VIEW STATE PARTS NOT SHOWING UP IN SECTION VIEW

[Anthony_Zepeda]

Running CREO 8.0

I have a section view with 2 components not showing up in view. They are there but will not appear.

I have tried excluding and including back and forth in VM States tab. I even cleared out my workspace and did the work all over again it was only a (5 minutes task)..

I also created the view state all over again. and nothing.

See screenshot of bodies in green that will not appear.

I did notice in modelling that when I try to add the parts to the section they will not select but other parts will.

[Dale_Rosema]

I've seen display issues more in regular views than section views, but are the (2) parts in question interfering/overlapping with each other?

[Anthony_Zepeda]

No. They actually were present in the view when I originally opened. However, the view state contained extra bodies that did not need to appear in the view. But when I created a new SIMPLIFIED REP the 2 parts do not show up.

[Dale_Rosema]

Can you check your constraints and verify that the two parts are not constrained to a part that is not in the simplified rep?

[Anthony_Zepeda]

Yes. And they are not.

[Anthony_Zepeda]

Just curious. Would that cause them to not appear?

[Dale_Rosema]

If parts are constrained to a part in an instance on which you are not working, then even if you choose to have those parts in the assembly, they will not appear since the parts to which they are constrained does not appear. The logic to constrain them is missing since that part is missing.

[Anthony_Zepeda]

This was not the issue. No instances were used. Issue already resolved. Thanks.

[Dale_Rosema]

Thanks. I saw that, but still wanted to answer your question. Glad you got it resolved.

[StephenW]

The green parts might be surface models (my surface models are magenta but you may have differenet color settings).

In the edit definition on the section, under the Options tab, select Include all Quilts. 

In the drawing, under view properties, under View Display, set Yes for Hidden Line Removal for Quilts

[Anthony_Zepeda]

The option is greyed out.

[StephenW]

Which option is greyed out? Under the view display in the drawing or in the section definition for Include quilts. Also, the include quits doesn't work on offset sections, only planer sections.

There may be a draiwng option, go to File - Prepare - Drawing proerties - detail options Change

Look for Show_quilts_in_total_xsecs  change the value to YES

On a section view in a drawing, surface models (aka quilts) don't section correctly by default...it's an odd thing creo does. 

I may be mistaken, they may not be surface models, so all my advice wouldn't be helpful.

[StephenW]

Also, check your layers. A layer that is blanked in the drawing that contains surfaces will make them not show...again, based on my surface model assumption.

[Anthony_Zepeda]

Got it. Thanks!

[StephenW]

@Anthony_Zepeda If any one post got you to the answer, set that as the solution. If it was multiple posts or something different, go ahead and explain what was done in a post and then set that one as the solution.

Thanks

[Anthony_Zepeda]

In the Drawing View, View Display.

How do you know this is an offset section? I did not create the section. I am only revising this drawing to add some notes. But noticed hte view was not updated correctly.

I will try these suggestions.

[Anthony_Zepeda]

[Anthony_Zepeda · Accepted solution]

Figured it out. It was something different. Lower sub assy's had some constraint errors. But parts were locked and released. Temporarily unlocked to fix constraints in or for drawing views to update properly.

Parts will will go back to error state but for now to get my drawing to publish correctly this work around will work.