In context edits don't update when configuration changes

david_brophy

I have a drawer front that can be various widths. Latches on either side need a complex recess routed into the wood. I've positioned the latches in the assembly, then used in-context edit to cut the recess. This works great, until I change the width of the drawer-front by changing the configuration variable. The recesses are now in the wrong place. I've made a simplified demo:

https://cad.onshape.com/documents/6b3201709c47974d980be713/w/ea2c99aee6826c0087e36cbc/e/785d95cc34fdef7dcd38a873

chad_schmidt

I tried a little different approach.  I know this doesn't help you much but it didn't work for me either.  I don't think in-context and configurations works very well in OnShape.  No matter what I do I still had to update the context.  Hopefully someone can explain how to do this correctly.

https://cad.onshape.com/documents/aa96484937e4b35f1a7bcc1a/w/6208b1d9e94f9a42f046f598/e/4613c58510384a1dfb09964e?configuration=default&renderMode=0&uiState=660f01f6c6a1e66a0e340230

NeilCooke

That's really the whole point of in-context editing, it only updates when requested.

david_brophy

People have suggested adding a different context for each variation... I tried this with my 10 variations, and it turned into a giant mess... Now I have to update ten contexts every time there's a change. 🤔

NeilCooke

I wouldn’t do that. Could you not just put the cutouts for the latches in the part first then assemble the latches into them? Then there would be no need for in-context at all. 

dirk_van_der_vaart

Have look at Assembly configurations
https://cad.onshape.com/help/Content/assembly_configurations.htm?tocpath=Assemblies|_____6

david_brophy

NeilCooke said:

I wouldn’t do that. Could you not just put the cutouts for the latches in the part first then assemble the latches into them? Then there would be no need for in-context at all. 

The cut-outs for the latches are complex:

https://cad.onshape.com/documents/16dd5c53137283ef24438b7c/w/36da66510257517b8f92b61b/e/338da39250746a962d89c618?renderMode=0&uiState=6611f60da802425600ccee47

The cut-out is defined by the hidden "Recess" part, which I use with the boolean feature to cut out material from the shelf.

dirk_van_der_vaart said:

Have look at Assembly configurations
https://cad.onshape.com/help/Content/assembly_configurations.htm?tocpath=Assemblies|_____6

I'm not sure how assembly configurations will help things?

eric_pesty

@david_brophy
You already did the hard part with creating the part to boolean from the shelf. Now you just need to derive that part into your shelf part and transform it (by mate connector) to be offset the correct distance from the end. Or use the super derive to derive and locate in one step...

Like this:
https://cad.onshape.com/documents/b9a1b78d24da28b71b9dd10b/w/2b4e1bc0b6f818e30d16ffd7/e/c027b7fd4a12c00a59e14e88?configuration=length=0.129+meter&renderMode=0&tangentEdgeStyle=1&uiState=6612cccb34b161494406371e

In context definitely not the best option in this case.

david_brophy

OK cool I'll try that. I hadn't thought of deriving and simply translating it. I guess by tying everything together with explicit mate connectors, the recess and the part can be aligned identically. 

david_brophy

That worked great. Super Derive is awesome. Problem solved! Thanks very much Eric!