Accuracy

[bvanhiel]

Is there any way to manually change the accuracy of SW models?

I'm doing some fairly large surface models with small details. Features that should work are frequently failing. Which means I'm spending most of my time devising work arounds.

Pro/E allows control over the model accuracy. It seems that SW users are "protected" from this feature.

-b

 

[TheTick]

Can you post a picture?

In my experience, it is rare (= never) for SW to have this type of problem due to the reason stated above. I did see it plenty in Pro/E, though.

Is there source geometry that is imported? Perhaps there is anther source of corruption causing the smaller features to fail.

 

[bvanhiel]

All geometry was created in SW. Can't post a picture due to the proprietary content. In this particular case I was attempting to create a .010 debossed area on a 50" long part by copying the surface and and using the cut-thicken command. The command failed with the "accuracy not good enough" (I'm paraphrasing) error message.

I frequently get errors in SW when dealing with non-planar coincident surfaces. I spend lots of time arranging surface trims to avoid that situation. Typically I just get the "geometry error" message when trying to create the feature. The above error occured after exiting the feature creation mode, so it was unusual.

-b

 

[TheTick]

Is it a lofted surface?

This could be due to interpolation errors inherent to the way parasolid looks at non-analytic surfaces. If the defining points of a B-surface are too far apart, the .010" offset may be larger than the applied tolerance.

I understand the error. I've just never seen SW do it before. (UG would cough this one up once in a while).

Another possible approach:
Copy your surface, trim it down to a swatch close to the size you need. Offset that so it is the "bottom" of your emboss and then thicken outward. Use a thickness that is as large as possible, not just .010".

Honesty may be the best policy, but insanity is a better defense.

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-SolidWorks API VB programming help

 

[bvanhiel]

Tried offset and then larger thickness cut. It failed as well. Also tried thickening as a solid and then subtracting. What finally worked was offsetting the surfaces and manually constructing a connecting edge surface, then knitting and cutting. Overall I figure I wasted about 2 hours trying varous scenarios and watching regens.

I spend much of my time modeling fairly involved ID shapes. Bloated SW files sizes and slow regens are offsetting any usability gains. I love SW for lots of reasons, but I think I'm going back to Pro/E for the next surface intensive project.

-b

 

[Heckler]

Pro/Engineer employs a variable tolerance model. The maximum gap is a fraction of the total model size. So for large models, such as jet engines, Pro/E allows larger gaps, while for small models, such as watch parts, only small gaps are permitted. The relative tolerance model is a clever one, and it enables Pro/E to run fast. Unfortunately, no other major CAD firms have adopted this strategy.

Heckler
Sr. Mechanical Engineer
SWx 2007 SP 3.0 & Pro/E 2001
XP Pro SP2.0 P4 3.6 GHz, 1GB RAM
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

(In reference to David Beckham) "He can't kick with his left foot, he can't tackle, he can't head the ball and he doesn't score many goals. Apart from that, he's all right." -- George Best

 

[Heckler]

The Parasolid kernel employed by Unigraphics, SolidWorks, Solid Edge, and Microstation employs a concept called "tolerant modeling." The tolerance is fixed, but larger gaps may be permitted on a face-by-face basis.

Heckler
Sr. Mechanical Engineer
SWx 2007 SP 3.0 & Pro/E 2001
XP Pro SP2.0 P4 3.6 GHz, 1GB RAM
NVIDIA Quadro FX 1400
o
_`\(,_
(_)/ (_)

(In reference to David Beckham) "He can't kick with his left foot, he can't tackle, he can't head the ball and he doesn't score many goals. Apart from that, he's all right." -- George Best