Creating Assy Dwgs - Is there a way to pre-set the Simplified Rep?

[mkelley-2]

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?

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[dschenken]

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.

[gkoch]

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.

[TomD.inPDX]

Sounds to me like an Idea should be submitted

Gunter, maybe you can prod a technical committee?

[gkoch]

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":

http://communities.ptc.com/community/create-idea!input.jspa?container=2023&containerType=14

(i.e. View refers to Creo View, not drawing views, so it should not be selected for this idea)

[TomD.inPDX]

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?

[gkoch]

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.

[TomD.inPDX]

Thanks Gunter.

I suppose extra effort is required to use simplified reps, specifically of assemblies, to have significant overhead savings. With part models, simplified reps would have to be fully loaded anyway since you are "suppressing" features; but in assemblies, I could see a significant saving of resources if only the parts in the representation are loaded (and maybe the parts used for constraints).

From a user perspective, you get the option to show a simplified rep when placing the view if one exists. Actually it asks if you want to use a Combined State... making this less user friendly. I don't use these often so I wonder if the answer to the user interface is more a question of usability of view manager dialog.

[mkelley-2]

The OP observed precisely the same behavior as you did.

What the OP would *like* to see is a pop-up on the drawing creation dialog box that permits one to select a Simp Rep (other thatn the Master Rep) upon drawing creation...! Not having this forces adding the Master Rep to the drawing - whereuopn I need to "Add Rep" tochoose the desired Simp Rep, and then DELETE the Master Rep. YUK!

[ChristopherLewi]

What if you made a drawing of an External Simplified Rep assembly instead?

[mkelley-2]

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?

[TomD.inPDX]

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.

[StephenW]

If you start your drawing with just the format or empty (NOT A TEMPLATE) you should get a chance to choose your simplified rep before it brings anything in to memory. I tested with with our template and it does not give you the option to choose a rep before it brings the master into memory.

I do have the open simplified rep by default option set, not sure if that is required for this to work also.

Just don't use the drawing template.

[mkelley-2]

eeeehhhhgg - not a good workaround IMO...

If I don't use the template then the drawing parameters in the format are not auto-populated correctly.

Why does one even need drawing templates in that case?

The right way to address this would be the ability to specify a simp rep on-the-fly as a drawing is created.

Looking forward to having PTC implement this!

[TomD.inPDX]

I think that this is more of a user experience request than a performance improvement request.

Although I fully agree with you, why not have this load by default, combined states addresses this.

Regardless, it appears that the full model, part or assembly, will be loaded so the performance is not enhanced in any way.

Maybe you can get the results you want if you add the simplified rep to a combined state in the model so it can be considered at the time of view creation in the drawing.

Just a tip in how to get what you want without the code changing.

Most times, I don't hold my breath for code change requested in the Ideas section.

The ripple effect in R&D can be significant.

[mkelley-2]

Got to disagree w/ you regarding the performance - unless one is willing to fix any auto-populated format fields (rev, part parameters, etc.) you NEED to use the drawing template. If you use the drawing template, you are FORCED to add Master Rep. Not really an issue on small assemblies - but if you add the Master Rep of a LARGE Assy you WILL pay the price - in terms of the time required to retrieve the entire assembly (I have even had crashes occur as a result) so I think it should be fixed.

[TomD.inPDX]

Maybe I am not understanding what is going on under the hood very well, but it is my impression that to use simplified reps in drawings, you still have to load the entire assembly into memory anyway.

I fully agree with you as posted before, that -if- indeed you can only load a subset to obtain a simplified rep assembly (like external simplified reps), then indeed there would be a performance improvement.

The other issue you touched on is something to consider, but probably not part of a simplified rep solution, and that is the use of different parameters depending on the condition of the simplified rep. For instance, in family tables, each member can have different parameters to populate the format. I am not aware that this can be done with simplified reps.

Sorry that I do not have any relevant use cases on hand to try illustrating where I am coming from. Can you show where your performance and productivity would be improved? Have you tried using the combined states instead? Do your templates have predefined views? If so, can they not have a predefined name and combined state already coded in the template?

I am not trying to smart here because I am certainly no expert on simplified reps... but I do like it when these forum discussion can open new avenues in a Pro|WorkAround^tm Arena. Often times, a little difference in thinking can create excellent discussions. My face would be bluer than this guy if I waited for PTC to fix things!

[mkelley-2]

Antonius Dirriwachter wrote:

Maybe I am not understanding what is going on under the hood very well, but it is my impression that to use simplified reps in drawings, you still have to load the entire assembly into memory anyway.

Nope, you can start with an "empty" session and create a drawing. And that would be the way to do it for a LFAD (Large Freakin Assy Dwg), IMHO...

I fully agree with you as posted before, that -if- indeed you can only load a subset to obtain a simplified rep assembly (like external simplified reps), then indeed there would be a performance improvement.

The other issue you touched on is something to consider, but probably not part of a simplified rep solution, and that is the use of different parameters depending on the condition of the simplified rep. For instance, in family tables, each member can have different parameters to populate the format. I am not aware that this can be done with simplified reps.

