Cycle 258 POLYGON STUD

ISO programming

G258

Application

Use Cycle 258 to machine a regular polygon by machining the contour outside. The milling operation is carried out on a spiral path based on the diameter of the workpiece blank.

Cycle sequence

  1. If, at the beginning of machining, the work piece is positioned below the 2nd set-up clearance, the control will retract the tool back to 2nd set-up clearance  
  2. Starting from the center of the stud the control moves the tool to the starting point of stud machining. The starting point depends, among other things, on the diameter of the workpiece blank and the angle of rotation of the stud. The angle of rotation is determined with parameter Q224
  3. The tool moves at rapid traverse FMAX to the setup clearance Q200 and from there with the feed rate for plunging to the first plunging depth
  4. The control then machines the circular stud with a helical infeed motion, taking the path overlap into account
  5. The control moves the tool on a tangential path from the outside to the inside
  6. The tool will be lifted in the direction of the spindle axis to 2nd set-up clearance in one rapid movement
  7. If several plunging depths are required, the control returns the tool to the starting point of the stud milling process and then plunges the tool to the programmed depth
  8. This process is repeated until the programmed stud depth is reached
  9. At the end of the cycle, first a departing motion is performed. Then the control will move the tool on the tool axis to 2nd set-up clearance

Notes

 
Notice
Danger of collision!
If you enter the depth in a cycle as a positive value, the control reverses the calculation of the pre-positioning. The tool moves at rapid traverse in the tool axis to set-up the clearance below the workpiece surface! There is a danger of collision!
  1. Enter depth as negative
  2. Use the machine parameter displayDepthErr (no. 201003) to specify whether the control should display an error message (on) or not (off) if a positive depth is entered
 
Notice
Danger of collision!
In this cycle, the control performs an automatic approach movement. If there is not enough space, a collision might occur.
  1. Use Q224 to specify which angle is used to machine the first corner of the polygon stud. Input range: –360° to +360°
  2. Depending on the angle of rotation Q224, the following amount of space must be left next to the stud: At least tool diameter +2 mm
 
Notice
Danger of collision!
At the end, the control returns the tool to the set-up clearance, or to 2nd set-up clearance if one was programmed. The end position of the tool after the cycle need not be the same as the starting position. There is a danger of collision!
  1. Control the traversing movements of the machine
  2. In the Simulation workspace of the Editor operating mode, check the end position of the tool after the cycle
  3. After the cycle, program absolute coordinates (no incremental coordinates)
  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • The control automatically pre-positions the tool in the tool axis. Make sure to program Q204 2ND SET-UP CLEARANCE correctly.
  • This cycle finishes Q369 ALLOWANCE FOR FLOOR with only one infeed. Parameter Q338 INFEED FOR FINISHING has no effect on Q369. Q338 is effective in finishing of Q368 ALLOWANCE FOR SIDE.
  • The control reduces the plunging depth to the LCUTS cutting edge length defined in the tool table if the cutting edge length is shorter than the Q202 plunging depth programmed in the cycle.
  • This cycle monitors the defined usable length LU of the tool. If the LU value is less than the DEPTH Q201, the control will display an error message.

Notes on programming

  • Before the start of the cycle you will have to pre-position the tool in the working plane. In order to do so, move the tool with radius compensation R0 to the center of the stud.
  • The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.

Cycle parameters

Help graphic

Parameter

Q573 Inscr.circle/circumcircle (0/1)?

Define whether the dimension Q571 is referenced to the inscribed circle or the circumcircle:

0: Dimension is referenced to the inscribed circle

1: Dimension is referenced to the circumcircle

Input: 0, 1

Q571 Reference circle diameter?

Enter the diameter of the reference circle. Specify in parameter Q573 whether the diameter entered here is referenced to the inscribed circle or the circumcircle. You can program a tolerance if needed.

Input: 0...99999.9999

Q222 Workpiece blank diameter?

Enter the diameter of the blank. The workpiece blank diameter must be greater than the reference circle diameter. The control performs multiple stepovers if the difference between the workpiece blank diameter and reference circle diameter is greater than the permitted stepover (tool radius multiplied by path overlap Q370). The control always calculates a constant stepover.

