New Custom feature: Publish geometry

GregBrown

I'm pleased to announce that my Publish geometry Custom feature is now… published.

https://cad.onshape.com/documents/40d43cad542dccfa4772d7e1/v/856bd2b631f7e35c4a2b34ad/e/788996d08647863b81b2ff61

Like many other CAD systems (Creo, CATIA etc) the Publish geometry is intended to make Top Down Design workflows much more efficient by providing an easy way to collate references (bodies, faces, curves, sketches, mate connectors) needed for certain downstream activities into a single feature. This feature creates a (composite) part that can be Derived into other Part Studios, into the same or other documents.

Because the Publish geometry creates a part, it can be version/revision managed, ensuring that downstream collaborators always are working with the correct references.

The Publish geometry can also be inserted into an assembly to provide a "scaffold" for assembly of other instances. For this reason, the "Exclude from BOM" property is set by default, though you can override this.

Intended usage is for this feature to be used on high level, skeleton (early concept/layout) parts, and NOT at the end of a multi-hundred feature epically detailed Part studio. The reason for this? When a Derive feature is used, it regenerates and carries along with it the contents of the whole part studio. So even if you only "published" one face, it will carry the weight of everything else in the Part studio. Hence it should be used early in skeleton/layout Part Studios where you are laying out the interfaces, the key keepin/keepout bodies, the key csys/datums (Mate connectors!) and so on.

If you do have a complex assembly (either from a an existing native Onshape assembly or a giant imported STEP file) then it can be used in the following way: create an in-context Part studio (ICPS) of the assembly, then in that ICPS, use the Publish geometry feature on only the key references you need! The double good whammy here is that 1) the ICPS will ensure that the Part studio is lightweight, and 2) you get all the benefits of the Publish geometry workflow.

I made a quick video to introduce this:

https://www.youtube.com/watch?v=nWUE4qCElNg

EvanReese

Yes! Thanks so much, Greg. This is a fantastic workflow. I was hoping you'd release your version eventually.

MichaelPascoe

Woot! Thanks for this Greg. Looks awesome.

John_Arb

I love this custom feature and it has solved a big workflow issue. It also makes deriving parts much less of a headache trying to dig through the standard menu and find what's needed. However I am also finding some limitations when using it. I think most of this stems from the resulting derived geometry being a "closed" composite part perhaps?

Being able to select a singular surface vs. faces would be handy (this could be a problem with the surface model i assume.).

I cannot select or use curves if they match a surface edge without using the "select other"

The sketches also get grouped as one singular sketch which makes it difficult to filter through.

There may be other work arounds for this that I'm just not aware of yet.

Thank you @GregBrown for putting in the work to make this, it really is a powerful feature.

MichaelPascoe

So what are the main benefits of using this feature when comparing it to the native Composite part feature?

GregBrown

https://forum.onshape.com/discussion/comment/119253#Comment_119253

1. you can’t include sketches in a regular composite part, or mate connectors.
2. The feature creates a single composite part of all the references and automates a couple of other handy steps for the workflow

Basically #2 adds convenience and encourages a good workflow. #1 is not doable in any other way. Unless you write your own custom feature.

GregBrown

https://forum.onshape.com/discussion/comment/119248#Comment_119248

John, thanks so much for the comments! Glad it can unlock some workflows for you.

Regarding the limitation you mention, this is intentional in order to reduce the clutter, and reduce the derive to only need a single part. More specifically, the idea behind this all is to create a single "skeleton" part that has all the references you need for a particular downstream activity, a specific function, or that a certain collaborator would need. A classic use case is where different functional areas of the model are going to be addressed by different folks, in different documents. Think of chassis design, versus powertrain design, versus interior, etc. They will share certain common references, but also have some of their own. In other words, feel free to make multiple Publish geometries with the curves separated into their own groups… These can be named appropriately (like in the custom feature's test part studio) and thus there will be multiple Composite parts in available for downstream use as necessary.

As for sketches, I deliberately used the reference to a whole sketch feature. If you want to peel off a subset of entities from a sketch, or indeed choose a surface edge (like the edge from a face blend) then you could first create a Composite curve of the individual edge(s), then select these curves for the Publish geometry. They are always associated to the original geometry, and will update properly.

eric_pesty

Haven't played with it yet but that looks really useful (a couple weeks too late to use on my current project!)

One thing I don't see and I think could be handy is the ability to include variables…

I know you can use variable studios but if you are going to use configurations (which would work for a "publish", that's not an option… You could also use this to derive in measured variables or "strings" to use in downstream features.