linear element as reference

N..G25 H..I..K.. .. /Undercut contour

N..G1 X.. /Next surface element

Form elements

for contour description

Parameters

Undercut form U (H=4) Parameters

I: Depth of undercut (radius) K: Width of undercut R: Inside radius (in both corners of recess) – default: 0 P: Outside radius/chamfer – default: 0

■ P>0: radius of the rounding

■ P<0: width of the chamfer

H: Type of undercut – default: 0

■ H=4: undercut form U

■ H=0, 5: undercut form DIN 509 E

■ H=6: undercut form DIN 509 F

■ H=7: thread undercut DIN 76

■ H=8: undercut form H

■ H=9: undercut form K

Continued

Undercut form U (H=4)

Undercut DIN 509 E (H=0, 5) Parameters

I: Depth of undercut (radius) K: Width of undercut R: Undercut radius (in both corners of the undercut) W: Undercut angle

If you do not enter any parameters the CNC PILOT calculates the values from the diameter (see User's Manual, section “Undercut Parameters DIN 509 E”).

Undercut DIN 509 F (H=6) Parameters

I: Depth of undercut (radius) K: Width of undercut R: Undercut radius (in both corners of the undercut) P: Transverse depth W: Undercut angle A: Transverse angle

If you do not enter any parameters the CNC PILOT calculates the values from the diameter (see User's Manual, section “Undercut Parameters DIN 509 F”).

Continued

Undercut DIN 509 E (H=0, 5)

Undercut DIN 509 F (H=6)

Form elements

for contour description

Undercut DIN 76 (H=7) Parameters

I: Depth of undercut (radius) K: Width of undercut R: Undercut radius (in both corners of the undercut) – default:

R=0.6*I

W: Undercut angle – default: 30°

Form elements

for contour description

Undercut form H (H=8)

If you do not enter W, it will be calculated on the basis of K and R. The final point of the undercut is then located at the ”final point contour.”

Parameters

K: Width of undercut R: Undercut radius – no value: the circular element is not machined W: Plunge angle – no value: W is calculated

Undercut DIN 76 (H=7)

Continued

Undercut form H (H=8)

Undercut form K (H=9) Parameters

I: Undercut depth R: Undercut radius – no value: the circular element is not machined W: Undercut angle A: Angle to linear axis – default: 45°

Thread (standard) G34-Geo

G34 defines a simple or an interlinked external or internal thread (metric ISO fine-pitch thread DIN 13 Series 1). Threads are interlinked by programming several G01/G34 blocks after each other.

Parameters

F: Thread pitch – no value: pitch from the standard table

• You need to program a linear contour element as a reference

before G34 or in the NC block containing G34.

• The thread is cut with G31.

Undercut form K (H=9)

Form elements

for contour description

Thread (general) G37-Geo

G37 defines the different types of thread. Threads are interlinked by programming several G01/G34 blocks after each other.

Parameters

Q: Type of thread – default: 1

■ Q=1: metric ISO fine-pitch thread (DIN 13 Part 2, Series 1)

■ Q=2: metric ISO thread (DIN 13 Part 1, Series 1)

■ Q=3: metric ISO taper thread (DIN 158)

■ Q=4: metric ISO tapered fine-pitch (DIN 158)

■ Q=5: metric ISO trapezoid thread (DIN 103 Part 2, Series 1)

■ Q=6: flat metric trapezoid thread (DIN 308 Part 2, Series 1)

■ Q=7: metric buttress thread (DIN 13 Part 2, Series 1)

■ Q=8: cylindrical round thread (DIN 405 Part 1, Series 1)

■ Q=9: cylindrical Whitworth thread (DIN 259)

■ Q=10: tapered Whitworth thread (DIN 2999)

■ Q=11: Whitworth pipe thread (DIN 2999)

Form elements

for contour description

■ Q=12: nonstandard thread

■ Q=13: UNC US coarse thread

■ Q=14: UNF US fine-pitch thread

■ Q=15: UNEF US extra-fine-pitch thread

■ Q=16: NPT US taper pipe thread

■ Q=17: NPTF US taper dryseal pipe thread

■ Q=18: NPSC US cylindrical pipe thread with lubricant

■ Q=19: NPFS US cylindrical pipe thread without lubricant

F: Thread pitch – must be entered for Q=1, 3..7, 12. P: Thread depth – enter only for Q=12. K: Runout length (for threads without undercut) –

default: 0

• Program a linear contour element as a reference before G37.

• The thread is cut with G31.

• For standard threads, the parameters P, R,

A and W are defined by the CNC PILOT.

• Use Q=12 if you wish to use individual parameters.

The thread is generated to the length of the reference element. For the machining of threads without an undercut, it is necessary to program an additional linear element so that the overrun can be executed by the CNC PILOT without danger of collision.

Continued

D: Reference point (position of thread runout) – default: 0

■ D=0: runout at end of reference element

■ D=1: runout at beginning of reference element

H: Number of grooves – default: 1 A: Edge angle left – enter only for Q=12. W: Edge angle right – enter only for Q=12. R: Thread width – enter only for Q=12. E: Variable pitch (increases/reduces the pitch per revolution by E) –

default: 0

Form elements

for contour description

Bore hole (centered) G49-Geo

G49 defines a single bore hole with countersink and thread at the turning center (front or end face).

Parameters

Z: Starting position for hole (reference point) B: Bore hole diameter P: Depth of hole (excluding point) W: Point angle – default: 180° R: Countersinking diameter U: Countersinking depth E: Countersinking angle I: Thread diameter J: Thread depth K: Thread runout length

Form elements

for contour description

F: Thread pitch V: Left-hand or right-hand thread - default: 0

■ V=0: Right-hand thread

■ V=1: Left-hand thread

A: Angle (position of bore hole) – default: 0

■ A=0: front end

■ A=180: tail end

O: Centering diameter

• G49 is programmed in the FINISHED PART section (not in the FRONT or REAR SIDE section).

• The contour defined with G49 is machined with G71...G74.

Overview: Help commands for contour description

G7 Accurate stop ON G8 Accurate stop OFF G9 Accurate stop blockwise G10 influences finishing feed rate for total contour G38 influences finishing feed rate for basic contour elements block

by block

G39 Only for form elements:

■ influences finishing feed rate

■ additive compensation values

■ equidistant finishing allowances

G52 Equidistant finishing allowances – blockwise G95 defines finishing feed rate for total contour G149 additive compensation values for total contour

Accurate stop ON G7-Geo

G7 switches the ”precision stop” on modally. In a ”precision stop,” the CNC PILOT does not start the next block until the ”tolerance window” around the end point is reached (for tolerance window, see machine parameters 1106, 1156, ...).

• The NC block containing G7 is also executed with a precision stop.

•”Precision stop” is used for basic contour elements that are executed with G890 or G840.

Precision stop OFF G8-Geo

G8 switches the precision stop off. The block containing G8 is executed

without a precision stop.

Blockwise accurate stop G9-Geo

G9 activates a precision stop for the NC block in which it is programmed (see also ”G7 Geo”).

Peak-to-valley height (surface texture) G10-Geo

G10 influences the finishing feed rate of G890 and thus determines the surface roughness of the workpiece.

Basics of programming

■ The peak-to-valley height activated with G10 is mo-

dal.

■ G10 without parameters deactivates peak-to-valley

height.

■ G95 Geo deactivates peak-to-valley height.

■ G10 RH... (without ”H”) overwrites the valid peak-

to-valley roughness block by block.

■ G38 Geo overwrites the valid peak-to-valley

roughness block by block.

Parameters

H: Type of surface texture (see also DIN 4768)

■ H=1: general roughness (profile depth) Rt1

■ H=2: average roughness Ra

■ H=3: mean roughness Rz

RH: Peak-to-valley roughness (in µm, inches: µinch)

The peak-to-valley height applies only for basic contour elements.

Help commands for

contour description

Feed rate reduction factor G38-Geo

G38 defines a special feed rate for G890.

Parameters

E: Special feed-rate factor (0 < E  1) – default: 1

(special feed rate = active feed rate * E)

Basics of programming

■ G38 is a non-modal function.

■ G38 is programmed before the contouring

element for which it is destined.

■ G38 replaces another special feed rate or a

programmed peak-to-valley height.

The ”special feed rate” applies only for basic contour elements.

Attributes for superimposed elements G39-Geo

G39 influences the machining of G890 for the superimposed

Help commands

for contour description

elements (form elements):

✲■ Chamfers/rounding arcs (for connecting base elements)

■ Undercuts

■ Recesses

Influence on machining:

■ Special feed rate

■ Peak-to-valley height

■ Additive D compensation

■ Equidistant oversizes

Parameters

F: Feed per revolution V: Type of surface texture (see also DIN 4768)

■ V=1: general roughness (profile depth) Rt1

■ V=2: average roughness Ra

■ V=3: mean roughness Rz

RH: Peak-to-valley height (µm, inch mode: µinch) D: Number of the additive compensation (901  D  916)

P: Finishing allowance (radius) H: (Translation of P) absolute / additive – default: 0

■ H=0: P replaces G57/G58 allowances

■ H=1: P is added to G57/G58 allowances

E: Special feed-rate factor (0 < E  1) – default: 1

(special feed rate = active feed rate * E)

Basics of programming

■ G39 is a non-modal function.

■ G39 is programmed before the contour element

for which it is destined.

■ G50 before a cycle (MACHINING section) switches

G39 oversizes for this cycle off.

Only use peak-to-valley height (”V, RH”), finishing allowance (”F”) and special feed rate (”E”) alternately!

Blockwise finishing allowance G52-Geo

G52 defines an equidistant finishing allowance which is taken into consideration in G810, G820, G830, G860 and G890.

Basics of programming

■ G52 is a non-modal function.

■ G52 is programmed in the NC block containing the contour element

for which it is destined.

■ G50 before a cycle (MACHINING section) switches G52 oversizes for

this cycle off.

Parameters

P: Finishing allowance (radius) H: (Translation of P) absolute / additive – default: 0

■ H=0: P replaces G57/G58 allowances

■ H=1: P is added to G57/G58 allowances

Feed rate per revolution G95-Geo

G95 influences the finishing feed rate of G890.

Basics of programming

■ G95 is a modal function

■ G10 switches the G95 finishing feed rate off.

