How to accept failed feature; setting?

[bnemec]

Hello,
Frequently I'm in a failed feature, usually a new one, and I'd like to leave the feature and save my changes even though the feature cannot build. I'm fine with that, I want to leave the feature to go back and try a change upstream (sketch or other feature) that I believe will let the failing feature build. But I cannot figure out how to get Solidworks to let me do that. I've searched settings and web; the only thing I find is the "Allowed failed features" in the FeatureWorks->Opttions->Advanced Controls settings, I had that turned on but I'm guessing that only applies to FeatureWorks features which we don't use. But it looks like that's the behavior I would like. Hopefully it's a simple checkbox I'm not finding.

Thanks.

[SPerman]

I don't think that is possible. NX had a similar feature and it is very convenient at times.

[bnemec]

I don't think that is possible. NX had a similar feature and it is very convenient at times.

Yeah, it was a common workflow in Solid Edge. Makes the iterative process of seeing what makes a down stream feature build or fail. Now I have to go do all the selections and insert all the parameters for a new feature that I don't know the magic recipe needed upstream to make it build, yet. I have to cancel to get out of that feature manager just to go back and make a tweak then redo all the feature inputs. Was way faster to just accept the new feature even if it didn't build then keep editing upstream things until the new feature built.

I don't understand why people think failed features are fatal in history based modeling. All these things to block failed features is like neutering history based modeling IMO.

[SPerman]

Sometimes it is as simple as missing something in the sketch for an extrude. It would be preferred if you could create the (failed) extrude feature and then go back and fix the sketch.

[JSculley]

Sometimes it is as simple as missing something in the sketch for an extrude. It would be preferred if you could create the (failed) extrude feature and then go back and fix the sketch.

I can't think of a way that a new extrude would fail based on the content of the sketch. You can extrude a single line. There's not much less you can have in a sketch. Now, there is the problem of not being able to change between thin and regular extrude (known limitation), but if you would need to go back fix the sketch later anyway, you may as well throw in a temporary sketch entity to close the contour.

I'm not trying to say there is no scenario where this would be helpful, I'm just having a hard time thinking of one.

[SPerman]

Here's one example:

image.png (12.55 KiB) Viewed 690 times

[TTevolve]

Learning how to manage fixing features and sketches when you change something is somewhat an art-form and is very hard to teach. It alos goes back to how you layout your parts originally and your work flow.

This is where knowing that doing this

is not a good idea vs doing it this way for most things

[JSculley]

Here's one example:

image.png

You can just click the 'Selected Contours' box and choose one or more closed contours and continue on your way. I'm not sure how you would end up with that error in a new feature though.

[SPerman]

I've had it happen more than once. Typically an extremely complicated sketch, somewhere there is a tangency that I assumed was created but wasn't, so when I trim the sketch there is a tiny sliver of overlap that isn't easily seen.

I'm not saying there aren't workarounds. I'm not saying sloppy cad work isn't a contributing factor. All I'm saying is it would be nice if it would go ahead and create the feature with a red x and let me fix the sketch afterwards.

[AlexLachance]

The only way to "accept" failed features is to tell SolidWorks that you do not want them displayed, which I doubt is your intention.

[bnemec]

I've had it happen more than once. Typically an extremely complicated sketch, somewhere there is a tangency that I assumed was created but wasn't, so when I trim the sketch there is a tiny sliver of overlap that isn't easily seen.

I'm not saying there aren't workarounds. I'm not saying sloppy cad work isn't a contributing factor. All I'm saying is it would be nice if it would go ahead and create the feature with a red x and let me fix the sketch afterwards.

