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

[Patriot_1776]

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...

[MartinHanak]

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]

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.

[MartinHanak]

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.

[MartinHanak]

https://www.ptc.com/en/support/article/CS360627

[Patriot_1776]

Hey Martin!  That option doesn't seem to exist, at least not normally.  You can't add it via the detail menu (at least in my Ceo 8).  So, thinking it might be a "hidden" option, I added it manually to the bottom of my .dtl file using notepad.  Is that how you had to add it?  At this point it's too late, and I can;t even test it, but we'll see in the future because I'll certainly be keeping my eye out for that bug.

See, I KNEW something was FUBAR'd, thanks for finding that BUG report.👍

Creo 8.0.5.0

I wonder if this is fixed for Creo 10?  Oh wait, that would be WAY too much to ask....I mean, they're FAR too busy giving us fancy new menu graphics...*sarcasm*

[StephenW]

This post explains some of those options:

https://community.ptc.com/t5/3D-Part-Assembly-Design/Fast-Facts-Quick-Tips-for-Using-PTC-Creo-Drawings-Part-3/td-p/443939

[Patriot_1776]

Man, PTC just HAS to make it a complete PITA.  Turns out those settings need to be in the config.sup, NOT the .dtl file:

• enable_auto_drawing_update yes *(required to use the options below)
• auto_drawing_update all

Thanks for the heads up Stephen!  Too late for me, but "maybe" they'll work next time...maybe.

[StephenW]

Wait!  Not exactly. There are some options available for the config.sup but the one Martin mentioned is a drawing setup file option.

You add the option as it shows and then apply it and then it goes away after applied. It's not something that stays or should stay.

I always tell people to SAVE before applying the option and the check your drawing to make sure there are no unexpected changes before saving again so you have an easy way to get back to what you had before. I've never had any problems but its just good practice.

Detail Options:

1. File
2. Prepare
3. Drawing Properties
4. Detail Options

• User_command delete_erased_dimensions
• User_command delete_erased_axes
• User_command clean_duplicate_axes
• User_command update_note_text_padding
• Update_drawing 1808656 (remove extra spaces in basic dimensions)
• Update_drawing 2119624 (Crosshatching break across text)
• Update_drawing 2140864 (secondary dimensions show at maximum decimal places)
• Update_drawing all (applies all updates. Use caution as this command may make more changes than are desired)

[Patriot_1776]

Ok, now I'm even more confused.  I just added the 2 settings I mentioned to the config.sup and whatever happens, happens.  Sick of monkeying with it...  Makes no **bleep** sense to even have the .sup file, why not just put all that into the 1 config.pro file?  Again, just a total PITA

HOPEFULLY they fixed that so when I move to Creo 10 it's not an issue.

[StephenW]

The problem with setting them in the config (.sup or .pro) is you may not realize something changed within a drawing that the user may not want to change. 

I suppose, in other words, one problem for one user may be something another user wants.

I don't really see how your specific problem would fit that description but some of those "fixes" listed may mess up your drawing unexpectedly, it'll just be changed.

[Patriot_1776]

Yeah, I just set that one setting.  Honestly, I can't ever think of a scenario where a user would NOT want a simplified rep dwg view to update, esepcially knowing that the BOM DID.  I was pi$$ed that my neat new technique didn't work....because of the buggy software.

[BenLoosli]

The funny thing is, even though PTC says enable_auto_drawing_update  must be in the config.sup file (CS31562), it does not show as an error if placed in the config.pro. We are testing a new Creo setup and I noticed this in the config.pro file that they sent out for testing.

I don't know if the auto_drawing_update all still works if the enable_auto_drawing_update is in the config.pro.

Note that enable_auto_drawing_update is obsolete in Creo+! Does that mean it is also obsolete in Creo 12.4.0.0?

[Patriot_1776]

'Sup Ben!  Since it was unclear, I initially put it in the config.pro file because the article Martin referenced didn't mention anywhere else and that's where you USUALLY put these settings.  But then it showed that weird green icon with the lines which if I remember means that it's a setting that's unused/unknown.  So then I found the other PTC article, and put those 2 in the config.sup, but THAT'S stupid because while our users get the config.pro from a central location, the config.sup is loaded locally on people's systems (and who knows if PTC loads it in several locations or not) so it now falls to the individual to make sure they have that setting.  In my 29 years on Pro/E, I've NEVER had to add settings to the config.sup, ever.  Effing stupid.  As to your question, I don't know if "THEY" know.  Best of luck!

[StephenW]

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]

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.

[StephenW]

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.

[Patriot_1776]

Yup, same issue with both very different assemblies.  The BOM updated just fine, the views refused to.  I wonder if there's some setting that's maybe causing an issue.  I don't ever remember seeing this.

Can't get into too much detail for security reasons.  It would be easy to not notice the missing parts though, it was only a handful in 1,300 total.