Laser post-processor for Fusion 360?

I was given a diode laser for Christmas, and am slowly working on getting it up and running. I primarily use Fusion 360 for my CNC routing projects, but it looks like the Mach 4 post-processor doesn’t support laser. What are other Fusion 360 users doing? I’ll probably buy LightBurn too, but it would be nice to have the option of working in Fusion 360 for projects that combine routing and laser operations. Thanks for the advice!

Mach4 is Func compatible. Just download the Func post processors and port over what you need.

But my limited understanding is that is already there and you are needing to change profiles in Mach4 to output the control signals to the laser. So that would also be ESS configuration as well.

I can answer your post processor questions but how everyone has it set up in Mach4 and the ESS is something I haven’t found the desire to do yet.

Sorry, I’m a total noob with this kind of thing. What do you mean by “porting over what I need?” I tried googling “func post processor,” but it’s not really a SEO term; I didn’t find much.

I think I’m up and running on the ESS configuration. There’s pretty good documentation available there. I can successfully test fire the laser through Mach4.

Well, it would help if I spelled it correctly :rofl:

lol ok yes that makes way more sense!

Do you have any suggestions for resources discussing porting/customizing post-processors? I have zero experience with it, but it seems like it would be a very useful thing to know.

One thing with Lightburn is that it does not support the ESS control board, so you can’t do any of the direct control stuff (like turning on the laser for a test, running a square around the area to burn, jogging, etc.). However, you can use the design part of the software to create Gcode. If you are an F360 user, I suspect you can do just as well using that (I’m not sure of F360’s capabilities around creating vectors around bitmap images and such though) if you get the right post processor (there are people out there that have them). I use Vectric and it does everything around the creation part already, and then mach 4 with the ESS plugin does the realtime control stuff just fine.


So you are in luck, the post processors in Fusion 360 are in fact written in ECMA-262 Script or more commonly known as JavaScript. So its a very easy to learn scripting language. It is also very forgiving and generally there are a lot of resources on the internet for it since its very mature.

You will find that the structure of the post processors are generally well organized. The exposed objects from F360 are very natural language named. Unlike the stupid Lua stuff in Mach4 :rofl:

You WILL NOT be making major changes. The vast majority of the script will remain the same. You just need to identify (and somebody like @jjneeb can help you figure what you need) what is missing, if anything.

So lets agree on a simple 50mm circle for our first exercise. It will be centered X 60mm and Y 60mm into the work space. That way we can eliminate differences in CAM packages.

Now, using the laser tool operations, produce a g-code file and lets see what the differences between what @jjneeb has and what you have. Even better, before we get to that point, see if you can run Jim’s file!

So we have two issues, first being the machine setup. Second being the CAM output. Lets eliminate the machine setup first. Jim will get that part for you. He is better at that stuff than I am. I can figure out the post processor but I need examples of what is different.

1 Like

Hi Jim, big fan of your content!

Thanks for the heads up. I’ll download the 30-day trial and see if I like it enough.

F360 is good at a lot of things, but pretty clunky when it comes to more graphic-design-y things. I was just hoping to get some basic functionalities (cutting contours and maybe engraving simple text) up and running in Fusion, and then handle more elaborate images either with LightBurn or directly through the Mach4 raster process you’ve been discussing.

Vectric might be worth it in the long run (that video you did on getting laser engraving to follow the surface of spoons was very cool) I was just trying to dip my toe in with something cheaper.

Laser is very new to me and I’m still figuring out the workflow.

Not better, just been through it a lot on the laser already :slight_smile:

I’m gonna assume your machine has the regular AVID electronics kit with the ESS controller. I have a full set of instructions for setting up the laser in SW and signals there, as well as a combined laser/spindle screen and some Vectric post processors. This is at: Public CNC Docs - Google Drive

Also, you’ll want to visit Warp9’s website on laser setup. They go through the Mcodes and other setup info that will help you with your postprocessor journey: FAQ Mach4

Now post processors. Vectric post processors are very simple (and they have a great manual), but as such are a little more limited. I haven’t actually modified any F360 ones (because I suck at F360 so I don’t use it much), but I have looked at the post processors and they are very capable and probably won’t be too hard to get something working.

It looks like F360 has specific laser support, so you have two choices. You can make a “laser endmill” tooltype with a 0.005" (or whatever your laser is) diameter, and then set your rpm for the spindle speed to 0-100, which you will use as your power percentage in the post processor to pass to the laser command (M67). There are a few things to add to the header to enable the laser, and then you’ll basically add a laser command to your feedrate command (turns the laser on to a given power level), and one to turn it off for the rapid moves. You’ll also remove your M3/M5 commands to leave the spindle alone.
If you want to use a laser type tool, then it will probably have a power setting that you can pass to the M67 instead of spindle rpm, and it will likely also have the laser commands in the right place (feed and rapid moves), so you’ll probably just need to add the ESS specific commands in the right places.

If you send me an email at, I can share what the vectric post processors look like, and what the end Gcode should look like so you can figure out what you need to do to the F360 PP. If you really don’t want to edit anything, I know there are people out there (I just can’t think of one off the top of my head) that have PPs for F360, so if you ask over at the Opt lasers or AVID CNC user groups on FB you might find someone that will offer you theirs.

That’s very encouraging!

