topic Re: problems designing a toolpath in Fusion Manufacture Forum

problems designing a toolpath

maker9876 — Fri, 17 Aug 2018 15:44:13 GMT

Hi, wondering if anyone would explain how to machine a fiddly little channel?

The piece will first have been machined from the other side which will have given it's overall shape and taken out the big hole below the feature we're looking at in the image below.

Now from this, the "top" side, we remove a small wedge of material. I lazily did an adaptive with an 8mm cutter since that fits into the tightest curve.

small wedge removed with adaptive leaving the "tricky" channel

Since the channel (see RED arrow) is about 4.75mm wide figured it should be possible with a 4mm cutter. Couldn't get adaptive to work but pocket looked as though it might (simply by selecting the bottom of the channel).

Since the channel bottom is intersected by a diagonal hole and because it has squared ends that won't be milled properly selecting the boundary as is, created a projection of the bottom of the channel and tried extending it a bit (see below).

What results is a proper "area" in F360 terms (it shades when you select it) but am unable to use this as the basis for some pocket or adaptive or contour milling to cut out the channel.

What am I doing wrong?

tried creating a sketch "pocket milling" - a projection of the bottom of the channel with some additions

Re: problems designing a toolpath

Steinwerks — Fri, 17 Aug 2018 15:53:08 GMT

You can use 3D geometry for 2D selections. Faces work sometimes, but obviously not all the time. I would give this a shot, a sketch shouldn't be necessary.

I can take a closer look (or someone else might beat me to it) in about an hour if this doesn't get you there.

Re: problems designing a toolpath

maker9876 — Fri, 17 Aug 2018 16:05:07 GMT

Aha. It has to be 2D-contour to make segment by segment selections?

Now am a lot closer. Thanks! (The sketch seems nonetheless necessary because of the aforementioned awkward corners and the diagonal hole.)

Need to figure out why the arrows are going in lots of different directions....

Re: problems designing a toolpath

Steinwerks — Fri, 17 Aug 2018 16:23:41 GMT

You can edit chains for any toolpath like this, not just 2D Contour. It was simply an example Screencast I had made before.

Hide your sketch first or you risk selecting sketch and model geometry. Also you don't want to do single selections, you want to start with one and then edit it: click it a second time to "help" the CAM find the chain you want it to use - make sure you click the green "+" button or it will not take!

Re: problems designing a toolpath

maker9876 — Fri, 17 Aug 2018 16:36:22 GMT

Great. It's all working now....

Well except one tiny detail.

For some reason "Multiple depths" doesn't work as expected here. It refuses to PLUNGE to more than one depth. It only works if "ramping" is selected. Have tried selecting completely different geometries and it works as expected there, but not here. Why might it be insisting on ramping?

Re: problems designing a toolpath

Steinwerks — Fri, 17 Aug 2018 17:24:56 GMT

Can you export your part in its current state as a .F3D and attach it here? It will be much simpler to troubleshoot that way. It should be possible to fix though.

Re: problems designing a toolpath

maker9876 — Fri, 17 Aug 2018 17:39:14 GMT

Not able to export so here's the live reference

https://a360.co/2MV9FoI

Promise not to touch it!

In fact the 2D toolpath does have a relevant warning. It's set to multiple depths but is only performing the first of them.

If one goes in and turns on Ramping then it does both OK.

Don't see what the collision it's postulating would be?

Re: problems designing a toolpath

Steinwerks — Fri, 17 Aug 2018 18:48:35 GMT

So when I open your file I still see a lot of separate contours selected (which is why there are a lot of arrows). Turning on Ramp shows this in better detail as it attempts to ramp every contour chain (the toolpath geometry says there are 11):

Ideally for a 2D Contour here you should have two:

For some odd reason in order to get this to behave appropriately this was how I had to modify the chain:

But here's your collision, which is because of the lead-in settings on the inner profile. When you were using the sketch geometry the toolpath overlapped itself, which the CAM does not allow for, so it trimmed your lead geometry and added the warning.

Re: problems designing a toolpath

maker9876 — Fri, 17 Aug 2018 19:31:21 GMT

Fantastic. Thank you so much. There is no way I was getting that but, after a lot of trying have managed to replicate what you've done. Then noticed that the bit was knocking somewhere it shouldn't and changed the lead-in/out to correct that. Now quite pleased. All coming together. Looking forward to try. 😄 Thanks again!