Hello,
I am new to CNCs, so this might be a simple error. I am using a Mac book pro running High Sierra, fusion 360, with firecontrol. I am getting sn error of " The following error happened at line 30168: Two G-Code commands that both require the use of the XYZ axis words were detected in the block." What is causing this? Also when I click “run from here” I get the error, no speed detected, and I have to end the program. This seems to be a bigger issue since this always happens when I click the run from here option, as I a not sure why it will not detect its speed. Any help or recommendations would be helpful thanks.
Are you using the fusion 360 post processor for the crossfire pro?
Hello, if that means exporting it into a gcode in fusion 360 to upload into crossfire then yes.
Not exactly. Fusion allows you to use different files (“post processors”) to control the generation of the GCode to match the specific requirements of the machine you’re going to use to cut.
There is a special post-processor file you need to install and setup in order to get GCode that is compatible with the Crossfire. The file & setup instructions are on the Langmuir download site.
1 Like
Ok, should have said the full version. I then upload it into FireControl to do the actual cut. It stops randomly, so I am unsure why. I have gotten this error a few times when cutting the outline of the pig. Here is s copy of the file, and G-code. I read that it might be the [LS-THC Firmware Update for Bug Fixes (Current Version is V1.08 on 4/9/20), but this only shows windows, and I am not sure how to check it on my Mac. I download the latest versions of software from your downloads site last week, but cannot find a Mac version of the LS-THC Firmware, or is included in one of the downloads already? Also when running FireControl if a cut stops I click on run from here, but this is where I get the error no speed detected, so it cancels the cut, which I think might be a different error since it happens if I loose arc voltage as well. I know my USB ports/drives are correct and working, since I checked them with your guide info if this helps.
Pig-GiGi-75IPM.nc (586.7 KB) Pig - Gigi.zip (1.5 MB)
I’m not 100% sure, but I believe you are using an old Fusion 360 post processor for Firecontrol. Your .nc file has no version information in it. I believe the Fusion one should be writing out a line that looks like:
( description: FireControl Plasma v1.5)
but yours has:
( description: Generic Cutting Machine)
But I haven’t tried a post from Fusion yet to be sure. I know Sheetcam definitely has a similar line in it. To verify see step A5 onward from:
https://www.langmuirsystems.com/software/fusion#post-firecontrol
And make sure you are using the lastest post, which is version 1.5. If you are not using 1.5, install it and then generate your .nc file again.
I believe that is a known bug.
1 Like
Hello, Thanks for the feed back. I checked the post process control and I have uploaded the screen shot. I believe it is correct, and the values are the same as the ones shown in their set up. This maybe dumb, when exporting the g-code does it matter if I do it in the “Additive” tab or “Fabrication” tab. I am re-uploading the file with it being exported in Fab tab instead of the Add tab. How do you see the file version description? If I didn’t have one in the set up section of post-process would it affect it? Thanks for the info on the bug I hope they fix it soon. Also I just updated Fusion 360, since there was an update for it. I will try to cut tomorrow to see how it goes.
/Pig - Gigi.zip (1.8 MB)
From your screen shot it looks like you are using the correct post v 1.5.
I’m not using Fusion (yet) so hopefully someone else can fill you in on that.
Are you able to ‘dry’ run without errors? To do that: turn off your plasma and disable THC in Firecontrol. Make sure to have a sheet on the table. Then run it. If you are able to consistently make it through without errors this may point to an interference problem. If you run into the problem in the dry run then this could be: problem in original image, problem in the generated gcode, or problem with Firecontrol.
1 Like
Ok, thanks for the dry run tip, I didn’t know how to do that. So I did a few dry runs and still get the error. I have zipped screenshots of the error code, line it says there is an issue on, and some I took of the top and bottom line of code, in the attached file. I check the LS-THC and I am running the most current version V1.09. The program always gets through the lettering, it just gets stuck on the pig some places more than others for some reason. Do you know of a good site that has files I could import and try besides this one?
Screenshots.zip (3.6 MB)
@Greg9504, This may be totally off base but… I don’t have FireControl so I’m not familiar with it, but, from the screenshots it seems that all the moves are microscopic (<=0.001 in one or more axis). Is there some kind of limit in FireControl to flag these moves as errors?
2 Likes
@TomWS, that is probably it. I loaded the file into a gcode viewer and it seemed to kill it too.
There’s no user setting for any limits like that, there may be some internally.
@JJacobson I haven’t looked at the drawing closely enough to know the problem, but as Tom suggests it seems the generated gcode isn’t optimized well. This could a problem with the drawing or some setting with Fusion. Unfortunately I’m not familiar with the gcode generation settings in Fusion, so I can’t offer you any suggestions. Hopefully some of the Fusion experts will take a look. The good news is it is not interference which can be hard to track down.
I’ve attached two dxf files that you should be able to import into Fusion. One is some circles and the other has come circles and squares and some lettering. If you are just looking for something to test try one of those.
testshapes.zip (3.3 KB)
@TomWS @Greg9504 Funny you mention that. Fusion has a setting call tolerance and smoothing, it was in one of Langmire tutorials LOL, I will revise the tolerance to be bigger, they suggested .0004, I guess that was very straight cuts, and I might add in smoothing to see if it works. I will also try with your files to see what changes happen thanks. Where can I get a gcode view, or is it in a seperate application?
Did you generate with the smoothing option? Might want to try that too. on edit, nevermind I see you said you are going to try that.
See this post for a gcode viewer:
you can also try this online one https://ncviewer.com/ which seemed to handle your pig fine. Although it does simulate very slow.
Quick look at the gcode - yeah - I’d definitely play with the smoothing setting. You could probably reduce that g-code file to 1/50th of it’s size and make it much easier to cut. When you’re getting to line 30,168, something’s not right unless your cutting parts for the space x rocket. Pretty sure pigs don’t fly 
2 Likes
I did a quick load in F360 to take a closer look, and turned smoothing on.
Pig-GiGi.nc (21.6 KB)
This file is 878 lines. The original was 32,362. Something going on with the imported outline of the pig.
2 Likes
Hello,
Well that was the issue. I did a few test cuts and this is what I found,
.04 w/ smoothing - 1216 lines of code = completed
.04 w/ out - 28930 lines of code = completed
.004 w/ smoothing - 474 lines of code = completed
.004 w/ out - 28930 lines of code = completed
.0004 w/ smoothing - 478 lines of code = Completed
.0004 w/ out - 28930 lines of code = did not complete
I guess if you have any curving you are going to want to keep this on.
Thanks for all the replies and help.
3 Likes
Normally your path won’t be broken up into that many small segments. For some reason that outline was broken into thousands of tiny line segments - not sure where it came from, but that’s not typical for a vector file. Smoothing takes all those tiny line segments and combines them into a longer, “smoother” path that doesn’t require all the g-code commands and really simplifies the cut. It’s usage really depends on what your source design consists of. It’s not needed most of the time.
I’m not sure without seeing it, but I’d guess the torch moves much slower when it’s processing the big files without smoothing - that can affect cut quality as well.
1 Like
I’ll bet it’s an artifact from file type conversions. DXF does that a lot. One of the reasons I try to get to SVG as soon as possible in the workflow 
2 Likes