Is it possible to put a sketch relation from a part into an assembly design table?
ie.
I have a part called "gusset" in an assembly. I want to be able to turn off sketch relation "Coincident1" in "Sketch1" of "gusset" from within the assembly's design table. I tried using "$STATE@Coincident1@Sketch1 @gusset" but the design table complains about the part name.
If I can't do it this way I'll just have to use two configurations of "gusset".
TIA
Yes, that's the way you'll have to do it. The basic rule is that for every geometric state of a component, you need a different configuration. If a part can be round or square, it can't be both round and square in the same configuration.
This will be the rule until SW implements statistical quantum mechanics in the "physical dynamics", in which case the part can be both round and square, but only until you open the file and look at it. Then it will still be either round or square.
Tia,
You can utilize $state@sketch_relation@sketchname in an assembly if it refers to a sketch created in the assembly.
Example in Assem1, I create Sketch1. Sketch1 has 2 configurations: With Coincident and No Coincident. The parameter, $state@coincident1@sketch1 in the design table would be able to control the state of the Sketch1. You would develop the Gusset from these 2 sketches in the assembly by developing a part in context. A Gusset part is probably note a great example of top down design. So if you aready have the part, you will have to create two configurations of the part and control the part in the assembly design table.
You can only go one level down in the assembly design table - unless it is a entity created in the assembly.
Regards, Marie
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