expose part parameters in assembly

[jonkon]

hi,

i have the following problem.

i design a simple part - an extruded base, so i have a parameter in this part that i can control the extrusion distance - i call this parameter D.

Then i create an assembly and place the part in it.

How can i access the parameter D of the part from within the assembly?

I want to place multiple instances of this part in my assembly and control each parameter D of an instance using an excel worksheet that is linked with the assembly. How can i do it ?

My aim is to design a very simple manipulator. Each link has the same shape but a different length. I want to control each length from an excel worksheet and not from an ipart table.

I want to have only one worksheet that controls the parameters of my assembly such as constraint  angles , and link lengths.

Thank you.

[Steve_Bahr]

You didn't mention which version you have, so I'll assume you have 2010.  You'll be able to do it with previous versions, but I don't remember where the Parameters function is anymore.

In your part file, under the Manage tab, click on the Parameters button. Find the parameter you want to see in your assembly and check "export parameter".  Save the file.

In your assembly file, place your part, then under the Manage tab, click on Parameters button.  Select "link" at the bottom of the pop-up and browse to your part file.  The parameter you selected in your part file will have a little green arrow over it, click on that parameter to change it to "+".

What you've just done is told the part to export a parameter and your assembly to receive it.

Why do you want to avoid using an iPart family?  Make your part into an iPart family, just for fun, then try to do it using a spreadsheet.  Place more than one copy of your spreadsheet part into an assembly and watch your parameters go berserk renaming themselves.  Then try to get your drawing to understand all that spreadsheet info.  IMO, you'll make yourself nuts going the spreadsheet route.

[jonkon]

hi,

thanks for the reply.

i tried to do it this way . I can see the part's parameters but i can't change their values.

However i can do it with rules because i can work with part parameters in the rule editor.

I create some new parameters in my assembly and then i create an iLogic form so i can control them with sliders or textboxes. I also insert a rule button in this form. So when i change these assembly parameters i press the rule's button and this rule assigns their values to the part's parameters that i point to. I think this can be done faster using itrigger.

[Steve_Bahr]

I don't have any experience with iLogic yet, but whatever you said sounds good to me!  Glad I was almost able to help.

[CalvinDay]

I have a tray part that has been brought into an assembly. I did the linking as suggested but the part parameters are not editable. Is it possible to edit the part parameters from within the assembly? Or, what is the best way to do it?

[drguitarum2005]

As far as I can tell, you have to drill down into the part to edit the paramters. When I make an assembly, I always pick/name a part 01 and that has ALL my parameters for the entire assembly. I build all my other parts from those linked parameters. That way when I need to adjust something, I double click part 01, edit its parameter, and all changes.

I agree it would be nice to be able to edit those parameters from the assembly.

Or better yet, it would be nice to be able to set all the parameters in the ASSEMBLY parameter menu and link THAT to all the parts. It errors something about cyclic dependency which doesn't make sense. Oh well, perfect world eh?

[jamieborder01]

Hi drguitarum2005, do you know whether this issue has been resolved in updated versions of Inventor, such as 2016 or 2017? Or is it still only editable through the parts and not through the assemblies?

Thanks

[JimmyDoe]

This is possible to do and I think you can do it in previous versions.

In your assembly, create a new rule. At the top, on the 'Model' tab click on the model parameters or user parameters, depending on which type of parameter you would like to access. Double click on the part parameter you want to control from your assembly. Once it is in the rule dialogue set it equal to a user parameter that you have in your assembly(usually named the same as the part parameter to avoid confusion) Then you can add the assembly parameter to a form and changing that assembly parameter will, in turn, change the value of the associated parameter in the part 🙂

I have attached a part and assembly with the above steps done to control 'LENGTH' 'WIDTH' and 'THICKNESS' I think it should be easy enough to follow. I hope this helps!