Pattern definition with PATTERN DEF

Application

You use the PATTERN DEF NC function to easily define regular machining patterns, which you can call with the CYCL CALL PAT NC function. Just like in cycle definitions, help graphics are available for pattern definition that clearly indicate the input parameters required.

 
Notice
Danger of collision!
The PATTERN DEF function calculates the machining coordinates in the X and Y axes. For all tool axes apart from Z there is a danger of collision in the following operation!
  1. Use PATTERN DEF only in connection with the tool axis Z

To navigate to this function:

Insert NC function Special functions Contour/point machining Pattern PATTERN DEF

Possible setting

Definition

Further information

POS and /POS

Point

Definition of up to any 9 machining positions

ROW

Row

Definition of a single row, straight or rotated

PAT

Pattern

Definition of a single pattern, straight, rotated or distorted

FRAME

Frame

Definition of a single frame, straight, rotated or distorted

CIRC

Circle

Definition of a full circle

PITCHCIRC

Pitch circle

Definition of a pitch circle

Programming PATTERN DEF

To program the PATTERN DEF functions:

  1. Select Insert NC function
  2. The control opens the Insert NC function window.

  1. Select the desired machining pattern (e.g., PATTERN DEF CIRC for a full circle)
  2. The control opens the dialog for entering PATTERN DEF.
  3. Enter the required definitions
  4. Define the machining cycle (e.g., Cycle 200) DRILLING
  5. Call cycle with CYCL CALL PAT
 
Tip

While you are programming a machining pattern, you can switch to a different machining pattern in the Form column.

Calling PATTERN DEF

As soon as you have entered a pattern definition, you can call it with the CYCL CALL PAT NC function.

Calling cycles

The control performs the most recently defined machining cycle on the machining pattern you defined.

Program structure: Machining with PATTERN DEF

0 BEGIN SL 2 MM

...

11 PATTERN DEF POS1 (X+25 Y+33.5 Z+0) POS2 (X+15 IY+6.5 Z+0)

12 CYCL DEF 200 DRILLING

...

13 CYCL CALL PAT

Notes

Programming note

  • Before CYCL CALL PAT, you can use the GLOBAL DEF 125 function with Q345=1. Then, between the holes, the control always positions the tool to the 2nd set-up clearance that was defined in the cycle.

Operating notes:

  • A machining pattern remains active until you define a new one, or select a point table with the SEL PATTERN function.
  • Selecting the point table in the NC program with SEL PATTERN

  • The control retracts the tool to the clearance height between the starting points. Depending on which is greater, the control uses either the tool axis position from the cycle call or the value from cycle parameter Q204 as the clearance height.
  • If the coordinate surface in PATTERN DEF is larger than in the cycle, the set-up clearance and the 2nd set-up clearance reference the coordinate surface in PATTERN DEF.
  • You can use the mid-program startup function to select any point at which you want to start or continue machining.
  • Block scan for mid-program startup

Defining individual machining positions

 
Tip

Programming and operating notes:

  • You can enter up to 9 machining positions. Confirm each entry with the ENT key.
  • POS1 must be programmed with absolute coordinates. POS2 to POS9 can be programmed as absolute or incremental values.
  • If you have defined a Workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.
  • You can use the /POS syntax element to hide positions that are already defined. The control will then skip these positions.

Help graphic

Parameter

POS1: X coord. of machining position

Enter the X coordinate as an absolute value.

Input: –999999999...+999999999

POS1: Y coord. of machining position

Enter the Y coordinate as an absolute value.

Input: –999999999...+999999999

POS1: Coordinate of workpiece surface

Enter the Z coordinate as an absolute value at which machining starts.

Input: –999999999...+999999999

POS2: X coord. of machining position

Enter the X coordinate as an incremental or absolute value.

Input: –999999999...+999999999

POS2: Y coord. of machining position

Enter the Y coordinate as an incremental or absolute value.

Input: –999999999...+999999999

POS2: Coordinate of workpiece surface

Enter the Z coordinate as an incremental or absolute value.

Input: –999999999...+999999999

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 PATTERN DEF ~

POS1( X+25 Y+33.5 Z+0 ) ~

POS2( X+15 IY+6.5 Z+0 )

Defining a single row

 
Tip

Programming and operating note:

  • If you have defined a Workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

Help graphic

Parameter

Starting point in X

Coordinate of the starting point of the row in the X axis. This value has an absolute effect.

Input: –99999.9999999...+99999.9999999

Starting point in Y

Coordinate of the starting point of the row in the Y axis. This value has an absolute effect.

