Access a part parameter from an assembly?

[kmckenney]

There is a part with a model parameter in an assembly
Is there a way to access the part's parameter from within the assembly?

Thank you.

[pcrawley]

Would a line of iLogic be OK?

Something like:

assemblyParameterName = Parameter("Part1", "d0") 

Hopefully it's self explanatory.  If not, just ask.

Peter

[Logos_Atum]

Hello there,

this adds up to the previous post and shows how the part "single deep rack"

has some of it´s parameters linked to the assembly level of the *.iam file.

Simply add lines like theese to a new iLogic rule and it´s done in no time.

Parameter("single deep rack close:1", "standwidth")=Standwidth
Parameter("single deep rack close:1", "standdepth")=Standdepth
Parameter("single deep rack close:1", "rackheight")=RackHeight

[ic198 · Accepted solution]

Assuming I've understood your problem, you can do this without using iLogic:

- Open your assembly

- Open the assembly Parameters browser

- At the bottom left of the browser, hit the button marked 'Link'

- Change the file type to Inventor Files and browse for your part

- You should now be able to import that part's Parameters into your assembly and use them for driving constraints etc.

Hope this helps

[jtylerbc]

ic 198 is correct.  You can link parameters from a part to an assembly without iLogic, using the Link button in the Parameters dialog box.

What you can't do is go the other way - linking a parameter from an assembly to a part.  If the part is in the assembly, this causes a circular reference, and Inventor will not allow it.  In that situation you must use iLogic to transfer the parameter value from the assembly to the part.

[kmckenney]

Thanks ic 198. That was easier than expected, worked like a charm.

[gconley]

That worked, but the downfall is now you can not change the length of the parameter that you linked to the assembly.

How can you do this and still be able to modify the length of the imported parameter?

[ic198]

You have to change the parameter in the part you imported it from. Open that part, change the parameter, go back to the assembly, update and the new value will link through.

[gconley]

I tried that multiple times and it didn't update, it kept reverting back to the original length.  It won't keep the change nor will it update.

Anything else that I can try?

[ic198]

When I said update, you have to manually hit the button shown below (or the matching one on the Manage tab) for the new value to come through. Sorry if this is obvious and you've already done it, it's hard to judge experience on a forum... It might also be worth saving the part after modifying the parameter, though I just tested a quick assembly and that didn't seem to matter.

If you are already doing that I'm not sure what else to suggest, other than to upload your part and assembly here

[ic198]

In case it helps I've attached my test assembly