Generated parallel toolpath is cutting into the part itself?

[jw.hendy]

I recently made a 4-sided case and used a new technique for the mitered corners. I've used the 90-deg v-bit trick before, but I don't like the variability in re-zeroing after a tool change, and I wondered if I could get away with a parallel toolpath using the 1/4in bit used for everything else. It worked great! ...

...except it cut into my part in the surrounding area during the operation. Like all things I suspected myself, but I just looked more closely before I go to make a second, and it looks to be real in the generated toolpath.

Can anyone illuminate on why it would generate a path that cuts into the final model?

Here's the part for reference. I will note that this was made in SolidWorks and imported to Fusion. Not sure if that matters or not.

Here is the parallel operation cutting my miter:

I adaptive clear to rough everything out, then run the miter parallel toolpath, and then clean up the "shelf" and walls with this 2d conI also have this contour cleaning up the "shelf" and protruding walls after this miter operation:

Now I'm orienting to the front view (looking at the miter/shelf from the side) and zooming way in:

Here's the contour, which makes that shelf disappear behind the toolpath lines:

Now here's that parallel path highlighted, which is clearly below the shelf as I experienced in real life:

Here's the geometry tab, which I'd think is the most relevant?

I thought it might have been the use of touch surfaces, but here's with turning them off. In this view from the side, you can see the toolpath line disappear right into the part!

Any other information that would be helpful for me to provide? All other cuts/passes seem correct, and in checking other dimensions, things seem well within what I'd expect. My walls should be 4.37mm and I get 4.34-4.37mm with my caliper away from the ends, but 4.19-4.22mm where the parallel path hit.

I appreciate any suggestions, and again am happy to provide other details/settings that would be needed to troubleshoot further. I've never had this happen so I'm not sure how to diagnose!

[daniel_lyall]

To check for deflection stick a dti against an axis and pull and push that axis a cutter can put more forces into a cut than you can buy pull and pushing an axis, then you need to find why it is deflecting most times with hobby machines like yours its the frame its self or the wheels not being tight enough.

[jw.hendy]

And for heaven's sake man, I did ask:

"""
Thanks for the idea on the extra surface. Do you have a quick shot of the model, or how you added it? I've not used a "dummy surface," so I'm curious if this is a sketch or full on e.g. extrude to pad the surfaces. And then does one have to export the miter toolpath, then suppress the feature, then re-export the other toolpaths? Cool technique.
"""

Again, a workaround is not an explanation. We indeed solved "how does one work around Fusion?," which is required either with a ball or a flat end mill. You've been harping away on how a ball end magically solves this... but it doesn't. The fundamental flaw in how Fusion is computing the path for this part is still present, it's just less obvious.

Perhaps this was purely suited for a bug report. I thought I was essentially doing that, but filing it in the manufacturing category. Turns out I messed up. Now it's fixed.

I, too, long ago had a satisfactory solution. I made another case this weekend with no issues, and with no ball end mills required.

[Anonymous]

I saw your issue from the start, I solved it in two ways but then we got into..... "why does Fusion!?"

Because you used odd tool choice to do something, there are consequences that need to be dealt with, that's not workaround, that is simply counteracting result of bad choice, one that would not be within preferred choice of tool for type of operation but still works within narrow margin of side effects that need attention.

Fusion has more than one way to do nearly anything, only limited by bugs, lock of full development, user's skills and imagination.

Here is one way again, flat end mill, tool overlaps edges of model by 1 mm, tool does not go below model bottom, absolutely no intrusion into unwanted surfaces as you can see, Fusion rocks. 😎

We just made it to third page, there is nothing productive coming out of this and I think there is no need to go on.

[jw.hendy]

Cool. I'm sure it's significant, particularly in z. I updated x/y belts to steel core, but z has a thinner belt so I left it. Is DTI "dial [tramming?] indicator"?

[jw.hendy]

That picture could be a sail on a sailboat for all I know. Means nothing. 😛

For realz, good to know, but you still didn't explain it, nor when I asked the last time. And a ball end mill wouldn't solve anything. By accident it would handle the oddity in the software of machining the surrounding part (because it doesn't go as far so it's less noticeable), but I'd have a janky miter at the tip or swiss cheese for wasteboard. And a tool change.

[Anonymous]

Read that post with picture (of sail 😋) again so I don't have to repeat myself again and again.

You'll have to look elsewhere for details regarding dummy surface, remember?,.... my solutions don't work for you.

I have no desire to continue this, it is becoming annoying and pointless waste of my time.

[jw.hendy]

I ask, you don't tell. Later, you complain I don't ask. Ask what I mean and seem confused, I explain (again). Then you don't read because I'm repeating [what you asked me to tell you].

I can only wonder what you're like in real life. I'm feeling grateful I'll never have to find out.

