"Missing Profiles" On Revolve After Changing Sketch Parameter

[therealsamchaney]

I am having an issue with my model where Fusion 360 gives a "missing profiles" error for a revolve feature when I change the profile sketch using a parameter. The sketch is just an ellipse and the parameter I'm modifying just changes the width and height of the ellipse being used for the revolve feature. Changing these parameters does not delete the profile I had selected so I'm not sure why it causes this error. Re-selecting the profile fixes the error and all subsequent errors down the timeline. However, I really need to be able to change this parameter dynamically from the Parameters menu as this model will be used by others who are not savvy in fixing Fusion 360 errors.

The parameter in question is ConcaveIntensity and the sketch it affects is called Sketch Ellipse

If anyone, especially a developer could tell me how Fusion 360 keeps track of sketch profiles when they are modified by parameters that would be very valuable. It seems for some reason after changing the size of the ellipse, Fusion can no longer recognize the profile as the same entity.

Any help would be greatly appreciated. Screen cast is attached and I will upload my model to the post.

Thanks!
-Alterius

[HughesTooling · Accepted solution]

Definitely something odd there. I experimented redrawing the ellipse because I think you've deleted one of the original construction lines used to constrain the ellipse and you have 2 horizontal lines where the rotation axis is but that didn't the new ellipse was no more reliable.

What I did find works is draw another line across the ellipse like below. Sketch also becomes fully constrained with the extra line.

Even this is a bit screwy because when you first draw the line the end points do not generate coincident constraint and need to be added before adding the dimension for the offset from the centre line. If you add the dimension first you can't add the coincident constraints after! I tried this in a new sketch in a new design and had no problems so something real odd! @jeff_strater  Can you take a look at the revolve and odd sketch behaviour? File's attached.

Thanks Mark

[davebYYPCU]

From the video I figure, sketch not defined, from the file, I found, 

Your sketch is not fully defined.

Your horizontal dimension is tied to one line.  One is a construction line.   

Revolve requires a normal axis line, Just read Marks post so adding a pic, 

Reduce the line count to one, when you constrain the ellipse to become black, I can't break the parameter updates, in a range of 3 to 6, scratch that 6 is failing now.

Might help...

[HughesTooling]

@davebYYPCU  Like I said above I redrew the ellipse so it has its original constructions lines only and it still fails. Odd thing is it seems to only fail on odd number, seems to fail reliably with 5, 7 and 9. File's attached. My other file in my first post seems pretty reliable with the extra line.

Mark

[davebYYPCU]

Will leave it to Jeff, seems that I took the screenshot, (no further edits was working fine) and now the file is unreliable.

Might help...

[jeff_strater]

I'll take a look at this.  My theory is that this is just a "profile tracking" issue.  The profile in question is bounded by 2 curves - the ellipse, and the horizontal line in the middle.  But, that description is ambiguous - it can describe either the top or bottom half of the ellipse, and I wonder whether that is confusing the algorithm somehow...

[therealsamchaney]

@HughesTooling, thanks so much for taking the time to find this solution. I have re-drawn this ellipse before to try to fix the issue and I may have accidentally removed one of the construction lines this time, but I was having the same issue even when the sketch was fully defined as you found.

Adding the extra horizontal line is a good idea, I'm not sure I understand why it works though. I would think that line would be redundant if the height and width of the ellipse are already constrained, but Fusion 360 is mysterious sometimes. Hopefully Jeff can shed some light on this.

Anyway I have marked your answer as an accepted solution while we wait for Jeff to get back with some more insight.

Thanks!
-Alterius

[therealsamchaney]

Thank you very much @jeff_strater. I would be very interested to know how Fusion 360 achieves this "profile tracking". I thought Fusion would have some metadata about the center line and be able to tell which "side" of the line the selected profile half sits on, but without that information you're right that there would be 2 possible solutions for that profile, even if the sketch is fully constrained.

I have also found that if I change this parameter to some more extreme values, the entire ellipse will invert and flip over because there are two "stable" and constrained states it could be, one above the top of the key surface as it is now and one below. I was hoping there was something like a "stay above/below sketch line" constraint but there isn't. I should be able to get the same affect by projecting another line from lower down on the model and adding a dimension from the center line to that projected line. Still, I think this could be a valuable constraint and can think of many situations where it would be useful, like having a circle or polygon constrained above a projected or construction line. In any of these situations there would be 2 possible solutions for a constrained sketch. But if Fusion doesn't have any way of knowing which side of a line some entity is on this would not be possible.

Alternately, an elliptical arc would be perfect for my scenario, but there are only circular arcs available which will not work in this case which is why I'm just using an ellipse and a center line.

Anyway, I appreciate you digging into this and look forward to hearing what you find. 

Thanks!
-Alterius

[therealsamchaney]

@HughesTooling I tried implementing your extra offset line approach but I was still getting the same error.

I then modified the plane that the ellipse sketch was on so it went through the top opposite corners of the keycap model. This simplifies the sketch as I no longer need to control a vertical distance dimension for the ellipse and instead can just have it constrained to be coincident with the projected points from the corners. I only needed to make sure that the resulting concave didn't leave any of the top surface untouched and this achieves that goal more elegantly. However this also means that the revolve axis must now be the vertical line and your offset line approach is no longer possible.

This still didn't fix the issue though and I still get the "missing profiles" error when changing the ellipse dimensions. I did find that with this new arrangement, only changing the height causes the error. Changing the ellipse width does not cause the error. This leads me to believe that Fusion 360 is using the vertical positioning of the sketch to do the profile tracking. I would have thought the profile tracking would be independent of the position of the profile but that doesn't appear to be the case. I've attached the newer version of my model.

[HughesTooling]

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@therealsamchaney wrote:

@HughesTooling I tried implementing your extra offset line approach but I was still getting the same error.

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Did you add the coincident constraint after drawing the line? There is a problem with the sketcher where it's not creating the coincident constraints automatically.

See screencast, after adding the constraints I try several sizes without any problems.

Mark

[therealsamchaney]

Since I switched to revolving the ellipse about the vertical centerline, I can't use the exact same solution you provided. However, I did try adding an arbitrary vertical line on the opposite side of the profile that I'm using and constraining it fully (the coincident constraints are working normally for me, not sure why you had to add them manually), and this seems to have made it at least more stable than it was. Strangely, the first time I changed the ConcaveIntensity value to 12 it broke, but then I did it again and it didn't break. It seems to be mostly stable between 1 and 10 so its definitely an improvement, thank you. I'm still not really sure why this helped, as I'm just adding an arbitrary line on the unused profile in the sketch. Perhaps Fusion can now distinguish between the two profiles where before it was ambiguous?

@jeff_strater have you had any luck in your investigations? It seems like this is a corner case where Fusion doesn't know exactly how to keep track of the sketch profile.

Thanks!

-Sam