I have been working on a part and all of a sudden some features(i.e. a sketch or a fillet, so anything really) cant be unsuppressed or suppressed. There is no option for it. Does anybody know why this is?
When I open the part and immediately perform a CTRL-Q, there is a warning:
If I select 'Continue', several features fail, others have warnings. At this point, it's time to start deconstructing the model, removing features until the bad behavior goes away. Step one is to eliminate all the folders. They just get in the way at this point. Next, starting from the bottom of the tree and working your way up, delete features until the bad behavior goes away. Also, delete any features that have no children, regardless of where they are in the tree. This takes the model from 233 features, down to 28, but still exhibits the bad behavior. Delete all the other configurations, just to make things even simpler. Your feature tree now looks like this:
All six items at the bottom exhibit the bad behavior (can't unsuppress). If you delete the last feature, the bad behavior goes away. You can't unsupress the last feature because its suppression state is controlled by an equation.
If you delete the equation, the problem goes away and everything can be unsupressed. So, I made a simple test part with three extrude features stacked up. I made an equation that set the suppressed state of the last feature to always be suppressed. I see the same behavior. Any features that are parents of the feature controlled by an equation cannot be suppressed/unsuppressed. This is most definitely a bug in 2017, since 2016 doesn't exhibit the behavior. The complexity and errors in your model made it difficult to find the problem, but that's why saving a copy and deconstructing it is worth doing.
Update: I see that you can go to feature properties and change it there but it not showing up in the first thing is still weird. and still my question. I should add that it doesn't happen to all my features just some random ones.
Can you share the part? And maybe exactly where you were and what process you tried to use to suppress/unsuppress?
The reason that I ask, is, as an example, that if you are in an assembly and are modifying a part in context, then the suppress/unsuppress buttons don't show up for the components until you exit the in context modification of the part.
Is it something like that?
I would share it but its pretty complex so I wont. But that could be the case. I wasn't in an assembly though. The part is referenced in an assembly though so maybe that is it. even though the sketch that I couldn't unsuppress didn't have anything to do with the assembly.
Well, it all depends on the specific scenario. It sounds like the example that I gave is NOT the issue here, if I understand correctly.
The reason that I am asking for more details is that I am not sure how much of a user you are. Giving more information will clue us in to what things to try.
How about a screen shot of the issue?
I understand your concern. I'm really sure hot to explain my level of being a user besides that ive had 3 semesters of solidworks classes at college 1 and a half years in industry and 2 training courses. One specific to assemblies.
Here is the screen shot you asked for.
Its a sketched I used so that later down the tree I had a consistent location for a specific feature which only has one child(which is in a different configuration that is not being used in the assembly).
Alex, from the picture you posted below, this really isn't a complex model and sharing it would be the best way to get a complete and accurate answer to you question.
Does it have any parents that are suppressed?
My first intuition matched Dan's, that of assembly in-context editing focusing only on that context.
Do any other users have access to the PC you're using? More specifically, could someone have customized the Solidworks UI that you are using? Do you have an OCD intern? It appears to me that your missing commands from the RMB pane could simply have been removed by someone's customization. This is very odd to me, as I usually consider customization for adding icons, not removing them.
Try adding it back in with UI Customization. If my UI was really messed up, I would revert it to a saved Settings Wizard file, or reset the UI, depending on how many other options need restored.
The other thing that I notice, is that it looks like (its hard to see, but I think I am right ) Flat tree view enabled.
If this is true, then it is extra hard to see what is linked to what. If this IS the case, try turning it off.
No but its connected to a somewhat complex assembly consisting of 5 other parts
No one else has access or are able to accesses my computers files. And it will work on the other features as shown. This is not the only one in the tree that does not show the suppress option though. There are a couple others but all of their parents are unsuppressed.
And no. Flat Tree is not enabled. Hope this is easier to see as well.
In this picture you are RMB selecting the sketch. That popup menu is correct for the sketch.
RMB on the feature one position up.
In fact if I do the feature above it which I believe is what you are saying it also doesn't give me the option to suppress.
I was trying to show that it also showed that I could suppress on other features.
Select the feature in the tree.
Then select Edit>Suppress>This Configuration...
Actually doesn't work. As stated earlier I did find a way around it. But not sure why it doesn't show up in the beginning.
Alec the feature in this screen shot is a combine and I do not think you can suppress that. Edit feature and delete would be the 2 options available.
I could be mistaken on that one, but I am pretty sure you cannot suppress it.
Sorry but you can suppress a combine. But even if you couldn't it doesn't explain the sketch not being able to unsuppress.
I just made a test part and I can suppress a Combine feature...
Alec, at this point I am out of ideas until you post your Part file here. Sorry.
Can you upload a simple file which is showing this behavior? Does you part has configuration, multi bodies or exploded view?
Check #18 of Forum Posting on how to attach files while replying to a post.
Alright Ill see what I can do tomorrow.
stupid question but did you shut down SWX and restart. Nine times out of ten when it starts acting buggy this fixes it. Then there's that one time out of ten that who knows...
Thanks for your input but I have tried that. Still doesn't work.
Okay Here are the files. The file in which the problems are are in the "Assurpack Bar Shallow Clam". I'm assuming you can tell where the feature is from the screenshots. Thanks
Sorry I forgot to add that I am using SW 2017 SP1
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