Parameters

F: Feed per revolution

• Use peak-to-valley height and finishing feed rate alternatively.

• The G95 finishing feed rate replaces a finishing feed rate

defined in the machining program.

Additive compensation G149-Geo

The CNC PILOT manages 16 tool-independent correction values.

To activate the additive correction function, program G149 followed by a „D number“ (for example, G149 D901). ”G149 D900” resets the additive compensation function.

Basics of programming

■ Additive compensation is effective from the block

in which G149 is programmed.

■ An additive compensation remains active until:

• the next ”G149 D900”

• the end of the finished part description

Parameters

D: Additive compensation - Default: D900

Range: 900 to 916

Note the direction of contour description!

Help commands for

contour description

Start of pocket/island G308-Geo

G308 defines a new reference level/reference diameter for hierarchically nested front face or lateral surface contours.

Parameters

P: Depth for pocket, height for islands

The algebraic sign of ”Depth P” defines the position of the milling contour:

■ P<0: Pocket

■ P>0: Island

Section P Surface Milling floor

FRONT END P<0 Z Z+P FRONT END P>0 Z+P Z REAR END P<0 Z Z–P

Overlapped contours

REAR END P>0 Z–PZ CYLINDER SURFACE P<0 X X+(P*2) CYLINDER SURFACE P>0 X+(P*2) X

The milling cycles machine from the ”surface” toward the ”milling floor.”

X: Reference diameter from the section code Z: Reference plane from the section code P: ”Depth” from G308 or from the cycle parameters

• Note with ”P”: the addition of a negative number reduces the result, and the subtraction of a negative number increases the result.

• Island: The area-milling cycles machine the complete area specified in the contour definition. Islands that are defined within this area are not considered.

End pocket/island G309-Geo

G309 ends a reference level. Every reference plane defined with G308

must be ended with G309!

Starting point of end face contour G100-Geo

G100 defines the starting point of an end face contour.

Parameters

X, C: Starting point in polar coordinates (diameter, starting angle) XK,YK: Starting point in Cartesian coordinates

Linear segment in end face contour G101-Geo

G101 defines a line segment in an end face contour.

Parameters

X, C: End point in polar coordinates (diameter, end angle) XK,YK: End point in Cartesian coordinates A: Angle to positive XK-axis B: Chamfer/rounding

■ B is undefined: Tangential transition

■ B=0: Nontangential transition

■ B>0: Rounding radius

■ B<0: Chamfer width

Q: Select point of intersection – default: 0

■ Q=0: Near intersection

■ Q=1: Far intersection

Base elements for

front/end face contour

Circular arc in front end contour G102-/G103-Geo

G102/G103 defines a circular arc in a front/end face contour. The direction of rotation is visible in the help graphic.

Parameters

X, C: End point in polar coordinates (diameter, end angle) XK,YK: End point in Cartesian coordinates R: Radius I, J: Center in Cartesian coordinates Q: Selection of intersection – default: 0

■ Q=0: Far intersection

■ Q=1: Near intersection

B: Chamfer/ rounding at end of circular arc

■ B no entry: tangential transition

■ B=0: no tangential transition

Base elements for

front/end face contour

■ B>0: Radius of rounding

■ B<0: Width of chamfer

The end point may not be the same as the starting point (not a full circle).

G102-Geo

G103-Geo

Bore hole on end face G300-Geo

G300 defines a bore hole with countersink and thread on the front/end face.

Parameters

XK,YK: Center of hole B: Hole diameter P: Depth of hole (excluding point) W: Point angle – default: 180° R: Countersinking diameter U: Countersinking depth E: Countersinking angle I: Thread diameter J: Thread depth K: Thread runout length F: Thread pitch V: Left-hand or right-hand thread - default: 0

■ V=0: Right-hand thread

■ V=1: Left-hand thread

A: Angle (reference: Z-axis)

■ Front end – default: 0° (range: –90° < A < 90°)

■ Rear end – default: 180° (range: 90° < A < 270°)

O: Centering diameter

Use G71...G74 to machine bore holes defined with G300-Geo.

Figures on end face contour

Linear slot on the end face G301-Geo

G301 defines a linear slot on the front/rear end face.

Parameters

XK,YK: Center of slot A: Angle of slot length (reference: XK-axis) – default: 0° K: Slot length B: Slot width P: Depth/height – no entry: ”P” from G308

■ P<0: Pocket

■ P>0: Island

Figures on end face contour

Circular slot on the front end G302-/G303-Geo

G302/G303 defines a circular slot on the front/rear end face.

Parameters

I, J: Center of slot curvature R: Curvature radius (reference: center point path of the slot) A: Angle of slot starting point (reference: XK-axis) – default: 0 W: Angle of slot end point (reference: XK-axis) B: Slot width P: Depth/height – no entry: ”P” from G308

■ P<0: Pocket

■ P>0: Island

Example: G302-Geo

Full circle on front end face G304-Geo

G304 defines a full circle on the front/rear end face.

Parameters

XK,YK: Circle center R: Circle radius P: Depth/height – no entry: ”P” from G308

■ P<0: Pocket

■ P>0: Island

Rectangle on end face G305-Geo

G305 defines a rectangle on the front/rear end face.

Parameters

XK,YK: Center of rectangle A: Angle to longitudinal axis of rectangle (reference: XK-axis) – default:

0° K: Length of rectangle B: (Height) width of rectangle R: Chamfer/rounding - default: 0

■ R>0: Radius of rounding

■ R<0: Width of chamfer

P: Depth/height – no entry: ”P” from G308

■ P<0: Pocket

■ P>0: Island

Figures on end face contour

Regular polygon on end face G307-Geo

G307 defines a regular polygon on the front/rear end face.

Parameters

XK,YK: Polygon center point Q: Number of edges (Q3) A: Angle to a polygon side (reference: XK-axis) – default: 0° K: Edge length

■ K>0: Edge length

■ K<0: Key width (inside diameter)

R: Chamfer/rounding - default: 0

■ R>0: Radius of rounding

■ R<0: Width of chamfer

P: Depth/height – no entry: ”P” from G308

■ P<0: Pocket

Figures on end face contour

■ P>0: Island

Linear pattern on end face G401-Geo

G401 defines a linear pattern on the front/rear end face. G401 is effective for the bore hole/figure defined in the following block (G300..305, G307).

Parameters

Q: Number of figures XK,YK: Starting point of pattern I, J: End point of pattern Ii, Ji: Distance between two figures (in XK, YK direction) A: Angle to the longitudinal axis of the pattern (reference: XK-axis) R: Total length of pattern Ri: Distance between two figures (pattern distance)

Circular pattern on end face G402-Geo

G402 defines a circular pattern on the front/rear end face. G402 is effective for the figure defined in the following block (G300..305, G307).

Programming notes

■ Program the hole/figure in the following block without a center –

exception: circular slot.

■ The milling cycle (MACHINING section) calls the hole/figure in the

following block - not the pattern definition.

Parameters

Q: Number of figures K: Pattern diameter A, W: Starting angle, end angle – position of first/last figure (reference:

XK-axis) – default: A=0°; W=360° Wi: Angle between two figures V: Direction (orientation) – default: 0

■ V=0 – without W: Distribution over complete circle

■ V=0 – with W: Distribution over long arc

■ V=0 – with Wi: Algebraic sign of Wi defines the direction

(Wi<0: Pattern in clockwise direction)

■ V=1 – with W: Pattern in clockwise direction

■ V=1 – with Wi: Pattern in clockwise direction (algebraic sign of

Wi is without meaning)

■ V=2 – with W: Pattern counterclockwise

■ V=2 – with Wi: Pattern counterclockwise (algebraic sign of Wi

has no effect) XK,YK: Center of pattern H: Position of figures – default: 0

■ H=0: Normal position – figures are rotated about the circle

center (rotation)

■ H=1: Original position – position of figure remains the

unchanged with respect to the coordinate system (translation)

Figures on end face contour

Starting point of lateral surface contour G110-Geo

G110 defines the starting point of a lateral surface contour.

Parameters

Z, C: Starting point of contour (starting point, starting angle) CY: Starting angle as linear dimension

Program either Z, C or Z, CY.

Basic elements of

lateral surface contour

Straight line in a lateral surface contour G111-Geo

G111 defines a line segment in a lateral surface contour.

Parameters

Z, C: End point, end angle CY: End angle as linear dimension A: Angle (reference: negative Z axis) B: Chamfer/rounding

■ B is undefined: Tangential transition

■ B=0: Nontangential transition

■ B>0: Rounding radius

■ B<0: Chamfer width

Q: Select point of intersection – default: 0

■ Q=0: Near intersection

■ Q=1: Far intersection

Program either Z, C or Z, CY.

Circular arc in lateral surface contour G112-/G113-Geo

G112/G113 defines a circular arc in a lateral surface contour. The direction of rotation is visible in the help graphic.

Parameters

Z, C: End point, end angle CY: End angle as linear dimension R: Radius K: Center point (in Z direction) W: Angle of the center point J: Angle of the center point as a linear value Q: Selection of intersection – default: 0

■ Q=0: Far intersection

■ Q=1: Near intersection

B: Chamfer/rounding

■ B is undefined: Tangential transition

■ B=0: Nontangential transition

■ B>0: Rounding radius

■ B<0: Chamfer width

• Program either Z, C or Z and CY, or K, W or K and J.

• Program either center or radius.

• For radius: only arcs  180° possible

G112-Geo

Basic elements of

lateral surface contour

G113-Geo

Bore hole on lateral surface G310-Geo

G310 defines a bore hole with countersink and thread on the lateral surface.

Parameters

Z, C: Center point of bore hole (position, angle) CY: Angle as linear dimension B: Hole diameter P: Depth of hole (excluding point) W: Point angle – default: 180° R: Countersinking diameter U: Countersinking depth E: Countersinking angle I: Thread diameter J: Thread depth

Figures on the

lateral surface

K: Thread runout length F: Thread pitch V: Left-hand or right-hand thread - default: 0

■ V=0: Right-hand thread

■ V=1: Left-hand thread

A: Angle (reference: Z axis) – default: 90° = vertical hole (range:

0° < A < 180°)

O: Centering diameter

Use G71...G74 to machine contours defined with G310.

Linear slot on lateral surface G311-Geo

G311 defines a linear slot on the lateral surface.

