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Mirror feature does not work properly with sketches and configuration variables

oleksandr_slovakoleksandr_slovak Member Posts: 6
Hi!

There is a very annoying issue that breaks completely our workflow.
The mirror feature in the part studio does not work properly with sketches if a configuration variable was used in a sketch geometry.
When the first time created it does its job, but once I try to change the configuration - it fails.

1. Sometimes it just mirrors the default sketch ignoring changes of the configuration variable.
2. Sometimes it does crazy shifts like in the image below. There is a simple fully defined sketch with a center point rectangle parametrized by #a and #b. The sketch is mirrored with respect to the plane which is parallel to the sketch plane. With default config, two rectangles are the same and coincide when looking from the top.





But once I change config - it starts looking like this:




Dimensions are correct (sometimes not) but the center of the mirrored sketch is placed randomly.

https://cad.onshape.com/documents/5557cd846b03bea657c7c535/w/e0a4a3a9bd81ab729eca63ff/e/e485c2a6a8f46b5983eacd3b

In both situations, mirror guaranty does not hold anymore which is unacceptable for mechanical CAD, as far as I understand. I might be wrong, please correct me in such a case.

Does anybody, except me, experience similar behavior?
Is there a way to work around it?

Many thanks!

Comments

  • Evan_ReeseEvan_Reese Member Posts: 918 PRO
    This is a strange one. I did reproduce it, and look for workarounds and I'm ready to call it a bug. As a workflow thing, can you get away with using a linear pattern (feature pattern) instead? it seems to hold up to change. It's not as simple as mirroring about a plane since you'll have to know what distance to move it. An even hackier workaround is to use your sketch to create a surface (Offset tool set to 0 is good for this), then mirror the surface body.

    Evan Reese / Principal and Industrial Designer with Ovyl
    Website: ovyl.io
    Instagram: @evan.reese.designs
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,639
    When patterning sketches, we must remove external constraints.  As an example of why this is important, if you were to "linear pattern" your sketch to the right, you would not expect that centerpoint to stay affixed to the origin.

    It seems that in this case removing the constraint is causing the sketch to move undesirably.  Could you try removing the external coincident constraint between the origin and the centerpoint of the rectangle (if you hover over the centerpoint it is the constraint that looks blue instead of grey, blue meaning "constrained to something outside the sketch") and replace it with a "fix" constraint instead?
    Jake Rosenfeld - Modeling Team
  • dirk_van_der_vaartdirk_van_der_vaart Member Posts: 110 ✭✭✭
    Here's a workaround, the rectangle not centered on the origin, but with a corner on the origin.
    https://cad.onshape.com/documents/0a8bce7c901ee33d26fcea8b/w/024b2f0fd3343771763a4155/e/3a49ef413d4c7243fc0922cd

  • oleksandr_slovakoleksandr_slovak Member Posts: 6
    When patterning sketches, we must remove external constraints.
    Hi, Jake! Thank you for the suggestion!
    I do partially agree with you, all the external constraints must be removed.
    But the new, "mirror" constraint, has to be added. It perfectly and intuitively works inside the sketch by mirroring geometry with external references. You can find a simple example here. There is a circle, with external constraint (Origin) which is mirrored wrt some line. Obviously, there is no "coincide with origin" constraint at the center point of the new circle, but there is a new mirror constraint added to all three parties: circles and line.

    How this example is fundamentally different from the 3d case with the plane?



    >> Could you try removing the external coincident constraint between the origin and the centerpoint of the rectangle

    That works, but it is obviously not practical and significantly restricts the functionality of the sketch.

    Best regards,
    Oleksandr Slovak

  • oleksandr_slovakoleksandr_slovak Member Posts: 6
    As a workflow thing, can you get away with using a linear pattern (feature pattern) instead? it seems to hold up to change. It's not as simple as mirroring about a plane since you'll have to know what distance to move it. An even hackier workaround is to use your sketch to create a surface (Offset tool set to 0 is good for this), then mirror the surface body.

    Hi, Evan! Many thanks for the suggestion!

    The linear pattern indeed works for some cases. You must know distance and direction.
    But it does not work for the case when the mirror plane is not parallel to the sketch plane.

    The surface trick does not work as it does not preserve all the geometry from the original sketch.

    Best regards,
    Oleksandr Slovak

  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,639
    When patterning sketches, we must remove external constraints.
    Hi, Jake! Thank you for the suggestion!
    I do partially agree with you, all the external constraints must be removed.
    But the new, "mirror" constraint, has to be added. It perfectly and intuitively works inside the sketch by mirroring geometry with external references. You can find a simple example here. There is a circle, with external constraint (Origin) which is mirrored wrt some line. Obviously, there is no "coincide with origin" constraint at the center point of the new circle, but there is a new mirror constraint added to all three parties: circles and line.

    How this example is fundamentally different from the 3d case with the plane?



    >> Could you try removing the external coincident constraint between the origin and the centerpoint of the rectangle

    That works, but it is obviously not practical and significantly restricts the functionality of the sketch.

    Best regards,
    Oleksandr Slovak

    The functionality of the mirror constraint is to mirror planar entities across a line within the same sketch.  It does not have the ability to mirror entities from another plane across 3d space onto a different sketch plane.  The situations are different because constraints are a function of a single sketch, that allow that sketch to solve within itself.  When you are mirroring the entire sketch across 3d space, we now have two sketches, and then need to solve independently.  There is no magic "mirror constraint" to apply, because the two sketches, on two different sketch planes, in two different features, are not solved as one.

    I agree though it is clear that this case is not working as intended, and we are discussing a more robust solution internally.


    Jake Rosenfeld - Modeling Team
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,639
    For a bit of additional context:

    You may be asking "Well why do you even solve the second sketch, giving it the opportunity to look different once the external constraints are removed?? We already know what it looks like, just make a mirrored copy of that!"

    That's basically the gist of the solution we are discussing :) 
    Jake Rosenfeld - Modeling Team
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