Fusion 360 Guide For Multi-Pass 3D Engrave

In a bit of a follow up to my Laser Guide and Rotary CNC Guide, I’ve decided to do a quick 3d relief guide for the snapmaker using Fusion 360. This guide assumes you know some basics of running the CNC, such as being able to jog the machine with the control app, set work origin, and set origins for the axes independently. There will also be some optional G-code changes and sizing done in other programs to achieve a better result.

Disclaimer: I am in no way responsible for any possible damage to your machine or materials, although risk is very minimal if you follow along exactly as I am going to include images of my settings, setup, and results as I’ll be carving this. Please read the entire guide before attempting.

Materials and Machinery in this tutorial:
Snapmaker A350 + Enclosure
Tools: 3.175mm (1/8") 2-flute up-spiral flat end mill for roughing; 20 Degree Engraving bit for finishing.
Material: Solid Maple Wood - 152.4mm X 152.4mm X 19mm (6" x 6" x 3/4")
Model to be machined: Owl CNC High Detail by billywoodworks found here: Owl CNC High Detail by billywoodworks - Thingiverse
Software: Prusaslicer 2.4.0 (for optional STL modification) & Autodesk Fusion 360
Required Downloads: Snapmaker Configuration & Tool Libraries

I: Preparation

1: Download the software, model, and measure the stock you will be carving into.
1a: If you’ve never used Fusion 360 before sign up for and download the personal/hobbyist version here: Fusion 360 for Personal Use | Fusion 360 | Autodesk
1b: If you’ve never used Prusaslicer, learn to, it’s a much better slicer than Luban and is actually quite powerful and easy to use/learn: Original Prusa 3D printers directly from Josef Prusa
1c: The thickness of the material isn’t as critical, as the engrave will always be from the surface, just ensure it’s thicker than the height of the model.
2: Follow the quick start guide for setting up the bit and workpiece.
2a: Go ahead and mark the center of your material and get it clamped down.
2b: You should be loading the Flat End Mill for the initial roughing pass.
3: Go ahead and set your work origin following the quick start guide and use the control app to move Z up from the workpiece about 10mm.

II: Editing The Model

1: My material is 152.4mm square (6" Square), and I want a border of 12.7mm (1/2").
1b: 152.4 subtract 12.7 x 2 (25.4) = 127mm (5") will be the size of my model, open in Prusaslicer.
2: Use the size/scale boxes to take the larger size (in this case the Y dimension) and change it to our target size of 127mm.
PS Sizes

2a: You will notice all the other sizes change in scale, if they do not, undo with the back button in the upper toolbar and make sure the lock icon by scale is “locked”
3: Since the model has a thick base, you can use the trim tool to remove most of it, the cut tool is at the very left.
3a: Uncheck “keep lower part” and either use the handles or input a size to cut off (I cut off 3.5mm)
PS Cut

4: Check the Z height back in the size/scale box, this is how deep it will carve.
4a: You can adjust how deep you want the carve, the deeper the carve, the more details you get, but the longer it will take. An average of 5-8mm is pretty decent I find.
4b: To adjust depth, UNLOCK the lock by the scale and modify the Z size. Since it was 6.4mm and the model looks good already, I’ll leave it.
5: Export the modified STL by either right clicking > export as STL, or clicking in the menu File > Export > Export plate as STL.

III: Preparing The Model in Fusion

1: Open Fusion 360 and get a drink.
1a: If your beverage contains alcohol, drink it slowly.
1b: If you’ve never used Fusion before, you need to add the post processor and tool libraries you downloaded above.
1c: Installing the post processor.
1d: Installing the tool library.
1e: Fusion is well documented and most functions will have a very nice explanation if you hover over them.
2: Import the model into Fusion 360 by clicking the arrow in the toolbar under insert > Insert Mesh
2a: In the insert mesh window that comes up, click the buttons in the position section Center > then Move to Ground
2b: Click Ok.
2c: Click the little home icon by the control cube in the upper right to recenter on the model.

