Emboss: Sketch profiles are not coplanar

[Anonymous]

Hi there,

I'm encountering a strange error I'm hoping someone can help whether is a strange bug or something I'm missing.

I have a curved surface that I want to emboss some text (imported as .SVG). At first this worked perfectly fine (see "Emboss working.f3d"). However, I wanted to scale down my text a bit. I used the scale command in the sketch workspace to scale it down. After doing so, when trying to emboss the "U" letter it gives me the error "Sketch profiles are not coplanar. Deselect sketch profiles that are not on the same plane." Even when selecting only the "U" letter (only one sketch profile selected, it still says that multiple are selected and that they are not coplanar. Model "Emboss failure.f3d" shows this error.

Has anyone experienced this before? I assume it must be something with the sketch profile of that specific letter that Fusion has issues with, but I can't figure out what's wrong with it.

Also if someone could confirm that the "U" letter cannot be embossed using the emboss command it would be very helpful.

Thanks

Alfred

EDIT: I tried deleting the old text sketch geometry and reinserting the .svg. Scaled it to correct size and now the "U" embosses fine. Still interested in seeing why it doesn't work in the attached files

[jeff_strater]

yes, that looks like a bug.  Can't see anything wrong with the sketch or design here, but will continue to investigate.  My suspicion is that the error message is misleading, and that some other error is happening.  The fact that the preview succeeds makes me think there is some other underlying cause that is not that the profiles are not co-planar

[jeff_strater]

it looks like the "U" is the problem profile:

[Anonymous]

Yes I also found that the "U" was the issue. I tried inspecting it but didn't see anything immediately wrong with it. I also concluded that the error message was misleading, but without knowing the actual error I find it a difficult to diagnose what's wrong with the sketch

[jeff_strater]

even more so, it's the lower curve in the U.  I tried deleting and re-adding a curve there, but that still seems to have the same problem.

[jeff_strater]

I created bug FUS-87340 to investigate this.  Thank you for reporting it.  Very strange...

[Anonymous]

Hi Jeff,

I tried reproducing your method and it seems to work but somewhat randomly. First time it didn't allow me to emboss, but as I tried clicking some of the other letters it worked. As soon a sketch line is placed around the position where you put it, the whole thing allows to be embossed it seems. Very strange.

Should I accept the solution or wait until a fix has been made?

[TrippyLighting]

I believe Fusion 360 encounters a problem intersecting the sketch curves with the curved surface.

Extruding the text to combine with a flat surface works fine and is a stable workaround:

[TrippyLighting]

@jeff_strater I believe this isn't per-se a bug, but a near tangency problem.

The sketch is an imported SVG and all the imported curves are 3-degree splines that seem to be tangent.

I modified the bottom curves of the U in that I made the construction lines that form the spline control cage,

 colinear with the construction lines of adjacent  splines,. Then it works fine.

[Anonymous]

As I mentioned in the original post, the SVG worked fine at first, but as I scaled it the "U" suddenly messed up. I created a new part where I imported the exact same SVG and resized it the exact the same and didn't get any issues. So somewhere in Fusion's handling of the SVG a bug occurs

[TrippyLighting]

I understand what you wrote in your initial post. It does not change what I've observed.

CAD software works internally with all sort of tolerances in order to make sure tangencies and other conditions are maintained.

The problem with imported geometry is that it does not have to adhere to these tolerances and the problem can be exasperated, for example when modifying the sketch , e.g. scaling it, before 3D geometry is created from it.

If you apply proper constraints to the sketch it is unlikely that you run into these problems, as one of the functions of these constraints is is to make sure the sketch geometry will maintain these internal tolerances. 

I understand that this is often not practical, but that explains the likely root cause and one way to fix it.  

It happens only very rarely but sometimes  those internal tolerances can get adjusted adjusted in the code. 

A bug indicates that something is wrong with the code, but that might not be the case here.

As general guideline I never scale imported sketch geometry to avoid such situations. Most of the time that helps, but not always. I create 3D geometry from the original sketch and then I might scale that. 

[jeff_strater · Accepted solution]

yes, @Anonymous - I saw some of the same flakiness in when it would, and would not work with that U character.

"Should I accept the solution or wait until a fix has been made?" - that's kind of up to you.  It might take a while to diagnose and fix the problem, to be honest.

[bryn.parrott]

That is un-&^%&^% believable. This problem was known about back in 2021, and yet today I get the exact same error.