Parameters

Z, C: Center point of slot (position, angle) CY: Angle as linear dimension A: Angle to longitudinal axis of slot (reference: Z-axis) – default: 0° K: Slot length B: Slot width P: Pocket depth – no entry: ”P” from G308

Circular groove on lateral surface G312-/G313-Geo

G312/G313 defines a circular slot on the lateral surface.

Parameters

Z, C: Center of curvature of slot (position, angle) CY: Angle as linear dimension R: Curvature radius (reference: center point path of the slot) A: Angle of slot starting point (reference: Z axis) W: Angle of slot end point (reference: Z axis) B: Slot width P: Pocket depth – no entry: ”P” from G308

Figures on the

lateral surface

Example: G312-Geo

Full circle on lateral surface G314-Geo

G314 defines a full circle on the lateral surface.

Parameters

Z, C: Circle center (position, angle) CY: Angle as linear dimension R: Circle radius P: Pocket depth – no entry: ”P” from G308

Figures on the

lateral surface

Rectangle on lateral surface G315-Geo

G315 defines a rectangle on the lateral surface.

Parameters

Z, C: Center point of rectangle (position, angle) CY: Angle as linear dimension A: Angle to longitudinal axis of rectangle (reference: Z-axis) – default: 0° K: Length of rectangle B: Width (height) of the rectangle R: Chamfer/rounding - default: 0

■ R>0: Radius of rounding

■ R<0: Width of chamfer

P: Pocket depth – no entry: ”P” from G308

Regular polygon on lateral surface G317-Geo

G317 defines a regular polygon on the lateral surface.

Parameters

Z, C: Center point of polygon (position, angle) CY: Angle as linear dimension Q: Number of edges (Q3) A: Angle to a polygon side (reference: Z-axis) – default: 0° K: Edge length

■ K>0: Edge length

■ K<0: Key width (inside diameter)

R: Chamfer/rounding - default: 0

■ R>0: Radius of rounding

■ R<0: Width of chamfer

P: Pocket depth – no entry: ”P” from G308

Figures on the

lateral surface

Linear pattern on lateral surface G411 Geo

G411 defines a linear pattern on the lateral surface. G411 is effective for the bore hole/figure defined in the following block (G310..315, 317).

Parameters

Q: Number of figures Z, C: Starting point, starting angle of pattern K, W: End point, end angle of pattern Ki: Distance between the figures (in Z-direction) Wi: Angular distance between the figures A: Angle of pattern length axis (reference: Z axis) R: Total length of pattern Ri: Distance between two figures (pattern distance)

Figures on the

lateral surface

If you program Q, Z and C, the bore holes/figures will be ordered in a regular manner along the circumference.

Circular pattern on lateral surface G412 Geo

G412 defines a circular pattern on the lateral surface. G412 is effective for the bore hole/figure defined in the following block (G310..315, 317).

Programming notes

■ Program the hole/figure in the following block without a center –

exception: circular slot.

■ The milling cycle (MACHINING section) calls the hole/figure in the

following block - not the pattern definition.

Parameters

Q: Number of figures K: Diameter of circle A, W: Starting angle, end angle – position of first/last figure (reference:

Z-axis) – default: A=0°; W=360° Wi: Distance between two figures V: Direction (orientation) – default: 0

■ V=0 – without W: Distribution over complete circle

■ V=0 – with W: Distribution over long arc

■ V=0 – with Wi: Algebraic sign of Wi defines the direction

(Wi<0: Pattern in clockwise direction)

■ V=1 – with W: Pattern in clockwise direction

■ V=1 – with Wi: Pattern in clockwise direction (algebraic sign of

Wi is without meaning)

■ V=2 – with W: Pattern counterclockwise

■ V=2 – with Wi: Pattern counterclockwise (algebraic sign of Wi

has no effect) Z, C: Position, angle to midpoint of pattern H: Position of figures – default: 0

■ H=0: Normal position – figure is rotated about the circle center

(rotation)

■ H=1: Original position – position of figure remains the

unchanged with respect to the coordinate system (translation)

Figures on the

lateral surface

G Functions for Machining

The following functions must be preceded with the section code MACHINING.

For contour-based turning cycles define the reference to the contour description in ”NS, NE.” You can determine this reference as follows:

Activate contour display (menu item ”Graphic”). Place the cursor on the ”NS/NE” field and press the

Continue key.

Select the desired contour element with the left/right arrow

key.

The up/down arrow keys can be used to switch between

several contours (also end face contours, etc.)

Transfer the block number of the contour element (”Enter”

key).

Overview: machining part

If you activate the up/down arrow keys, the CNC PILOT also considers contours that are not displayed on the screen.

Tool positioning without machining Page G0 Positioning in rapid traverse 45

G14 Approach to the tool change position 45 G701 Rapid traverse to machine coordinates 46

Simple Linear and Circular Paths Page G1 Linear path 46

G2 Circular path 47 G3 Circular path 47 G12 Circular path 47 G13 Circular path 47

Feed rate and spindle speed Page Gx26 Speed limit * 48

G48 Acceleration (slope) 48 G64 Discontinuous feed rate 49 Gx93 Feed rate per tooth * 49 G94 Feed per minute 49 Gx95 Feed in revolutions 49 Gx96 Constant surface speed 49 Gx97 Spindle speed 49

Cutter radius compensation (TRC/MCRC) Page G40 Switch off TRC/MCRC 50

G41 TRC/MCRC left 50 G42 TRC/MCRC right 50

* ”x” = number of the spindle (0...3)

Datum shift Page Overview Datum shifts 51

G51 Datum shift (relative) 51 G53 Parameter-dependent datum shift 52 G54 Parameter-dependent datum shift 52 G55 Parameter-dependent datum shift 52 G56 Additive datum shift (relative) 52 G59 Datum shift (absolute) 63 G121 Contour mirroring/shifting 54 G152 Datum shift C-axis 82

Allowances, safety clearances Page G47 Set safety clearances 55

G50 Switch off allowance 55 G57 Paraxial allowance 56 G58 Contour-parallel allowance 56 G147 Safety clearance (milling) 55

Tools, types of compensation Page T Tool change 57

G148 (Changing the) correction of cut 57 G149 Additive correction 58 G150 Compensate right tool tip 58 G151 Compensate left tool tip 58

Simple turning cycles Page G80 End of cycle 59

G81 Simple longitudinal roughing 59 G82 Simple face roughing 59 G83 Simple contour-parallel roughing 60 G85 Undercuts 61 G86 Simple recessing cycle 63 G87 Transition radii 64 G88 Chamfers 64

Contour-determined turning cycles Page G810 Longitudinal roughing cycle 65

G820 Face roughing cycle 65 G830 Contour-parallel roughing cycle 67 G835 Contour-parallel with neutral tool 68 G860 Universal recessing cycle 69 G866 Simple recessing cycle 70 G869 Recess turning cycle 71 G890 Finishing cycle 72

Thread cycle group Page G31 Thread cycle 74

G32 Single thread cycle 75 G33 Single thread cut 76

Drilling cycle group Page G36 Tapping 77

G71 Simple drilling cycle 78 G72 Boring, sinking, etc. 79 G73 Tapping cycle 80 G74 Deep drilling cycle 81

C axis Page G120 Reference diameter for cylinder

surface machining 82

G152 Datum shift C-axis 82 G153 Standardize C-axis 82

End face machining Page G100 Rapid traverse, front/rear face 83

G101 Linear movement, front/rear face 83 G102 Circular arc, front/rear face 84 G103 Circular arc, front/rear face 84

Overview: machining part

Cylindrical surface machining Page G110 Rapid traverse, cylindrical surface 85

G111 Linear movement, cylindrical surface 85 G112 Circular arc, cylindrical surface 86 G113 Circular arc, cylindrical surface 86 G120 Reference diameter for cylinder

Milling Cycles Page G840 Contour milling 87

G845 Pocket milling – roughing 89 G846 Pocket milling – finishing 89

Other G Functions Page G4 Dwell time 90

G7 Accurate stop ON 90

Overview:

G-functions for machining part

G8 Accurate stop OFF 90 G9 Block precision stop 90 G60 Deactivate protection zone 90 G65 Chucking equipment for graphics 91 G98 Assignment spindle – workpiece 91 G121 Contour mirroring/shifting 54 G702 Regeneration of contour storing/loading 92 G703 Regeneration of contour ON/OFF 92 G720 Spindle synchronization 92 G905 Measuring C-angle offset 92 G918 Feedforward control ON/OFF 93 G919 Spindle override 100% 93 G920 Deactivate datum shift 93 G921 Deactivate datum shift and tool

surface machining 82

dimensions 93

Other G Functions Page G980 Activate datum shift 93

G981 Activate datum shift and tool

dimensions 93

Subprograms Page

Subprogram call 94

See User's Manual G15 Moving a rotary axis

G30 Converting G62 One-sided synchronization G63 Synchronous start of slide G119 Select C axis G162 Set synchronizing mark G192 Minute feed rate for rotary axes G204 Wait for moment G600 Tool preselection in magazine/chain G601 Inserting tool from magazine into carrier G710 Linking tool dimensions G711 Activate magazine tool G717 Update nominal values G718 Servo lag G900..999 Special G functions

Rapid traverse G0

The tool moves at rapid traverse along the shortest path to the ”target point.”

Parameters

X, Z: Diameter, length to target point (X diameter)

Tool change point G14

The slide moves in rapid traverse to the tool change position. In setup mode, define permanent coordinates for the tool change.

Parameters

Q: Sequence – default: 0

0: Diagonal path of traverse

1: First in X axis, then in Z

2: First in Z axis, then in X

3: X axis only

4: Z direction only

Tool positioning

without machining

Rapid traverse to machine coordinates G701

The slide moves at rapid traverse on the shortest path to the ”target point.”

Parameters

X, Z: End point (X diameter value)

Simple linear

and circular paths

Linear path G1

The tool moves at the programmed feed rate on a line to the ”end point.”

Parameters

X, Z: Diameter, length to end point (X diameter) A: Angle (angular direction: see graphic support window) Q: Selection of intersection – default: Q=0

B: Chamfer/rounding

E: Special feed-rate factor (0 < E  1) – default: 1

”X, Z” refer to the machine datum and the slide datum.

