I did an extruded cut in an assembly as an assembly feature. then deleted it and the feature is gone from the tree but my model didnt revert to back before the cut... any help?
Did you try a Ctrl+Q update with the Part open? If that doesn't fix it, can you post the Part here? See How can I attach a file to a forum post?. And welcome to the forum.
yep...tried the traffic light and ctrl+q and neither worked. its an assembly. i will try to pack an go it and post it.
Here is the file. The top level assembly is called "dually flatbed frame.sldasm"
I made an extruded cut to the boards and a piece of sheet metal but didnt like how it worked and was going to redo it. i deleted the feature in the tree and it went away. the cut to the boards went away but the cut to the C-channel member of the frame itself did not. it still shows it being cut. if you open the frame by itself you do not see the cut (assembly feature).
hope that helps. thanks for the welcome and hope you guys can figure this one out because its eluding me...
I've seen a lot of weird stuff in the almost 10 years that I've been using this software, but never that. I can't figure it out either. I even tried saving the Part as a new name and using the "Replace Components" feature, but the new one came in with the same cut. I finally just deleted the original, reinserted the newly saved one, and mated it's three primary planes to the same planes in the Assembly. You can do that too, but it will require replacing a bunch of lost mate references. If you do decide to do that be sure to not delete the child features when you delete the original or they'll be completely gone instead of just suppressed because they can't find the face, edge, or whatever. Hopefully someone else will take a look and figure out what's going on before you go to that much trouble.
Nice work, by the way.
I posted a link to this somewhere else hoping someone there will see it and solve the problem, so please wait a while before you swap out components as I suggested above.
Thanks! i did the same thing with trying to rename the frame and replace it. I've been a CAD user since '98..everything from solid works, solid edge, Autocad and a bit of inventor and this one has me stumped. there is no logical reason for what its doing. I would hate to have to re-create the assembly.
Its like the assembly doesn't want to let go of the deleted extruded cut assembly feature.
Do you have a version of the file from before you deleted it?
I am thinking.. narrow the scope of the feature, i.e. to which components it applies, so that it only applies to some fake thing put there to absorb its target.
I'm checking out the file now; haven't seen it yet.
Tom Gagnon wrote: Do you have a version of the file from before you deleted it?I am thinking.. narrow the scope of the feature, i.e. to which components it applies, so that it only applies to some fake thing put there to absorb its target.I'm checking out the file now; haven't seen it yet.
Tom Gagnon wrote:
That won't work. The feature has been deleted, and is no longer in the tree, in the Assembly or Part. It's scope can't be edited if it's no longer there.
Must be blind or something, I couldn't see where you mean, could you take some snapshots and show us the placement??
If you open up the assembly then open up the steel frame by itself it will be clear. look at the rear most members. in the assembly the outer frame is cut off... in the part file it is not.
Hence why I was considering a file Restore Previous Versions to an earlier version of the file. This is available in Windows Pro or Enterprise, depending on your environment. That's what I'd do, in my environment, depending on time frames of design vs backups. Otherwise, start over with that component or replace as Glenn said. I tried save_as copy and replace component, with no change in results.
I opened it up and was as mystified as you, Glenn. I have no idea why or how it is doing that.
Jason Moyer This should be brought to your VAR's attention. File is in Student version, so I doubt you really know who that would be.
unfortunately i do not have an older version
May be I'm not able to see or overlooking something; so could you post a picture of the issue?
Also you've double bodies in the frame due to extension option in the trim command. See the overlap in the picture below
So edit the trim feature and removed the option "allow extension"
Tom.. Its a student version because i work for a university. This is just a personal project for my pickup as i have extra time here and there. ill just swap the component out and reattach all the mates. Time consuming yes but it works. Either way the problem baffled me. Because it deleted the reference in the tree... deleted the cuts to the boards...but left the C-channel member cut. Unless it has something to do with the frame command since that's how i made the structural frame.
I found it!
I don't know why, but if you edit the C channel C5X6.7(1) in the main deck frame and select "Merge miter trimmed bodies", the missing portion comes back in the assembly.
Richard Doyle wrote: I found it! I don't know why, but if you edit the C channel C5X6.7(1) in the main deck frame and select "Merge miter trimmed bodies", the missing portion comes back in the assembly. Richard
Richard Doyle wrote:
holy crap your my hero!!!
never would have thought to look there! talk about a brain teaser!
Thank you...I owe you a cold one!
You're welcome Jason, I like to chase things like this down every now and then.
It still doesn't solve your entire problem, I assume you still need to cutoff the deck planks.
I'd try a different method
typically i would drive down and make unique components for those parts... since this is just for me i'm being a bit lazy if i were completely honest.
It show up but still not correct
To me it looks like a graphical bug as bodies are still there.
Seems like a similar problem has already been reported under SPR 753564 in the SOLIDWORKS Knowledge base (which is accessible only to commercial customers on subscription, so you may not be able to check/vote )
Take the Frame, Form New Subassembly. Then Dissolve Subassembly.
Agreed - there is something else going on with those corners. And..that's probably why the whole thing failed.
Jason - play around with the corner settings, trimming, etc. and see if that helps.
I'll redo the assembly. Or Form New Subassembly with everything.
You never know what else is wrong with the file.
Retrieving data ...