IV: Using Fusion CAM to Assign Toolpaths For Roughing

1: In the upper left where it says “Design”, click this button followed by “Manufacture”
2: If you have not already, import the Snapmaker tool library as outlined above. If you have problems, feel free to post on this thread and I’ll see if I can help.
2a: If you finished your beverage by now, get another.
3: On the left list, right click setups > New setup.
3a: In the new setup window, click the 2nd tab for stock, change the stock side and top offset to 0.
3b: Also make sure the origin point is still in the center of the model on the very top and click ok.
4: On the upper toolbar click the arrow in the 3D tools > Pocket Clearing to bring up a new pocket process.
5: In the first tab, Tool, click select next to tool.
5a: If you still haven’t imported the tool files yet, right click local > import libraries. Select the 3.175mm Double Flat Endmill and click ok.

5b: Click coolant and select disabled, the snapmaker does not have any air or fluid coolant.
5c: The feeds & speed can be left alone if you desire, but they ARE a bit conservative. I bumped Cutting Feedrate to 600, Ramp Feedrate to 300, and Plunge Feedrate to 200.
6: Second tab, Geometry.
6a: Machining Boundary will be Silhouette, since the surrounding square is already part of the model. Bounding box would make a square the extents of the model, hover over for a good visual. Bounding Box is really good for things with organic shaped edges.
6b: Tool Containment: You’ll generally want inside boundary, unless the very edges are not really part of the model, such as using bounding box. Leave the other options.
7: Third tab, Heights, don’t change anything here, but it’ll give you a view of where every movement will be.
8: Fourth Tab, Passes. This will be the meat of the setup and can make or break your project (and tools).
8a: The first thing to change will be checking “Manual Stepover” and change the Maximum Stepover to 30-40% the cutter diameter (1.25mm works nicely)
8b: Next is the Maximum Roughing Stepdown, the Snapmaker can handle 1mm fine, but you can reduce this a smidge to 0.5-0.6mm to be a bit smoother.
8c: Flat Area Detection is at your discretion, hover over and see if you want it. It could increase machining or computation time, but I usually leave it on.
8d: Ensure Stock to Leave it checked. Radial is horizontal stock, Axial is vertical stock. Somewhere between 0.3-0.5mm is fine for these.
8e: Fifth tab, Linking. Nothing to do here really, it’s to setup how the bit enters and leaves the material, defaults are good unless you have specific needs. Click Ok.
9: It will now generate the toolpath. In the list on the left, you will see the pocket added. You can right click > simulate and watch a simulation of how it will run, under the statistics tab you can see an ETA of how long it will take.
10: Post Process. Right click the pocket > Post Process > in the post click the “…” and select the snapmaker.cps and click Post at the bottom to save the file with a name like OwlRough3.175 (this tells you the model, rough pass, and bit to use).

V: Using Fusion CAM to Assign Toolpaths For Finishing

1: You have a few options for the finishing pass, under the 3D menu you can use Parallel (goes back and forth like Luban), scallop (similar), or Morphed Spiral (my preferred and will be using)
2: First tab, Tool, select tool to bring up the tool list.
2a: Snapmaker’s tool list does not include any of their V bits… Sigh. Refresh your drink.
2b: Click the + above the tool list for a new tool and select Engrave/Chamfer Mill.
2c: Name it what you want, in this setup I’m using a 20 degree engraving bit (this is the cheap bit that comes with a lot of chinese CNCs like the 3018 and is very cheap to buy)
2d: Under the Cutter and Cutting Data tabs, use the information I’ve provided in these screenshots, click Ok, then Ok again to select the tool. Leave everything else under the tool tab.

3: Second tab, Geometry. We do have a couple specific things to do here!
3a: It should already be setup as silhouette, you can do tool center on boundary to ensure the walls are cleaned up.
3b: Contact only is a personal preference, but since we have no openings/through cuts, uncheck it.
3c: Check “Rest Machining” and make Adjustment Offset 0.
4: Fourth tab, Passes (ignore tab 3 and 5)
4a: Reduce stepover to 0.1, the other options should be good. Click Ok.
4b: Refresh your drink again, since by the time it finishes, so will your current drink. Morphed spiral takes a lot longer than Parallel, but the results I find are much better.
4c: It’s still generating, pet your cat and/or dog. It’s making a path one tenth of a mm at a time.
5: Watch the simulation, check the time, etc as you want. Then Right click > Post Process. Snapmaker should still be there, if not, select with the drop-down.

