Hello, when I suppressed a feature in a part, other related features were also suppressed (as a result of a generated error). This was done without notification and caused me a lot of trouble later. When I delete this feature I can see the generated errors notifications. How can I avoid this situation?
As a side note, i do apologize if my answer seems vague, it is just that your are asking a tough question. Design intent is one of the hardest things to learn/teach, if can even be learned/taught.
Thanks Jody. It just seems odd to me that when suppressing a feature there is no warning regarding the other features being suppressed as a result of that action.
For future reference, you can right click the feature or sketch and choose parent/child to see these things. Or a round about way of doing what you ask, a window asking if you wish to suppress features driven from the one you wish to suppress is to act as if you were going to delete the feature/ketch. If there are not any driven features from it the confirm delete window will be empty. If there are features listed within the confirm delete window, then these same features would be suppressed if this feature is suppressed. Then cancel/no out of this window and you've been informed of it's children.
You just have to understand that SolidWorks is a history-based solid modeler so that, chances are, if you suppress a feature then features below it will probably be suppressed as well.
As for a warning, if suppressing the feature doesn't cause errors then the system doesn't have anything to warn about. However, by deleting the feature you've created dangling relationships that will generate an error. A bit confusing perhaps but, as Jody mentioned, a lot of it has to do with design intent coupled with modeling technique.
I was going to submit a SWx improvement idea, but missed the deadline & don't want to wait a whole year. I'd like the capability to the effect of: where possible, when you delete a parent feature, dangle the child features instead of deleting them. When I say "where possible", I mean that, for example, if you delete all of the faces, edges, etc. that are later used to create a fillet, then there's nothing you can do about that: the fillet needs to be deleted or at least the error needs to be dealt with (e.g. select replacement faces) before subsequent features can be rebuilt. But for situations where a child sketch has dimensions or relations to a parent feature, couldn't SWx let the dimensions or relations dangle? I can't recall the specific situation when I encountered it, but I've had child features deleted (without a warning prompt) when deleting a parent feature when it seemed unnecessary to delete them.
1. you can submit enhancement requests year-round. "ideas" are special for SWW
2. this is already available as of SW 2014 - when you delete a feature, hit the advanced button in the delete dialog.
Jeremy, I believe what Zachi is looking for is the same kind of interface/options you get when deleting a feature except for simply suppressing a feature. So that when you suppress a feature you could choose to keep dependent sketches and features unsuppressed but with dangling relations. As it is, no such option is available for suppressing, all dependents automatically get suppressed.
I wasn't replying to Zachi, but to David.
Oh yeah, that makes sense.
re: 1. you can submit enhancement requests year-round. "ideas" are special for SWW Thanks, but I'm not the only one that likes the SWW Ideas area as a single place for enhancement requests: one of the active Ideas this year is to keep the Top Ten Ideas area open year round as an area for enhancement requests.
re: 2. this is already available as of SW 2014 - when you delete a feature, hit the advanced button in the delete dialog. Thanks for your suggestion, but I just tried this on SW 2014 SP 4. I deleted a cut-extrude, and two boss-extrudes that referenced the cut were also deleted. The cut sketch remained. The boss-extrudes could have easily have remained in the model built from dangling/under-defined sketches. I highlighted the cut & pressed the delete button, and tried Edit menu, and right-click - Delete and I was not presented with a delete dialog or an Advanced button. Maybe you need to delete a feature another way to access this capability?
I think you could do the same thing for suppressed features, but SWx would have to keep track of which dangling dimensions have parents which may be unsuppressed at any moment. That might be useful from time to time.
the "advanced" button is right here:
I get it anytime I hit delete key with a feature selected - it is greyed out occasionally when it would not apply.
Great - nice tip. I looked up Confirm delete in SWx help. This dialog must be disabled on my system (note the 'Do not show again" check box). There must be a system options switch somewhere to turn the box on, but I haven't found it yet.
Thanks,
Dave
system options - messages/errors/warnings
checking the box next to the messages undoes the "don't show again" for that message.
Great, thanks. It was the "Do you really want to delete this item?" message that needed to be restored. I'd been looking for "Confirm Delete".
FWIW, 2015 is going to have a feature where when you hover your mouse over a feature, it will draw arrows to any dependent features (children).
As other have said, part of the deal with history-based modelling, is that you end up with parent/child relationships as you start modeling. You can always delete a parent feature and choose which children will not be deleted. This will leave dangling references and underconstrained geometry that will need to be fixed.
It is all about parent/child relationships, the nature of history based modeling and your design intent when you start designing something. The only way to avoid it is to check the parent/child relationships before suppression (right click on a surface in the model, or a sketch or feature in the tree and then select parent child), then determine how these will be impacted by the suppression. Sometimes you may have to go back and change where a feature sketch is dimensioned from or how it is related to existing features.