Well, as applied to this situation - what happens is you need to use the proposed workaround (i.e. empty drawing, add model, choose rep, do NOT use template) the various drawing fields do not get populated (I should add here that I am living within a Windchill environment). Thus, to use the workaround requires one to a) be savvy enough to fix ALL of the broken fields and b) actually remember to do it! (which is no mean feat at my age! ).

This is actually what I now do when faced with this challeng - but I was hoping there was a better way.

Sorry that I do not have any relevant use cases on hand to try illustrating where I am coming from. Can you show where your performance and productivity would be improved? Have you tried using the combined states instead? Do your templates have predefined views? If so, can they not have a predefined name and combined state already coded in the template?

IMO it is a bad idea to include pre-defined views - particularly for assembly drawings -as you get will get killed by creating a large assy dwg & furthermore you can never count on wanting to use the same Simp Rep for every dwg. Consequently, my drawing templates do NOT contain pre-defined views, since it is easy enough to make them.

I think that combined states will not help here, because this is irrelevant once the drawing has been created. Someone please correct me if i am mistaken!

I am not trying to smart here because I am certainly no expert on simplified reps... but I do like it when these forum discussion can open new avenues in a Pro|WorkAround^tm Arena. Often times, a little difference in thinking can create excellent discussions. My face would be bluer than this guy if I waited for PTC to fix things!

Yeah, I'm not holding my breath either - but hope springs eternal, as they say...!

[TomD.inPDX]

Good! We are in agreement on the predefined views. A few organizations can make use of this in a template but this is the exception for sure.

I never bothered with trying to populate all the format variables if indeed I forgot to create the parameters in my model (I start with empty parts). The easy way around this is to "change" the format by reloading it and letting the process delete the existing tables with the now-added parameters in my model. Yes, two times the work, but everything populates and maintains relationships back to the model (not true if you try to enter the data at the drawing level).

So the last question is, does the LFAD (love that!) load the assembly fully into memory if you only want to use a simplified rep with a subset of the assembly. Here I maintain that the full assembly (master rep) is still loaded into memory. And I will maintain that you can use a combined state for your view definition to keep the entire assembly from having to go through the display routine.

Time for Gunter to weight back in

[StephenW]

No, absolutely not. When using a simplified rep in a drawing, only the components active in the simplified rep are brought in to memory. It's just like using a simplified rep in an assembly. The main purpose of a simplified rep is for large assembly management. Some people have gotten creative and used it for product variation more commonly associated to family tables.

I also work on large assemblies and their associated drawings. For a while, we could not open the master rep of our large assemblies mostly due to lack of enough memory. I think that was right after one of the major upgrades, either WF4 to WF5 or WF5 to Creo 2 (not sure which, old man memory is awesome). Our only option until we convinced IT and the boss to upgrade RAM was to aggresively manage our simplified reps.

You if care, you can test this easily by making a simple 2 or 3 part assembly. Make a simplified rep of that assembly by excluding all the components except one. SAVE the assembly. Close the assembly and erase not displayed. Make a new drawing (empty or with format, not with a template), with the assembly as the model and set the rep to the one that only includes the single part. View what has been loaded in to memory using the FILE - MANAGE SESSION - OBJECT LIST. It should only show the drawing, the assembly and the one part, not the other part(s) excluded using the simplified rep.

[TomD.inPDX]

Thanks Stephen. Definitely good to be wrong about this one

[gkoch]

And I could not have been clearer or more definite about this than Stephen. Thanks from my side, too!

Just a question:

Has someone from the thread created the Product Idea by now? I don't see a link posted.

Note:

As I mentioned before, PTC employees have been explicitly asked to refrain from filing Product Ideas, as this mechanism is supposed to fully reflect customer needs.

[StephenW]

Please see product idea:

http://communities.ptc.com/ideas/4627

[TomU · Accepted solution]

Weird, I thouht PTC fixed the double URL thing. Guess not. Trying this:

Create drawing with template with a simplified rep (not master rep)

[StephenW]

LOL. And I thought I made sure that it didn't get the double URL. Now I know I'm still screwing it up.

How did you do it Tom?

[TomU]

I had no confidence I could create it either. Since I had just viewed the idea (by manually editing the URL), it was listed in my recent places. Adding that link directly seems to work okay.

[StephenW]

I'll use that next time. I did make the link back to this conversation correctly in the idea. I thought I did them exactly the same though. I thought it worked to simply hightlight the link as its pasted in, right click and unlink. I guess it doesn't work every time or ?? Thanks for the browser history suggestion.

[Dale_Rosema]

Or you can click on the URL link (in your post) just before posting and "Un-click" the "A" with the little piece of chain. That re-establishes the correct link and doesn't double it up.

(I also then go and click the link on my post to make sure I did it correctly).

[mkelley-2]

Great Discussion!

Thanks for submitting the Product Idea - I had missed PTC's request, so you've saved me the trouble.

One question - is it in fact possible to specify a specific Simp Rep for a drawing view when defining a drawing template?

(Not that I would be able to use this to solve my current problem, but I can see where this ability could come in very handy!)

[TomD.inPDX]

Probably not since the template requires a model, and the only model that can be added at the time of creation has to be a master rep.

But I could be wrong again