VI: Optional G-Code Optimization

1: If you’ve followed my laser guide, you’ll already have Notepad++ as it’s what we’ll be using in this section.
2: The free version of Fusion 360 reduces rapid non-cut movements to the same speed… but we know how to get around that.
3: Open the OwnRough3.175.cnc file in Notepad++ and stare at it a bit.
4: We’ll be changing the feedrate of our “Clearance Height” and our “Retract Height” so when the bit is above the workpiece, it can move faster.
4a: In Notepad++ press Ctrl+H to bring up the replace window.
4b: Find box: “Z15.000 F300” Replace box: “Z15.000 F3000”, replace all (should be about 2 instances).
4c: Find box: “Z5.000 F600” Replace box: “Z5.000 F3000”, replace all (should be about a bunch).
4d: NOTE: the F600 is the feedrate we set in the roughing pass, if you left it at default, or changed to a different feedrate, use that. You can check what it is by just looking for “Z5.000” and the feedrate that follows it.
4e: The finish pass does not need this, the tool never lifts and rapids.
5: Save the file, use either Luban or the USB stick to transfer the file to the snapmaker.

VII: Beginning the Rough, and Getting a Snack

1: If your beverage contains alcohol, and you’ve had several by now, it might be wise to get a snack… or another drink, I’m not your mom.
2: Since the workpiece has already been setup, clamped, and origin set, you should be able to go ahead with running the rough pass file. You can run a boundary if you wish to ensure it doesn’t collide.
3: Remember to periodically clean dust to prevent the chips from being recut and reduce heat, both which shorten tool life.

VIII: Swapping Bits, and Running the Finish

1: After the rough pass finishes, use the control app to move the toolhead into a position where you can swap in the V-bit.
2: Jog the toolhead back down above an uncarved area (like the border we set up earlier) of the workpiece.
3: Use the calibration card to set the Z height, then tap the set origin tab and ONLY set the Z origin.
4: Move the Z axis up ~10mm, then tap go to work origin. It should move back to the center and down to where the tip of the bit is at the top of the stock.
4a: If it does not… oof. You might have accidentally tapped set origin for all, or x/y individually.
4b: Hopefully the roughing pass left the center mark you made so you can try realigning the center so the entire engrave is not lost, otherwise you may have to get tricky with a ruler or similar to try centering it to the best of your ability.
5: Run the finishing pass.

IX: Afterthoughts

1: IF THE BIT BREAKS, follow section VIII steps again to put a new bit in and set a new Z height and make sure to remove any shards, try slowing the feedrate down.
2: Marvel at how short of a time it takes vs just loading it in Luban. (seriously)
2a: Fusion’s ETA for the roughing pass was 0:59:19
2b: Fusion’s ETA for the finishing pass was 9:59:28 (total 10:58:47, but the ETAs, while somewhat accurate, have always seemed to be a bit longer than it actually takes YMMV)
3: If you can get past Luban sticking at “Loading object 52.5%” (alright, I never did. Luban 4 sucks, let’s load into 3)
3a: Loading the STL into Luban 3.15.2 (which still takes a decade), selecting the carving V bit with the defaults of 300mm/min, and 0.5mm stepdown. We put in a density of 10 (to match our 0.1mm stepover, default is 5 or 0.2 which would leave flakes with the grain of the wood), and finally under height/tabs we put our target depth at 6.4 to match our model (by default luban squishes it to 2mm).
3b: It was a long road to get here, but our Luban ETA is 105 Hours 46 Minutes. Eesh. (for funsies, at the default 2mm it would still take 30 hours 31 minutes)

I’m sorry this guide a bit longer, I likely went into some details that weren’t required, or I may have forgotten something. Once you get the hang of it, it’s pretty easy and quick. Please feel free to post any questions about specific things you have a problem with. This guide was very quick and dirty, leaving out a lot of potential things, but it’s for basic engraving. Larger projects will require more thought in the setups and maybe messing with some settings we glazed over here. Maybe even adding in additional passes. However, I feel this is a good start to making your projects faster, and look better. :slight_smile: Bonus image of the finished product with clearcoat.


Mood :joy:. This is a great set of instructions, thanks for making these.

