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Document stuck in "Loading Studio Data" after Circular Pattern timed out generating

john_hackingtonjohn_hackington Member Posts: 41 ✭✭
edited February 10 in Community Support
Hi everyone,

My Document is currently stuck in "Loading Studio Data" when I open it, after one of my Circular Face Patterns timed out during generation.

I've tried to use Versions to go back to an earlier state and try again, but I repeatedly run into this problem.

Do note that the Circular Face Pattern could be generated properly with the default 4 iterations, but gets stuck when I increase the iteration to 54.

The document is here:
https://cad.onshape.com/documents/e3a279a3a61f9eb98e166e1d/w/968bf2f032f637f35846302a/e/49a0e4e7ddd04ec75a83692e

Best Answers

  • john_hackingtonjohn_hackington Posts: 41 ✭✭
    Accepted Answer
    Onshape support has kindly looked into the issue and suggested an alternative way to generate my object using a surface approach:
    https://cad.onshape.com/documents/e3a279a3a61f9eb98e166e1d/w/968bf2f032f637f35846302a/e/e277222d67903f8731ffee57

    My previous method caused too much of a strain on the system and could only inevitably be timed out
  • philip_thomasphilip_thomas Posts: 1,081
    Accepted Answer
    Singularities are bad in Star Trek and CAD!

    Your solution to making square cuts on a hemispherical face was fine - a small offset and a profile tangent to the offset .
    A problem arises however on the last square - the one that spans both the hemispherical portion of the shuttlecock AND the straight portion.
    Because the straight line is offset, half of the square (to make matters worse) touches the face at its tangent - solid modellers dont like either.



    The solution is VERY simple - remove the singularity - edit EXTRUDE 1 and change the end condition to Symmetric (from blind) - i also for good measure also doubled the extrusion depth (from 1mm to 2 mm so that it would be 1mm in each direction).

    This took longer to type than to fix.

    I hope this helps :)

    https://cad.onshape.com/documents/dfdd5df5f2dd1710b56be229/w/27d75b00d95ec33893debc06/e/a752eb3fbd710be46803535a

    @john_hackington


    Philip Thomas - Onshape
  • john_hackingtonjohn_hackington Posts: 41 ✭✭
    edited February 22 Accepted Answer
    Hi Philip, thanks for the help! Sorry for the late response, I was away overseas for a few days.

    I've tried to implement your suggestion of using the Symmetric condition for Extrude 1, but it appears that it still didn't solve the problem of the last Circular Pattern not being able to generate to completion:
    https://cad.onshape.com/documents/e3a279a3a61f9eb98e166e1d/w/968bf2f032f637f35846302a/e/49a0e4e7ddd04ec75a83692e

    I do see your example document though, and it displayed successfully. I then made a copy of your document and am also able to successfully see the final product in that copy.

    As noted, I could generate 4 iterations of the Circular Pattern, but it became stuck when I increased the number to 54. I suspect that the hurdle here could be that the hardware on my client side somehow could not support the generation of the Circular Pattern before timeout. However, if the Pattern was already successfully generated, I would then have no issue seeing it. This is my hypothesis based on what I've observed so far.

    Still thanks again for your help and time taken to help me look into this! :smile:

    philip_thomas

Answers

  • john_hackingtonjohn_hackington Member Posts: 41 ✭✭
    Accepted Answer
    Onshape support has kindly looked into the issue and suggested an alternative way to generate my object using a surface approach:
    https://cad.onshape.com/documents/e3a279a3a61f9eb98e166e1d/w/968bf2f032f637f35846302a/e/e277222d67903f8731ffee57

    My previous method caused too much of a strain on the system and could only inevitably be timed out
  • philip_thomasphilip_thomas Member, Onshape Employees, Developers Posts: 1,081
    Before you do that - you might want to know how easy it is to fix! :)
    It took me 5 mins to find the problem and 15 seconds to fix.


    Philip Thomas - Onshape
  • philip_thomasphilip_thomas Member, Onshape Employees, Developers Posts: 1,081
    Accepted Answer
    Singularities are bad in Star Trek and CAD!

    Your solution to making square cuts on a hemispherical face was fine - a small offset and a profile tangent to the offset .
    A problem arises however on the last square - the one that spans both the hemispherical portion of the shuttlecock AND the straight portion.
    Because the straight line is offset, half of the square (to make matters worse) touches the face at its tangent - solid modellers dont like either.



    The solution is VERY simple - remove the singularity - edit EXTRUDE 1 and change the end condition to Symmetric (from blind) - i also for good measure also doubled the extrusion depth (from 1mm to 2 mm so that it would be 1mm in each direction).

    This took longer to type than to fix.

    I hope this helps :)

    https://cad.onshape.com/documents/dfdd5df5f2dd1710b56be229/w/27d75b00d95ec33893debc06/e/a752eb3fbd710be46803535a

    @john_hackington


    Philip Thomas - Onshape
  • philip_thomasphilip_thomas Member, Onshape Employees, Developers Posts: 1,081
    Full regen - 49 seconds
    Philip Thomas - Onshape
  • john_hackingtonjohn_hackington Member Posts: 41 ✭✭
    edited February 22 Accepted Answer
    Hi Philip, thanks for the help! Sorry for the late response, I was away overseas for a few days.

    I've tried to implement your suggestion of using the Symmetric condition for Extrude 1, but it appears that it still didn't solve the problem of the last Circular Pattern not being able to generate to completion:
    https://cad.onshape.com/documents/e3a279a3a61f9eb98e166e1d/w/968bf2f032f637f35846302a/e/49a0e4e7ddd04ec75a83692e

    I do see your example document though, and it displayed successfully. I then made a copy of your document and am also able to successfully see the final product in that copy.

    As noted, I could generate 4 iterations of the Circular Pattern, but it became stuck when I increased the number to 54. I suspect that the hurdle here could be that the hardware on my client side somehow could not support the generation of the Circular Pattern before timeout. However, if the Pattern was already successfully generated, I would then have no issue seeing it. This is my hypothesis based on what I've observed so far.

    Still thanks again for your help and time taken to help me look into this! :smile:

    philip_thomas
  • Jake_RosenfeldJake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 941
    @john_hackington

    Your local hardware does not affect geometry regeneration times.  The only thing that should be affected by your local hardware is graphical performance (frame rate, responsiveness, etc.).

    Are you using the 'Feature pattern' option?  Notice that in @philip_thomas 's copy he has used 'Face pattern'.  It is much faster and does exactly what you need.
    Jake Rosenfeld - Modeling Team
  • john_hackingtonjohn_hackington Member Posts: 41 ✭✭
    @Jake_Rosenfeld

    Hi Jake, thanks for your input too. Yes, I'm using 'Face pattern', I selected all the 12x4 faces from the Extrude for the 54x circular pattern.
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