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... 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. 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... 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!
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.
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.
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.
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).
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.
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: I just selected the top shoulder of the bore and selected Tool Inside Boundary. Does exactly what it's supposed to do!
I must be missing something, I tried to replicate but maybe something was lost on translation, so to say... My result: My settings:
Hmm, odd. Here's mine: 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.
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.
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...
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!
