Cycle 28 CYLINDRICAL SURFACE SLOT (#8 / #1-01-1)

ISO programming

G128

Application

 
Machine

Refer to your machine manual.

This function must be enabled and adapted by the machine manufacturer.

With this cycle you can program a guide slot in two dimensions and then transfer it onto a cylindrical surface. Unlike Cycle 27, with this cycle, the control adjusts the tool in such a way that, with radius compensation active, the walls of the slot are nearly parallel. You can machine exactly parallel walls by using a tool that is exactly as wide as the slot.

The smaller the tool is with respect to the slot width, the larger the distortion in circular arcs and oblique line segments. To minimize this process-related distortion, you can define the parameter Q21. This parameter specifies the tolerance with which the control machines a slot as similar as possible to a slot machined with a tool of the same width as the slot.

Program the center path of the contour together with the tool radius compensation. With the radius compensation you specify whether the control cuts the slot with climb milling or up-cut milling.

Cycle run

  1. The control positions the tool above the infeed point.
  2. The control moves the tool vertically to the first plunging depth. The tool approaches the workpiece on a tangential path or on a straight line at the milling feed rate Q12. The approaching behavior depends on the ConfigDatum CfgGeoCycle (no. 201000), apprDepCylWall (no. 201004) parameter
  3. At the first plunging depth, the tool mills along the programmed slot wall at the milling feed rate Q12 while respecting the finishing allowance for the side
  4. At the end of the contour, the control moves the tool to the opposite slot wall and returns to the infeed point.
  5. Steps 2 to 3 are repeated until the programmed milling depth Q1 is reached.
  6. If you defined the tolerance in Q21, the control then re-machines the slot walls to be as parallel as possible
  7. Finally, the tool retracts in the tool axis to the clearance height.
 
Tip

The cylinder must be set up centered on the rotary table. Set the preset to the center of the rotary table.

Notes

 
Machine

This cycle performs an inclined machining operation. To run this cycle, the first machine axis below the machine table must be a rotary axis. In addition, it must be possible to position the tool perpendicular to the cylinder surface.

 
Notice
Danger of collision!
If the spindle is not switched on when the cycle is called a collision may occur.
  1. By setting the displaySpindleErr machine parameter (no. 201002) to on/off, you can define whether the control displays an error message or not in case the spindle is not switched on.
 
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.
  • This cycle requires a center-cut end mill (ISO 1641).
  • The spindle axis must be perpendicular to the rotary table axis when the cycle is called.
  • This cycle can also be used in a tilted working plane.
 
Tip

The machining time can increase if the contour consists of many non-tangential contour elements.

Notes on programming

  • In the first NC block of the contour program, always program both cylinder surface coordinates.
  • The algebraic sign for the DEPTH cycle parameter determines the working direction. If you program DEPTH=0, the cycle will not be executed.
  • The set-up clearance must be greater than the tool radius.
  • If you use local QL Q parameters in a contour subprogram, you must also assign or calculate these in the contour subprogram.

Note regarding machine parameters

  • Use machine parameter apprDepCylWall (no. 201004) to define the approach behavior:
    • CircleTangential: Tangential approach and departure
    • LineNormal: The tool approaches the contour starting point on a straight line

Cycle parameters

Help graphic

Parameter

Q1 Milling depth?

Distance between cylindrical surface and contour floor. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q3 Finishing allowance for side?

Finishing allowance on the slot wall. The finishing allowance reduces the slot width by twice the entered value. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q6 Set-up clearance?

Distance between the tool face and the cylindrical surface. This value has an incremental effect.

Input: –99999.9999...+99999.9999 or PREDEF

Q10 Plunging depth?

Tool infeed per cut. This value has an incremental effect.

Input: –99999.9999...+99999.9999

Q11 Feed rate for plunging?

Traversing feed rate in the spindle axis

Input: 0...99999.9999 or FAUTO, FU, FZ

Q12 Feed rate for roughing?

Traversing feed rate in the working plane

Input: 0...99999.9999 or FAUTO, FU, FZ

Q16 Cylinder radius?

Radius of the cylinder on which the contour will be machined.

Input: 0...99999.9999

Q17 Dimension type? deg=0 MM/INCH=1

Program the rotary axis coordinates in degrees or mm (inches) in the subprogram.

Input: 0, 1

Q20 Slot width?

Width of the slot to be machined

Input: –99999.9999...+99999.9999

Q21 Tolerance? (optional)

If you use a tool smaller than the programmed slot width Q20, process-related distortion occurs on the slot wall wherever the slot follows the path of an arc or oblique line. If you define the tolerance Q21, the control adds a subsequent milling operation to ensure that the slot dimensions are as close as possible to those of a slot that has been milled with a tool exactly as wide as the slot. With Q21, you define the permitted deviation from this ideal slot. The number of subsequent milling operations depends on the cylinder radius, the tool used, and the slot depth. The smaller the tolerance is defined, the more exact the slot is and the longer the re-machining takes.

Recommendation: Use a tolerance of 0.02 mm.

Function inactive: Enter 0 (default setting).

Input: 0...9.9999

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 28 CYLINDRICAL SURFACE SLOT ~

Q1=-20

;MILLING DEPTH ~

Q3=+0

;ALLOWANCE FOR SIDE ~

Q6=+2

;SET-UP CLEARANCE ~

Q10=-5

;PLUNGING DEPTH ~

Q11=+150

;FEED RATE FOR PLNGNG ~

Q12=+500

;FEED RATE F. ROUGHNG ~

Q16=+0

;RADIUS ~

Q17=+0

;TYPE OF DIMENSION ~

Q20=+0

;SLOT WIDTH ~

Q21=+0

;TOLERANCE