Fusion360 CAM-Layout Checklist

[mrfugu]

Hey,

I found that creating a CAM-Layout Assembly for each workpiece (thickness or sheet) was pretty handy. I worked up a few more ‘best practices’ into a checklist to be completed prior to entering the Fusion360 CAM environment.

I made a PDF of the checklist that others might find handy.

This assumes that you’ve created your Fusion360 Model with ALL parts to be cut as independent Components and arranged them within a ‘3D-Model’ Component. (below the top level component of the project.)

You then create a CAM-Layout component for each sheet or thickness of sheet you’re planning on milling.

Then copy/paste the Model Components into the CAM-Layout (preserving their edit-ability within the Model Component, with changes flowing through to the CAM-Layout)

Align and Nest the Components on the CAM-Layout sheets.

Create Dog-Bone radiuses on inside corners (it is important to do this last so as to not effect your model assembly. The Dog-Bones are a function of the material (plywood) and not a function of the model (in most cases) and are therefore part of the CAM preflight, not Model creation process.

review and save and you’re off to the CAM environment.

I hope to follow up by posting similar checklists for MaslowCNC specific settings for the various common CAM operations (Drilling, 2D-Pockets, 2D-Contours, etc) in the near future.

Fusion360 Pre-CAM Checklist.pdf (37.4 KB)

hope this helps,

[LakeWorthB]

Great, I am still learning how to do CAM with fusion 360, and like your checklist, but have a question:

1. What do you mean by arranged within a “3D model” component?

This might be useful for you, but I bought an addon for $2 that does the flattening and nesting, called MapBoards https://apps.autodesk.com/FUSION/en/Detail/Index?id=7055850008078104945.

[mrfugu]

I set up some Components just to keep parts organized and some to keep processes organized.

ex: 3D-Model (contains all the components and subassemblies and collections of parts to make a working model, or the most complete/detailed version i need.

Every part to be milled is here, but so are imported McMaster-Carr hardware parts, and I’m trying to build the model so that i’m taking advantage of everything Fusion360 offers (weather or nort I can take full advantage of that now is a different matter, but I’m getting better at Joints, and other ‘part to part relationships’)

That component tho is ill suited for laying up parts for CAM processing, so I use the paste command to bring parts into a CAM-Layout component for each different material thickness I might be intending the Maslow to cut.

This lets me keep the process of building the part in Fusion360 completely separate from all the other considerations of Machining.

I add to each CAM-Layout, a component that is the dimensions of the Stock as well, which makes it easier to ensure everything is the correct orientation and whatnot, and that it all fits and is the intended thickness, sizes and distances if >1 part is being laid out.

I end up with a ‘top level component assembly’ for the 3D-Model and one for each material thickness or whole sheet to be milled.

To layout everything, I turn off the model and sketches and only work on a a single CAM-Layout at a time, and do the same when in CAM mode

Then, when moving to the CAM portion of the process I’m only messing with a single material thickness, which in and of itself dictates some of the tools and operations used and is best kept together.

[Jamtek]

@LakeWorthB Nice add-in, two got have time savers are a dogbone generator and a Nester. The one you found in the app store looks like it does good job laying out the parts.

Im using the Nester add-in from here, also check out Patrick Rainsberry youtube video, link is on his github page below.

tapnair/NESTER

Dogbone generator.

DVE2000/Dogbone

Neither one of these add-ins are in the app store, you just have to unzip the folders and drop them in the Fusion add-ins folder, instructions also on the github pages.

[K3IH1]

Is there an step by step on Fusion360 cam specific to the maslow? I walk through most of the steps I see in other tutuorials but can never get Gcode out of Fusion. Hoping theres a video somewhere that can walk me through taking a part and creating g-code in fusion on the maslow.

[mrfugu]

From the CAM environment within Fusion360:

Make a new ‘Setup’ Folder and begin adding CAM operations (generally from the inside > out with small holes and pockets 1st and contours last)

You’ll want to make sure your CAM operations are sensible, ie: use the simulator a lot, know the limits of the maslow (x/y/z speeds) and those of your router (spindle speeds) and bits (which should be measured, named and numbered, and saved in the Fusion Tool Library, a lot of organization here goes a long way).

Remember that Fusion360 is suitable for MANY completely and utterly different types of CAM operated machines, from heavy duty 2 axis Lathes to 3d printers to building sized 5 axis machining centers and everything in between. I recommend spending a fair amount of time looking through the different options available in each CAM operation until you feel comfortable with what each setting purports to give you control over. Much of it is not terribly important to a machine of MaslowCNC’s ‘accuracy’, but IS for machines that measure their success by 10000’ths of an inch. Spend some time to understand the scale of the numbers in the CAM operations settings.

Taking all this into account, along with observation from both the simulator and in practice on the machine will lead you to begin to save pre-defined settings for each of the major CAM operations (2d pocket, 2d adaptive, and 2d contour are what you’ll be using 99% of the time.)

In each of the CAM operation setting’s tabs, right clicking in an input box will let you save a setting as a preset for that operation, then once an operation is complete and in the Setup Folder on the left, you can right click there and Save that whole operation (sans the contours/paths) as a preset for that type of CAM Operation. eventually you’ll have a list of operations, ex: “MaslowCNC 1/4” 2 Flute Compression Bit 2D Contour", “MaslowCNC 1/8” Hole Drill", etc.

It’s probably a good idea to write out a list of things that need to be done for ‘changing a tool’, ‘adding a tool’, to check before machining’, it’s helped me, and I’m finding that adding a few checks and steps to each process happens with each mistake or unintended error.

Install the maslowCNC Post Processor to your Fusion Post Processor Cloud. I’m not sure why but this is now unavailable on Autodesk’s Post Processor Site, but a search of the forum should give you a link… its around here somewhere.

Once you have the CAM Setup Folder populated with operations, each having been meticulously doted over in the simulator and triple checked for having numbers that make sense, you can right click the Operation and Post Process it.

This is where you would select the MaslowCNC post processor file and save the result as ‘filename.nc’, which is then opened by and run in Ground Control.

hope this helps,

[K3IH1]

Wow… Thank you @mrfugu. Extremely thourough explaination. After trying this I’ve got most of it. The post process (Maslow specific one) is a little tricky on a Mac but I’ll keep working on it.

Thanks again. Tons of value here.

[Jatt]

if you’re using the mac app store version of fusion 360, here is how to install the maslow post processor:

1. Open terminal.app (located in Applications/Utilities) and enter
   mkdir -p ~/Library/Containers/com.autodesk.mas.fusion360/Data/Autodesk/Fusion\ 360\ CAM/Posts/
   hit return.
2. Close terminal and go back to the finder. Press command-shift-G
   In the dialog box that opens, enter ~/Library/Containers/com.autodesk.mas.fusion360/Data/Autodesk/Fusion 360 CAM/Posts/
   and press return or hit “go”.
3. Download this if you don’t already have it.
   Take the downloaded “maslowcnc.cps” file and drag it into that folder you opened in step 2. You can now close this folder.
4. Launch Fusion 360 and select the path you wish to use with the post processor.
   Select Actions > post process and under “Source” select “Personal Posts”
   The “MaslowCNC” post should appear in the Post processor dropdown.
   

[K3IH1]

That was extremely helpful and straightforward. I was looking for that folder in a bunch of different locations and wasn’t able to find it. Thank you! It looks like it worked. I did get a compatibility error for bridge but the code looks great!