Compute failed with parameter that previously worked

[Anonymous]

Hi,

I have drawn a little box for wafers (see attached file). The design is parametric, and one of the parameters is called waferwidth. While drawing I had it set to 166 mm, everything rendered fine. I then subsequently set it to 83 mm to check if smaller sizes worked. Nothing exploded, so I set it back to 166 mm, only for the design to fail with the message "Warning: Sketch1 Compute Failed: Failed to solve. Please try revising dimensions or constraints."

Unfortunately this is all the detail I get, no mention of which constraint failed. This is especially annoying since I did not change anything in the design that previously worked. Help?

[TrippyLighting · Accepted solution]

1. You should avoid sketching with overlapping colinear line segments. This form of "lazy sketching" almost always leads to problems.

2. You only need to model 1/4 of this sketch without the pattern.

3. Do not pattern, or mirror in a sketch when it can be achieved with modeling features.

[daniel_lyall]

Whatever the problem is changing the dimensions to a small number a big number then again a small number then back to 144 it seems to come right.

Example attached

[Anonymous]

Hi, thanks for your input. Regarding your first point, what would be best practice? Coincidence? I don't understand how colinearity for colinear lines is the wrong choice.

So if I understand correctly I should do the pattern for the bodies - this is more robust?

Cheers,

Boris

[g-andresen]

Hi,

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@Anonymous  schrieb:

So if I understand correctly I should do the pattern for the bodies* - this is more robust?

* features in your case!

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This minimises the effort for the sketch, makes it clearer and puts less strain on the Sketch solver.
In addition, the features are updated directly when changes are made (e.g. number).
If you change the sketch, you have to change the features manually.

günther

[TrippyLighting]

The keyword is not collinear but overlapping. 

For example there are 2 sketch lines here where one would be enough. This avoids confusion when dimensioning.

It might not be a problem in this sketch, but it would be very difficult to debug it it was.

As such, it is best avoided.

[Anonymous · Accepted solution]

Thanks everybody for your help. For reference, what worked in my case (thanks Autodesk support) was removing and re-applying the dimension in question. This will teach me to keep my sketches as simple as possible...

Cheers,

Boris

[TheCADWhisperer]

@Anonymous 

See my example Attached.

I kept the sketches simple - I didn't make the dimensions parametric, but I think you have that figured out.

Of course you could simplify the sketches even more by utilizing Mirror Features.

Another real advantage to Pattern Features rather than Sketch elements is you could tie the number of slots to the height and it would update automatically.

Ha! I just realized I did this all wrong.  There is a much better way.

[Anonymous]

Thanks for taking the time to redo my design! That helped quite a lot for my understanding.

[TheCADWhisperer]

Did you find my mistake?

How will you manufacture this?

As one component or as an assembly of several components?