Parameters

[ASchlaack]

I would like to have a user parameter in an .iam and I need that to control certant parameters on parts within that assembly. When I do it i get this error message:

Is there a way to get around this at all?

Thanks.

[Hochenauer]

Could you please post an example where you see this issue?

Thanks,

Gerald

[ASchlaack]

The rails parameter "d303" is linked to "LENGTH_1" from the .iam file. I'd like to be able to change "LENGTH_1" and have that change the rails length or "d303".

Thank you Gerald.

[ASchlaack]

If you try to put the rail into the .iam it comes up with the error.

[wimann]

Hey there Schlaack,

So I'm not sure what you're doing that's causing that message to pop up or how exactly you're trying to transfer the parameter from the assembly into the part file, but to my knowledge this can be done 1 of 3 ways.

1) If your rail is a standard structural shape, then having a frame generated model may be helpful so long as one side of your sketch is similar to the other. That way changing the dimension in the frame-driving sketch will change all the associated rail lengths.

2) Adaptivity. Now I personally do not prefer adaptivity. It's created issues for me in the past so I've tried to work around it as much as I can but it would work. You'd project a work plane, geometric face, or edge into your part file from the assembly and use it to drive the length of the rail.

3) My favorite, iLogic. I've used this code a few times to pass a parameter from an assembly into a part file and I find it to be the best way IMO. I don't know how familiar you are with iLogic but if you wanted to use it, you'd go the the manage tab on your ribbon and select Add Rule. Name the rule as you please. Then in the dialog you would type out something like this:

'

Parameter("15-0000 - 20#_RAIL:1","RailLength") = LENGTH_1

iLogicVb.UpdateWhenDone = True

'

Then you could set up an Event Trigger to run the rule under certain conditions and/or run it manually by right clicking it in the iLogic Browser and seleting Run.

That's my input anyway.

[wimann]

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@ASchlaack wrote:

If you try to put the rail into the .iam it comes up with the error.

---

I hadn't seen this post yet. But the error should only exist if the file your grabbing is also the file you have open. I can't imagine why it would show you that otherwise.

PS. I can't open your rail file. Maybe it is corrupt and that is the problem? My computer does not recognize it as an inventor file.

[ASchlaack]

That's really odd, my computer won't open the rail file off here either.. Well, here's the rail again. Could you do the iLogic to this file for me so I can see exactly what you did? I'm going to have to do this for a few other parts so I'd like an example to go by. Thank you!!

[wimann · Accepted solution]

I still can't open that file. But I've attached a quick assembly that has the short iLogic code in it so that when you change the parameter in the assembly, it updates the part.

Hope this helps.

[ASchlaack]

Will you are awesome! I've spent so muchtime trying to do this. Thank you!

[wimann]

No problem. Glad I could help.

[Hochenauer]

Thanks for providing this solution Will!

I think one other possible way would be to use a skeloton sketch part and drive everything from there through derived workflows.

However, I am not an expert on this topic and was waiting for some internal feedback while you already provided an answer.

Nice work :o).

Gerald

[wimann]

Gerald,

Thank you for the kudos (both literal and written).

I'd like to clarify that I understand the approach you've briefly described in your response. It sounds similar to frame generator but without using that specific tool. Instead it sounds like using the .ipt that contains the skeleton sketch and deriving it into other part(s) to create the individual pieces. And by doing that, your individual pieces will be dependent on the original part containing the skeleton sketch. Is this about right?

Thanks,

Will

[Hochenauer]

Correct.

[johnsonshiue · Accepted solution]

Hi! The reason Inventor pops up the dialog is because Inventor recognizes linking the parameter could violate parent and child relationship. The parameter in this case is in the assembly. And,linking (deriving) the assembly parameter associates the assembly containing the part to the part itself. Please note that the paradigm applies to geometry (solid, surface, and sketch) also. It could create a cycle. As a result, Inventor blocks it from happening.

You may ask why iLogic can handle it. It is because iLogic manages the parameters in a different way. Basically, it operates at each document level and it is able to allow parameters to exchange across different levels.

The skeletal modeling technique can also be used here. You simply need to keep all the parameters in an Excel file or a part file. Then in each assembly or part file requiring to reference these parameters, simply link to this Excel file or part file to Parameters dialog. Essentially, you have one Excel file or part file driving all other part or assembly files.

Thanks!