Can't Change Sketch Dimension

JDMather · ‎01-13-2017

I can drag the line to any length and add a dimension, but then can't edit that dimension?

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cekuhnen · ‎01-13-2017

@JDMather

I highly suspect that this is part of the sketch engine - maybe a bug or misbehavior in the solver.

The sketch should work - look below

From time to time happened in my class yesterday - it can happen that dimensioning just refuses. What worked was

deleting the sketch part and redoing it and dimensioning it. again - this time with success.

Claas Kuhnen

Faculty Industrial Design – Wayne State Universit

Chair Interior Design – Wayne State University

Owner studioKuhnen – product : interface : design

HughesTooling · ‎01-13-2017

Sometimes the DOF colour status makes things like this fail, can you try turning it off in your preferences and see if it's still a problem.

Mark

Mark Hughes
Owner, Hughes Tooling
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jeff_strater · ‎01-13-2017

Hi @JDMather,

I have not yet been able to reproduce this. Can you share the design, if you still have it, in that bad state?

thanks,

Jeff

Jeff Strater
Engineering Director

JDMather · ‎01-14-2017

Edit Sketch1 and delete the 31mm dimension on the left side.

If you dimension from the symmetrical point illustrated in the video on the right side to the corner of the rectangle and then attempt to edit the dimension - I get an error.

If I dimension from endpoint to endpoint of the angled line - I do not get an error.

If I dimension selecting only the angled line - I do not get an error.

If I dimension the symmetrical line on other side of the sketch endpoint to rectangle corner - I do not get an error.

If I turn off constrained sketch color (which of course I would not do this, just as I would not turn off my airbags or anti-lock brakes) - I do not get an error.

So the issue is between those two particular points.

I run into similar issues with nearly every part that I attempt to model in Fusion.

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jeff_strater · ‎01-15-2017

Thanks for the design, @JDMather, I've filed bug FUS-29943 to track it internally.

The interesting thing about this case is that if I create the dimension differently, (as a vertical dimension to the ends of the angled line), it is fine:

Jeff

Jeff Strater
Engineering Director

jms30 · ‎02-11-2022

This was just happening with me. I know how to fix it. One of the points included in the dimension is fixed, you can know which one by dragging the point ( point A) and not being able to. After locating which point is pivoted, redraw the line (line AB) but starting from B to A to make point A flexible to move.

maccleery · ‎08-09-2022

I also ran into this problem and had to revert to an earlier saved version in order to continue the design. Please see attached "sketch_bug.f3d". Try changing one of the dimensions. It throws a "failed to solve" error asking to delete a Rectangular Pattern. Actually, one of the rectangular patterns I deleted did not disappear. Different bug or same bug? Also, if I try adding sketch items such as a box and dimensioning, the dimensioning fails. Please let us know when this bug is fixed. I hope the attached sketch is useful for reproducing.

etfrench · ‎08-09-2022

Deleting the rectangular pattern icon at the origin will allow you to change dimensions. You may be better served by using multiple sketches instead of one.

ETFrench

Fusion