Undercut Causing Headaches - Fusion 360

[Anonymous]

I am trying to machine a part with an undercut an I am having trouble getting Fusion 360 to recognize the area I need removed before cutting the undercut.

I am trying to run a 2D Adaptive roughing tool path and an 2D Pocket finishing tool path. In both cases the only pocket selections that I can get to generate a valid tool path is the floors of the different levels of the pocket I'm trying to cut out. Since the floor extends under the undercut the tool path is trying to also cut out my undercut.

Is there another tool path I should be using?

Any suggestion on how to pocked out an area with an undercut?

[Laurens-3DTechDraw]

DataProto wrote:

I am trying to machine a part with an undercut an I am having trouble getting Fusion 360 to recognize the area I need removed before cutting the undercut. I am trying to run a 2D Adaptive roughing tool path and an 2D Pocket finishing tool path. In both cases the only pocket selections that I can get to generate a valid tool path is the floors of the different levels of the pocket I'm trying to cut out. Since the floor extends under the undercut the tool path is trying to also cut out my undercut. Is there another tool path I should be using? Any suggestion on how to pocked out an area with an undercut?

3D Adaptive? To be honest the masterpiece of the software.

[fredsi]

If you want to use the pocketing routine....

Create a sketch on the bottom of the pocket and project the edges needed to give the desired 'profile' for the pocket; then use that sketch in CAM to drive the pocketing routine.

Fred

Edit: Took a moment to duplicate a simple version of your setup. Although I usually find it easier to create a sketch (old habits), you can actually use the selection tools in Fusion to get the desired tool path (check this forum and Youtube for videos by Scott Moyse and others on using the selection menu).

For your situation, click on the bottom of the pocket to get the default profile. Click on the profile that appears, to bring up the 'advanced' selection menu. Hold down the Alt key and select the individual edges needed to create the desired closed profile - regardless of the level they are at in the model. Have attached an example of what you can get working in this way.

[scottmoyse]

Thanks Fred.

I would probably use 3D Adaptive here, but even then you may need to use the edge selection chaining to contain it. So 2D Adaptive may still be a pretty good option.

Our YouTube channel is here. There are a couple of edge selection videos. I hope to get up a more comprehensive one soon.

[Anonymous]

Thank you for the advice. I had a chance to mess around with it a little tonight but I am still running into problems. I'll try some more tomorrow and let you know how it goes.

[Steinwerks]

Select the top of the pocket, set bottom height via selection.

[scottmoyse]

N. Stein wrote:
Select the top of the pocket, set bottom height via selection.

Yup...

If you export your file as an f3d file, and attach it here, I'll do a quick video to show you how.

[Anonymous]

N. Stein wrote:
Select the top of the pocket, set bottom height via selection.

This method works but not for machining multiple bottom heights at the same time.

I attached the file if you have time to look at it. 

[Steinwerks]

Not at a computer, but try 3D Adaptive and Horizontal. Finish with 2D Contour, it might just take separate operations.

[scottmoyse]

I hope this video gets you going https://youtu.be/9Q0KsPPycsc

And I've attached the f3d file so you can check out the settings.

I suggest getting some quick start training from your local reseller to get you moving along as quickly as possible, so you can spend more of your time making chips.

[Steinwerks]

Very nice, Scott!

[Anonymous]

Thanks a lot Scott, that was great.

The part I sent you was exported from a bigger assembly. When I try your suggestions on the part in the assembly a tool path doesn't generate (Empty Toolpath)  :-\. This is one of the problems I have having previously. I tried programming with the base part as its own file and everything worked fine. So I guess I have something messed up in my assembly.

Thanks for you help, for the time being I'll just program this part separately.

[scottmoyse]

Hi mate, you can use Autodesk Screencast for free to show us what's happening and the workflow you are using.

[fredsi]

It has been our experience that putting toolpaths on parts that are in an assembly does not work very well. That is not to say you can't put a part into a vise (designated as a fixture) and get tool paths, you can. But we find that trying to keep multiple parts with CAM paths in a single file causes all sorts of problems with regard to stock and multiple WCSs.

