Assembly-level modifications, post-part studio. Discussion/Question.

don_williams909

Hi all,

I'm a reasonably new user to OS, but have been a Creo user for several years. 
One great feature in Creo is that you can make geometry changes to the assembly that won't affect the individual parts.

I'll explain.  I work for a company that makes high-end speaker systems.  We use 2D Acad to create files of parts that will be imported into CAM software to make files for cutting on the CNC router.

Once those parts are cut, they are assembled/glued together to form a raw cabinet.  That cabinet, now an assembly, then goes through the process of having all the corners radiused.  It is then sanded, prepped and painted.  Then, it is loaded with drivers and crossover and other components. 

My issue: 

What I need to accomplish with OS / CAD:

1. Create files for creating CAM code for individual parts.

2. Create an assembly from the CNC cut parts, and then modify the assembly to show corner radii or whatever else may change, without affecting the individual parts for creating the CAM code.

3. Create a 3D model of the Final Assembly, including imports from other manufacturer's parts into it.

4. Derive an accurate Center of Gravity of the Final Assembly, so that I can add internal hardware and holes for mounting the speakers, based on the CoG.

5. Create a Customer Drawing with the located CoG, and product weight and basic measurements from that accurate Final Assembly 3D model.

With OS, you can't make assembly-level modifications, at all. 

Any changes, like putting a radius on the cabinet affects the parts individually, and then the drawings won't represent the actual shape of the machining of the individual parts.
Critical in our industry, is getting an accurate Center of Gravity (Center of Mass in OS language) of the full assembly, which is used to created rigging and mounting brackets. I have to create a Customer Drawing which gives accurate measurements, as well as the CoG.  In order to get an accurate CoG, every part must be in the model.  I can't make a "dummy" model to appear like what the cabinet should look like, as that won't get me an accurate CoG. 
Making a copy of all the parts and modifying them to get the radii seems like creating a lot more work than is really necessary.  Plus, adding radii to the assembly requires sketches and sweeps to make happen, instead of just adding a radius.  If there was some way of turning an assembly into a part, then perhaps that would help speed up the process.

Has anyone out there encountered similar needs, and have you found any reasonably quick ways of getting this type of functionality to work in OS?

All comments and advice appreciated...

Thanks.

NeilCooke

Hi @don_williams909 - welcome to Onshape!

In this document I created the basic shapes in one part studio, then "derived" them into a second part studio and added fillets. I then assembled the second part studio, inserted a speaker from the public library, then edited the second part studio "in-context" (right click "edit in-context") to position the speaker holes. Shout if you need more clarification.

don_williams909

So I guess the only method available is to copy the original Part Studio and make the changes there.

I guess it works, but not an ideal solution.  One still has to create sketches to add the radii if they affect more than one part instead of simply using a radius command.  Kind of a round-about way of doing it, but it works I guess.

owen_sparks

Configurations on the PS would sort you here.

Config 1 - In condition for CNC

Config 2 - As finished (ie fillets enabled.)

You can then show either config in the assembly.

Cheers,

Owen S.

NeilCooke

@don_williams909 - if you open my doc in the link above, you will see how it's done. This doc will be view only, so you must make a copy first to edit the features to see more detail.

"copy the original Part Studio" - it is derived, not a copy, so when the original updates so does the filleted version (Owen's config solution is also a good one)
"create sketches to add the radii if they affect more than one part" - you can use the fillet tool to add rads to all the parts in one go (something that Creo cannot do). If the fillet crosses two parts you would have to sketch/extrude/sweep just the same as in Creo.

Hope this helps.

EDIT: I changed the second part studio by boolean-ing all the parts together (since once glued they are one part, right?) - now you can use the fillet tool to your heart's content.

don_williams909

NeilCooke said:

EDIT: I changed the second part studio by boolean-ing all the parts together (since once glued they are one part, right?) - now you can use the fillet tool to your heart's content.

So you can merge the parts of an assembly into one part, and then treat it as a part?

Can someone please explain "Configurations"?

ilya_baran

I'd suggest starting with the video on configurations here: https://forum.onshape.com/discussion/7975/improvements-to-onshape-january-2nd-2018/p1

NeilCooke

@don_williams909 I wouldn’t say “parts of an assembly” - when in a part studio they are just parts designed in relation to each other. 

Configurations = Family Tables

NeilCooke

@don_williams909 another way to do this project could be to model the box as one solid, fillets and all, then later reverse engineer it into its constituent parts using derived/delete face (to remove fillets)/split part.