Post processor

71taa

Using F360 with Fanuc postprocessor w/o subprograms, helical movements should be disabled (it's a matter of gcode processing, the controller will use helical movements in the end).

Removing o1001 sub call in the result, and that's all.
https://madmodder.net/index.php/topic,11598.900.html - here is a long discussion, pp's are discussed there as well as controller limitations.

71taa

yehanv71 Posted at 2018-7-14 17:30
Hello 71ta

What is meaning of removing o1001, where is this in the result?

Typical workflow:
1. Choose the target setup in CAM module
2. Ensure that operation names doesn't contain symbols that aren't allowed in g-code comments (like parentheses and so on)
3. Select the 'Post Process'
4. Select "FANUC / fanuc" postprocessor
5. Set following properties:
5.1 Allow helical moves - No
5.2 G28 Safe retracts - No (it's a matter of taste)
All other options by default
6. Open the generated file. In the beginning you'll see the following (depends on your setup):
%
O1001
(T1 D=1. CR=0. - ZMIN=-2.5 - FLAT END MILL)
G90 G94 G17 G49 G40 G80
G21
G53 G00 Z0.
7. Remove the 'O1001' line
8. If you haven't setup home switches on your CNC and doesn't use homing sequence before the work - remove G53 lines - both in the beginning and in the end of file - otherwise you could hit limits easily.

That's all. Works for all trajectories I've tested. With custom T.nc (simple M5 M0) manual tool change with probe is working and so on.

And one more thing (see other discussions in this forum) - I'm not using the diameter correction in the controller, using F360 CAM for this.

71taa

fanuc.cps.zip (16.68 KB, Down times: 1425)

2020-2-12 13:30 Uplaod

Click on the file name to download attach

Slightly modified fanuc PP.
Helical moves are on (since the old post time I haven't found any problems with it)