What is the easiest way to make two identical parts with different sized holes at one point?

RChilcoat

I'm a neophyte, although I once was fluent in SDRC Ideas.  I'm designing a mechanism to help learn this new software.  The mechanism has two concentric shafts, and two nearly identical cranks.  The only differences between these two cranks is the size of the hole that attaches to the shaft ends.  Since the shafts are concentric, one crank has to have a different sized hole to account for the concentricity of the shafts.  I would like to be able to adjust the length of the two cranks at a later time to adjust them to fit later parts of the mechanism.  I've designed one crank "In Context" using the assembled concentric shafts, but when I try to sketch the new crank In Context  using the first crank as a pattern, it makes the relevant hole the same size as the first crank, and I cannot figure out how to make it fit the smaller shaft.  I would like to be able to adjust the new crank length on one crank and have it change the other length automatically.  Is there a better way to do this?  Thanks.

michael_mcclain

Can you share a link to the document in this thread? I think I understand you, but I would like to see it to understand. I think what you are referring to could be done using a configuration and changing one part in the assembly to a different configuration from the first part. Here's a video explaining them:
https://www.onshape.com/videos/introducing-onshape-configurations

RChilcoat

I believe this link will let you see what I'm trying.  https://cad.onshape.com/documents/8fa0b6717471c2cb96e829f5/w/e6d4854c8f833a45a9519975/e/512032ff7d1ff3f1cb32536a  I would like to continue to use In Context sketching because I believe at some point I can specify clearance between the mating parts.  Thanks for your help.  This is a terrific program, that I would like to teach at our local high school.  I need to get very much more conversant with it before I can do that.   

michael_mcclain

I'll check this out in a bit. You can also look into the Onshape educator program for teaching it at your high school

michael_mcclain

Also, if you are learning the program I would suggest to look at the video library and also the learning center: https://learn.onshape.com/learn/dashboard

kevin_o_toole_1

@RChilcoat
I don't have permission to open the document you shared (could you make it public?).

Regardless, I think this is a really informative use case for configurations. So I whipped up an example on how you could use configurations to solve this type of problem in this document:
https://cad.onshape.com/documents/c465a6b998854e12d5b373ed/w/0fa1d54a1394f41db2e3fc84/e/a1d1e67e4a65f3ebcd8b0949

The document has two different strategies for modeling the two cranks. The first strategy uses configurations and In Context editing both together, and the second strategy uses just configurations.

Configurations + In context
For this design (the "Cranks (In context)" folder), I did the following:

1. Create a crank with two configurations: Large hole and small hole, and model the cranks without the hole.
2. Assembled the cranks and the shaft, making sure to add one of each configurations, and mate them in place
3. Edit the first crank in context, add a boolean with offset to create the properly sized hole.
4. Right-click the "tools" in the boolean feature and click configure. This allows the tools to be different in different configurations
5. Edit the second crank in context. This takes you back to the Crank Part Studio in the other configuration. Edit the boolean, delete the old tool, click the shaft in the new context
   

And voila! You have a configured shaft whose geometry is dependent on two different assembly contexts, one for each configuration.



Just configurations
For this design (the "Cranks (In context)" folder), I changed the hole size with a single configured dimension.



If your hole is simple, you could model this hole directly in the configured crank's Part Studio and configure the size of that hole.

However, my hole was complicated. I did the following:

1. Use derived to bring in all the shaft's geometry, and do a boolean subtract with offset (just like we did in the in context case).
2. Next, I utilized the fact that the shaft itself was configured. Right-click to configure the "Shaft diameter" input on the derived, and, in the table on the right pane, set the shaft diameter it to the two values needed for the assembly.

This is a pretty interesting design. The only thing controlled by the crank's configuration... is the shaft's configuration!

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In both designs, the crank geometry is defined once, and the shaft geometry is defined once. Making a change to that base geometry will update all configurations and all assemblies.

Additionally, in the "No context" version, the crank will update automatically if you change the shaft.

In the "In context" version, you will need to manually update the two contexts in order for the holes to update. However, these updates could let you make changes to the design that are more aware of the full assembly (like, say, changing the angle between the crank and the shaft).

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Now... I built this document based off of my interpretation of your description, since I thought it made a cool example of Onshape's newly release configurations. My interpretation is probably off, so please share the document to let us see your real use case!

Configurations are an extremely flexible tool in Onshape's toolbox, so I'm confident we can come up with a good solution for your case.