Problem using Thicken on a simple surface

john_robinson568

Hi All,

I've been using onshape for a few months now and have been getting the hang of it, but today I ran into a problem that has me stumped. 

I have created a simple surface using a sweep. The sketches used to define the profile and path for the sweep are mostly constrained, but are simple with no sharp corners. If I try to use thicken on the surface in the inward direction, it fails. However if I mirror the surface, I can use thicken on the mirrored surface without any issues. 

Could someone take a look at this really simple document and give me some hints please?

https://cad.onshape.com/documents/0824b97bad2a52c026499cde/w/4d7a37b5aa599b4ab4e6ef7d/e/1628b5a69b6ab5e46d8edaf8?renderMode=0&uiState=61fb6f29307158015c87649b

Many thanks, John

brooke_spreen

Gave it a shot, but no luck. Strange that extra faces are being created on the underside of the successfully thickened part. Would guess this delves into the mysterious world of surface quality...

NeilCooke

Can that point on the left be removed? Causing horrendous curvature

john_robinson568

Thanks guys for taking a look at this for me.

You're on the money Neil, it was the point on the left causing the issue. I lowered it by 0.1mm and that fixed the issue. I am surprised by how sensitive it is, I have done a reasonable amount of surface modeling in onshape, and never encountered anything like this before. this one really had me stumped.

I didn't realise you could visualise the curvature within a sketch, so thanks for the tip, that really helps a lot.

Cheers John

EvanReese

If you can at all afford to remove the point instead of nudging it down it will make your model much more stable.

john_robinson568

Evan_Reese said:

If you can at all afford to remove the point instead of nudging it down it will make your model much more stable.

Thanks Evan,

I do need that point, but I will see if I can find another way. But what I don't understand is what is it about that particular point that makes it unstable? Is it that it is too close to the next point? Or is it because that point is "behind" the sweep profile sketch? Or something else altogether? Just trying to understand so that I don't make the same mistake again. 

Cheers John

S1mon

@john_robinson568

If you turn on the "minimum radius" check box in the show curvature dialog, you will see a very small radius near that end. If the radius is smaller than the offset/thickness value, it's difficult to do the offset. Some CAD systems can approximate the result in that situation, but it's more of a challenge.