This tutorial will explain how to generate a toolpath in Fusion 360 and send it to your Handibot.

This allows for a completely "Mac only" solution without resorting to VCarve. Also, there are many other capabilities in Fusion 360 that make it a complete 3D Design package, so in some cases it can be more powerful.

PLEASE provide feedback so I can make this more useful for everyone.

You can download the sample CamClamp.f3d file above so you can follow along with this example in Fusion 360.

Step 1: Enable Cloud Libraries

First, Cloud Libraries must be enabled in Fusion 360. This allows you to store both your tool files and your post processor on your A360 drive rather than on a local directory, which makes everything much simpler.

Enable Cloud Libraries in Fusion 360 by going clicking your account (top right) and going to Preferences. Click CAM from the sidebar and check the box for Enable Cloud Libraries.

[Instructions leveraged from Inventables FAQ on Fusion 360]

Step 2: Download Tool Files and Post Processor

First, you must download both the tool files (which represent the bits available for sale on the Handibot site, including the ones that come with the Handibot, and the two other sets).

The Post processor should also be downloaded. The post processor allows Fusion 360 to output toolpaths in OpenSBP file format.

Here is the link to the Grabcad site , where these files are stored.

Download the F360toHBPP.cps file (the post processor) under the "Fabmo" directory on Grabcad. Download the files to a location where you can later find them to upload.

Then navigate to "Handibot Adventure Edition" and the "Fusion 360" subdirectory, and download the relevant "tools" files for the bits you have, at least the Handibot 3 Piece Bit Kit.tools file for the base bits of the Handibot.

Step 3: Upload Tool Files and Post Processor

  1. First, login to your A360 Drive Account and navigate to "A360 Drive".
  2. An "Assets" Library should automatically be created if you set the Cloud Library preferences flag and saved it correctly.
  3. Within this library, Fusion 360 may or may not create these directories:
    • CAMPosts - hold Post Processors (.cps)
    • CAMTools - holds Tool files (.tools)
  4. If they are not created, create them.
  5. Upload the Post processor you downloaded from the prior step (F360toHBPP.cps) to the CAMPosts directory (use the Upload file button or drag and drop).
  6. Upload any/all of the tool files you downloaded from the prior step to the CAMTools directory.

Step 4: Load or Create Your Drawing in Fusion 360

Create or load an existing drawing in Fusion 360.

Before creating a drawing it helps to make sure you've set your "Z" orientation correctly.

Under Fusion 360->Preferences, set the "Default Modeling Orientation" to "Z Up".

It is also preferable to set the units to "inches" at the overall model/sketch level.

Step 5: Switch to CAM Mode, Generate a "Setup"

Switch Fusion 360 to CAM mode by selecting it from the main dropdown where you normally select "Model" or "Sketch".

To begin CAM operations, first generate a "Setup" that determines the basic parameters for the CNC operations.

From the Setup menu at the top, choose "New Setup".

On the Setup tab on this window:

  • Operation type should be "Milling" for standard Handibot routing. I suspect eventually the rotary indexer might be able to be supported with the "Turning" operation type, but for now and for basic functionality, use Milling.
  • Orientation should be "Model" orientation if you followed the prior advice and created your design with "Z Up". If you did not, you can choose one of the other available options and choose which direction is X/Y/Z in terms of the Handibot.
  • Origin should be "Stock Box point", then select which corner you want to be the X/Y zero.

Choose the "Stock" tab in the Setup window to set additional options:

  • For mode, choose "Relative Size Box".
  • For Stock Offset Mode, choose "Add Stock to Sides and top/bottom".
  • Typically, you would want to add a little to the sides, say the width of the bit just to be sure.

If you want to change the relative position of your stock, for instance if you want to cut down into a piece of wood that the Handibot is resting on, and not cut out a block of wood that is on top of this position, you can change the stock's relative position:

  • For mode, choose "Fixed Size Box".
  • Set the X/Y/Z width values to absolute values as needed - including a bit extra on x/y as we did above.
  • For Z Model Position, choose "Offset from Bottom (-z)", and set a value to the depth of your wood - i.e. .5"

Although this last mechanism would seem to be the most flexible, at current I don't recommend it (unless I'm missing something --- please let me know if you are a real Fusion 360 expert that can help). Right now, if you offset the stock significantly as noted above, the toolpaths are not consistent or the same as they are when the stock is occupying the same space as the model. Could be a bug? Not sure. The alternative is to simply move the whole model/body to the desired offset, which is what I did -- for instance if you are cutting this out of plywood that the Handibot is sitting on directly, I put the model at Z -.5" to Z 0, so basically under the normal Z axis. This works well and is what the rest of these steps assume.

Step 6: Create Toolpaths

This is where you need to do some "playing" with the toolpath generation options to get Fusion 360 to do what you want. I'll show you what I did for this simple clamp as well as link to some other tutorials.

