Pattern definition with PATTERN DEF
Application
Related topics
- Cycles for pattern definition
- 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 |
---|---|---|
| Point Definition of up to any 9 machining positions | |
| Row Definition of a single row, straight or rotated | |
| Pattern Definition of a single pattern, straight, rotated or distorted | |
| Frame Definition of a single frame, straight, rotated or distorted | |
| Circle Definition of a full circle | |
| Pitch circle Definition of a pitch circle |
Programming PATTERN DEF
To program the PATTERN DEF functions:
| ||
|
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.
The control performs the most recently defined machining cycle on the machining pattern you defined.
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.
Defining individual machining positions
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.
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.
11 PATTERN DEF ~ |
POS1( X+25 Y+33.5 Z+0 ) ~ |
POS2( X+15 IY+6.5 Z+0 ) |
Defining a single row
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.
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.
11 PATTERN DEF ~ |
ROW1( X+25 Y+33.5 D+8 NUM5 ROT+0 Z+0 ) |
Defining an individual pattern
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.
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.
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
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.
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.
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
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.
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.
11 PATTERN DEF ~ |
CIRC1( X+25 Y+33 D80 START+45 NUM8 Z+0 ) |
Defining a pitch circle
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.
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.
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.
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 ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
6 CYCL DEF 240 CENTERING ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
7 GLOBAL DEF 125 POSITIONING ~ | |||
| |||
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 ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
| |||
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 ~ | |||
| |||
| |||
| |||
| |||
| |||
| |||
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 |