Configuration to Chose a Shape in a Sketch

neobobkrause

I have a shape that includes a surface with a pattern of holes. Sometimes I want the holes to be round, but other times I want them to be hex shaped, and so on. Prior to OnShape configurations showing up on our doorsteps, I've managed this set of variations using a sketch that included all the various hole patterns I might be interested in, but set all but the "current" pattern as Construction lines. Something like this...

In all that clutter, you'll notice that the only non-Construction element in the sketch is the hexagonal shape. Changing the hexagon to a Construction, then converting the circle, diamond, or smaller hexagon to be non-Construction will result in the shape having cutouts of those shapes.



My question is how/whether OnShape's new Configuration capabilities can be used to cleanly select the cutout shape of this object. 

- Bob

mahir

@neobobkrause, construction lines are just that - for construction. Someone correct me if I'm wrong, but they don't contribute to the creation of usable contours. You can't currently use configs to switch between construction/solid sketch lines, and I doubt you ever will. You can definitely configure different contour selections, but they need to actually be selectable. To do this, you either need different sketches for the different outlines, or you need to make all the construction lines into solid lines. I'd use the first option. It adds lines to the feature tree, but it makes selecting contours much simpler.

mahir

Here's an example. The config option called "Base Shape" selects between either the square or pentagon contour from the same sketch. As mentioned above, this can more easily be done with separate sketches.

https://cad.onshape.com/documents/57acdfaae4b005c413ed9b6f/w/3fd585a46d3af1b3ba413c53/e/b02ec721136c6121c1a02cc1

owen_sparks

Personally (and it's just a preference) I'd have either:-

Simple method
(i)  An initial sketch with just hole location vertices.
(ii) Individual sketches for each hole type, and select these using configs.

Nicer Method
Make a simple featurescript with a "Hole Shape" drop down list, and then configure that input.

This has the option that you can then use "created by" with an edge filter to add a chamfer to the hole.

Cheers,

Owen S.

andy_morris

The way I would suggest achieving this result is to configure the selections used for the extrude feature.

All you need to do is to add the selection list for the extrude to the configuration input, which will then display the selection count in the table. When you double click on this cell in the table you can change the selections to a different sketch, or you can add or remove regions from the selection list.



See this simple example of configured selections:
https://cad.onshape.com/documents/7e5e83e6885dae5776260b9a/w/2339a1a63af248955ab9d648/e/0d31f7998ae62e42f60df3ff

Andy

owen_sparks

Nice :-) :-)

OwS

neobobkrause

andy_morris said:

The way I would suggest achieving this result is to configure the selections used for the extrude feature.

Yeah, that’ll work. Thanks.

bikr7549

This is a neat way of doing things, but I cannot get my part model to work in an assembly, tho it works fine in part mode. In assy one is correctly config is displayed and the other shows an error 'failed to resolve instance' with no geometry shown. The demo shown above is moving way to fast for me to follow, is there a step by step written down?

I have tried a number of things, all with the same results. 

Thanks

Jake_Rosenfeld

@bikr7549

Could you post the URL of your document?  Then we can take a look.  Maybe these instructions will help:
https://cad.onshape.com/help/Content/configurations.htm

bikr7549

Hi Jake, How do I post the URL, literally copy and paste here the https://... ?

owen_sparks

bikr7549 said:

Hi Jake, How do I post the URL, literally copy and paste here the https://... ?

Yup, more detail here:- https://forum.onshape.com/discussion/9107/forum-post-checklist

O.S.