Input: –99999.9999999...+99999.9999999

Spacing of machining positions

Distance (incremental) between the machining positions. Enter a positive or negative value

Input: –999999999...+999999999

Number of operations

Total number of machining operations

Input: 0...999

Rot. position of entire pattern

Angle of rotation around the entered starting point. Reference axis: Main axis of the active working plane (e.g., X for tool axis Z). Enter a positive or negative absolute value

Input: –360.000...+360.000

Coordinate of workpiece surface

Enter the Z coordinate as an absolute value at which machining starts

Input: –999999999...+999999999

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 PATTERN DEF ~

ROW1( X+25 Y+33.5 D+8 NUM5 ROT+0 Z+0 )

Defining an individual pattern

 
Tip

Programming and operating notes:

  • The Rotary pos. ref. ax. and Rotary pos. minor ax. parameters are added to a previously performed Rot. position of entire pattern.
  • If you have defined a Workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

Help graphic

Parameter

Starting point in X

Absolute coordinate of the pattern starting point in the X axis

Input: –999999999...+999999999

Starting point in Y

Absolute coordinate of the pattern starting point in the Y axis

Input: –999999999...+999999999

Spacing of machining positions X

Distance in X direction (incremental) between the machining positions. You can enter a positive or negative value

Input: –999999999...+999999999

Spacing of machining positions Y

Distance in Y direction (incremental) between the machining positions. You can enter a positive or negative value

Input: –999999999...+999999999

Number of columns

Total number of columns in the pattern

Input: 0...999

Number of rows

Total number of rows in the pattern

Input: 0...999

Rot. position of entire pattern

Angle of rotation by which the entire pattern is rotated around the entered starting point. Reference axis: Main axis of the active working plane (e.g., X for tool axis Z). Enter a positive or negative absolute value

Input: –360.000...+360.000

Rotary pos. ref. ax.

Angle of rotation around which only the main axis of the working plane is distorted with respect to the entered starting point. You can enter a positive or negative value

Input: –360.000...+360.000

Rotary pos. minor ax.

Angle of rotation around which only the secondary axis of the working plane is distorted with respect to the entered starting point. You can enter a positive or negative value

Input: –360.000...+360.000

Coordinate of workpiece surface

Enter the Z coordinate as an absolute value at which machining starts.

Input: –999999999...+999999999

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 PATTERN DEF ~

PAT1( X+25 Y+33.5 DX+8 DY+10 NUMX5 NUMY4 ROT+0 ROTX+0 ROTY+0 Z+0 )

Defining an individual frame

 
Tip

Programming and operating notes:

  • The Rotary pos. ref. ax. and Rotary pos. minor ax. parameters are added to a previously performed Rot. position of entire pattern.
  • If you have defined a Workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

Help graphic

Parameter

Starting point in X

Absolute coordinate of the frame starting point in the X axis

Input: –999999999...+999999999

Starting point in Y

Absolute coordinate of the frame starting point in the Y axis

Input: –999999999...+999999999

Spacing of machining positions X

Distance in X direction (incremental) between the machining positions. You can enter a positive or negative value

Input: –999999999...+999999999

Spacing of machining positions Y

Distance in Y direction (incremental) between the machining positions. You can enter a positive or negative value

Input: –999999999...+999999999

Number of columns

Total number of columns in the pattern

Input: 0...999

Number of rows

Total number of rows in the pattern

Input: 0...999

Rot. position of entire pattern

Angle of rotation by which the entire pattern is rotated around the entered starting point. Reference axis: Main axis of the active working plane (e.g., X for tool axis Z). Enter a positive or negative absolute value

Input: –360.000...+360.000

Rotary pos. ref. ax.

Angle of rotation around which only the main axis of the working plane is distorted with respect to the entered starting point. You can enter a positive or negative value.

Input: –360.000...+360.000

Rotary pos. minor ax.

Angle of rotation around which only the secondary axis of the working plane is distorted with respect to the entered starting point. You can enter a positive or negative value.

Input: –360.000...+360.000

Coordinate of workpiece surface

Enter the Z coordinate as an absolute value at which machining starts

Input: –999999999...+999999999

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 PATTERN DEF ~

FRAME1( X+25 Y+33.5 DX+8 DY+10 NUMX5 NUMY4 ROT+0 ROTX+0 ROTY+0 Z+0 )

Defining a full circle

 
Tip

Programming and operating notes:

  • If you have defined a Workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

Help graphic

Parameter

Bolt-hole circle center X

Absolute coordinate of the circle center point in the X axis

Input: –999999999...+999999999

Bolt-hole circle center Y

Absolute coordinate of the circle center point in the Y axis

Input: –999999999...+999999999

Bolt-hole circle diameter

Diameter of the bolt hole circle

Input: 0...999999999

Starting angle

Polar angle of the first machining position. Reference axis: Main axis of the active working plane (e.g., X for tool axis Z). You can enter a positive or negative value

Input: –360.000...+360.000

Number of operations

Total number of machining positions on the circle

Input: 0...999

Coordinate of workpiece surface

Enter the Z coordinate as an absolute value at which machining starts.