I know this flies in the face of Fusion's philosophy of keeping everything in one file. I'd be glad to be proven wrong and see the work flow involved. Scott...time for another video?  🙂

Fred

[Steinwerks]

I guess it might be an issue with lots of parts? I have done two 3D parts in assemblies in Fusion, one of which involved three modified vise models, a subplate and two setups, and had zero issues.

Designating things as Fixture and Model is important. For one of the programs (two parts in a soft jaws) I modeled the stock as well.

[fredsi]

N. Stein wrote:
I guess it might be an issue with lots of parts? I have done two 3D parts in assemblies in Fusion, one of which involved three modified vise models, a subplate and two setups, and had zero issues. Designating things as Fixture and Model is important. For one of the programs (two parts in a soft jaws) I modeled the stock as well.

Ok, good so far. Now insert two new and different parts into the assembly, adjust the vises as needed, etc. Don't remove the previous parts, just hide them or whatever. Now program up the new parts with appropriate WCSs, stock, etc. When done, hide or suppress this second group of parts and turn on the first group - anything happen to the setups? Toolpaths?

It's not machining parts in an assembly where you designate fixture(s) that has caused us difficulties, its multiple different parts in their original assembly being kept in a single file along with all the CAM data that has been problematic. I may be misinterpreting the OP's remarks, but thought that was the gist of his later comments to Scott.

Confess, I haven't pursued this in depth so it may be easily accomplished; just haven't found the way of enlightenment yet.

Fred

[Steinwerks]

Fred Siedenburg wrote:

Ok, good so far. Now insert two new and different parts into the assembly, adjust the vises as needed, etc. Don't remove the previous parts, just hide them or whatever. Now program up the new parts with appropriate WCSs, stock, etc. When done, hide or suppress this second group of parts and turn on the first group - anything happen to the setups? Toolpaths? It's not machining parts in an assembly where you designate fixture(s) that has caused us difficulties, its multiple different parts in their original assembly being kept in a single file along with all the CAM data that has been problematic. I may be misinterpreting the OP's remarks, but thought that was the gist of his later comments to Scott. Confess, I haven't pursued this in depth so it may be easily accomplished; just haven't found the way of enlightenment yet. Fred

Trying to follow your workflow in that scenario... are you trying to reuse fixturing or...?

I think I'd move fixturing around before trying to add parts to existing part/fixture assemblies. I have a specific project to store basic fixtures (subplate, vise models, softjaw blank, etc) that I can add to assemblies and break the associativity (on purpose).

I concede that I may simply be misunderstanding the purpose of your workflow though.

[scottmoyse]

I'm struggling to understand as well.

I would only have one assembly per component run on the machine. That would cover tombstone machining, or multiple setups for the same part. But not two or more completely different parts in the same assembly.

[fredsi]

Time to take a step back...

Say I've just designed an instrument or device that contains a dozen parts or so. The Fusion philosophy is that you can have all your data in a single file (or it seems so). Thus, I switch to the CAM environment, hide all but one of the parts and put setup, toolpaths, etc. on that one part. OK, first part programmed and all is fine.

Now, in the same file, turn off visibility of first part, make a second part visible and put setup, paths and so forth on the second part. In my experience, if I later switch back to the first part to make changes, the setup, stock and paths are 'corrupted'.

We're talking about two versions of 'assembly' - one is working in an assembly of parts trying to keep all the design, CAM, simulation, and other data in one file versus an assembly of a part to machine and other items that are used for fixtures.

I got the impression, maybe wrongly, that the OP was being successful working with an individual part but was having trouble containing the CAM data inside the assembly for the complete device.

Apologies if I caused a lot of confusion...just talented that way  🙂

Fred

[daniel_lyall]

the same thing can happen in single part files, it is in part something to do with how it is saved you have to do it a certain way otherwise when you go back to that file the tool paths need regend