■ Q=0: Near intersection

■ Q=1: Far intersection

■ B is undefined: Tangential transition

■ B=0: Nontangential transition

■ B>0: Rounding radius

■ B<0: Chamfer width

(special feed rate = active feed rate * E)

Circular path

G2, G3 – incremental, G12, G13 – absolute center coordinates

The tool moves in a circular arc at the feed rate to the ”end point.” The direction of rotation of G2/G3 or G12/G13 is shown in the graphic support window.

The special feed rate applies to chamfer/rounding.

Parameters

X, Z: Diameter, length to end point (X diameter) R: Radius (0 < R  200 000 mm) Q: Selection of intersection – default: Q=0

■ Q=0: Far intersection

■ Q=1: Near intersection

B: Chamfer/rounding

■ B is undefined: Tangential transition

■ B=0: Nontangential transition

■ B>0: Rounding radius

■ B<0: Chamfer width

E: Special feed-rate factor (0 < E  1) – default: 1

(special feed rate = active feed rate * E)

With G2, G3:

I, K: Center point incremental (distance starting point – center point;

I radius)

With G12, G13:

I, K: Absolute center (I radius)

Example: circular path G2

Simple linear

and circular paths

Example: circular path G12

Speed limitation

G26: Spindle; Gx26: Spindle x (x: 1...3)

G26/Gx26 limits the speed of spindle x. The speed limit remains in effect until program end or until it is replaced by a new G26/Gx26.

Parameters

S: (Maximum) speed

The ”absolute maximal speed” is specified in machine parameter 805 and following. If S > parameter value, the parameter value takes applies.

Acceleration (slope) G48

G48 specifies the approaching acceleration, braking acceleration, and the maximum feed rate. G48 is a modal function.

Without G48 the following parameter values apply:

Feed rate and spindle speed

■ Acceleration at approach/deceleration at departure: Machine

parameter 1105 ff ”Acceleration/deceleration of linear axis”

■ and the maximum feed rate from: Machine Parameter 1101 ff ”Maxi-

mum axis speed”

Parameters

E: Acceleration at approach – no input: the parameter values take

effect.

F: Deceleration at departure – no input: the parameter values take

effect

H: Programmed acceleration On/Off

■ H=0: switch off programmed acceleration after next traverse

■ H=1: switch on programmed acceleration

P: Maximum feed rate – no input: Parameter value

• If P > parameter value, the parameter value applies.

•”E, F and P” refer to the X or Z axis. The acceleration/feed rate for the slide is not higher with axis-parallel traverses.

Interrupted (intermittent) feed G64

G64 interrupts the programmed feed for a short period of time.

■ For switch-on, program G64 with E and F.

■ For switch-off, program G64 without parameters.

Parameters

E: Duration of pause (range: 0.01 s < E < 99.99 s) F: Duration of feed rate (range: 0.01 s < E < 99.99 s)

Feed rate per revolution Gx95

G95: Spindle; Gx95: Spindle x (x: 1...3) G95/Gx95 defines the feed rate as a function of drive.

Parameters

F: Feed rate in mm/revolution or inch/revolution

Feed rate per tooth spindle x Gx93

Gx93 (x: spindle 1...3) defines the feed rate drive-dependent, depending on the number of teeth of the cutter.

Parameters

F: Feed rate per tooth (mm/tooth or inch/tooth)

The actual value display shows the feed rate in mm/rev.

Feed rate constant G94 (minute feed)

G94 defines the feed rate as a function of drive. Parameters

F: Feed rate per minute (in mm/min or inch/min)

Constant cutting speed Gx96

G96: spindle; Gx96: spindle x (x: 1...3)

G96/Gx96 defines a constant cutting speed. The spindle speed is dependent on the X position of the tool tip or on the tool diameter (with driven tools).

Parameters

S: Cutting velocity (in m/min or ft/min)

Speed Gx97

G97: spindle; Gx97: spindle x (x: 1...3)

G97/Gx97 defines a constant spindle speed.

Parameters

S: Speed (in revolutions per minute)

Feed rate and spindle speed

Tooth and cutter radius

Tooth and cutter radius compensation (TRC/MCRC) G40, G41, G42

G40: Switch off TRC/MCRC

■ The TRC is effective up to the block before G40.

■ In the block with G40, or in the block after G40, only one straight line

segment permitted (G14 is not permitted).

G41/G42: switch on TRC/MCRC

■ In the block with G41/G42 or after the block with G41/G42, one

straight line segment (G0/G1) is to be programmed.

■ The TRC/MCRC is included after the next contour element.

G41: Switch on TRC/MCRC – displacement of the tool radius in the direction left of the contour.

G42: Switch on TRC/MCRC – displacement of the tool radius in the

compensation (TRC)

direction right of the contour.

Parameters

Q: Machining plane – default: 0

■ Q=0: TRC on the turning plane (X-Z plane)

■ Q=1: MCRC on the end face (X-C plane)

■ Q=2: MCRC on the cylindrical surface (Z-C plane)

■ Q=3: MCRC on the end face (X-Y plane)

■ Q=4: MCRC on the cylindrical surface (Y-Z plane)

H: Output (only with MCRC) – default: 0

■ H=0: Intersecting areas which are programmed in directly

successive contour elements are not machined.

■ H=1: The complete contour is machined – even if certain areas

are intersecting.

O: Feed rate reduction – default: 0

■ O=0: Feed rate reduction active

■ O=1: No feed rate reduction

• If the tool radii > contour radii, it can result in tool path loops during CRC/MCRC. Recommendation: Use the finishing cycle G890 / milling cycle G840.

• Never select MCRC during a perpendicular approach to the plane.

• Note when calling subprograms with active TRC/MCRC: Switch the TRC/MCRC off in the main program if it was switched on in the main program. – Switch the TRC/MCRC off in the subprogram in which it was switched on.

Overview

G51 ■ Relative shift

■ Programmed shift

■ Reference: set workpiece datum

G53, G54, G55

G56

G59

■ Relative shift

■ Shift from parameters

■ Reference: set workpiece datum

■ Additive shift

■ Programmed shift

■ Reference: current workpiece datum

■ Absolute shift

■ Programmed shift

■ Reference: machine datum

Zero point shift G51

G51 displaces the workpiece datum by ”Z” (or ”X”). The shift is referenced to the workpiece datum defined in setup operation.

Even if you shift the zero point several times with G51, the displacement is still always referenced to the workpiece zero point from the setup mode.

The zero point shift applies until the end of the program or until it is canceled by another zero point shift.

Parameters

X, Z: Displacement (X radius value) – default: 0

Zero point shift

Parameter-dependent zero point shift G53, G54, G55

G53, G54, G55 displace the workpiece zero point by the value defined in the setup parameters 3, 4, 5. The shift is referenced to the workpiece zero point defined in setup operation.

Even if you shift the zero point several times with G53, G54, G55, the displacement is still always referenced to the workpiece datum from the setup mode.

The datum shift applies until the end of the program or until it is canceled by another datum shift.

A shift in X must be indicated as a radius value.

Zero point shift

Additive zero point shift G56

G56 shifts the workpiece zero point by ”Z” (or ”X”). The displacement is referenced to the currently active workpiece zero point.

If you shift the workpiece zero point several times with G56, the displacement is always added to the currently active zero point.

Parameters

X, Z: Shift (X radius value) – default: 0

Absolute zero point shift G59

G59 sets the workpiece datum to ”X, Z”. The new datum is valid to the end of the program.

Parameters

X, Z: Datum shift (X radius dimension)

G59 cancels all previous zero point shifts (with G51, G53..G55 or G59).

Zero point shift

G121 contour mirror and shift

G121 mirrors and/or shifts the position of roughed and finished part contours. The contour is mirrored in the X axis and shifted in the Z direction. The workpiece datum is not affected.

Parameters

H: Mirroring – default: 0

■ H=0: Contour shift – no mirroring

■ H=1: Contour shift, mirroring, and reversal of the direction of

contour description

Q: Mirroring the coordinate system (direction of the Z axis) - default: 0

■ Q=0: No mirroring

■ Q=1: Mirroring

Z: Shift – default: 0 D: Mirroring XC/XCR (mirroring/shifting the front and rear face

contours) - default: 0

Datum shift

■ D=0: No mirroring/shifting

■ D=1: Mirroring/shifting

• Lateral surface contours are mirrored/shifted like turning contours.

• Auxiliary contours are not mirrored.

• Please note for Q=1: The coordinate system including the contour is mirrored – H=1 mirrors only the contour.

Safety clearance G47

G47 defines the safety clearance for the turning cycles: G810, G820, G830, G835, G860, G869, G890; drilling cycles G71, G72, G74 and milling cycles G840...G846. G47 without parameters activates the parameter values (machining parameters 2, ... – safety clearances).

Parameters

P: Safety clearance

G47 replaces safety clearance set in the machining parameters or that set in G147.

Safety clearance (drilling and milling cycles) G147

G147 defines the safety clearance for milling operations with G840...G846. Parameter ”K” influences the safety clearance for drilling operations (G71, G72, G74). G147 replaces the safety clearance set in ”;Machining parameter 2, ... – safety clearances.”

Parameters

I: Safety clearance in milling direction K: Safety clearance in approach direction (feed)

G147 replaces safety clearance set in the machining parameters or that set in G47.

Switch off allowance with G50

G50 switches off allowances defined with G52/G39Geo for the following cycle.

Allowances, safety clearances

Axis-parallel allowance G57

G57 defines different allowances in X and Z. G57 is programmed before the cycle.

After cycle execution, allowances are

■ deleted: G810, G820, G830, G835, G860, G869, G890

■ not deleted: G81, G82, G83

Parameters

X, Z: Allowance (X diameter value)

If the allowances are programmed with G57 and in the cycle itself, the cycle allowances are used.

Allowances, safety clearances

Contour-parallel allowance (equidistant) G58

G58 defines a contour-parallel allowance. A negative allowance is permitted with G890. G58 is programmed before the cycle.

After cycle execution, allowances are

■ deleted: G810, G820, G830, G835, G860, G869, G890

■ not deleted: G81, G82, G83

Parameters

P: Allowance

If an offset is programmed with G58 and in the cycle, the offset from the cycle is used.

Tool call T

The ”T” is followed by the WAPP number. You can enter the T number directly or select it from the tool list (switch with the CONTINUE key).