Input: –999999999...+999999999

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 PATTERN DEF ~

CIRC1( X+25 Y+33 D80 START+45 NUM8 Z+0 )

Defining a pitch circle

 
Tip

Programming and operating notes:

  • If you have defined a Workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

Help graphic

Parameter

Bolt-hole circle center X

Absolute coordinate of the circle center point in the X axis

Input: –999999999...+999999999

Bolt-hole circle center Y

Absolute coordinate of the circle center point in the Y axis

Input: –999999999...+999999999

Bolt-hole circle diameter

Diameter of the bolt hole circle

Input: 0...999999999

Starting angle

Polar angle of the first machining position. Reference axis: Main axis of the active working plane (e.g., X for tool axis Z). You can enter a positive or negative value

Input: –360.000...+360.000

Stepping angle/Stopping angle

Incremental polar angle between two machining positions. You can enter a positive or negative value. As an alternative you can enter the Stopping angle (switch via the selection possibility on the action bar or in the form)

Input: –360.000...+360.000

Number of operations

Total number of machining positions on the circle

Input: 0...999

Coordinate of workpiece surface

Enter the Z coordinate at which machining starts.

Input: –999999999...+999999999

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 PATTERN DEF ~

PITCHCIRC1( X+25 Y+33 D80 START+45 STEP+30 NUM8 Z+0 )

Example: Using cycles in conjunction with PATTERN DEF

The drill hole coordinates are stored in the PATTERN DEF POS pattern definition. The control calls the drill hole coordinates with CYCL CALL PAT.

The tool radii have been selected in such a way that all work steps can be seen in the test graphics.

Program sequence

  • Centering (tool radius 4)
  • GLOBAL DEF 125 POSITIONING: This function is used for CYCL CALL PAT and positions the tool at the 2nd set-up clearance between the points. This function remains active until M30 is executed.
  • Drilling (tool radius 2.4)
  • Tapping (tool radius 3)

Cycles for Drilling, Centering and Thread Machining and Milling cycles

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

0 BEGIN PGM 1 MM

1 BLK FORM 0.1 Z X+0 Y+0 Z-20

2 BLK FORM 0.2 X+100 Y+100 Z+0

3 TOOL CALL 1 Z S5000

; Tool call: centering tool (tool radius 4)

4 L Z+50 R0 FMAX

; Move tool to clearance height

5 PATTERN DEF ~

POS1( X+10 Y+10 Z+0 ) ~

;

POS2( X+40 Y+30 Z+0 ) ~

;

POS3( X+20 Y+55 Z+0 ) ~

;

POS4( X+10 Y+90 Z+0 ) ~

;

POS5( X+90 Y+90 Z+0 ) ~

;

POS6( X+80 Y+65 Z+0 ) ~

;

POS7( X+80 Y+30 Z+0 ) ~

;

POS8( X+90 Y+10 Z+0 )

;

6 CYCL DEF 240 CENTERING ~

Q200=+2

;SET-UP CLEARANCE ~

Q343=+1

;SELECT DIA./DEPTH ~

Q201=-2

;DEPTH ~

Q344=-10

;DIAMETER ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q211=+0

;DWELL TIME AT DEPTH ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+10

;2ND SET-UP CLEARANCE ~

Q342=+0

;ROUGHING DIAMETER ~

Q253=+750

;F PRE-POSITIONING

7 GLOBAL DEF 125 POSITIONING ~

Q345=+1

;SELECT POS. HEIGHT

8 CYCL CALL PAT F5000 M3

; Cycle call in connection with the point pattern

9 L Z+100 R0 FMAX

; Retract the tool

10 TOOL CALL 227 Z S5000

; Tool call: drill (radius 2.4)

11 L X+50 R0 F5000

; Move tool to clearance height

12 CYCL DEF 200 DRILLING ~

Q200=+2

;SET-UP CLEARANCE ~

Q201=-25

;DEPTH ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q202=+5

;PLUNGING DEPTH ~

Q210=+0

;DWELL TIME AT TOP ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+10

;2ND SET-UP CLEARANCE ~

Q211=+0.2

;DWELL TIME AT DEPTH ~

Q395=+0

;DEPTH REFERENCE

13 CYCL CALL PAT F500 M3

; Cycle call in connection with the point pattern

14 L Z+100 R0 FMAX

; Retract the tool

15 TOOL CALL 263 Z S200

; Tool call: tap (radius 3)

16 L Z+100 R0 FMAX

; Move tool to clearance height

17 CYCL DEF 206 TAPPING ~

Q200=+2

;SET-UP CLEARANCE ~

Q201=-25

;DEPTH OF THREAD ~

Q206=+150

;FEED RATE FOR PLNGNG ~

Q211=+0

;DWELL TIME AT DEPTH ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+10

;2ND SET-UP CLEARANCE

18 CYCL CALL PAT F5000 M3

; Cycle call in connection with the point pattern

19 L Z+100 R0 FMAX

; Retract the tool

20 M30

; End of program

21 END PGM 1 MM