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How would you configure a multi-feature option?
tom_auger
Member Posts: 129 ✭✭
Hi folks, I've been learning about Configurations and I'm loving them. I noticed a recent improvement / shortcut that allows you to multi-select features that are in a folder by selecting the folder and adding all those features to a configuration. I've also noted there is an improvement request for actually making the configuration suppression toggle at the folder level, which I think is what's needed.
My question then is a workaround. I am wondering whether I'm approaching something the wrong way.
Suppose I design a part that can, for the sake of this example, have multiple different kind of bases or footings - all very different from one another and all requiring many features. So I'd like to add a configuration that lets me choose which of the footings gets created / added to this part.
Currently I can imagine grouping the features for a specific type of footing into a folder and then using the suppression configuration on those features, but if I have 3 different kinds of footings each with a dozen features to create them, thats 30+ features being added to the configuration and that seems, well, a bit silly.
Is there another way I should be thinking about this? Can you suppress an entire part, as in, create each footing, but then suppress just the final part and boolean the one that's left with the orginal part?
Is there another approach? Perhaps using an assembly instead (assuming I can still export the assembly as a single monolithic part for production)
Best Answers
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S1mon
Member Posts: 3,188 PRO
Creating separate parts and using the configuration to control a boolean or boolean operations seems like a possible approach, although it means that all the features are being regenerated which takes more time. If you're concerned about regen time, you probably want to suppress by folder. The trick is that you have to be careful to redefine the suppression if you add or remove features from the folders.
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eric_pesty
Member Posts: 2,049 PRO
You can't "re-derive" something that would create a circular reference.
However you can have a "master" part studio with some layout sketch that has all the shared info for the base and other part. You can then derive that into multiple part studios to drive the design.
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Answers
Creating separate parts and using the configuration to control a boolean or boolean operations seems like a possible approach, although it means that all the features are being regenerated which takes more time. If you're concerned about regen time, you probably want to suppress by folder. The trick is that you have to be careful to redefine the suppression if you add or remove features from the folders.
This sample uses S1mon's description of Boolean with the regen time issue.
https://cad.onshape.com/documents/e1437c11e27dfdbe8eeef114/w/8e22d667f2ff4ead531b4c80/e/f43f46b03336f7bd62d1bcc7
Adding on to @glen_dewsbury 's great example, it's a matter of trading modeling time vs regen time. If you have to carefully redo the folder suppression each time you make a change, that takes a bit more modeling time, but the regen time is lower. If you configure the booleans, it's much cleaner from a modeling perspective, but you lose a bit on regen times.
I tend to favor things that make the modeling tree easier to understand at the expense of regen time, but it depends on your overall environment and needs.
One more thing to consider if regen time is an issue, you can model the "bases" in another part studio and then derive the different ones in for the different configurations. If you then switch to a version for the derive you effectively bypass the regen time for the bases.
Thanks @S1mon , @glen_dewsbury , @eric_pesty ! Really good info here.
I'll have to see about the regen time, which I imagine is proportional to the number of features / complexity of each part. it might not be an issue at the level I'm working at.
@eric_pesty - in your approach, if the "bases" needed to be derived from the original part, or at least use projected elements from the original part to get the dimensions right, is that still possible? Or do things get uncomfortably circular in that scenario?
Like, in Glen's example, for the "Stretch" option - the width of the "stretch" piece is clearly based on the diameter of the original cylinder. If the "Stretch" piece were modeled in its own Part Studio to be later brought back into the original part studio, would it still be possible to base its geometry / original sketch dimensions on geometry from the original part studio?
You can't "re-derive" something that would create a circular reference.
However you can have a "master" part studio with some layout sketch that has all the shared info for the base and other part. You can then derive that into multiple part studios to drive the design.