Cycle 221 CARTESIAN PATTERN

ISO programming

G221

Application

This cycle enables you to define a point pattern as lines. It can be used for a previously defined machining cycle.

 
Tip

Instead of Cycle 221 CARTESIAN PATTERN, HEIDENHAIN recommends using the more powerful PATTERN DEF function.

Cycle run

  1. The control automatically moves the tool from its current position to the starting point for the first machining operation.
  2. Sequence:

    • Move to 2nd set-up clearance (spindle axis)
    • Approach the starting point in the working plane
    • Move to set-up clearance above the workpiece surface (spindle axis)
  3. From this position, the control executes the last defined fixed machining cycle.
  4. Then, the tool approaches the starting point for the next machining operation in the negative direction of the reference axis. The tool stops at the set-up clearance (or the 2nd set-up clearance).
  5. This procedure (steps 1 to 3) will be repeated until all machining operations from the first row have been completed. The tool is located above the last point of the first row.
  6. The tool subsequently moves to the last point on the second row where it carries out the machining operation.
  7. From this position, the tool approaches the starting point for the next machining operation in the negative direction of the reference axis.
  8. This procedure (step 6) will be repeated until all machining operations of the second row have been completed.
  9. The tool then moves to the starting point of the next row.
  10. All subsequent rows are machined in a reciprocating movement..
 
Tip

If you run this cycle in Program Run / Single Block mode, the control stops between the individual points of a point pattern.

Notes

 
Machine

Cycle 221 CARTESIAN PATTERN can be hidden with the optional machine parameter hidePattern (no. 128905).

  • Cycle 221 is DEF-active. In addition, Cycle 221 automatically calls the last defined machining cycle.

Notes on programming

  • If you combine Cycle 221 with one of the machining cycles 200 to 209 or 251 to 267, then the set-up clearance, the workpiece surface, the 2nd set-up clearance, and the rotary position that you defined in Cycle 221 will be effective for the selected machining cycle.
  • Slot position 0 is not allowed if you use Cycle 254 in combination with Cycle 221.

Cycle parameters

Help graphic

Parameter

Q225 Starting point in 1st axis?

Coordinate of starting point in the main axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q226 Starting point in 2nd axis?

Coordinate of starting point in the secondary axis of the working plane. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q237 Spacing in 1st axis?

Spacing between the individual points on a line. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q238 Spacing in 2nd axis?

Spacing between the individual lines. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q242 Number of columns?

Number of machining operations on a line

Input: 0...99999

Q243 Number of lines?

Number of lines

Input: 0...99999

Q224 Angle of rotation?

Angle by which the entire pattern is rotated. The center of rotation lies in the starting point. This value has an absolute effect.

Input: –360.000...+360.000

Q200 Set-up clearance?

Distance between tool tip and workpiece surface. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q203 Workpiece surface coordinate?

Coordinate on the workpiece surface referenced to the active datum. This value has an absolute effect.

Input: –99999.9999...+99999.9999

Q204 2nd set-up clearance?

Distance in the tool axis between tool and workpiece (fixtures) at which no collision can occur. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q301 Move to clearance height (0/1)? (optional)

Specify how the tool moves between machining processes:

0: Move to the set-up clearance between operations

1: Move to the 2nd set-up clearance between operations

Input: 0, 1

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 CYCL DEF 221 CARTESIAN PATTERN ~

Q225=+15

;STARTNG PNT 1ST AXIS ~

Q226=+15

;STARTNG PNT 2ND AXIS ~

Q237=+10

;SPACING IN 1ST AXIS ~

Q238=+8

;SPACING IN 2ND AXIS ~

Q242=+6

;NUMBER OF COLUMNS ~

Q243=+4

;NUMBER OF LINES ~

Q224=+15

;ANGLE OF ROTATION ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q301=+1

;MOVE TO CLEARANCE

12 CYCL CALL