I create a solid brep cylindrical primitive object on a plane, and on the same plane I later create. a sketch, which contains some text along a path.
When I finish the sketch, and then select the "emboss" command, select first the text object, then the face of the cylinder, and select the "deboss" (indent) button, Fusion tells me that the text is not coplanar with the cylinder face.  This has cost me hours trying to work around it.
Why the heck can't it be fixed ?!!!

<!angry!>

[g-andresen]

Hi,

please start a new topic and share the file

günther

[bryn.parrott]

Nope, not going to do that.  The problem is well described, and its easy to replicate.  I got around the problem by extruding the text, then using the extruded text to cut the object needing to be debossed.  But its a work-around.  

[TrippyLighting]

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@bryn.parrott wrote:

Nope, not going to do that.  The problem is well described, and its easy to replicate.  

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Almost all of the folks who help here on the forum do this on a voluntary basis.

We don't have to do this and anything you as a user can do to help us help you, is appreciated.

[bryn.parrott]

Yeah sure, I understand that.  But the request is totally unreasonable, as it involves packing up a rather large file and somehow attaching it to a message here, when in fact the foregoing messages indicate the problem has been around for quite some time, and thus likely to be well known.  But somehow the actual answer never got posted.

Seems like the person that requested me to do that does so out of habit without thinking, its an easy way out to dismiss a question.  Seems to me that if thats the response, then just say nothing.

[TrippyLighting]

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@bryn.parrott wrote:

... But the request is totally unreasonable, as it involves packing up a rather large file and somehow attaching it to a message here ...

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And how could we possibly assess the complexity of your design without you posting it here on the forum?

Exporting a .f3z file and attaching it to the forum is rather simple ( you might have to zip it to attach it). 
That isn't an unreasonable request. Even complete beginners manage to do that.

If your full design is too complex, create a simpler one we can look at. If there is a bug, we can tag someone from Autodesk. They'll add the data to the ticket if the problem has already been posted and recorded as a bug.

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[bryn.parrott]

OK, I specially made this attached text file.  It contains just a disk shaped primitive cylinder, and a sketch with the debossed (ie inset) text curved on a path in Brush script font.  So, its really simple, and the model file contains nothing else.  The sketch was made on the planar surface of the cylinder. So there is no doubt at all that the sketch is indeed coplanar with the model surface.

The test model  bears some similarity to the real model, which I chose not to share because of its size and the fact it contains a lot of stuff not relevant to the issue at hand.

And yes, with this model the sole opened object on my Macbook Pro Max, which has only Google Chrome (this window) and Outlook running.  So it's not a resources issue.

I found that I was able to "deboss" the text by extruding the lettering and using that extruded model to cut into the surface of a disk using the combine command.  But the resulting model does not print well, as the slicer wants to surround the text with several walls that are visible on the model surface. This makes the text difficult to read, and it looks very odd.
So, I'd like to see what the inbuilt emboss tool can do, and how the text looks when printed.

In an effort to see whats going on. I edited my own copy of the file.  I deleted the original sketch, and made a new sketch on the face of the cylinder. This time I used "Arial Narrow" font. Upon saving the sketch, I found that it was possible to use the emboss command.  So I edited the sketch, selected the text, and opened "edit text".  I changed the font to "Brush Script".  I saved and closed the sketch.  Then cound I was no longer able to use the text to emboss the surface, I got the "not coplanar" error.  So, I make the theory that it something to do with the font used.  But the client requirement is to use the "handwriting" style of font, as this model is made as a replica of something that has handwritten engraving on it.  So the curvy font isn't negotiable.


Now, I am able to emboss text using Prusa Slicer, but PS does not have the facility to curve text along a path in the same way as Fusion.  So, this does not meet client requirements.

As I said in the original post, this issue has been around for several years, and it seems not to have been corrected.
Really, for software that uses the timed payment system that's completely unacceptable.

[jeff_strater]

"So, I make the theory that it something to do with the font used."

Your theory is correct.  We have no control over the quality of the font outline produced by various fonts.  In this case, the error message is misleading.  Has nothing to do with co-planar profiles.  It is just that the "x" here does not define a valid profile outline.  The other letters are fine.  You can tell this by "exploding" the text.  I can emboss those letters just fine:

using the "divide and conquer" method, I tracked it down to this section of the "x":

and further identified this line:

as the culprit.  Deleting that one and replacing it with a sketch line allowed the whole string to be embossed:

The repaired model is attached.