I try to keep my sketches simple and break out elements that don't need to be there into other sketches. What that looks like is different in SW than SE. I'm used to what SE expects and allows in sketches, but SW not so much. I'm slowly learning what SW allows and doesn't allow For example, I need to go back and edit sketch when SW doesn't allow extra lines that for some features that SE didn't mind at all. All I need to do is go back and make them construction lines. Cut features in SE do fine with open profiles, SW that seems to be a hard no. SE would gladly add a sheet metal tab with open profile terminating on the existing body, but SW says no. One could argue that open profiles are always evil; that's fine. They were not a problem in SE and lead to simpler fixes when things changed, IF done properly. Again, need to know what the program is expecting and how it handles things. I'm still learning what those are with SW, but it's painful when I have to set up the feature several times before SW will accept it and save the inputs.

[bnemec]

The only way to "accept" failed features is to tell SolidWorks that you do not want them displayed, which I doubt is your intention.

You are correct, that's certainly not my intention.

[Frederick_Law]

I can't think of a way that a new extrude would fail based on the content of the sketch.

ZTG

[JSculley]

ZTG

Again, you can simply select one or more regions (they can even have ZTG)and carry on:

I would never do it, but if the goal is to preserve a couple of property manager values while you go fix something else, it works.

[bnemec]

Again, you can simply select one or more regions (they can even have ZTG)and carry on:
image.png
I would never do it, but if the goal is to preserve a couple of property manager values while you go fix something else, it works.

We avoid using regions. Testing that we have done indicate they lead to more changes in geometry IDs when editing the profiles.

However, good example of how to get over the feature not accepting. Usually at this point there are not a lot of references to that geometry in where used assemblies and drawings so the risk is very low. So long as I change from region back to profile selection once things are fixed. This is similar to what I did in the most recent case of trying to apply Dimple feature, I was playing around with the tool body to find what caused the Dimple to fail or not. I found that checking the "Cut" checkbox would allow the feature to build so I could save the dimple feature edits. Then I could return and uncheck that box after editing the tool body for example. Good suggestion to find things to temporarily tweak in the feature to get it to build.

[JSculley]

We avoid using regions. Testing that we have done indicate they lead to more changes in geometry IDs when editing the profiles.

Absolutely. This is just a means to allow you to create the feature that will fail otherwise while you go and fix the problem. I made extensive use of regions on one model years ago and it was a nightmare that I never wish to see again.

[matt]

I requested this enhancement many times in the past, which might be why it never made it into the software. Complex fillets, lofts, take a lot of clicks to set up. And when they don't work, it becomes a research project. Failed features would also be helpful for macros.

SolidWorks users have always been afraid of errors. In asseblies, errors are often automatically hidden because in general, a lot of users just don't deal with errors. Sw chased the ease-of-use rabbit so hard that for a lot of users, errors were just too much to deal with.

[Frederick_Law]

We avoid using regions. Testing that we have done indicate they lead to more changes in geometry IDs when editing the profiles.

SW lost track of which one is which when number of regions changed (add or delete in the sketch).

[Dwight]

SolidWorks users have always been afraid of errors.

Yes. I hit that wall hardest in sheet metal, when I've made extensive changes in a flange sketch and then have to dump the sketch if it causes an error.

Dwight

[SPerman]

This was timely (and unintentional.) I created this sketch (with an unintended self-intersection), attempted an extrude cut and got this error:

No problem, I thought. I can just select a region.

image.png (4.01 KiB) Viewed 352 times

So I'm back to cancelling the operation, fixing the sketch and trying again.

[JSculley]

This was timely (and unintentional.) I created this sketch (with an unintended self-intersection), attempted an extrude cut and got this error:

image.png

No problem, I thought. I can just select a region.

image.png

image.png

So I'm back to cancelling the operation, fixing the sketch and trying again.

image.png

You can just select both the large region and that little triangular region and it won't error.

[bnemec]

Absolutely. This is just a means to allow you to create the feature that will fail otherwise while you go and fix the problem. I made extensive use of regions on one model years ago and it was a nightmare that I never wish to see again.

Ok, good to know. I see regions mentioned now and then and I wonder if we were just using them wrong causing geom ID to change more than they should or the other's use case didn't care about updating where used.