Great Idea for a study project. I’ll start poking around and see how it goes.

I’m still waiting on a few last fittings for the air assist plumbing on my machine, but hopefully by mid-week I can test meaningful g-code on it.

I like your idea of making a “laser endmill” tooltype. From what I can tell, the laser specific operations that Fusion offers are pretty bare bones, so using endmill operations could give a lot more control.

I took a look at the Vectric post processors on your Google Drive - wow that format is so much more legible than F360 post processors.

NYCCNC has a video on editing post processors for F360, which I found pretty helpful. I’ve just been peeking under the hood of different post processors, seeing how they’re structured etc.

I also found a post on the Autodesk post processor forum discussing a similar project, which had some useful advice.

Vectric is the same way. I like the rest of their software a lot, but they underachieved on the laser module. They charge $50 extra for it, and they don’t even let you set your Z height (it just defaults to whatever Z zero is). You get more capability just using the engraving and routing toolpaths. Its too bad since they could literally copy the capability from their other toolpaths.

@shopratsneedshopcats Welcome to the laser club!

I’ve been digging into this a lot… including starting (but not completing the process) of getting a post to work with Fusion with laser cutting.

The solutions suggested by folks above, like custom posts for Vectric, Fusion, or even hacking Lightburn to work all of their merits but it might be worth asking the question:

What do you want to do?

More specifically, do you see yourself doing mostly vector work? (logos, text, etc) or burning images into things?

If it’s the latter there are actually are some ways you can use Mach 4/ESS to do some pretty good image burning (@jjneeb has documented this well).

If you want to do vector work there are some reasonably good ways you can use Vectric products to do what you want, either with, or without the laser module. That will involve some post-processor work, but it’s not too bad. And lucky for you some others have already done a little work on that front.

I just wanted to step back and see what you had in mind…

1 Like

Well the short answer is: it’s a new toy and I’m not quite sure how my workflow will evolve.

Longer answer: I’ll definitely etch some logos etc into wood projects, but I’m also really excited to play around with cutting fabric.

Certainly for more elaborate image burning, I want to explore that Mach4 ESS rastering process.

But since I do the vast majority of my CAD/CAM in Fusion, I’d really like the ability to generate both laser and milling toolpaths in the same model, at least for simple vector work. I realize that Vectric might be better suited to this, but I had just assumed there would be some kind of off-the-self solution for F360 and Mach4. Are we laser-having-fusion360-using-mach4-controlling-avid-cnc-owners really that rare??:rofl:

This process of editing F360 post processors is really interesting, but I’m definitely still at the part of the learning curve where it feels like a cliff.

Fair answer! :slight_smile:

Check out this link: FAQ Mach4

You should follow that for laser setup options, but specifically for laser image rastering there is a section that explains how you do that. Essentially you need to prep an image and write a little G Code to make it work. (I think @jjneeb posted this link earlier)

If you want to do image rasters to my knowledge this is the only way you can do it with the ESS/Mach 4. As they explain in that link, a lot of G Code is needed to do an image raster. If you create an image raster with a 3rd party program the G code generated is too much for the ESS to handle, and it either won’t work or you will get a poor image.

To image raster G Code generated with programs like:


Won’t work. (or won’t work well)

Now if you want to do vector lasering you can do that well with Vectric. You can do that in two ways: use the laser module OR you can hack together a pretty good post processor that fakes out an endmill into being a laser. Using that link to Warp 9 above will get you the G codes needed to pull this off. If you don’t already have @jjneeb 's posts he has done a lot of work on this front.

If you’re going to get your feet wet editing posts Vectric posts are FAR easier to edit than Fusion’s posts.

I would say the vector editing abilities of Vectric for “laser things” are far better than what is in Fusion so I’d focus your energy on Vectric if I were you.

Do keep us up to date with how things go. I’d be interested in hearing.

I just found, buried over in the Autodesk forum, a partially functional F360 Mach4 pp. It seems like it was only partially updated from the Mach3 laser commands, so I’m working on tidying it up. But it’s been very helpful to look over, and I figured other people might want to check it out. I’ll let you know if I make any more headway on this sidequest.

Read the Warp 9 and Jim Neebs work carefully. There have been a LOT of laser changes in Mach 4 alone. Mach 4 also was a total rewrite of Mach 3 so the post may be a good start, but likely not something you want to use out of the box.

There are different versions of the ESS plugin you can have as well and they have different commands and laser capabilities. The ESS version that Avid ships has some older laser support. Like Jim you can upgrade that to a newer version of the ESS that has far more up to date laser commands (and capability)

Save your currrent Mach/Avid directory though as running non support versions isn’t supported by support (ha!) but you can swap out your install directory from one version to another whenever you want.

I will! They’re a treasure trove of information. I’m thankful they’ve put so much effort into it, and shared that with everyone. I’d be even lost-er than I am now without it.

Definitely. I’m going cautiously, just editing typos, updating the conflicting Mach 3, and posting test code. But it’s been very helpful to me to have something to fix, instead of building from scratch.

1 Like

Let us know how it goes, and there’s a good helpful group here if you need anything!

For sure. One of the nicest things about Mach4 is how easy it is to backup/keep multiple versions on your machine. Going back and fourth is just a matter of renaming one directory.

1 Like