WAPP number:

W: Tool carrier number A: Number of the location group PP: Pocket number in the tool carrier

If you are working with multi tools, program

”T PP.S” or ”T WAPP.S” (S = number of the side tooth).

(Changing the) cutter compensation G148

”O” defines the wear and tear compensation values to be compensated. DX and DZ become effective after program start and after a T command.

Parameters

O: Selection – default: 0

■ O=0: DX, DZ active – DS inactive

■ O=1: DS, DZ active – DX inactive

■ O=2: DX, DS active – DZ inactive

The recessing cycles G860, G866 automatically take the ”correct” wear compensation into account.

Tools, types of compensation

Additive compensation G149

The CNC PILOT manages 16 tool-independent compensation values. To activate the additive compensation function, program G149 followed by a „D number“ (for example, G149 D901). ”G149 D900” resets the additive compensation function.

Parameters

D: Additive compensation - default: D900

Range: 900 to 916

Tools, types of compensation

Compensate right tool tip G150 Compensate left tool tip G151

G150/G151 defines the workpiece datum for recessing and button tools.

G150: datum is on right tip G151: datum is on left tip

G150/G151 is effective from the block in which it is programmed and remains in effect up to

■ the next tool change

■ end of the program

• The displayed actual values always refer to the tool tip defined in the tool data.

• Be sure to switch the direction when you work with TRC

Basics of programming

■ The compensation becomes effective only after the

tool has actually moved in the compensation direction by the compensation value. You must therefore program G149 one block before the block in which you want the compensation to apply.

■ An additive compensation remains effective until:

■ The next ”G149 D900”

■ The next tool change

■ The end of the program

End of cycle G80

G80 concludes fixed cycles.

Simple longitudinal roughing G81 Simple face roughing G82

G81/G82 machines (roughs) the contour area described by the current tool position and ”X, Z”. If you wish to machine an oblique cut, you can define the angle with I and K.

The tool moves to clearance at the end of the cycle:

■ G81: X – last lift-off coordinate; Z – cycle start point

■ G82: X – cycle start point; Z – last lift-off coordinate

Parameters

X/Z: Contour target point (X diameter) Q: G-function Infeed – default: 0

■ 0: infeed with G0 (rapid traverse)

■ 1: infeed with G1 (feed rate)

G81:

I: Maximum infeed distance in the X direction

■ I<0: with machining the contour line

■ I>0: without machining the contour line

K: Offset in Z direction – default: 0

G82:

I: Offset in X direction – default: 0 K: Maximum infeed distance in the Z direction

■ K<0: with machining the contour line

■ K>0: without machining the contour line

Simple turning cycles

Simple longitudinal roughing G81

• Cutter radius compensation: is not carried out

• Offsets (G57): are calculated and remain effective after end of cycle.

• Safety clearance after each step: 1 mm.

Simple contour repeat cycle G83

G83 carries out the functions programmed in the following blocks (simple traverse or cycles without contour description) more than once. G80 ends the machining cycle.

If the number of infeeds differs for the X- and Z axes, the tool first advances in both axes with the programmed values. The infeed is set to zero if the target value for one direction is reached.

Notes on programming G83

■ Stands alone in the block

■ Must not be programmed with K variables

■ Must not be nested, not even by calling subprograms

Tool position at end of cycle: Cycle starting point.

Parameters

X/Z: Contour target point (X diameter) - no input: transfer the last X/Z

Simple turning cycles

coordinate

I/K: Maximum infeed (I: radius) – default: 0

• Cutter radius compensation: is not carried out – You can program the TRC separately with G40..G42.

• Offsets: G57-offsets are calculated; G58-offsets only have effect if you are working with TRC. Allowances remain in effect after the end of cycle.

• Safety clearance after each step: 1 mm.

Danger of collision !

After each pass, the tool returns on a diagonal path before it advances for the next pass. If required, program an additional rapid traverse path to avoid a collision.

Undercut cycle G85

With the function G85, you can machine undercuts according to DIN 509 E, DIN 509 F and DIN 76 (thread undercut). The CNC PILOT decides the type of undercut using ”K.” For undercut parameters, see table.

The adjoining cylinder is machined if the tool is positioned at the cylinder diameter (”X”) ”in front of” the cylinder.

The undercut roundings are executed with the radius 0.6 * I.

Parameters

X, Z: Destination point (X as diameter value) I: Depth/wear allowance (radius)

■ DIN 509 E, F: wear allowance – default: 0

■ DIN 76: undercut depth

K: Undercut width and type

■ K no input: DIN 509 E

■ K=0: DIN 509 F

■ K>0: undercut length for DIN 76

E: Reduced feed (for machining the undercut) – no input: active

feed rate

• Cutter radius compensation: is not carried out

• Allowances: are not considered

Continued

Undercut DIN 76 (thread undercut)

Simple turning cycles

Undercut DIN 509 E

Undercut angle for undercuts according to DIN 509 E and F: 15° Transverse angle for an undercut according to DIN 509 F: 8°.

where: I = depth of undercut

K = width of undercut R = undercut radius P = depth of end face

Undercut according to DIN 509 E Diameter I K R

 18 0.25 2 0.6

> 18 – 80 0.35 2.5 0.6

> 80 0.45 4 1

Simple turning cycles

Undercut according to DIN 509 F Diameter I K R P

 18 0.25 2 0.6 0.1

> 18 – 80 0.35 2.5 0.6 0.2

> 80 0.45 4 1 0.3

Undercut DIN 509 F

Recessing G86

G86 machines simple radial and axial recesses with chamfers. From the tool position the CNC PILOT calculates a radial/axial or an inside/outside recess.

If you program an allowance, the control always rough-machines the recess first. In the second step, the recess is then finish-machined.

G86 machines chamfers at the sides of the recess. If you do not wish to cut the chamfers, you must position the tool at a sufficient distance from the workpiece. Calculation of the starting position XS (diameter):

XS = XK + 2 * (1,3 – b) XK: Contour diameter

b: Chamfer width

Tool position at end of cycle:

■ Radial recess: X – Starting position; Z – last recess position

■ Axial recess: X – last recess position; Z – start position

Parameters

X, Z: Target point (X diameter)

Radial recess:

I: Allowance

■ I>0: Allowance (roughing and finishing)

■ I=0: No finishing

K: Recess width – no input: a single cut is machined (recess width

= tool width)

Simple turning cycles

Axial recess:

I: Recess width – no input: a single cut is

machined (recess width = tool width)

K: Allowance

■ K>0: Allowance (roughing and finishing)

■ K=0: No finishing

E Period of dwell (dwell time for chip breaking) –

default: Duration of on revolution

■ With finishing allowance: Only for finishing

■ Without finishing allowance: for every

recess

• Cutter radius compensation: is not carried out

• Allowances are not considered.

Transition radii G87

G87 machines transition radii at orthogonal, paraxial inside and outside corners. The direction for the rounding is taken from the ”position/ machining direction” of the tool.

A preceding longitudinal or transverse element is machined if the tool is located at the X or Z coordinate of the corner before the cycle is executed.

Parameters

X, Z: Corner point (X diameter) B Radius E Reduced feed rate – no input: active feed rate

• Cutter radius compensation: is carried out

• Allowances are not considered.

Simple turning cycles

Chamfer G88

G88 machines chamfers at orthogonal, paraxial outside corners. The direction for the chamfer is taken from the ”position/machining direction” of the tool

A preceding longitudinal or transverse element is machined if the tool is located at the X or Z coordinate of the corner before the cycle is executed.

Parameters

X, Z: Corner point (X diameter) B Chamfer width E Reduced feed rate – no input: active feed rate

• Cutter radius compensation: is carried out

• Allowances are not considered.

Longitudinal roughing G810 / Face roughing G820

G810/G820 cuts (roughs) the contour range defined by ”NS, NE.”

Parameters

NS, NE: Starting block number, end block number (from the contour

description) P: Maximum approach - Maximum infeed distance I, K: Allowances (I diameter value) – default: 0 E: Approach behavior

■ E=0: descending contours are not machined

■ E>0: approach behavior

■ no input: feed rate reduced depending on approach angle –

maximum reduction: 50% X/Z: Cutting limit (X diameter value) H: Type of contour smoothing – default: 0

■ H=0: smoothing after each cut

■ H=1: lift off at under 45°, smoothing after last cut

■ H=2: lift off at under 45°, no smoothing

A: Approach angle (reference: Z axis)

■ G810 – default: 0°/180° (parallel to Z axis)

■ G820 – default: 90°/270° (perpendicular to Z axis)

W: Departing angle (reference: Z axis)

■ G810 – default: 90°/270° (perpendicular to Z axis)

■ G820 – default: 0°/180° (parallel to Z axis)

Q: Type of retraction after machining – default: 0

n Q=0: return to starting point (G810: first X and then Z direction;

G820: first Z and then X direction)

■ Q=1: position in front of finished contour

■ Q=2: move to clearance height and stop

Contour roughing, longitudinal G810

Contour-determined

turning cycles

Continued

V: Machining chamfers/roundings at start/end of contour – default: 0

chamfer/rounding is machined:

■ V=0: at beginning and end

■ V=1: at beginning

■ V=2: at end

■ V=3: no machining at start or end

■ V=4: only single chamfers/roundings are machined – not the

base element (requirement: the contour consists of a contour element)

D: Omit element (influences the machining of undercuts, free

rotations: see table) – default: 0

B: Slide feed for 4-axis machining

■ B=0: Both slides work on the same diameter – at double feed

rate

■ B<>0: Distance from the ”leading” slide (the lead). The slides

work at equal feed rate on different diameters.

■ B<0: The slides with larger number leads

Contour-determined

turning cycles

■ B>0: The slide with smaller number leads.

D G22 G23 G23 G25 G25 G25 = H0 H1 H4 H5/6 H7..9

0 •••••• 1 •••––– 2 ••–••• 3 ••–––– 4 ••––•–

„•“: Hide elements

Contour face roughing G820

• Cutter radius is compensated

• Offsets (G57/G58): are effective

• On 4-axis cycles, ensure that the tools are

identical (tool type, cutting edge radius, cutting edge angle, etc.).

Contour-parallel roughing G830

G830 machines (roughs) the contour area defined by ”NS, NE” parallel to the contour.

