remember when a part has been copied but not changed

david_lang457

I am doing a project where I am designing some complex bookshelves to fit a room, and as I am generating things with mirror, transform(with copy) and patterns, OnShape doesn't remember that these are the same item, so when I finally put things into the assembly, the BOM shows each shelf as a separate item, not a couple hundred of the same thing.

I expect the reaction to be that I should just model one in the parts studio and put multiple copies in the assembly.

There are a couple of problems with this approach

1. the number and spacing is determined by variables (including measured variables) in the parts studio, information I don't have in the assembly.
2. I need to use the many copies of the parts for boolean operations
3. setting up all the fasteners for so many parts is quite a lot of work

In some ways, I am looking to gain some of the capabilities that are only available in the assembly (bom, and it would be really nice to be able to insert standard parts in a parts studio, bolts, etc to be able to then reference for clearances)

https://cad.onshape.com/documents/d5a9827f1b61fec371e262ce/v/d5f4f4a88560188774ce6b54/e/902b0119d1ee43890ff53924

glen_dewsbury

Here is a beginning using structured assemblies. Repeating parts in the part studio requires a a lot of regen time and all parts copied will be given individual names and part numbers. Much easier to use subassemblies and a variable studio. You can retrieve variables in a part studio and reuse in the assembly. Overall this seems to be a much more coordinated and easier to deal with. Also you can switch between structured and flattened BOMs. Top level BOM flattened will give a complete material take off including the subassemblies. This method also means hardware is placed in one subassembly and will be multiplied automatically in the next level assy. You also have Booleans are don't do anything. If the parts don't intersect or a least touch the Boolean does nothing.

https://cad.onshape.com/documents/0f5a9770d998c9ab325cff71/w/ed1809b9141ecef20627262f/e/fb8cf6c2c72f2b65213c2792

jelte_steur814

with variable studio's as glen suggests, a variable can be used both in the part-studio and the assembly.

Parsing measured variables from a part studio to an assembly is an open issue in Onshape.

But most often this can be circumvented through the addition of a helper-sketch to drive a 'replicate' in the assembly.
Or (like in your case) the measured variable could be easily calculated by a formula in the variable studio using the other variables iso measured.

david_lang457

how do I deal with things like needing the shelves to cut slots in the vertical sides/back of the bookshelf via booleans?

the image that @glen_dewsbury shows above superficially looks the same, but it's missing the key features needed to be able to machine the parts (the results of the booleans that will make the parts fit together)

I don't see where I have booleans that don't do anything.

I see three

1. spine making vertical groove in the ends
2. shelves making horizontal grooves in the spine and ends
3. trucks making pockets in the ends

david_lang457

in my original, I can suppress the last linear pattern and unsuppress the auto-layout and produce a cut sheet for cutting all the components for one moving shelf from 2 sheets of pluwood, and in this you can also see the slots to be carved on a CNC for assembling everything together

david_lang457

I added a 'show cut sheet' checkbox config to toggle the auto layout on and off. I have to disable the last linear pattern as auto layout can't handle that many pieces (it gives up after about 5 shelves worth)

glen_dewsbury

There was mirrored parts like back to back shelves mirrored that were fine. There was a follow up Boolean that did nothing in the part studio because they had a gap between. Better to use assembly to place 2 of the same shelf.

One place where a Boolean works well is to cut (Boolean/subtract) shelves into end board while editing in context. The slots in he spine can be done at the sane tine and will adjust with the shelves if the spacing is changed.

I made no adjustment for pockets at all but provided a sample for you to study and continue on your own.

https://cad.onshape.com/documents/0f5a9770d998c9ab325cff71/w/ed1809b9141ecef20627262f/e/fb8cf6c2c72f2b65213c2792

david_lang457

hmm, I wonder if you looked while I was editing things.

I see:

extrude a shelf/thicken edges

mirror around the center of the spline (now replaced by a 2 dimensional pattern)

pattern up the spline

boolean to cut all the slots in the spline and both ends. it's not a boolean of the two shelves with each other (there was a point in time where I experimented with doing the spline in two halves, you may have looked at it during that point in time when the mirrored shelf didn't touch the half of the spline)

I think I see how the edit in context does it by creating the ghost shelves from the context that don't exist in the parts studio.

I think this trick is worth a video example :-)

One thing I looked at was using a linear pattern in the parts studio to cut all the slots from a single shelf, but that consumes the shelf and I would then need to create it again. am I missing something?

david_lang457

auto layout doesn't detect these 'ghost shelves' created in the context

david_lang457

I've sent a comment to the auto layout author about that.

david_lang457

a note for anyone looking at this in the future. If you take this approach, every time you change a variable you then have to go to the assembly where you do the edit-in-context to create the boolean and do an 'update context'