- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Multiple Commands error running files on Stinger1 Camaster with FTC
Hello:
I am getting mixed results with using Fusion 360 and exporting a .tap file to go to Camaster Visualcnc / wincnc. Most of the posts work put then some do not work and I will get a Error- Multiple Commands. I understand the basics of G code but by no means a pro. Am I missing something. Why is it not all post failing instead of random ones. Also after I zero out a new tool does it always have to go back to measure the tool on the machines touch plate?
The post processor seems really buggy and any help on this would be greatly appreciated.
Many thanks
Erik
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Does it give you a line where there's a problem in the code.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
No it did not. Maybe I am not looking in the correct place but it just says "Error - Multiple Commands"
This is the beginning of the post that gives the error.
[1]
[T1 D=0.375 ball end mill]
G90
G20
[Parallel1]
M5
T1
G53 Z0.
S5000
M3
G54
G0 X6.0184 Y4.7316
Z2.4
Z-0.7792
This is the beginning post of a post that worked with no problem.
[1]
[T2 D=0.5 flat end mill]
G90
G20
[2D Contour13]
M5
T2
G53 Z0.
S1222
M3
G54
G0 X4.2625 Y0.2433
Z0.6
One out of many differences that I can see is the T value. I use a good amount of bits so I do not have my library setup with different numbers. All bits should be T1. But that said the post that works says T2. So I am very confused.
Is it the tool parameters that need to be changed? But I have had successful cuts with this tool.
Also every time I run a program even after I use the top plate on the material it still goes over to the machines touch plate and remeasures it. I would really like to disable the FTC. Would this help? When you are cutting many different parts with different setups FTC it seems not that helpful. But then again I might not be understanding something.
Thanks for you quick response. I have a job half way done and am now stuck because of this error.
Erik
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
To me the Multiple Commands error sounds like there are 2 M or G codes on one line that your control doesn't like, trying to find that if you don't get any feed back from the control is going to be quite hard.
The tool numbers are controlled in the library, you have a library in every document like this. Click the mange library icon then double click a tool to edit.
I don't know how the tool library on your control works or how the touch plate works with it so I can't help there.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Error, X5.9808 Z-0.8539 I-0.0265 K0.0266, Line 17
Sorry I found where the error is. I checked the post and it does not seem to have M or G codes on the same line that I see.
Any ideas what is giving the error.
Thanks
Erik
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
I seem to remember that WinCNC doesn't support arcs that are not on the XY plane, the line with the error the arc is on th XZ plane. Is the post you're using the one that comes with Fusion.
Mark
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
It's the Vertical lead-in radius that's causing the issue, I bet
Seth Madore
Owner, Liberty Machine, Inc.
Good. Fast. Cheap. Pick two.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Yes probably, I've allready modified a post for someone using that control.
A search for CAMaster_wincnc_m3xa.cps might find the thread.
Mark
Attached is the post I modifed for someone else, don't know if there are any other differences to the one you're using so be careful.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Hello:
This is the post processor that came from fusion 360 furum. Does Fusion 360 have a single tool postprocessor for Camaster? Does Fusion 360 make the postprocessors? I know that Camaster does not.
Many thanks
Erik
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
Attached it the post processor that I have.
The file that does not work is also attached, Inner_parallel002.tap
After talking to the company they noticed that the G3 and G2 codes are missing from the post. Wincnc does not know which direction to go ccw or cw. for example in line 17
X5.9808 Z-0.8539 I-0.0265 K0.0266
This seems to happen only when K value is involved.
It does not happen when it is the I J
Thanks
Erik
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report
I too have a Camaster stinger 1 with the Fast tool change ( FTC ) and I am looking for a working post processor.
@Madcow2 does the PP that was listed in the thread work?
I would like to use Fusion 360 on some projects that I am working on but I am not the person who is going to edit PP files.
Fusion