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References to instances

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References to instances

I'm starting a new library of components. I am going to have the following structure typically

Assembly_generic

    PartA_generic

    PartB_generic

and an instance of that assembly will be like this (in table format):

  PartA  PartB
Assembly_INST1 PartA_INST1 PartB_INST1
Assembly_INST2 PartA_INST2 PartB_INST2

   

PartA is a normal part with real dimensions that will be accurately modelled. PartB, however represents a consumable material (glue, shim or similar) so that its dimensions actually should come from Part A as well. Currently I have to define the same family table values in the tables of PartA and PartB, but I'm trying to find a way to define the dimensions only once, at the level of part A or at assembly level. Just to make the design clear and easy to update in the future. I want the partB to be a part because it has significant dimensions and properties for the BOM.

I've tried to define a sketch at assembly level and put its dimensions in the assembly family table, to use them as the master, but it doesn't work (see attached parts). And I think that the same will happen with an skeleton. I have also tried to use notebook params (for the first time) but I didn't get it either...I realised that params cant be used as values of my instance columns... Any idea or a different approach? Is this just not possible?

Thank you!

Carlos

1 ACCEPTED SOLUTION

Accepted Solutions

Re: References to instances

You need to use the 'reference model' column in your 'glue' part family table. This type of column tells the instance of the part which instance of the assembly it should be regenerated in the context of.

 

 

In my experience this can be difficult to get correct if you're copying dimensions using relations, as session IDs will sometimes stay 'stuck' to the generic. I think it will be more robust if you use copy geometry features.

 

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5 REPLIES 5

Re: References to instances

I would question putting consumable items into a family table. Why not use bulk item parts for your glue, sealant, etc. and have them go into your BOM with a quantity of As Required?

 

Assembly family tables can be tricky and consume a lot of time building to get all of the pieces right. I did one of a plastic cable tray that after about 8 different lengths got to be a real pain to maintain and add more instances to. There were 2 main parts, the tray and the cover, but then you had to add nuts to the assembly at certain intervals depending on the length because the tray had posts to secure the cover at intervals.

Re: References to instances

Thanks for your reply. Bulk items are an option but they don't cover all I want ... they will appear in the BOM but they don't have a 3D representation, and I want to define the dimensions of the glue because, in my use case, that is indeed an important part of the design and manufacturing information.
Kind regards
Carlos

Re: References to instances

You need to use the 'reference model' column in your 'glue' part family table. This type of column tells the instance of the part which instance of the assembly it should be regenerated in the context of.

 

 

In my experience this can be difficult to get correct if you're copying dimensions using relations, as session IDs will sometimes stay 'stuck' to the generic. I think it will be more robust if you use copy geometry features.

 

00001.png

 

Clipboard02.png

 

Clipboard03.png

 

Clipboard04.png

 

View solution in original post

Re: References to instances

It is exactly what I need!

Thank you!

 

Carlos

Re: References to instances

If you don't need to have a dimensionally accurate part drawing (which I doubt for glue) I'd use part flexibility.  Volume, mass, and relations that rely on dimensions which reside in the glue part will be updated accordingly to the new "flexed" dimensions.  The BOM will also update accordingly if setup correctly.  This saves the trouble of needing a family table for these types of parts at all.

 

The dimensions of the flexible part can be controlled a few ways but my preference is "by curve length".  I'll normally setup a base sketch in the driving part with curves that I intend to drive the flexible part with.

 

Flexibility can also change parameters and turn features off or on.  It's a very powerful tool.