topic Re: Trouble with simple machining operation in Fusion Manufacture Forum

Trouble with simple machining operation

JetForMe — Mon, 14 Nov 2016 02:42:45 GMT

I'm having a number of issues with the latest Fusion 360 (and the previous version). I a very shallow set of pockets I want to recess in aluminum. I'm making a plaque of sorts. The 2D pocket operation insists on doing a helix into the pocket, and doesn't draw the entire tool path it generates. Here's a screenshot:

It should show a lot of path inside each pocket, but it just shows these down-then-up patterns. If you simulate it, it seems to do the right thing.

It also insists on the helix, even though I specified a ramp.

Second, I'm trying to accomplish something like this. The guy who did this didn't explain his entire process, but he said he just did "a 2D tool path" using an engraving tool from Tormach (it's a single-flute V-bit). Keep in mind he's done a lot of polishing on this. But I'd like to create tool paths using a larger end mill to get the bulk of the material out, then get the detail and sidewall using the V-bit. Any suggestions? Thanks!

My file is enclosed.

Re: Trouble with simple machining operation

daniel_lyall — Mon, 14 Nov 2016 04:26:54 GMT

There is a few problems with how you did the toolpath settings.

The easy way to do 2D pockets if they have a flat bottom is your bottom hight use selected and select the bottom face.

The tool entry was to big changing the Helical ramp diameter and the minimum ramp diameter to 1 fixed that.

you had stock to leave set at .5 mm when the letters are .3 deep.

the above 3 fixed the 2D pocket.

The engrave you have your bottom height set to the bottom face of what you want to cut and the top hight use selection and select the top face, also you select the bottom profile not the top other wise it's just a chamfer.

The biggest problem for you with the engrave is the tool is to big to fit in.

I have attached your file with the changes done enjoy.

Re: Trouble with simple machining operation

JetForMe — Mon, 14 Nov 2016 23:17:48 GMT

Thank you. I realized a bunch of those things later in the day, too.

I finally ended up cutting the entire pocket with the single V-engraving bit. The problem now is that there is some material left behind. I may be able to address that with a smaller stepover, but the bit has a very small radius point, and for the most part, it cut well. A smaller stepover would dramatically increase the operation duration.

I'm going to try again with a small flat endmill, because the ridge is only in the middle of some of the pockets:

It's a bit blurry, but if you look in the "F" and the "L" in the bottom row, you can see the ridges I'm talking about.

But I have a very hard time getting Fusion to do the right thing with multiple tool paths in these pockets.

Another problem I have with using multiple tools is that my tool lengths are slightly off, making the results worse. I hope I can fix that on the machine.

Re: Trouble with simple machining operation

Steinwerks — Tue, 15 Nov 2016 00:28:24 GMT

Use a 3D Pocket operation and turn on Rest Machining from Previous Operations to go after just those ridges. Should do much better than running over the entire text again (even if just a couple characters).

Re: Trouble with simple machining operation

JetForMe — Tue, 15 Nov 2016 02:02:09 GMT

I'm not sure I understand. You mean use a 3D pocket operation instead of my other operations? Or in addition to, after the first 2D operation? What kind of tool, the same V-bit engraver?

In the case of the former, I put the 3D path in, and it's covering the entire part, not staying within the pockets.

Re: Trouble with simple machining operation

Steinwerks — Tue, 15 Nov 2016 02:04:29 GMT

Use it after the 2D operations, but inside the same Setup. You can also constrain it inside the letters with Machining Boundary -> Selection.

Re: Trouble with simple machining operation

daniel_lyall — Tue, 15 Nov 2016 02:42:41 GMT

@JetForMe like the pick below.

you can also just use the bottom height and use selected and select the bottom faces and that's it

Re: Trouble with simple machining operation

JetForMe — Tue, 15 Nov 2016 07:28:50 GMT

This is what I'm up to now (file attached). It rubs me the wrong way, to use the big tool (1mm end mill) after the tiny tool; I'd much rather use the large tool to remove the bulk of the material, then use the small tool to machine the remaining material. Doing the 3D pocket clearing operation after adds 5 minutes to the op (the initial 2D pocket is 10 minutes). This doesn't seem ideal, but I have yet to try it to see the results.

Re: Trouble with simple machining operation

JetForMe — Thu, 17 Nov 2016 07:13:39 GMT

I still can't get it to do the right thing. The second pocket operation, with a 2 mm end mill, ends up blowing out the boundary of each letter, destroying the fine detail. It also cuts too deep (and I've triple-checked my tool lengths).

Re: Trouble with simple machining operation

daniel_lyall — Thu, 17 Nov 2016 07:39:30 GMT

Have a look how I have done this.

Re: Trouble with simple machining operation

JetForMe — Thu, 17 Nov 2016 22:49:00 GMT

Thanks for that @daniel_lyall, but (assuming I understand it correctly), you've only done a single operation with a 1 mm end mill. I want to use the chamfering tool to get the chamfer and finer points in the corners of the font. I just don't want it leaving ridges of material in the middle of the pockets like it does in some instances.

I improved the appearance of the toolpath by reducing the maximum stepover (which was more than 3mm). The tool tip radius is 0.010", so I set it to 0.008" max stepover. I won't be able to try cutting until tonight.

I still think the toolpath generation itself could use a bit of improvement, but we'll see how this works out.

Re: Trouble with simple machining operation

daniel_lyall — Thu, 17 Nov 2016 23:07:06 GMT

You have the V bit part in hand.

Most times it is easier to use a 3D toolpath, 2D toolpaths do what you set them to do that's all they do.

3D toolpaths have some brain power behind them you can just pick the tool set what to cut and just tick stock contor and select the model and done.

some 3D toolpaths you just pick the tool, tick stock contor select the model and put the bottom height onto the bottom of a toolpath and done.

engrave is a bit different again it's a 2.5D toolpath