Parameters

NS, NE: Starting block number, end block number (from the contour

description) P: Maximum approach - Maximum infeed distance I, K: Allowances (I diameter value) – default: 0 X/Z: Cutting limit (X diameter value) A, W: Approach angle, departure angle (reference: Z axis)

■ Approach angle – default: 0°/180° (parallel to Z axis)

■ Departure angle – default: 90°/270° (perpendicular to Z axis)

Q: Type of retraction after machining – default: 0

■ Q=0: return to starting point (first X and then Z direction)

■ Q=1: position in front of finished contour

■ Q=2: move to clearance height and stop

V: Machining chamfers/roundings at start/end of contour – default:

0; chamfer/rounding is machined:

■ V=0: at beginning and end

D G22 G23 G23 G25 G25 G25 = H0 H1 H4 H5/6 H7..9

0 •••••• 1 •••––– 2 ••–••• 3 ••–––– 4 ••––•–

■ V=1: at beginning

■ V=2: at end

■ V=3: no machining at start or end

■ V=4: only single chamfers/roundings are

machined – not the base element (requirement: the contour consists of a contour element)

D: Omit element (influences the machining of

undercuts, free rotations: see table) – default: 0

• Cutter radius compensation: is carried out

• Offsets (G57/G58): are effective

Contour-determined

turning cycles

„•“: Skipping elements

Contour-parallel with neutral tool G835

G835 machines the contour area defined by ”NS, NE” parallel to the contour and bidirectionally.

Parameters

NS, NE: Starting and end block numbers (reference to contour section) P: Maximum approach - Maximum infeed distance

I, K: Allowances (I diameter value) – default: 0 X/Z: Cutting limit (X diameter value) A, W: Approach angle, departure angle (reference: Z axis)

Approach angle – default: 0°/180° (parallel to Z axis)

Departure angle – default: 90°/270° (perpendicular to Z axis)

Q: Type of retraction after machining – default: 0

Q=0: return to starting point (first X and then Z direction)

Contour-determined

turning cycles

V: Machining chamfers/roundings at start/end of contour – default: 0

Q=1: position in front of finished contour

Q=2: move to clearance height and stop

chamfer/rounding is machined:

V=0: at beginning and end

D G22 G23 G23 G25 G25 G25 = H0 H1 H4 H5/6 H7..9

0 •••••• 1 •••––– 2 ••–••• 3 ••–––– 4 ••––•–

V=1: at beginning

V=2: at end

V=3: no machining at start or end

V=4: only single chamfers/roundings are machined – not the base element (requirement: the contour must consist of one element)

D: Skip the element (influences the machining of

undercuts, free rotations: see table) – default: 0

• Cutter radius compensation: is carried out

• Offsets (G57/G58): are effective

„•“: Skipping elements

Recessing G860

G860 machines (indents) the contour area defined by ”NS, NE” axially/ radially.

Parameters

NS, NE: Starting block number, end block number (reference on contour

section or NS = reference on a recess described with G22-/G23-

Geo) I, K: Allowances (I diameter value) – default: 0 Q: Sequence – default: 0

Q=0: roughing and finishing

Q=1: roughing only

Q=2: finishing only X/Z: Cutting limit (X diameter value) V: Machining chamfers/roundings at start/end of contour – default: 0

chamfer/rounding is machined:

V=0: at beginning and end

V=1: at beginning

V=2: at end

V=3: no machining E: Finishing feed rate – no input: active feed rate H: Retraction at end of cycle – default: 0

H=0: return to starting point (axial recess: first Z and then X

direction; radial recess: first X and then Z direction)

H=1: position in front of the finished contour

H=2: move to safety clearance and stop

• Cutter radius compensation: is carried out

• Offsets (G57/G58): are effective

Contour-determined

turning cycles

Recessing cycle G866

G866 makes a recess defined with G22-Geo Calculation of the cut segmentation (SBF: see machining parameter 6):

Maximum offset = SBF * cutting edge width

Parameters

NS: Block number (reference to G22-Geo) I: Allowance (with precutting) – default: 0

■ I=0: recess is machined in one run

■ I>0: precutting is carried out in the first run; and finishing in the

second

E: Dwell time – no input: corresponds to a spindle revolution

■ With I=0: for each recess

■ With I>0: only during finishing

Contour-determined

turning cycles

• Cutter radius compensation: is carried out

• Allowances: are not considered

Recess turning cycle G869

G869 machines the contour described by ”NS, NE” axially and radially with alternating recessing and roughing movements.

Parameters

NS, NE: Starting block number, end block number (from the contour

description) P: Maximum approach - Maximum infeed distance R: Turning depth compensation for finishing – default: 0 I, K: Allowances (I diameter value) – default: 0 X/Z: Cutting limit (X diameter value) A, W: Approach angle, departure angle – default: opposite from the

recessing direction Q: Sequence – default: 0

Q=0: roughing and finishing

Q=1: roughing only

Q=2: finishing only

U: Direction of turning – default: 0

U=0: Bidirectional turning

U=1: Unidirectional turning in direction of contour

H: Retraction at end of cycle – default: 0

H=0: return to starting point (axial recess: first Z and then X

direction; radial recess: first X and then Z direction)

H=1: position in front of the finished contour

H=2: move to safety clearance and stop

V: Machining chamfers/roundings at start/end of contour – default: 0

chamfer/rounding is machined:

V=0: At beginning and end

V=1: At beginning

V=2: At end

V=3: No machining

O: Recessing feed rate – default: active feed rate

E: Finishing feed rate – no input: active feed rate B: Offset width – default: 0

• Cycle G869 requires type 26* tools.

• Cutter radius compensation: is performed

• Offsets (G57/G58): are effective

Contour-determined

turning cycles

Contour finishing G890

G890 finishes the contour area defined by ”NS, NE” parallel to the contour.

Parameters

NS, NE: Starting block number, end block number (from the contour

description)

E: Approach behavior

E=0: descending contours are not machined

nÿ

E>0: approach behavior

no input: feed rate reduced depending on approach angle –

maximum reduction: 50%

V: Machining chamfers/roundings at start/end of contour – default:

0; chamfer/rounding is machined:

V=0: at beginning and end

nÿ

V=1: at beginning

nÿ

Contour-determined

turning cycles

Q: Type of approach – default: 0

V=2: at end

nÿ

V=3: no machining at start or end

nÿ

V=4: only single chamfers/roundings are machined – not the base element (requirement: the contour consists of a contour element)

nÿ

Q=0: automatic selection – the CNC PILOT checks the possibilities for approach:

– diagonal approach – first X direction, then Z – equidistant around the barrier – Omission of the first contour element if the start position is

inaccessible

nÿ

Q=1: First in X direction, then Z

nÿ

Q=2: First in Z direction, then X

nÿ

Q=3: No approach – tool is in the proximity of the starting point of the contour section

nÿ

Q=4: Residual finishing

H: Type of retraction – default: 3

tool lifts off under 45° in the opposite direction to machining and moves as follows to the position ”I, K”:

nÿ

H=0: diagonal

nÿ

H=1: first X, then Z direction

nÿ

H=2: first Z, then X direction

nÿ

H=3: remains at safety clearance

nÿ

H=4: no retraction movement – tool remains

at the end coordinate

X/Z: Cutting limit (X diameter value) - no input: no

limit

D: Omit element (influences the machining of

undercuts, free rotations and recesses: see table) – default: 1

Continued

I, K: End point which is approached at the end of

the cycle – except for H=3 or 4 (I diameter value)

O: Feed rate reduction – default: 0

nÿ

O=0: No feed rate reduction

nÿ

O=1: Feed rate reduction active

During residual finishing (G890 – Q4), the CNC PILOT, checks whether the tool can access the contour recess without collision. The tool parameter ”width dn” is the basis of this collision check.

D G22 G23 G23 G25 G25 G25 G25 Form (H0) (H1) U E, F G, H K

0 ––––––– 1 ––•–••• 2 ––•–––– 3 ––––••• 4 ––•––•• 5 ––•–••– 6 ––•–•–– 7 •••••••

„•“: Skipping elements

Other D codes for skipping undercuts/recesses:

G-call Function D code

G22 Gasket recess 512 G22 Retaining ring recess 1.024 G23 H0 General recess 256 G23 H1 Free rotation 2.048 G23 H4 Undercut form U 32.768 G23 H5 Undercut form E 65.536 G23 H6 Undercut form F 131.072 G23 H7 Undercut form G 262.144 G23 H8 Undercut form H 524.288 G23 H9 Undercut form K 1.048.576

Contour-determined

turning cycles

Thread cycle G31

G31 machines threads defined with G24-Geo, G34-Geo or G37-Geo. G31 also machines successions of threads and multiple threads.

Chamfer length, overrun length: If you do not program ”B, P”,the CNC PILOT will automatically determine the lengths from adjacent undercuts or axis-parallel recesses. If no undercut/recess exists, the chamfer and overrun lengths from Machining Parameter 7 will be used.

Parameters

NS: Block number (from the finished part description containing the

basic block G1-Geo for thread contour definition)

I: Maximum approach - Maximum infeed distance B, P: Chamfer length, overrun length D: Cutting direction (reference: defined direction for basic element)

– default: 0;

Thread cycle group

■ D=0: same direction

■ D=1: opposite direction

V: Type of feed – default: 0;

■ V=0: constant cross section for all cuts

■ V=1: constant feed

■ V=2: with distribution of remaining cut – if the division thread

depth/feed provides a remainder, the first feed is reduced. The last cut is divided into four partial cuts: 1/2, 1/4, 1/8 and 1/8.

■ V=3: without remaining cut division – feed is calculated from

pitch and speed

H: Type of offset – default: 0

■ H=0: no offset

■ H=1: offset to the left

■ H=2: offset to the right

■ H=3: offset alternating left and right

Q: Number of air cuts after the last cut – default: 0 C: Starting angle – default: 0

•”Feed rate stop” becomes effective only at the end of a thread cut.

• Feed rate override is not effective.

• Do not use the spindle override if the

feedforward is switched off!

Danger of collision!

An excessive overrun length P can cause collision. You can check the overrun length in the simulation.

Simple thread cycle G32

G32 cuts a simple thread in any desired direction and position (longitudinal, tapered or transverse thread; internal or external thread). G32 calculates the thread to be cut from the ”thread end point,” ”thread depth” and the current tool position.

