Post-processor choice 3d toolpaths from fusion360 on the Multicam

Hi all, I have a job using a 3d toolpath that I would like to use on the multicam. I have designed the part and the toolpaths in Fusion 360, and need to make sure the post processor is correct.

There is another thread about this but it didn’t seem resolved. Fusion has a postprocessor from multicam called “MultiCam ISO” as is described in the previous thread that could be similar.

In order to figure this out, I have designed two identical sample parts in Fusion 360 and vcarve and exported the gcode through both of their respective post-processors. I have attached:

*The Fusion 360 file with the model and CAM setting
*The Vcarve file with model and CAM settings
*Screenshots of the fusion model
*Both outputed Gcodes
*screenshots of the gcodes side by side (658.5 KB)

My questions:
Has anyone had sucess with using Fusion360 CAM on our machine?
@CalvinStence - did you end up figuring it out from the previous post?
Has anybody used a 3d toolpath on the Multicam, how did you do it?
What is the exact machine model and info in case I need to ask another forum or the manufacturer?

I hope this has enough information and feel free to reach me at 512-201-7446 directly if needed.


So Kee Fedak had great success with a fusion 360 post processor…I don’t know which one.

1 Like

In comparing the two g code files, I don’t see anything scary in the Fusion file. It does appear to have one issue in that line N30 is specifying tool 4 (N30 G0 T4) where the VCarve file is correctly specifying tool 1 in the 6th line (G00T1). Since DMS does not have an automatic toolchanger, Tool 1 is the only viable DMS option.

I’d probably fix the tool specification, then run the Fusion file in dry run mode and then set Z Surface and Z Max Depth artificially high and run an air cut. If those runs look OK, then proceed to cut normally.

Don’t use Multicams post processor from the fusion website, it has several problems some of which are subtle.

Here is the post processor I modified to work with our machine.


Chris, would you please run Adrian’s sample through your post processor and send me the gcode file?
Would like to see what differences occur. Thanks, Bert

1 Like

Thanks Chris, I will look through that post. I tried the fusion360 postprocessor yesterday and it worked fine on the small part as is, but then when I went to the main job is ended up doing some really bizarre stuff during the cut. Specifically, it would randomly lose position and shift the cuts like a half an inch every once in a while, (ruining the peice). It looked similar to a belt slip, but the multicam is obviously not belt driven so I am inclined to think its a gcode problem. I will try out the new post-processor and see what happens.


This is the same part using Chris processor: (2.9 KB)

The big difference I see in Chris’s processor is getting the speed right. I missed that the first time. I vaguely remember hearing someone say there was a unit of measure problem on the Fusion processor and that the number generated was beyond what the Multicam can handle … maybe that’s the reason for the skips? Example: Vcarve F0.7, Fusion F20

What I don’t understand is why Chris omitted the arc functions (J & I ) and went with point-to-point directions for the curves. @Chris_Wischkowsky, can you explain?


20 / 25.4 = 0.7874015748

Metric versus American difference / mistake?

Just for the record the post processor provided by @Chris_Wischkowsky worked like a charm. Thanks all for your help!
My job did not have any arcs btw, so if it was curvy the finish might have been less desirable.

edit. I reworded in response to @Brian. Thanks for that.

1 Like

Just so there is no confusion … Is that the post processor @Chris_Wischkowsky provided?

Uhh, I’d call the circles an arc function … you call them something else???

1 Like

My apologies, I only ran my bigger job on the machine, which is just regular polygons. I only uploaded the test design for reference. Sorry for the confusion.

Next time I’m on the machine I will run it and let y’all know how it goes.

So Chris’ processor is the one to go with?

@Chris_Wischkowsky and

Does one of you have a tool library or crib for Fusion 360?

Have either of you done more testing with the post processors? Any good results?

Thank you in advance.


I haven’t done anymore testing with Fusion yet.
The post processor posted by Chris works fine, so if you would want to use it, go for it.

The problem we were discussing is that Chris’s processor doesn’t utilize the Gcode commands to program smooth arcs. From my understanding Chris’s just interpolates on curves by moving linearly between many points, which depending on your piece might yield sub optimal results.

It is like the difference between the “multicam Gcode post-processor” and the “multicam Gcode post-processor (arc)” in vcarve.

To my knowledge there is no tool library for fusion, but in the meantime I just find the comparable tool in the FusionCam example library and copy in the feeds and speeds from our existing library, which worked well for me. If you are unsure I would post a screenshot here and someone more qualified than I could probably give you the go ahead.

I was able to talk to Chris yesterday and he explained that he took the arc functions (gcode i’s and j’s) out on purpose. Says they are not needed due to controllers now having point smoothing functionality built into the system itself. (That’s my layman’s explanation and hopefully accurate.)

2 Likes and @bertberaht Thank you guys! I appreciate it.
Thank you.