Welcome to Our Community

Some features disabled for guests. Register Today.

Trochoidal Milling of Contour Slots with Fusion 360

Discussion in 'Tutorials' started by Scotty Orr, Mar 1, 2018.

  1. Scotty Orr

    Scotty Orr Master
    Builder

    Joined:
    May 21, 2015
    Messages:
    281
    Likes Received:
    135
    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).

    Screen Shot 2018-03-01 at 4.34.41 AM.png Screen Shot 2018-03-01 at 4.36.10 AM.png
    Screen Shot 2018-03-01 at 4.38.00 AM.png Screen Shot 2018-03-01 at 4.57.32 AM.png

    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.

    Screen Shot 2018-03-01 at 9.39.01 AM.png Screen Shot 2018-03-01 at 9.41.15 AM.png Screen Shot 2018-03-01 at 9.45.09 AM.png
    Screen Shot 2018-03-01 at 9.46.44 AM.png Screen Shot 2018-03-01 at 9.49.22 AM.png Screen Shot 2018-03-01 at 10.04.59 AM.png
    Screen Shot 2018-03-01 at 10.43.10 AM.png

    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.
    Screen Shot 2018-03-01 at 11.19.52 AM.png

    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.)
    Screen Shot 2018-03-01 at 11.11.34 AM.png

    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).
    Screen Shot 2018-03-01 at 11.17.09 AM.png

    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).
    Screen Shot 2018-03-01 at 11.12.34 AM.png

    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.
    Screen Shot 2018-03-01 at 10.03.11 AM.png

    Click OK, and hopefully you will be rewarded with a nice "trochoidal" tool path for your contour slot.
    Screen Shot 2018-03-01 at 10.04.09 AM.png Screen Shot 2018-03-01 at 10.08.01 AM.png

    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.
     
    #1 Scotty Orr, Mar 1, 2018
    Last edited: Mar 1, 2018
    Peter Van Der Walt likes this.
  2. Giarc

    Giarc Master
    Moderator Builder

    Joined:
    Jan 24, 2015
    Messages:
    925
    Likes Received:
    442
    I love designing in Fusion 360. I have generated gcode with it and it works great. I have not attempted to do trichoidal like you are yet. I make a lot of flat plates with holes, slots, or pockets in them, too. I thought it was kind of funny when I read this because I had an almost opposite issue. Recently, I wanted to use Estlcam with a part I designed in F360 and had to figure out how to convert my 3d object into a dxf so I could use Estlcam. The main reasons I wanted to use it is for the probing and edgefinding features and for trichoidal milling. Your tutorial looks like it should work though. What I always do (and is by no means a novel concept) is run two gcode files. The first is just the holes with the piece clamped down. Then when that is done, I screw the part down. Then I run the second file that does everything else. I rarely use tabs anymore. Also,I have never tried pausing a program. I am too scared. ;)

    Also, I have found that if you zero to the spoilboard with F360. you can cut completely through the part without damaging the spoilboard.
     
    #2 Giarc, Mar 1, 2018
    Last edited: Mar 1, 2018
    Scotty Orr likes this.
  3. Scotty Orr

    Scotty Orr Master
    Builder

    Joined:
    May 21, 2015
    Messages:
    281
    Likes Received:
    135
    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.)
     
  4. Giarc

    Giarc Master
    Moderator Builder

    Joined:
    Jan 24, 2015
    Messages:
    925
    Likes Received:
    442
    I have never tried a countersunk hole with F360 other than a shallow pocket for the head - unless that is what you mean. I have done them with Sketchucam, which is actually fairly simple to do. It is one of the hole options. I plan to try out Estlcam in a bit on this new 3D printer plate. It has some pockets for the springs in the corners. I plan to try 3 point leveling though.
    3d_printer_plate_2018-Jan-03_04-53-44AM-000_HOME_png.png
     
  5. Gary Caruso

    Gary Caruso OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    May 19, 2016
    Messages:
    546
    Likes Received:
    206
    Nice job Scotty, looks similar to what nycnc goes over in this video..

     
  6. Scotty Orr

    Scotty Orr Master
    Builder

    Joined:
    May 21, 2015
    Messages:
    281
    Likes Received:
    135
    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 :D ).

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

     
    #6 Scotty Orr, Mar 4, 2018
    Last edited: Mar 4, 2018

Share This Page

  1. This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
    By continuing to use this site, you are consenting to our use of cookies.
    Dismiss Notice