[Fabbunny69 · Accepted solution]

Blimey far to many egos bouncing around in here I really don't think the rhetoric is at all helpful to answering @jw.hendy  initial question 😴

Am I allowed to have a go without inviting some sort of challenge?

Along with studying the Z positions whilst running the simulation and also cross referencing the Z positions output to the ISO program I can see that Fusion is doing everything correctly, all Z heights in the problem areas are within 3 microns, ie. 4.375mm on the step and 12.500mm at the top surface. Fusion is not to blame.

In your file when  I run the second parallel toolpath I can see(as in your second picture) that the tool runs over onto the top and stepped surfaces as you have indicated where the problem is. 

Could it be possible that it is merely a matter of the tool running over those areas many more times than the full length areas? Taking a few more microns with every .5mm stepover?  We would even see a mismatch here on metal but I imagine it could be worse on wood. On aluminum with a precision ground sharp tool generating as little heat as possible we would probably get the minimal show.

[daniel_lyall]

DTI = Dial test indicator something like this https://www.mscdirect.com/product/details/44528008 these are the things you spend lots of $$ on.

At this stage @Fabbunny69 it could be ever the machine or fusion, so it is a bit hard to answer without the op running some tests.

[Anonymous]

Awesome, I am a terrible person,  ...... are we now officially divorced ?🤕🙄😊😇

[seth.madore]

Knock it off. This is a place of advice and assistance, leave the egos at the door. If this continues I'm going to get this thread locked.

[jw.hendy]

Thanks for taking a look. Very interesting find that the difference was so minimal. In the Support forum (where I transitioned to focus on whether or not this was a bug vs. how flat vs. ball end are best for this), someone observed the same and suggested it might have been the use of both ways in the machining option.

I used a downcut for this, so perhaps what you're saying and the other gentleman's observation align: more passes in that area + direction change/bit being pulled down and I end up eating away a bit each time. I've not seen anything like that before, and while it's nothing catastrophic by any means, it's sufficient to be ugly and perplexed me so I asked.

[jw.hendy]

Thanks for explaining. The finding it's 0.003mm is interesting indeed. I could try this with an upcut or only machining in climb and see if it's indeed the direction change and downcut getting pulled into the piece?

[daniel_lyall]

Yes definitely try that also look into the Z-axis touch plate it is a time saver and makes re-zeroing after tool changes simple as mud.

[Fabbunny69]

@jw.hendy 

I projected my own machining boundaries on to a sketch and then moved them the by the radius of the tool length ways along the model and added .5mm to the width ways profile and this seems to be giving a nice result.

Previously when trying to achieve something a little out the ordinary tooling wise I have had to created my own boundaries to get the result I was after.  A little bit more programming work involved but this has even been the case with the other CAM packages I have used.

 

[jw.hendy]

Ah, very interesting and thanks for clarifying and attaching the part. I noticed the same approach on @daniel_lyall 's model and wasn't sure how he did it. I figured I just didn't know how to e.g. select specific edges or maybe that miter face in the boundary? The selection dialog for boundaries always wants to select the full perimeter when I hover.

Daniel, did you use this technique as well? I didn't see a sketch in your model Design tab, but you were able to use a very similar geometry to @Fabbunny69 :

[HughesTooling]

Here's a quick screencast showing how to create extended surfaces so you can over machine the angled faces. Same as I suggested in the other thread. Note, it's a good idea to reset the extend surface tool to zero after the first selection to make it easier to select the other edges.

Mark

[daniel_lyall]

I used what is here to get the contour of the toolpath See this video for selecting toolpaths https://www.youtube.com/watch?v=ATs4rsI_TPc

[Anonymous]

I was gonna pass but could not resist, so..... the screencast does what it does, creates dummy surface to be used as geometry to cut, you filled the vacuum I deliberately left behind for operant reasons and I have no issues with that.

But, for wider audience, I wanna point out two things about the way you used option in this particular case.

1- Extending  bottom edges is not necessary because of flat end mill being used, OP had an issue with using ball end mill because it would cut into his spoil board, very upsetting part of "wrong vs right choice of tool" as we have seen.

2 - The main reason for creating offset surface is to isolate main body that caused odd tool path or "tool eating the model" under certain choices made in operation.

Therefore, when selecting model in operation, in this particular case, you wanna unselect option to use setup model which results in only machining duplicated surface.

Operantly, because you extended top edge of new surface, tool still avoids "eating the main model" even though you left setup model selected in operation.

Devil is always in the detail, isn't it ? 😁

[Fabbunny69]

@jw.hendy  No problem. All I did was project the face of your MITRE on to a new sketch plane (See Pic) then the outer profile will show as purple in color. After that you need to delete all constraints to change it to blue lines that you can then manipulate to achieve whatever boundary you are after.

If some body has advise of how to project a profile without constraints please share!

Sorry for short reply, apprentice has snapped drive belt on our big mill 😞