I’m trying to ‘form new sub-assembly’ but get an error :
Cannot add: one of components in rollback state.
So, couple thousand parts, how do I find the culprit without having to open every part?
you’re saying that assembly “TEMP-DWG-00023…” contains a couple thousand parts? If not should be able to drill down through sub assemblies there to find the offending part.
I looked for Component Status = Rolled Back among the “Search Criteria for Advanced Component Selection” (2018 link) https://help.solidworks.com/2018/english/SolidWorks/sldworks/r_search_criteria_advanced_selection.htm
I didn’t find it in 2018. I hoped this would be available. Maybe Component Status = (Has Errors, Had Warnings, or Needs Rebuild) can help find that needle, but I think it’d return more false positives than anything.
AFAIK, there is nothing at the assembly level to tell you which part is rolled back. You have to open (or edit) each individual component.
Why SW gets its panties all bunched up over a rolled back part, I will never understand.
I think in 2019 there was a bug where it would give you this error incorrectly. I think the fix was to open any part. Roll it back and then roll it to the end.
Haven’t tried the macro. Company PC, so we’re locked out of a lot of stuff like that.
I ended up trying ‘form new sub-assembly’ while deselecting one assembly at a time until I did not get the error. Then I went to the offending assembly and repeat. drilled down about 6 times to the final sub-assembly with parts. Checked about a dozen parts and found the bugger. About 15 minutes, but what a pain.
How about exploring to where the files are saved. The file would have to be one that was opened and saved recently.
Then again i have had a crash with a part in edit mode and it insisted that a part was still rolled back.
Well you should talk to your boss that how much time/money company is losing for not using the macros or similar tools.
I was cought with the same problem aswell.
Could not find a way to get the part that has the roll back state indeed.
Instead of searching a way to find one part I used an empty assembly and opened subs.
If I could not find it as an insert component it meant that the sub contained the part I searched for.
I’ve opened a few and came to a smaller sub wich was easier to verify, that way I found my part.
Hope it works for you aswell.
“One of the components of this assembly is in rollback state. The assembly is inaccessible now.”
…has been happening all day… only have a few components in the asm but what a pain in the butt!
No rhyme or reason… lame! 
I fought that same problem last week. Would it really be that difficult to tell us which part is rolled back?
I agree.
For some reason that download doesn’t work for me. It says the zip file is invalid. Can you share it another way?
See attached (I was able to download it, so I attached it here)
Edit: Never mind, it says that the zip file is invalid. Give me a few.
OK, here it is (see attached)
Find-Rolled-Back-Components.zip (11.1 KB)
Thanks. Unfortunately I’m having the same problem as the users in the other thread.
I think my problem is that no part is in a rolled back state, but SW thinks it is. From the other thread:
"Here is some discussion on why SW might display the rolled back message when nothing is actually rolled back:
https://forum.solidworks.com/message/143780 [This link doesn’t work for me]
(possibly related to using configure dimension while editing a sketch)"
I definitely have a few dimensions whose value changes based on the configuration.
After wasting half of the day on this, I finally found a work around, with a little help from my VAR.
- Open the problem assembly
- Suppress EVERYTHING
- Insert the problem assembly into the parent assembly
- Unsuppress everything.
(In my case, step 4 showed me which part was in a rolled back state, and gave me the option to roll it forward.)
I had the same problem last week.
Closing the assembly and solidworks and reooening solved it for me.
Eddy
I stumped on this problem recently and sometimes it is not a real rollback part to cause it, but you have to FORCE ROLLBACK and ROLLFORWARD on the part you opened. It needs just one step back and forward to force a rebuild and the error disappears…
Why does it seem like Solidworks has gone down hill in quality since 2014? Why not make the next upgrade be the 2014 version? Anyway has this always been a problem with SW. I don’t remember running into this issue in the past. The work around of suppressing everything in the Subassembly, inserting it into the assembly, and un-suppressing everything seemed to work for me. Thanks for that tip.