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Extrude From Vertex?
Maybe I'm missing something obvious, but is there a way to do the equivalent of Solidworks' extrude from vertex?
My Solidworks workflow over the years has evolved where I primarily sketch a few orthogonal layouts early in the model on the default planes, and then extrude from vertices in sketches up to vertices in the sketches. I do most of my extrusion sketching on the default planes, but extrude from/to vertices that are off of the sketch planes. I use this as a way of adding draft in the extrude feature from the tops of bosses or ribs. It's also a way to avoid adding a ton of planes.
I know there are interesting things that can be done with the "second direction" part of the extrude command and the offset option. What I'm not seeing is a way to have extrusion draft reference anything other than the sketch plane.
My Solidworks workflow over the years has evolved where I primarily sketch a few orthogonal layouts early in the model on the default planes, and then extrude from vertices in sketches up to vertices in the sketches. I do most of my extrusion sketching on the default planes, but extrude from/to vertices that are off of the sketch planes. I use this as a way of adding draft in the extrude feature from the tops of bosses or ribs. It's also a way to avoid adding a ton of planes.
I know there are interesting things that can be done with the "second direction" part of the extrude command and the offset option. What I'm not seeing is a way to have extrusion draft reference anything other than the sketch plane.
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So it sounds like @NeilCooke made this tool or feature you liked and used in SolidWorks
Did you know that Neil also made a Screw Boss FeatureScript for Onshape that has draft and ribs for the bosses and chamfer at the top of the ribs and it’s all adjustable
If you don’t have this tool yet, here is the link
https://cad.onshape.com/documents/5738c86de4b06c68b35e68a5/w/6c69df608d3406005d90482a/e/2b06e2e693176a3cc55be614
I've seen that screw boss featurescript. At some point, I'll take a pass at making my own version to create the other boss that accepts the thread-forming screws. There are a bunch of features necessary, and ideally the FS would also have a drop-down for material type to cover the percent of engagement.
https://www.design-engineering.com/the-thermoformed-plastic-boss-a-how-to-guide-141831/
@S1mon - It's been 4 years since your original post, and I'm still not seeing "extrude from vertex" as an option in Onshape. Have you changed your original SWX workflow to accommodate the lack of this option in Onshape? I'm coming from a SWX workflow that's similar to what you had described (start with orthogonal layouts, then extrude from one sketch vertex to another). Please advise, thanks!
There's a "starting offset" in the extrude tool now (added since this thread was started).
As @eric_pesty mentioned, "starting offset" is the key, but you also need to select "entity" from the drop down under starting offset to be able to select a vertex (or other reference) to extrude from. It takes more clicks than Solidworks, but it's at least as powerful. Because it also includes the option to create an implicit mate connector, you can even create new references which weren't there prior to the extrude feature.
One thing that's a bit weird (or is it useful?) is that if you use the direction option, it projects the original sketch to the starting offset along the direction. I would have preferred that it project normal the sketch, and then use the direction from that starting offset. The good news is that the draft option uses the starting offset as the draft reference plane.