Parameters

X, Z: End point of thread (X diameter) F: Thread pitch P: Thread depth I: Cutting depth B: Remainder cut – default: 0

■ B=0: division of the last cut into 1/2, 1/4, 1/8, 1/8 cut.

■ B=1: no remaining cut division

Q: Number of air cuts after the last cut – default: 0 K: Runout length – default: 0 (see G33) W: Taper angle (range: –45° < W < 45°) – default: 0; position of the

taper thread with reference to longitudinal or transverse axis.

■ W>0: Rising contour (in machining direction)

■ W<0: Falling contour

C: Starting angle – default: 0 H: Type of offset – default: 0

■ H=0: no offset

■ H=1: offset to the left

■ H=2: offset to the right

■ H=3: offset alternating left and right

Thread cycle group

•”Feed rate stop” becomes effective only at the end of a thread cut.

• Feed rate override is not effective.

• Spindle override is not effective.

• Create thread with G95 (feed rate per

revolution).

• Look-ahead control is switched off.

Individual thread cut G33

G33 cuts threads in any desired direction and position (longitudinal, tapered or transverse threads; internal or external threads). The thread starts at the current tool position and ends at ”X, Z”.

Parameters

X, Z: Diameter, length to end point of thread (X diameter) F: Feed rate per revolution (thread pitch) B, P: Chamfer length, overrun length – default: 0 (see G33) C: Starting angle – default: 0 Q: Number of the spindle H: Reference direction for spindle pitch - default: 0

■ H=0: Feed rate on Z axis (for longitudinal and tapered threads

up to a maximum angle of +45°/–45° to Z axis

■ H=1: Feed rate in X axis (for transverse and taper threads up

Thread cycle group

to a maximum angle of 45°/–45° to the X axis

■ H=2: Feed rate in Y axis

■ H=3: contouring feed rate

E: Variable pitch (increases/reduces the pitch per revolution by E) –

default: 0

•”Feed rate stop” becomes effective only at the end of a thread cut.

• Feed rate override is not effective.

• Do not use the spindle override if the feedforward is

switched off!

• Create thread with G95 (feed rate per revolution).

Calculation of ”thread run-in/runout distances”

The slide requires a run-in distance to accelerate to the programmed feed rate before starting the actual thread, and a runout distance at the end of the thread to decelerate again.

Calculation of chamfer (run-in) length:

BA > 0.75 * (F*S)² / a + 0.15

Calculation of runout length:

BE > 0.75 * (F*S)² / e + 0.15

BA: Minimum run-in length BE: Minimum runout length F: Spindle pitch in mm/revolution S: Speed in revolutions/second a, e: Acceleration in mm/s² (a = ”acceleration at

start of block”; e = ”acceleration at end of block” from Machine Parameter 1105, ff)

Tapping cycle G36

G36 can be used for axial and radial threads using driven or stationary tools. Depending on ”X/Z”, G36 decides whether a radial or n axial thread will be machined.

Parameters

X: Diameter – end point of thread for axial machining Z: Length – end point of thread with radial machining F: Feed per revolution - thread pitch Q: Number of spindle - default: 0 (main spindle) B: Chamfer length (see G33) H: Reference direction for thread pitch – default: 0

■ H=0: Feed rate on the Z axis

■ H=1: Feed rate on the X axis

■ H=2: Feed rate on the Y axis

■ H=3: Contour feed rate

S: Retraction speed

default: Same spindle speed as for tapping

•”Cycle STOP” becomes effective only at the end of a thread cut.

• Feed rate override is not effective.

• Do not use spindle override !

• With uncontrolled tool drive, a floating tap holder is required.

Drilling cycle group

Simple drilling cycle G71

G71 is used for axial and radial boring on the end faces or lateral surface using driven or stationary tools.

The cycle is used for:

■ A single hole without contour description

■ Boring with contour description (single hole or hole pattern)

Parameters

NS: Contour block number with boring geometry (G49, G300- or

G310-Geo) – no input: single hole without contour description X, Z: Position, length – end points of axial/radial hole (X diameter) E: Delay time in seconds (dwell time for chip breaking at end of

hole) – default: 0 V: Feed rate reduction (50%) – default: 0

■ V=0 or 2: Feed rate reduction at start

Drilling cycle group

■ V=1 or 3: Feed rate reduction at start and end

■ V=4: Feed rate reduction at end

■ V=5: No feed rate reduction

Exception for V=0 and V=1: No feed rate reduction when

boring/drilling with indexable inserts and twist drills with 180°

angle D: Retraction speed – default: 0

■ D=0: Rapid traverse

■ D=1: Feed rate

K: Retraction level (radial holes and holes in the YZ plane: Diameter)

– No input: Tool moves to starting position or safety clearance

• Single hole without contour description: Program „X or Z“ as alternative.

• Hole with contour description: Do not pro- gram „X, Z“.

• Hole pattern: ”NS” refers to the bore hole

contour (and not the definition of the pattern).

Boring, sinking G72

G72 can be used for boring, sinking, reaming, tapping or centering on the end faces or lateral surface using driven or stationary tools.

Parameters

NS: Contour block number with boring geometry (G49, G300- or

G310-Geo)

E: Delay (dwell time for chip breaking at end of hole)

default: 0

D: Retraction speed – default: 0

nÿ

D=0: Rapid traverse

nÿ

D=1: Feed rate

K: Retraction level (radial hole: diameter) – no input: tool returns to

starting position/moves to clearance height

Hole pattern: ”NS” points to the contour of the hole (not to the pattern definition).

Drilling cycle group

Tapping G73

G73 can be used for axial and radial threads using driven or stationary tools.

Parameters

NS: Contour block number with boring geometry (G49, G300- or

G310-Geo)

B: Chamfer length – default: Machining Parameter 7 ”Thread

chamfer length [GAL]” S: Retraction speed – default: tapping speed K: Retraction level (radial holes and holes in the YZ plane: Diameter)

– No input: Tool moves to starting position or safety clearance J: Pull-out length during use of collets with length compensation –

default: 0

Drilling cycle group

• Hole pattern: ”NS” refers to the bore hole contour (and not the definition of the pattern).

•”Cycle STOP” only becomes effective at the end of a thread cut.

• Feed rate override is not effective.

• Do not use spindle override !

Deep drilling G74

G74 can be used for axial and radial holes on the end faces or lateral surface using driven or stationary tools. The hole is drilled in several passes.

The cycle is used for:

■ A single hole without contour description

■ Boring with contour description (single hole or hole pattern)

Parameters

NS: Contour block number with boring geometry (G49, G300- or

G310-Geo) – no input: single hole without contour description X, Z: Position, length – end points of axial/radial holes (X diameter) P: 1st drilling depth I: Reduction value – default: 0 B: Return distance

default: Retract to ”starting point of hole” J: Minimum hole depth - default: 1/10 of P E: Delay (dwell time for chip breaking at end of hole)

default: 0 V: Feed rate reduction (50%) – default: 0

■ V=0 or 2: Feed rate reduction at start

■ V=1 or 3: Feed rate reduction at start and end

■ V=4: Feed rate reduction at end

■ V=5: No feed rate reduction

Exception for V=0 and V=1: No feed rate reduction when

boring/drilling with indexable inserts and twist drills with 180°

angle D: Retraction speed and infeed within the hole – default: 0

■ D=0: Rapid traverse

■ D=1: Feed rate

K: Retraction level (radial holes: diameter) – no

Drilling cycle group

input: tool returns to starting position/moves to clearance height

• Single hole without contour description: Program „X or Z“ as alternative.

• Hole with contour description: Do not program „X, Z“.

• Hole pattern: ”NS” refers to the bore hole contour (and not the definition of the pattern).

• A ”feed rate reduction at end” goes into effect only at the last drilling stage.

Reference diameter G120

G120 determines the reference diameter of the unrolled cylindrical surface. G120 is necessary if you are using ”CY” (with G110...G113). G120 is a modular function.

Parameters

X: Diameter

Datum shift in C axis (absolute) G152

G152 defines a datum shift for the C axis (reference: Machine Parameter 1005, ff ”Reference point C axis”). The datum is valid until the end of the program.

Parameters

C axis

C: Angle of the new C-axis datum

Standardize C axis G153

G153 resets a traverse angle >360° or <0° to the corresponding angle modulo 360° – without moving the C axis.

G153 is used only for cylindrical surface machining. An automatic modulo 360° function is carried out on the end faces.

Rapid traverse on end face G100

The tool moves at rapid traverse along the shortest path to the ”end point.”

Parameters

X, C: End point, end angle XK,YK: End point Z: end points

Program either X, C or XK, YK.

Linear segment on end face G101

The tool moves at the programmed feed rate on a line to the ”end point.”

Parameters

X, C: End point, end angle XK,YK: End point Z: End depth – default: current Z position

Program either X, C or XK, YK.

Front/end face machining

Circular arc on end face G102 / G103

The tool moves in a circular arc at the feed rate to the ”end point.”

Parameters

X, C: End point, end angle XK,YK: End point R: Radius I, J: Center point (in Cartesian coordinates) Z: End depth – default: current Z position H: Circular plane (working plane) – default:

■ H=0, 1: normal facing (XY plane)

■ H=2: Machining in YZ plane

■ H=3: Machining in XZ plane

K: Midpoint (Z-direction) – only for H=2, 3

Front/end face machining

• Program either X, C or XK, YK.

• Program either center or radius.

• Radius input: circular arc only possible  180°

• If the end point is the original coordinate starting point, enter

XK=0 and YK=0.

Circular arc G102

Circular arc G103

Rapid traverse on cylindrical surface G110

The tool moves at rapid traverse along the shortest path to the ”end point.”

Parameters

Z, C: End point, end angle CY: End point as linear value (referenced to unrolled reference

diameter G120)

X: End point (diameter)

Program either Z, C or Z, CY.

Linear movement on the cylindrical surface G111

The tool moves at the programmed feed rate on a line to the ”end point.”

Parameters

Z, C: End point, end angle CY: End point as linear value (referenced to unrolled reference

diameter G120)

X: End depth (diameter value) – default: current X-position

Program either Z, C or Z, CY.

Cylindrical surface machining

Circular arc on lateral surface G112 / G113

The tool moves in a circular arc at the feed rate to the ”end point.”