I may, or may not, have had to refresh my own drink while doing this guide… :wink:

Also; this guide SHOULD work for most any home CNCs, such as the 3018 models. (I do have a Sainsmart Genmitsu 3018-pro as well), the only real differences is reducing the speeds/feeds/stepdown/stepover a little (I use 600mm/m feedrate, 0.6mm stepdown, 0.5mm stepover for roughing) simply because it sounds more rattily and I have neighbors. I’m sure it can handle a bit more though. Also change the post-processor to GRBL, uncheck output M6 and tool number and set safe retracts to Clearance Height. Also in the Setup window (where the stock got setup) click the 3rd tab (post process), and set WCS offeset to 1. So there, if you have a 3018, these changes will let you use the above guide. Enjoy.

1 Like

Have you checked out GrblGru? I wonder if maybe it’d be less of a headache than F360.

I’ve yet to try out the CNC function, but I’m a little wary about further investing into f360, if they ever decide they want to just start charging for the CNC toolpathing, I’d hate to be so locked in.

GrblGru seems to only support Grbl, which the Snapmaker uses Marlin. Also in my testing, it seems quite frustrating and slow to use. A better alternative for those who do not want to use Fusion would be FreeCAD, it’s open source and Snapmaker does include a post processor in the config download. I don’t personally have experience with it, however, so I cannot be much help in this instance. It can be found here: https://www.freecadweb.org

Another option is Kiri:Moto, while not explicit in supporting Marlin, I’ve seen a lot of success in forums and other posts while searching for info. Even a forum post from the author who states they have several Marlin machines and it works. It’s also free and browser based found here: Kiri:Moto
However, snapmaker does not include setups or post processors, so you will have to test and figure that out yourself.

1 Like

Great guide! Thanks for sharing.

Why are you using manual stepover for clearing paths? Unless you’re looking for a smooth surface finish on a flat piece there’s no reason to have it default which ends up being just a little less than the cutting diameter. As long as you have ‘stock to leave’ set to on then you’re just trying to get rid of as much material as fast as you can.

I like to use both 1/4" and 1/8" bits for clearing to speed things up even more.


Mostly to help reduce tool wear and noise, and as a “safety catch” for newer people. Fusion likes to take 3mm per swipe and causes a bit of a racket and chatter, which can be scary. Although it doesn’t particularly matter if you have axial stock to leave, and you have the snapmaker in a garage or workshop. My own snapmaker is in my apartment, so I have to try to find a middle ground between speed and noise and this seems decent. How I wish to have my own workshop, sigh.

Overall, yes, you CAN let Fusion adjust your stepover and it’ll decrease time. :slight_smile: I should have pointed that out in my guide, thanks for bringing it up.

I’ve never had any problem with chatter as long as I kept my step-down less than 1mm and don’t push faster than 400-600 (hardwoods). I usually run .5mm stepdown.
You’ll dull your bits just as much if not more by having more passes and more time in contact where it’s still generating heat.


A couple changes/additions I’d suggest:

Once you’ve set your work origin and before starting the roughing pass, write it down or better yet, take a picture of it. That way if you accidentally hit “set work origin” you can simply go back to it. Even if you have a toolhead crash and lose steps you can usually get back to the same spot after homing. No need to fool around with 4a & 4b.

3 should read:
Swipe left on origin/boundary icons to get to “Set Z origin” ONLY change Z origin.


Facepalm I’ve used the method of taking a picture of the origin before, I don’t know why I forgot about it during this guide. Thanks for reminding me of that. I wish it was more rigid and I could setup machine 0,0 as the origin like I do the laser. I’m still sorta new to the hobby level machines, I’ve ran commercial CNCs for over a decade and miss some of the comforts. :stuck_out_tongue: I’ll eventually come up with a better method and do an updated guide. I just hope this is good enough to help beginners.

Is it possible to upload and use the Snapmaker 2.0 tool library with the snapmaker original?

It would be better to grab the tool library from the snapmaker original downloads: https://snapmaker.com/snapmaker-original/downloads

The problem is the SM original only has a library of three tools!!

It should work, just edit the tools to match the original specs, mainly the spindle speed (as I recall the original has a faster spindle). Import the 2.0 tool library and edit each tool to match RPM and you should be good to go.

Thanks will give it a go