Here are some other valuable tutorials that might provide some help:

Make Magazine Fusion 360 Milling tutorial

Youtube Video - CAM for CNC Router in Fusion 360

For this part, I first used a 3D Ramp toolpath, followed by a 2D Contour toolpath.

Although there are 3D toolpaths that could cut everything out in one pass, I chose the 2 step method here because only the 2D Contour option allows for automatic tab generation -- this is one area where Fusion 360 is not quite as powerful as VCarve. If you want tabs with other cutting methods, you would have to add them to the model itself. I haven't yet done that.

To generate a 3D Ramp Toolpath:

  • From the 3D Menu at the top, choose "Ramp".
  • From the tool box, click on the button to select a tool which opens the tool library. Click on the Library Tree button in the upper left. Make sure that under "Cloud" in the tree that all of the tools you uploaded are checked in the library, which will make the bits available for use. Then from the list of bits, choose the one you will use. Here, I select a 1/8 straight bit from the 3 bit kit.
  • Change coolant to "disabled"
  • The feeds and speeds will be loaded from the tool library - change the cutting feedrate and lead in/out if desired, or other values as well.
  • In the "Geometry" tab, choose Machining Boundary "Selection" and select the portions that the top of the model including the ramp section.
  • Select the "Heights" tab - if you have modified to use a "Z" offset, then you will want to change the "Bottom Height" to "Stock Bottom" so the appropriate adjustments will be made (not what was done in this example).

You should be able to now visualize the toolpath that was generated when you click on the tool action in the left hand tree (3D Ramp).

If you want to simulate the toolpath, choose Actions->Simulate after you have selected the main setup in the left hand tree. A couple of tips for simulate mode:

  • In the simulate options window, you can choose "Stock". The "transparent" checkbox allows you to see what is going on better. For an even better view, you may want to turn off visibility of the model itself (clicking the light bulb next to the model in the left hand tree).
  • Once in simulate mode, press the play button to see the tool in action. You can adjust the speed with the slider -- you probably want it faster than the default in order to get a good view.
  • At the bottom of the window, you can place your cursor to see overall machining time by operation

The Ramp toolpath should cut out, for this model example, the hole and slot and the 45 degree angle on one side will be cut out. Other experimentation here would be to use the

Now, generate the 2D Contour toolpath to completely cut out the clamp:

  • From the 2D Menu at the top, Choose "Contour".
  • Select the right tool and coolant (disabled) as above.
  • In the "Geometry" tab, select the base of the model/clamp.
  • Assuming you are using the 2D Contour path because you want tabs, select the tabs option and vary the options as appropriate. You probably will need to try the options to see how they work out. I needed to change the default height to be somewhat thicker than the original.
  • Go to the "Passes" tab and select "Multiple Depths". Check the values, but the defaults may work according to the tool selected.
  • Click on "OK"

You can see first just the 2D Contour toolpath by selecting it on the left hand side.

Then, to visualize the total toolpath, go back to the "setup" and choose Actions->Simulate.

Just to stress, this will take some playing around and practice and intelligent combinations between the available toolpath modes and "selections" of the model to execute. But there is substantial flexibility here.

Step 7: Export Toolpath Via Post Processor

First, select the entire setup on the left hand side of the model tree.

Then, from the top menu, choose Actions->Post Process.

Change the Source to "My Cloud Posts" to leverage the cloud post processor previously uploaded.

Change Post Processor to "F360ToHBPP.cps".

Change units to "inches" if it isn't already set.

If you want, open the NC file in the editor - this will allow you to preview the actual SBP file contents after it is generated. Helpful if you can "read" the OpenSBP format a bit.

Click on "OK", and save to a local file - probably want to change the default name to something other than 1001.sbp. Ensure you keep the .sbp extension.

Step 8: Optional - Preview Toolpath in ShopBot Control Software

If you are using Window, or have a virtual image, you might want to load up the .sbp file in Preview mode.

To download this software, check this Shopbot Link.

Open the software in preview mode only after choosing the Handibot specific option.

This will allow you to see exactly what will happen before sacrificing any material, and is a good test to see if the process has worked well so far.

Step 9: Upload File to Fabmo / CREATE!

Upload your final .sbp file exported out of Fusion 360 to the standard FabMo job queue and execute!

<p>Thanks, David. This is very helpful!</p><p>I could not find any way to do tiling with Fusion360. Did you?</p><p>(for jobs bigger than the 6&quot;x8&quot; working area of Handibot)</p>
<p>Nice tutorial. Do you have any pictures of parts that you have made using this technique?</p>

About This Instructable




Bio: Maker -- CNC (Handibot), 3DPrinting, LED Lamps/Light Projects, Particle Photons
More by DavidS1388:Fusion 360 Toolpaths for Handibot 
Add instructable to: