3D tool compensation during peripheral milling (#9 / #4-01-1)

Application

Peripheral milling is a machining operation carried out with the lateral surface of the tool.

The control offsets the tool perpendicular to the direction of movement and perpendicular to the tool direction by the total of the delta values from the tool management, the tool call and the compensation tables.

Requirements

Description of function

The variants below are possible with peripheral milling:

  • L block with or without programmed rotary axes, M128 or FUNCTION TCPM is active, define compensation direction with radius compensation RL or RR
  • LN block with tool orientation T without N vector, M128, or FUNCTION TCPM is active

The TNC7 basic can move up to four axes simultaneously. If an NC block commands movement of more than four axes, the control displays an error message.If the axis position does not change, you can nevertheless program more than four axes.

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 M128

* - ...

21 L X+48.4074 Y+102.4717 Z-7.1088 C+0 B-20.0115 RL

; Compensation is possible, compensation direction RL

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.

11 LN X+60.6593 Y+102.4690 Z-7.1012 TX-0.0807 TY0 TZ0.9366 RR M128

; Compensation is possible, compensation direction RR

Notes

 
Notice
Danger of collision!
The rotary axes of a machine may have limited ranges of traverse (e.g., between –90° and +10° for the B head axis). Changing the tilt angle to a value of more than +10° may result in a 180° rotation of the table axis. There is a danger of collision during the tilting movement!
  1. Program a safe tool position before the tilting movement, if necessary.
  2. Carefully test the NC program or program section in the Single Block mode
  • 3D tool compensation can be used in NC programs for peripheral milling with spatial or axis angles. It is also possible to use vector programs with tool vectors or NC programs without tool inclination.
  • If you combine vector programs with surface-normal vectors and tool vectors with RL or RR, the control will ignore the surface-normal vectors.
  • The control is not able to automatically position the rotary axes on all machines.
  • The control generally uses the defined delta values for 3D tool compensation. The entire tool radius (R + DR) is only taken into account if you have activated the FUNCTION PROG PATH IS CONTOUR function.
  • 3D tool compensation with the entire tool radius with FUNCTION PROG PATH (#9 / #4-01-1)

Example

Compensate re-worked end mill
CAM output at tool center

You use a re-worked Ø 11.8 mm end mill instead of Ø 12 mm.

The NC program has the following structure:

  • CAM output for Ø 12 mm end mill
  • NC points output on the tool center
  • Vector program with tool vectors
  • Alternative:

  • Klartext program with active tool radius compensation RL/RR

Proposed solution:

  • Tool measurement on tool tip
  • Suppress the error message with M107
  • Enter the tool compensation into the tool table:
    • R and R2 the theoretical tool data as from the CAM system
    • DR and DL the difference between the nominal value and the actual value

R

R2

DL

DR

DR2

CAM

+6

+0

Tool table

+6

+0

+0

-0.1

+0