Sketch Projection doesn't seem to work properly with Parametric Design

[heinzm64XF3]

I'm using Fusion Version 2.0.8335, but I have also seen this Bug in previous Versions.

Is there a summary somewhere that lists some of the Bugs / issues when using Parametric Designs?

I encountered this Bug in a much more complex design, the following simple design is for illustration purposes only.

Everything works as expected until I reduce User Parameter "Length" by more than (Key_Offset * 2 - 1) in a single Parameter Edit.  For example, leaving "Key_Offset" at 20 and reducing "Length" by only 30 several times doesn't cause any issues.

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However, if I change User Parameter "Length" to 150, I end up with this:

Incidentally, if I leave "Key_Offset" at 20, and change "Length" from 200 to 160, the same thing happens, but then there is no way to recover (i.e. Design remains broken even if "Length" is changed back to 200).

Does anyone have any suggestions?

Thanks

[jhackney1972]

If you change your the location dimension, of the small block, from the center of the hole to the end of the bar, the error will not occur.  I do not think this is a complete solution because different designs required different dimensional solutions and if you have to guess the one that will always work, well that could be difficult.  I think the solver is looking at the parameter of the bar length to solve all other parameters.  Your model modified under a different name is attached.

[jeff_strater]

@heinzm64XF3 - thanks for sharing the design.  I know that these kinds of "dimension flipping" cases exist, and we are very interested in finding and fixing them, so I was happy to get a case that we can use.  However, so far, I have been unable to reproduce this behavior.  Am I doing something differently?

[jhackney1972]

@jeff_strater   In your Screencast you seem to be using MY modified model.  His model references the edge center of the block from the hole center, not the end of the part as mine does.

[jeff_strater]

d'oh....   I just scrolled through the page looking for attachments, and downloaded the first one I saw...  OK, I'll try again, this time with the original file!!!

[heinzm64XF3]

This change to Sketch_Offset_4 also fixes the problem, but the fix makes the Sketch look kind of messy.

Instead of just using a dimension, I added a vertical construction line coincident with the end of the projection line. Then instead of using a dimension I used Offset from the above mentioned line, like this:

Below is the much more complex design and it exclusively used Offset for all the offset dimensions. The reason for the parametric design was to allow making several parts like the one shown below but with different dimensions.

[jeff_strater]

now that I have the correct design, I can reproduce the problem.  Thank you for sharing the design, @heinzm64XF3 , I've created FUS-66011  to track this problem.