I've noticed that in some cases, creating an extrusion will create unneeded edges on what should be an uninterrupted face which looks ugly and get in the way of other ops. I've never had an issue until starting to work on a component with an origin in a strange position. I'm pretty certain the problem is related to origin positioning because rotating it so that the geometry was re-calculated aligned to its Y axis partially fixes the issue (see attachments). It also only happens when extruding sketch geometry - extruding a face directly without creating a sketch doesn't cause it. I've worked around it so far, but that can only get me so far. Any ideas for how to get extrudes to behave properly?
please share your model here. Cannot tell anything from just images. I doubt it has anything to do with the design being at an angle - I've never seen that before. Planes will merge as long as the sketch lines that produced them are colinear.
@TheCADWhisperer All my important geometry is fully constrained.
@g-andresen I can confirm it's not anti-aliasing - toggling it has no effect. The faces created by the pointless edge can also be extruded like any other face, so I'm thinking it's not just visual.
For reference, I'm trying to create an enclosure to fit between an existing tube-based chassis component. I didn't share the original model because I reference another component that I can't share, but I've replicated the exact same problem in a brand-new file (attached) that's close enough to the original situation.
While doing that, I've also run into another (possibly related?) issue where re-computing will cause a coincident constraint with a projected line to disappear. I've fixed the relative point in the "ProofOfConcept.Enclosure" sketch, but added a floating line on the other side of the line that will exhibit the same problem.
He is complaining about all the body edge lines. He wants to know why they show up. If he wants to get rid of them he can use Delete Face on the areas of concern.
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thanks for the design. I just looked at this one area:
The reason for those edges are these projected curves:
I suspect that these 3 lines are at a VERY small angle from each other - even too small for Measure to see. And so, the resulting planes are not quite coplanar, and so are not merged. If you go back in and replace these with one line, the faces are merged.
@jhackney1972 That works! Seems like a workaround though - I'd prefer not to have face deletions littering my timeline.
@jeff_strater Interesting... Why don't those lines project colinearly? Those points are coplanar, so I'd assume they'd form a line... Either way, the extrude still causes a horizontal seam that breaks what should be an unbroken face.
I've done a bit more experimenting, and replicating the issue is pretty simple. I've included a screencast. These are the steps:
1) Create a component
2) Perform an "unusual" rotational transformation on it
3) Capture position
4) Create a sketch from the component's origin and extrude a body
5) Create a sketch on any (?) face of the new body and project the face.
Note that this only happens when the sketch is created in the already rotated position. Creating the sketch and geometry before rotating works as expected. Furthermore, creating another sketch from the origin and extruding it - even when rotated - won't create the seams (See the screencast: https://knowledge.autodesk.com/community/screencast/a9ab89b2-1ca4-486e-adf6-efdac23c7ecb ).
It seems that the common factor in my experiments is the creation of the sketch on a body face. If I may suggest a cause, is it possible there's some numerical precision error when calculating a face's normal to orient the sketch?
Having a similar issue recently, using delete face to delete a face that shouldn't exist in the first place and just clutters up the timeline and can potentially screw up parametric changes.
thanks for the design. I just looked at this one area:
The reason for those edges are these projected curves:
I suspect that these 3 lines are at a VERY small angle from each other - even too small for Measure to see. And so, the resulting planes are not quite coplanar, and so are not merged. If you go back in and replace these with one line, the faces are merged.
@jeff_strater There's another post here with the same problem but in a very simple sketch. Pretty sure the faces should merge, I've had designs where I've needed collinear segments like this and produce a single surface. Might be worth checking out in case something's regressed.
Thanks Mark
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Hi all! Any progress on this? I'm starting a new model in a similar situation and I wanted to check if this was on its way to being resolved. I've investigated some more in the meantime.
I decided created a couple of simple models to inspect generated STEP files for precision errors. The test model is as simple as it gets: A 1x1mm cube with a 1mm extrusion in +Z. One is created transformed, the other is left with the origin in the default position. The below photos should give you all the info you need.
The generated STEP for the untransformed model is as expected - a lot of nice, round numbers and unit vectors:
The transformed model's STEP is a different story, and just screams floating-point shenanigans to me. Now, I'm no expert on STEP, but when I see numbers with "E-17" and "E-8" at the end, the programmer in me starts to get a little suspicious:
(On a side note, it's interesting that the errors are either at around E-16 or E-7, which are very roughly the max precision of doubles and floats, respectively. )
Even a "simple" 45* rotated component displays some level of error - just not enough to trigger an edge creation on extrude, I'd assume:
@jeff_strater Of course I could be wrong, but this seems like more than enough to confirm unintended behavior. I think it's pretty clear that something floating-point related is going wrong and introducing tiny (almost epsilon level) errors into rotated-origin components.
It'd be nice to get this resolved quickly, because this seems like one of those errors that's very difficult (impossible?) to fix after a model is created.
It'd be nice to get this resolved quickly, because this seems like one of those errors that's very difficult (impossible?) to fix after a model is created.
I cannot say that I encounter such problems when I create models.
I use Fusion 360 every day in a professional environment for professional work and have done that in general with CAD software for over 30 years, 20+ of those in 3D.
Perhaps your modeling techniques might have something to do with this ?
"It'd be nice to get this resolved quickly, because this seems like one of those errors that's very difficult (impossible?) to fix after a model is created."
I can pretty confidently say that this will not be resolved quickly. It is possible that there are bugs here, but this, to me, feels like one of those that will take a lot of study to even determine the root cause, and if a fix is identified, it will take a long time to validate that it works. FWIW, I don't believe that this is a common problem, I don't believe that I have ever seen it reported before, but I don't see every single report.
I might quibble with the "impossible to fix". I believe there are fixes here, almost always involving re-sketching lines so they are not segmented. It may be unpleasant to have to fix them, but don't believe it is ever impossible.
@jeff_strater Ok, thanks! I appreciate the reply! You're right about it not being common - it surprised me to find no one mentioning it. It seems like something you'd run into pretty quickly on a moderately sized assembly if you were positioning your origins reasonably... Also, just to clarify, the segments aren't the cause - A seam occurs with continuous lines too (https://knowledge.autodesk.com/community/screencast/76966c60-0891-4749-8778-73efb859a06b)
@TrippyLighting I've narrowed the issue to sketching on a body face within a rotated component, then extruding. Unless working inside rotated components isn't intended in Fusion, there isn't much technique involved IFAIK. Here's a link to a screencast demonstrating the exact steps to create the problem - If you see anything obvious I'm missing please let me know! (https://knowledge.autodesk.com/community/screencast/76966c60-0891-4749-8778-73efb859a06b)
Unless there are any more developments or comments, I'll leave it here. Thanks everyone!
Don't suppose this is another bug related to having the Product Design add in active. Can you share your design?
Edit 2. OK, I can reproduce this. Seems like it only happens if the component is rotated in all 3 planes. Even a problem with fairly simple whole number transformations and using joint origins. @BertTheAvenger You might want to look at using joint and joint origins as capture positions can lead to other problems, although not what's causing the problem here. See attached file for example of problem and use of joint origins.
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I looked at the original design posted. The edges with the green arrows can be avoided, by re-projecting.
The ones with the red arrows cannot be avoided with the current sequence of operations, albeit a change in operations that create the same geometry would be able to achieve that. But obviously, that isn't possible in every scenario.