Input: 0...99999.9999

Q572 Number of corners?

Enter the number of corners of the polygon stud. The control distributes the corners evenly on the stud.

Input: 3...30

Q224 Angle of rotation?

Specify which angle is used to machine the first corner of the polygon stud.

Input: –360.000...+360.000

Q220 Radius / Chamfer (+/-)?

Enter the value for the radius or chamfer form element. If you enter a positive value, the control will round every corner. The value you enter here refers to the radius. If you enter a negative value, all corners of the contour will be chamfered with the value entered as the length of the chamfer.

Input: –99999.9999...+99999.9999

Q368 Finishing allowance for side?

Finishing allowance in the working plane. If you enter a negative value here, the control will return the tool to a diameter outside of the workpiece blank diameter after roughing. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q207 Feed rate for milling?

Traversing speed of the tool in mm/min for milling

Input: 0...99999.999 or FAUTO, FU, FZ

Q351 Direction? Climb=+1, Up-cut=-1

Type of milling operation. The direction of spindle rotation is taken into account.

+1 = climb milling

–1 = up-cut milling

PREDEF: The control uses the value of a GLOBAL DEF block

(If you enter 0, climb milling is performed)

Input: -1, 0, +1 or PREDEF

Q201 Depth?

Distance between workpiece surface and bottom of stud. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q202 Plunging depth?

Tool infeed per cut. Enter a value greater than 0. This value has an incremental effect.

Input: 0...99999.9999

Q206 Feed rate for plunging?

Traversing speed of the tool in mm/min while moving to depth

Input: 0...99999.999 or FAUTO, FMAX, FU, FZ

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?

Coordinate in the spindle axis at which a collision between tool and workpiece (fixtures) is impossible. This value has an incremental effect.

Input: 0...99999.9999 or PREDEF

Q370 Path overlap factor?

Q370 x tool radius = stepover factor k.

Input: 0.0001...1.9999 or PREDEF

Q215 Machining operation (0/1/2)?

Define the machining operation:

0: Roughing and finishing

1: Only roughing

2: Only finishing
Side finishing and floor finishing are executed only if the respective finishing allowance (Q368, Q369) has been defined

Input: 0, 1, 2

Q369 Finishing allowance for floor?

Finishing allowance in depth which remains after roughing. This value has an incremental effect.

Input: 0...99999.9999

Q338 Infeed for finishing?

Infeed in the tool axis when finishing the lateral finishing allowance Q368. This value has an incremental effect.

0: Finishing in one infeed

Input: 0...99999.9999

Q385 Finishing feed rate?

Traversing speed of the tool in mm/min for side and floor finishing

Input: 0...99999.999 or FAUTO, FU, FZ

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 258 POLYGON STUD ~

Q573=+0

;REFERENCE CIRCLE ~

Q571=+50

;REF-CIRCLE DIAMETER ~

Q222=+52

;WORKPIECE BLANK DIA. ~

Q572=+6

;NUMBER OF CORNERS ~

Q224=+0

;ANGLE OF ROTATION ~

Q220=+0

;RADIUS / CHAMFER ~

Q368=+0

;ALLOWANCE FOR SIDE ~

Q207=+500

;FEED RATE MILLING ~

Q351=+1

;CLIMB OR UP-CUT ~

Q201=-20

;DEPTH ~

Q202=+5

;PLUNGING DEPTH ~

Q206=+3000

;FEED RATE FOR PLNGNG ~

Q200=+2

;SET-UP CLEARANCE ~

Q203=+0

;SURFACE COORDINATE ~

Q204=+50

;2ND SET-UP CLEARANCE ~

Q370=+1

;TOOL PATH OVERLAP ~

Q215=+0

;MACHINING OPERATION ~

Q369=+0

;ALLOWANCE FOR FLOOR ~

Q338=+0

;INFEED FOR FINISHING ~

Q385=+500

;FINISHING FEED RATE

12 L X+50 Y+50 R0 FMAX M99