Trochoidal Milling of Contour Slots with Fusion 360

I'm pretty new to Fusion 360. In fact, I primarily use it to set up my CAM operations. I have yet to learn to design objects from scratch in F360. (I eventually will, but I'm much quicker with QCad.)

Most of the aluminum parts I make are pretty simple "plates" - an outline with a bunch of holes. My typical workflow goes like this:
1. Create a DXF using QCad.
2. Import the DXF into F360 and extrude to the thickness of my material.
3. Create tool paths using 2D pockets for holes, and 2D contours (with tabs) for outlines.
4. Clamp the aluminum to the table, and cut the holes and contour with the same bit (using multiple passes).

​

Now, the plate of aluminum that I use is usually rectangular in shape, and has often had another part or two already cut out of it. While setting up CAM, I set a zero top offset for the material thickness (for positioning my bit on the top of the aluminum). Then for the tool paths, I set a bottom offset of -0.2mm for the cuts (forcing a through-cut into my spoil board). This has worked pretty well, but the contour cuts are actually just slots and are hard on my bits. (When I break a bit, it is usually during the contour cut.)

I've been envious watching videos of EstlCam's trochoidal milling of contours/slots, but I really want to focus my attention on learning F360, and am not interested in switching to, or learning EstlCam for this feature.

I did some research on this with F360, and found that most of the stuff that applies uses "Adaptive Clearing", which is great, but contours typically require a fixture and milling away ALL the material outside the contour (then facing the other side). Well, I don't have "extra" aluminum to hold in a fixture and then "face" away the other side. (Plus, I'd have to pre-cut my plate of aluminum to a size closer to my part size.)

This "tutorial" is meant to show how I'm cajoling F360 to create a trochoidal tool path for my contour "slots". (And I thought also I'd record if here for my own reference, too.)

This will be my modified workflow:
1. Create a DXF using QCad.
2. Create a "box" in F360 that is 20mm longer and wider than my object and 1-2mm thicker than my material.
3. Create a sketch on the top surface of the box and import the DXF onto that sketch.
4. Select the outline of the DXF and create an outside offset wider than my bit diameter (4mm for a 1/8" bit).
5. Use press/pull tool to create pockets for the holes and new "contour slot" (0.2mm deeper than AL thickness).
6. Create tool paths using 2D pockets for holes, and 2D adaptive clearing for the contour slot.
7. (Optionally) Create a 2D contour path for a finishing cut.
8. Clamp the aluminum, and cut the holes. Secure the inside of the part with screws and cut the contour.

​

Notes: this will still cut into my spoil board by 0.2mm - that's OK with me. Adaptive clearing could be used for the holes as well. When creating the path for the "contour" pocket, you will need to select the floor of the pocket.

More details about creating the "trochoidal" tool path:
Select 2D Adaptive and choose your tool. For this tutorial, I am using a 3/32" endmill. For now, I am using the same feeds/speeds I used with my previous method. I will probably tweak these after experimenting some.


Under the Geometry tab, choose the floor of the contour "slot". (If you do a finish tool path later, you would choose the bottom edge of the part.)


Under the Heights tab, set a zero offset for the top and bottom (the excess cut depth was taken care of in the press/pull operation).


Under the Passes tab, set your optimal tool load and minimum radius. I used 0.762mm from something I read online (this may change). For radius, I just used half my tool diameter. In this example, I will not be doing a finishing operation, so I set material to leave to zero. Also notice this is a climb cut and NO multiple depths (sort of the point of doing this).


Under the linking tab, I didn't change anything except the Helical ramp diameter and the Minimum ramp diameter. If you get an "Empty toolpath" warning, these are probably set too high.


Click OK, and hopefully you will be rewarded with a nice "trochoidal" tool path for your contour slot.


I haven't actually performed a cut with this yet - I am waiting for more bits. I've also read something about a way to create "tabs" with something like this, and I may look into that more - but I suspect I will be using the "pause/add screws" method instead.

 

By "pausing", I actually planned to add some gcode to cause UGS to stop temporarily (like a tool change command that is "unsupported" in grbl). But separate files is probably a better idea...

I haven't experimented with Z-probing yet - I hope to, because I know setting z zero the way I do isn't consistent enough. Once (if) I get that working, I may well try the "zero to spoilboard" method. I also want to eventually ditch the step of creating the DXF in a separate program, but QCad just really works well for me (for now). However, I am beginning to want more complicated parts that will force me to use F360 more. (Something as simple as countersunk holes is not intuitive to do in F360 with an imported DXF.)

 

Thanks for that, Gary - I missed that one. I noticed that when he chose the objects for his path, he selected "edges" instead of the "floor". I tried that and kept getting an empty tool path. However, that may have been before I figured out which other parameters to tweak. I also didn't know that I could create a tool path based on just a top offset like he did. I may have to look at that some more and give it another go - would certainly simplify my process of creating an actual "contour pocket" in too-thick material (which felt like cheating ).

It was actually another of his videos that inspired me to figure this out.