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Patriot_1776
Patriot_177622-Sapphire II
22-Sapphire II
August 1, 2025
Question

Existing dwg views referencing a simplified rep will NOT update if you add new parts to the rep.

  • August 1, 2025
  • 3 replies
  • 6715 views

Creo 8:  I tried this earlier, in an admittedly more tricky version, that didn't work.  P!$$ed me off, but since I was trying something new, I figured it might be buggy, but this recent example is straight up modeling/dwg that DOESN'T WORK.  I had a simplified rep in an assembly where some parts were Excluded.  I made a bunch of dwg views of that rep.  I then had to change the assembly to add some parts and fasteners for them.  the BOM changed but the views DID NOT.  I was forced to DELETE all those views, and re-add them.  TOTALLY UNACCEPTABLE.  I've defended Pro/E against the SW guys for 20+ years, and now I find myself questioning why I continue to do so...

3 replies

M
MartinHanak24-Ruby III
24-Ruby III
August 3, 2025

Hi,

I do not have Creo 8 installed, therefore I tested Creo 9.0.2.0.

When I added new part into simplified rep in Assembly mode, this part was not displayed in drawing view.

In Assembly mode plus sign was displayed behind simplified rep name.

I saved simplified rep, this action removed plus sign behind simplified rep name.

After saving simplified rep new part was displayed in drawing view.

Patriot_1776
Patriot_177622-Sapphire IIAuthor
22-Sapphire II
August 5, 2025

Hey Martin!  I saved the Rep, still didn't update the views.  It "might" be because of the size of the assembly (1,300 parts), but it still did it on my much smaller assy of only about 9 parts.  Granted, I was trying a new technique out on a test assy, so, I "almost" expected issues, but I didn't on this assembly, and this one was a real assembly that needed to get done.

M
MartinHanak24-Ruby III
24-Ruby III
August 6, 2025

Hi,

just couple of notes ...

1.] Please provide exact information about Creo version ... Creo 8.0.?.0

2.] Does the drawing contain multiple drawing models?

3.] Just for testing purposes ... add  update_drawing  all detail option into the drawing and update it.

 

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
August 4, 2025

I haven't had an issue with this that I could remember so I tested this morning with a simple test assy and it updates without issue. It's a pretty common thing for me to have to add/remove simp rep components so I wanted to make sure I didn't miss anything

The issue you are having is likely data specific, the assembly or drawing probably has some sort of corruption (for lack of a better word).

The only other reason I can thing of is I forgot the save the simplified rep after modifying it, so the drawing doesn't see the update.

Patriot_1776
Patriot_177622-Sapphire IIAuthor
22-Sapphire II
August 5, 2025

Hey Stephen!  It's a pretty large assembly, 1,300 parts, a lot of small fasteners relative to the size of the table.  The new fasteners I added refused to show up no matter what I did.  I had to delete ALL the views and re-add them.  TOTAL PITA.  Good thing I saw that before I started adding all the 60 item balloons.

 

I had the same problem with a totally different assembly I was playing with using a different technique, but I expected there might be trouble with that one, but not this one that is much more "vanilla".  Have no idea what the issue is but to me it's a BUG.

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
August 5, 2025

Are you saying you were able to recreate the issue within a different assembly?

If so, please detail your process. I would like to see if I can recreate it.

I do large assemblies regularly and don't remember seeing an issue like this with reps. For me it is very common for lower level assemblies to be modified by other users and they destroy simplified reps that I am using, so I will either have them fix the rep or I will fix the rep later, which requires an update on the top level drawings.

R
ROpitz-24-Participant
4-Participant
December 18, 2025

Hi, here the answer:

since Creo 2 or 4 the standard rule of Simp Reps was changed from Master to Exclude for very good reasons. If you added 3 parts to a new SRep in former times the standard rule was "Master* and you hid components you did not want to see. Newly assembled components were shown. This is what you want but the Creo default changed.

Newer versions of Creo automatically will start Simp Reps with standard rule "Exclude", and they only show e.g. the 3 parts you marked as Master for all the times, but nothing else, and no newly assembled components.

What you need is to change the standard rule to Master, then hide objects you do not want to see. Now all newly adde components in your assembly will be shown in this (automatically updating) SRep. Use this Rep for drawing views and everything will run as you desire. Just understand the "standard rule" of Simp Reps - and life will be easier 😉

In this case forget "update_drawing all", "making" a bug out of it, complaining for PTC or Creo, do not try to figure out the bug with strange config options or something. The best way is to use the Creo default in this case and it works perfectly. This default change in Creo 4, I guess, was a very great enhancement to work with large assemblies, exactly made for what you need!

Good luck

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