Post processor

nzlowie · Posted at 2018-7-12 19:54:16

Hi there, I've just powered up my new 2.1 controller and I can't find a post processor that works with it. I use Vcarve pro which has a lot of processors but I can't find one that works properly.

Any idea's please.

Many thanks Dave

Lukasz · Posted at 2018-7-14 23:20:05

Hello,
Here is a post processor for Vectric Aspire. Maybe it will be helpfull for somebody...

Lukasz

71taa · Posted at 2018-7-12 23:18:18

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.

maxx2000 · Posted at 2018-7-13 23:47:15

for Mach3 fully supported. edit according to your requirements

yehanv71 · Posted at 2018-7-14 17:23:57

Hello

DDCSV 2.1........ any assistance with post processor please, i have tried every one in the Fusion360 list and the controller doesnt run. I used the sample file i got with the controller and it works perfect. It was created on Camotics. Also the code looks very different from what i have compared in fusion posts.

Anyone can assist please, PLEASE????, Pretty please??

YCAM-META-DATA: Filename: /home/jcoffland/projects/camotics/svn/trunk/camotics/examples/cat/tiny_cat_outline.svg

YCAM-META-DATA: Timestamp: 2012-01-27 20:11:57.397792

YCAM-META-DATA: Version: 0.5.1

yehanv71 · Posted at 2018-7-14 17:30:20

71taa Posted at 2018-7-12 23:18
Using F360 with Fanuc postprocessor w/o subprograms, helical movements should be disabled (it's a ma ...

Hello 71ta

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

Please guide

Thanks

71taa · Posted at 2018-7-14 23:33:08

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.

creisey · Posted at 2020-2-11 18:57:42

is there a postprocessor for Fusion 360? or do you just use the Fanuc basic and then later delete some lines?

and is there a postprocessor for rhinocam?

for any straigt forward solution i would be more than thankfull

71taa · Posted at 2020-2-12 13:31:47

fanuc.cps.zip (16.68 KB, Down times: 2400)

creisey · Posted at 2020-2-12 18:55:05

another little question, i read in the advertisments of DDCSV3.1 that USB hotplug is not possible. is that also with the DDCSV2.1 the case. or is it anyway a problem?

Post processor

TEL

0755-87654321