When creating a new drawing (using a template) the Creo dialog forces one to specify an assembly; unfortunatley there is no way to specify which Simp Rep should be used. The default is to add the Master Rep. Which is fine, unless one is working with a large assembly. In which case it is highly annoying, because then one first needs to wait for the drawing to be created; then switch any views to the desired Simp Rep; then remove the Master Rep; and finally use "Erase Not Displayed" to reduce memory usage. By which time one may have experienced a crash due to memory leakage. There's gotta be a better way! Does anyone else feel my pain?
Solved! Go to Solution.
Weird, I thouht PTC fixed the double URL thing. Guess not. Trying this:
There's a setting "open_simplified_rep_by_default" that may help; not sure about drawings, but it works like that in opening assemblies on their own.
What if you made a drawing of an External Simplified Rep assembly instead?
Interesting idea - my concern would be that you'd need to propogate versions of the assembly to accomplish this. I'll have to think thru the implications of this method. Anyone out there have experience doing it this way?
In the recent discussions of External Simplified Reps (ESR), I am not drawing a close relation between simplified reps and ESR's. It is an unfortunate naming convention. In a drawing, an ESR is simply an assembly that has to find some references from dependent assemblies.
Unfortunately not. It seems this option applies only to opening parts/assemblies (that contain a simplified rep).
There is a corresponding config.pro option for drawings (open_draw_simp_rep_by_default), allowing to simplify the drawing or use an existing simplification upon opening. However, there is no option to show the simprep dialog for the initial model that can be selected when creating a new drawing.
You can create a drawing without model and then add the model - this always invokes the simprep dialog (if a simprep exists in the model).
Of course, if you need drawing formats to be associated wth the model, you may have to re-apply the format after adding the model to the drawing.
Sounds to me like an Idea should be submitted
Gunter, maybe you can prod a technical committee?
Yes, I have checked the existing Product Ideas and there is seemingly no such request.
The only other idea around creating drawings with simplified reps selected, is this one about specifying reps in a template drawing: http://communities.ptc.com/ideas/3409
So you all are welcomed to file your ideas, how you would like this implemented!
(I have been told, that PTC employees are not supposed to file Product Ideas - this mechanism should be open for customers only)
About technical areas/committees, there is not much separation between Product Ideas.
When you Create a product idea, you can just roughly choose the product, in this case "Parametric":
(i.e. View refers to Creo View, not drawing views, so it should not be selected for this idea)
Thanks Gunter. Maybe the OP can make a better case than I but I will certainly vote for the idea.
So what happens when you only open the simplified rep (in memory) and create a new drawing?
Does the generic of the simplified rep get pulled in or does it add no model?
I did a test (using Creo Parametric 2.0 M110), opening the simplified rep of a model, then create a new drawing.
The model added, was the master rep, so I guess it makes no difference what is in memory:
The new dialog expects just a model name and always applies the Master Rep, whatever rep is in session.