New part associated drawing views not being populated

[Paul6]

I am using Creo Parametric Release 8.0 and Datecode8.0.3.0

Create a custom drawing when a new part is created. I have a start part and a drawing template with the same name and in the same directory. The drawing calls out 6 views which are named in the start part drawing. When the new drawing is created, I can see the views in the drawing tree, the model is shown in the model tree, however the drawing views are not populated with the models. If I select all the views in the drawing tree, and select edit properties, and change the display style to any other style than the drawing default and select apply, the views then become populated. I then have to re-select the display style back to the default style and select apply for the correct style view. Why would this be happening, and is there a solution to this issue? I get the same behaviour in Creo 4 M010 and Creo 8.0.3.0

[MartinHanak]

Hi,

please report your problem to PTC Support.

[hadardor]

Hello,

It looks like your drawing template is contains kind of corruption.

Try this :

1. Open your drawing template
2. Set the dtl option model_display_for_new_views to no_hidden
3. Save drawing
4. Create 3D model so that the drawing gets also created and check the output.

[Paul6]

Hi,

Thanks for your suggestion.

The dtl option model_display_for_new_views to no_hidden is already activated.

However I raised this issue with PTC support and they get the same behaviour from my start part and associated drawing.

Their suggested work round is to

1. create new part with associated drawing.
2. Do not create anything in the model.
3. Save model.
4. Close model
5. Erase model from session.
6. Open drawing.
7. Open model from drawing model tree
8. Create features in model, and drawing updates.

This is a lot of messing around.

Its easier just to create model and associated drawing, create the features etc. in the model, then open drawing and select all the views from the model tree, edit the properties and change the display style to any other style than the drawing default (no hidden) and select apply, the views then become populated. I then  re-select the display style back to the default style  and select apply for the correct style view. 

[hadardor]

Hello,

I still insist that drawing template has something wrong that should be fixed.
Please run this test :

1. Create your part geometry based on your part template
2. Open your drawing
3. Update sheet

=>I am pretty sure this will show the geometry on the views.

Let me know.

[Paul6]

Hi,

Yes, that seems to work by just updating the drawing sheet.

Definitely less clicks to see the model in the drawing, on first opening.

I would have expected it to populate the drawing views when bringing the drawing into session, without the need to update the sheet.

I note that any subsequent changes / additions to the model get populated to the drawing views ( in session) without the need to update the sheet.

You maybe right that there is an issue with the drawing template, PTC support did not comment on this in their evaluation of the issue. 

[StephenW]

By chance, do you have the config option auto_regen_views set to NO? I'm not sure it applies to your situation.

We use this option set to NO so our large assembly views don't regen views when switching windows.