Welcome to Our Community

Some features disabled for guests. Register Today.

Help with Fusion 360 Toopath

Discussion in 'CNC Mills/Routers' started by Felix_Hauser, Dec 3, 2020.

  1. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    27
    Likes Received:
    2
    Hi all,

    I was wondering if somebody would be able to give me a hand with a Fusion 360 toolpath I'm trying to do. The piece I want to machine is actually really simple, but because so far I have only dealt with easier toolpaths, it is quite challenging for me, even after many Youtube videos...
    Screenshot 2020-12-03 at 17.50.23.png
    It consist on a simple round hole with a chamfer at the bottom. I have already created a 2D Clearing in which the chamfer is left as a corner, which is what I expected and it is fine for removing large quantities of material.
    The problem is when I want the chamfer to look like a chamfer. The closes I got it a 3D contourm in which I selected the top and the bottom contours (edges?) of the chamafer and a 1/4" ball nose endmill as a tool. After calculating the toolpath, it doesn't look all that bad, but for whatever reason, wants to machine the whole contour, starting at the top.

    Screenshot 2020-12-03 at 17.55.49.png

    If I select the slope from 0 to 45 degrees, the thing goes nuts and instead of machining in circles, begins to plunge up and down...

    Screenshot 2020-12-03 at 17.57.56.png


    I would appreciate some help here. For the purpose of this piece, the chamfer is completely cosmetic, but I really want to improve my CAM skills. Any help is welcome. Thanks in advance!
     
    #1 Felix_Hauser, Dec 3, 2020
    Last edited: Dec 3, 2020
  2. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Aug 6, 2013
    Messages:
    3,461
    Likes Received:
    1,915
    I think you need a bullnose tool, with a 45 deg chamfer on the end. then ti can get to the sides and bottom and also do the chamfer without interfering with the sides as the ball does.
     
  3. Rob Taylor

    Rob Taylor Master
    Builder

    Joined:
    Dec 15, 2013
    Messages:
    1,470
    Likes Received:
    749
    Are you using Rest Machining, and Stock To Leave on the 2D clearance? A roughing op will always default to 0.5mm of stock to leave if you didn't touch it.

    Personally I'd actually let it do that and make sure the whole thing gets finished in the second op for a consistent finish.

    Those are rapids/positioning, not plunges, I'm not sure what it's trying to move between, but it may have something to do with your Stay Down settings in Linking.
     
  4. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    27
    Likes Received:
    2
    Thank you both.
    @David the swarfer I will have a look at the endmill you mention. However I don't really have a to-go store (online or otherwise) here in Germany.

    @Rob Taylor , yes, I'm using Rest Machining and Stock to leave. I will play a little bit with the linking settings to see if it changes anything.
     
  5. Rob Taylor

    Rob Taylor Master
    Builder

    Joined:
    Dec 15, 2013
    Messages:
    1,470
    Likes Received:
    749
    That would be why the entire thing gets redone, then. If you do a rough-finish strategy on the bores, zero stock to leave, and no Rest Machining on the chamfer op, it should (in theory) just do the chamfer itself (because the math should say it's the only thing remaining available to be cut).
     
  6. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    27
    Likes Received:
    2
    Well, to make it more clear. I use Stock to leave on the Adaptive clearing operation, followed by a 2D contour as a finishing step for the main bore. It is after the 2D Contour that I try to do the chamfer and in this operation I check the Rest Machining checkbox.
     
  7. Rob Taylor

    Rob Taylor Master
    Builder

    Joined:
    Dec 15, 2013
    Messages:
    1,470
    Likes Received:
    749
    Got it. I set it up the same, and a 3D ramp with a 0.1 degree (or less, whatever you want) helix angle seems to be the way to go:

    upload_2020-12-3_15-43-13.png

    I just selected the top shoulder of the bore and selected Tool Inside Boundary. Does exactly what it's supposed to do!
     
    David the swarfer likes this.
  8. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    27
    Likes Received:
    2
    I must be missing something, I tried to replicate but maybe something was lost on translation, so to say...

    My result:
    Screenshot 2020-12-03 at 21.57.43.png

    My settings:
    Screenshot 2020-12-03 at 21.58.42.png Screenshot 2020-12-03 at 21.58.30.png Screenshot 2020-12-03 at 21.58.22.png Screenshot 2020-12-03 at 21.58.11.png Screenshot 2020-12-03 at 21.58.01.png
     
  9. Rob Taylor

    Rob Taylor Master
    Builder

    Joined:
    Dec 15, 2013
    Messages:
    1,470
    Likes Received:
    749
    Hmm, odd. Here's mine:

    upload_2020-12-3_16-3-38.png

    upload_2020-12-3_16-4-25.png

    upload_2020-12-3_16-5-3.png

    upload_2020-12-3_16-5-34.png upload_2020-12-3_16-6-13.png

    The only difference the 1/4" bull vs 1/4" ball is gonna make is the length of that initial straight helix section, as the tool moves to touch the taper section tangentially.
     
  10. Rob Taylor

    Rob Taylor Master
    Builder

    Joined:
    Dec 15, 2013
    Messages:
    1,470
    Likes Received:
    749
    Either Slope or Max Stepdown, I guess, only differences I see.

    Ok, just tested, it is Slope. If you just click the down arrow to knock it down to 89 degrees, it takes out that entire sidewall.
     
  11. Felix_Hauser

    Builder

    Joined:
    Dec 7, 2019
    Messages:
    27
    Likes Received:
    2
    Got it!

    I think it was the Slope setting on the "Geometry" tab...

    Thanks @Rob Taylor ! I appreciate the time you took to help me out, I've been dealing with this a lot of time today...
     
  12. Rob Taylor

    Rob Taylor Master
    Builder

    Joined:
    Dec 15, 2013
    Messages:
    1,470
    Likes Received:
    749
    No worries! Usually when I spot a "specificity" setting like that I'll throw some loose numbers in there just to be on the safe side, like you saw with the 40-50 settings. Doesn't usually change anything at all, but sometimes, like here, it makes all the difference!
     

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