Parameters

Z, C: End point, end angle CY: End point as linear value (referenced to unrolled reference

diameter G120) R: Radius K, W: Position, angle to midpoint J: Center point coordinate as a linear value (referenced to unrolled

G120 reference diameter) X: End depth (diameter value) – default: current X-position

• Program either Z, C or Z and CY, or K, W or K and J.

• Program either center or radius.

Cylindrical surface

machining

• If you program a radius, the arc size cannot exceed 180°.

Circular arc G112

Circular arc G113

Contour milling G840

G840 mills, finishes, engraves or deburrs figures or ”free contours” (open or closed).

Parameters

Q: Cycle type (= milling location)

nÿ

Q=0: milling center on the contour (without radius

compensation)

nÿ

Q=1 – closed contour: inside milling

nÿ

Q=1 – open contour: left in machining direction

nÿ

Q=2 – closed contour: outside milling

nÿ

Q=2 – open contour: right in machining direction

nÿ

Q=3 (only with open contours): It depends on the ”cutting direction H” and the direction of tool rotation whether the tool cuts from the left or right of the contour.

NS: Block number – Beginning of contour section

nÿ

Figures: Block number of the Figure

nÿ

”free contour” (open or closed): first contour element (not starting point).

NE: Block number – End of contour section

nÿ

Figures: no entry

nÿ

Closed contours: entry unnecessary

nÿ

Open contours: last contour element to be milled

nÿ

Contour consists of one element: entry unnecessary

H: Cutting direction – default: 0

nÿ

H=0: up-cut milling

nÿ

H=1: climb milling

I: (Maximum) infeed – no entry: milling in one infeed F: Feed rate for infeed – default: active feed rate E: Reduced feed rate for circular elements – no entry: current feed

rate

Milling

R: Radius of approaching/departing arc – default: 0

nÿ

R=0: contour element is approached directly; feed to starting

point above the milling plane – then vertical plunge

nÿ

R>0: Tool moves on an approaching/departing arc that

connects tangentially to the contour element.

nÿ

R<0 for inside corners: tool moves on an approaching/

departing arc that connects tangentially to the contour element.

nÿ

R<0 for outside corners: length of linear approaching/departing

element; contour element is approached/departed tangentially.

P: Milling depth

nÿ

Milling, finishing – no entry: milling depth from the contour

description

nÿ

Deburring: plunging depth of the tool

K: Return plane – no input: Tool returns to the starting position

nÿ

Front or rear face: Return position in Z direction

nÿ

lateral surface: Return position in X direction (diameter)

B: Chamfer width for deburring the upper edges (sign has no

Milling

significance)

J: Preparation diameter (tool diameter from machining)

nÿ

Required for deburring of open contours.

nÿ

Not required, if diameter of deburring tool = diameter of milling

tool.

D, V: Beginning, end of element number for figures (only if partial

figures are machined)

See the ”CNC PILOT 4290 User's Manual” for the figure element numbers.

Pocket milling – roughing G845 Pocket milling – finishing G846

G845 roughs, G846 finishes closed contours and figures.

Parameters

NS: Block number (reference to contour section) P: (Maximum) milling depth (infeed in the working plane) R: Radius of approaching/departing arc – default: 0 (only with G846)

nÿ

R=0: contour element is approached directly; feed to approach point above the milling plane – then perpendicular feed to plunging depth

nÿ

R>0: mill moves along approaching/departing arc, which connects tangentially with the contour element

I, K: Allowance in X, Z direction (only with G845) U: (minimum) overlap factor – overlap of tool paths (overlap = U*

cutter diameter) – default: 0.5

V: Overrun factor – has no significance for machining with the C

axis

H: Cutting direction – default: 0

nÿ

H=0: up-cut milling

nÿ

H=1: climb milling

F: Feed rate for infeed – default: active feed rate E: Reduced feed rate for circular elements – no entry: current feed

rate

J: Return plane – no input: Tool returns to the starting position

nÿ

Front or rear face: Return position in Z direction

nÿ

lateral surface: Return position in X direction (diameter)

Q: Machining direction – default: 0

nÿ

Q=0: from the inside toward the outside

nÿ

Q=1: from the outside toward the inside

Milling

Period of dwell G4

The CNC PILOT interrupts the program run for the programmed length of time before executing the next program block. If G4 is programmed together with a path of traverse in the same block, the dwell time only becomes effective after the path of traverse has been executed.

Parameters

F: Period of dwell

Range: 0 sec < F < 99.999 sec

Precision stop ON G7

G7 switches the ”precision stop” on modally. With a precision stop the CNC PILOT does not run the following block until the last point has been reached in the tolerance window for position (tolerance window: machine parameter 1106, ff ”position control for linear axis”).

Other G Functions

A precision stop affects single contours and cycles. The NC block containing G7 is also executed with a precision stop.

Precision stop OFF G8

G8 switches the precision stop off. The block containing G8 is executed

without a precision stop.

Block precision stop G9

G9 activates a precision stop for the NC block in which it is programmed (see also ”G7”).

Switch off protection zone G60

resets protection zone monitoring. G60 is programmed before the traversing command that is to be monitored or not monitored.

Parameters

■ No input: Deactivate protective zone

monitoring for this block

■ Q=0: Activate protective zone (modal)

■ Q=1: Deactivate protective zone (modal)

Chuck selection G65

G65 shows the chuck in the simulation. G65 must be programmed separately for every chuck. G65 H.. without X, Z deletes the chuck.

Chucks are described in the database and are defined in CLAMPING DEVICE (H=1..3).

”Q” determines the degree and the type of clamping (external or internal).

Parameters

H: Chuck number (H=1..3: Reference to CLAMPING DEVICE) X, Z: Starting point – Position of the chuck reference point (X

diameter) – Reference: workpiece datum

D: Spindle number (reference: ”CLAMPING DEVICE” section) Q: Grip form for chuck jaws (H=2) – no input: Q from the

”CLAMPING DEVICE” section.

Spindle with workpiece G98

With G98 you can define which spindle is holding the workpiece. The assignment of workpiece to spindle is necessary for thread cutting,

boring and threading cycles if the workpiece is not being held by the main spindle.

Parameters

Q: Spindle number – default: 0 (main spindle)

Other G Functions

Storing/loading contour follow-up G702

G702 Q0 stores the current contour without influencing the contour follow-up function.

G702 Q1 loads the stored contour; follow-up continues with the new contour.

Parameters

Q: Store/load current contour

■ Q=0: store

■ Q=1: load

Other G Functions

Spindle synchronization G720

G720 controls the workpiece transfer from the master to the slave spindle and synchronizes functions such as polygonal turning jobs.

Where: Q * master speed = F * slave speed

Parameters

S: Number of the master spindle [1..4] H: Number of the slave spindle [1..4] – no input or

H=0: Switches off the spindle synchronization C: Offset angle [°] – default: 0° Q: Master speed factor – default: 1;

Range: –100  Q  100 F: Slave speed factor – default: Q take effect;

Range: –100  F  100

Regeneration of the contour G703

If changeable variables are used during run-time conditions ”{V...},” CNC PILOT switches off the contour regeneration function within an IF program branch and during a WHILE loop. It is switched on again after ENDIF/ENDWHILE.

With G703 you can switch on the contour regeneration function for THEN or ELSE branches.

Parameters

Q: Contour regeneration On/Off

nÿ

Q=0: Off

nÿ

Q=1: On

C-angle offset G905

G905 measures the angular offset which occurs during workpiece transfer with a ”rotating spindle”. The programmed ”angle C” is added to the measured offset and becomes effective as the datum shift value for the C axis.

Parameters

Q: Number of the C axis C: Angle of additional datum shift for displaced

infeed – Range: –360°  C  360°; default: 0°

Look-ahead G918

Look-ahead control can be switched On/Off with G918. G918 is programmed in a separate NC block before/after thread machining (G31, G32, G33).

Parameters

Q: Look-ahead On/Off – default: 1

nÿ

Q=0: off

nÿ

Q=1: on

Zero point shifts, deactivating tool lengths G921

G921 ”deactivates” the workpiece datum, all datum shifts and the tool dimensions. Traverse paths and position values are referenced to the distance slide

reference point – machine datum.

Spindle override 100% G919

The spindle override function can be switched On/Off with G919.

Parameters

Q: Spindle number – default: 0 H: Type of limit – default: 0

■ H=0: switch on spindle override

■ H=1: switch spindle override to 100% – modular

■ H=2: switch spindle override to 100% – for the current NC

block

Deactivating zero point shifts G920

G920 deactivates the workpiece zero point and all zeto point shifts. Traverse paths and position values are referenced to the distance tool tip

– machine datum.

Activate zero point shifts G980

G980 activates the workpiece datum and all datum shifts.

Traverse paths and position values are now referenced to the distance tool tip – workpiece datum, while taking the datum shifts into consideration.

Zero point shifts, activating tool lengths G981

G981 activates the workpiece datum, all datum shifts and the tool dimensions.

Traverse paths and position values are now referenced to the distance tool tip – workpiece datum, while taking the datum shifts into consideration.

Other G Functions

Subprograms

Calling a subprogram: L“12345678“ V1 Meaning:

nÿ

External subprograms are defined in a separate file. They can be called from any main program, other subprograms, or from TURN PLUS.

nÿ

Local subprograms are in the same file as the main program. They can only be called from the main program.

nÿ

Subprograms can be ”nested” up to 6 times. Nesting means that another subprogram is called from within a subprogram.

nÿ

Recursion should be avoided.

nÿ

You can add up to 20 „transfer values“ to a subprogram. The designations (parameter designations) are:

LA..LF, LH, I, J, K, O, P, R, S, U, W, X, Y, Z.

Subprograms

The transfer values are available as variables within the subprogram. The identification code is: „#__..“, followed by the parameter designation in lower-case letters (for example: #__la).

You can use the transfer values when programming with variables within the subprogram.

nÿ

The variables #256..#285 are available in every subprogram as local variables.

nÿ

If a subprogram is to be executed repeatedly, enter the number of times the subprogram is to be repeated in the parameter ”number repeats Q.”

nÿ

A subprogram ends with RETURN.

The parameter ”LN” is reserved for the transfer of block numbers. This parameter may receive a new value when the NC program is renumbered.

HEIDENHAIN CNC Pilot 4290 User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual