Unable to alter linked parameter in an assembly

[nstalker]

I have created a multi-value parameter in a part and exported it.  I then linked it in the assembly but I am unable to edit it.  I tried using iLogic but it also does not alter the part.  Please see the attached 3 jpegs.  I'm not sure what I'm doing wrong. I have been combing the discussion boards but I am unable to find an answer to my problem.  I'm certain that it just has to do with me not correctly understanding ilogic and parameters.  This is my first attempt at using them outside the tutorials.

[johnsonshiue]

Hi! If I understand this workflow correctly, the parameter source is in the part, not in the assembly ,right? If so, the linked parameter in the assembly will strictly follow the parameter value in the part. Any live linked parameter cannot be changed.

If you want to change the parameter value, you should create User Parameter instead.

Thanks!

[nstalker]

how do you use a user parameter in an assembly to alter a part?

[johnsonshiue]

There are multiple ways to achieve it. Here are a few that are commonly used in terms of parameters linking.

Option A: On the Parameters table in the part, link to the iam file. The exported assembly parameters will appear in the part.

Option B: Create an Excel table with all the parameters you would like to control. Then link it to the assembly and link it to the part. So you can drive the parameter from the Excel table.

Let me know if it works for you.

Thanks!

[nstalker]

Johnson,

Thanks so much for your response!  I tried linking the assembly to the part and I get a message that states "Selected component was rejected since it causes a cyclic dependency."

Also, ultimately I am looking to make a factory asset for roller conveyor.  I was planning on using the parts to drive the width and length of the conveyor.  From what I understand from what you are suggesting, using the Excel table will allow me to change the width and length of my conveyor by inputting different values in the Excel file.  However, that will just change my one assembly.  I would like my assembly to have parameters that I can alter when I insert it in Inventor or AutoCAD as a factory asset.  So I could have multiple instances of that assembly with different parameters.  Could you please point me in the right direction?

[johnsonshiue]

Hi! The reason you are getting "Cyclic relationship erorr" when trying to link an assembly to a part, is because I suspect the part also exists in the assembly. I thought you were just trying to reference an assembly parameter in a part.

I would like to understand your goal more clearly. It sounds like you would like to have a part driving the assembly width. To be exact, the width should be another part within the assembly, right?

Why do you need the part parameter to be linked to assembly? Would it be used to create assembly level features?

Thanks!

[nstalker]

Yes you have explained it correctly.  I want to use the parts to drive the assembly features.  So, for example, I could change the roller length to drive the width of the conveyor and change the leg height to drive the height of the conveyor frame.  How would I do that?

So far I have tried exporting the parameter from the parts but then when I link those part parameters to the assembly the parameters are not editable.  I'm trying to figure out the best practices for this application.

Thanks for all of your time and help so far.

[johnsonshiue]

Hi! I would like to get clarification on "assembly features" here. The "assembly features" I am talking about are the Inventor Assembly Features created at assembly level (Extrude Cut, Revolve Cut, Hole, and Sweep Cut). Are you talking about those? Or, you are referring to geometry on another part within the same assembly?

Thanks!

[johnsonshiue]

Hi! I look at the images you attached to the original post. It looks like the assembly constraints need to be adjusted when the part length changes. Could you confirm that?

If that is the case, there are two ways to do it. Either you change the way the assembly is constrained or link the part parameter to the assembly and reference the link parameter in the related constraints.

I guess it would be easier if you send me the assembly and I can take a quick look to see if there is a good workflow to achieve your goal.

Thanks!

[nstalker]

I am new to Inventor.  I didn't know I could extrude things on the assembly; I thought that all had to be done on a part level.  So my parameter that has a multi-value is on the part level.  By altering this part, I effectively create a different assembly.  I am using al of this in the context of Autodesk Factory Design Suite Premium.  Ultimately I would like to be able to insert multiple conveyors as factory assets based off of one assembly file and then just change the parameters to make them different size conveyors.

[johnsonshiue]

Hi! I think I understand your design requirement better now. Is your goal to create multiple assemblies with various width values? If yes, it sounds like using iPart and iAssembly might be a better choice here. If you need examples or tutorial, please go to Inventor Help and find topics related to "iPart" and "iAssembly."

If you still cannot figure it out, feel free to attach an example what you have so far. I will see how I can help.

Thanks!

[nstalker]

Johnson,

Thanks for the response!  I made my part an ipart.  Now it has two different part numbers for two different values for the parameter that I'm interested in.  Now how do I edit this ipart in the assembly?  I noticed that the part shows up as an ipart in my assembly and the default value (part number) is checked but I don't know how to change it.  

Regards,

Noel Stalker

[johnsonshiue]

Hi! I think you might want to spend a bit time reading through help documentation regarding iPart and iAssembly. You will understand this workflow better.

If I understand your issue correctly, it sounds like the part has been converted to an iPart factory. Go to the assembly browser -> right-click on the iPart factory -> Components -> Replace All -> pick the iPart factory file from disk. Then you will be prompted to select a member. Pick a member. Now the component becomes an iPart member.

As for variation at assembly level, you will need to turn the assembly into an iAssembly. On the author table, use "Table Replace" to control which iAssembly member uses which iPart member.

It is a bit hard to explain clearly in a posting. It is better to go through some documentation first. If you have hard time understanding it, please let me know.

Thanks!

[Anonymous]

I like use excel file to link with the assembly and parts. Open the assembly, edit 3rd excel, change parameters in excel and save it. The assembly automatically updated, and all part files do not neet to be opened.

[nstalker]

Johnson,

Thank you again for your time.  The help documentation is not useful.  Can you send me a direct link to a tutorial or video that goes through step-by-step procedures for using iparts and iassemblies?  I am also having difficulty finding useful information on youtube on this subject in particular.  Thanks!

Sincerely,

Noel Stalker

[nstalker]

MCM - what do you mean by edit 3rd excel?

[Anonymous]

in the assembly, open the linked excel file to edit to change parameters.

[johnsonshiue]

Hi! I think the following link is quite informative.

http://wikihelp.autodesk.com/Inventor/enu/2013/Help/1310-Autodesk1310/1655-Assembli1655/1656-Build_a...

Please take a look and let me know if you have any question.

Thanks!

[nstalker]

Thank you for the link.  I have read through it.  I created the ipart and now I am creating the iassembly but I am unable to select anything but the default value for the ipart (see attached screenshot).  How can I create an iassembly that uses either value 1 or value 2 of an ipart?

[johnsonshiue]

Hi! I am so glad you are able to go this far with the documentation link I sent you. It shows the documentation does help, right?

The first step you need to do is to swap out the iPart factory in the assembly with an iPart member. I still see the iPart factory placed in the assembly based on the image. Go to the assembly browser -> right-click on the iPart factory -> Components -> Replace All -> pick the iPart factory file (the one you convert it to an iPart). You will get prompted to pick a member. Then pick a member you like.

Next, edit  the iAssembly table -> right-click in a row on the table -> Insert a row. In upper left panel of the table, you should see the iPart member node with a subnode saying "Table Replace." Click on it and it will be added to the table as a new column. Then, you simply need to set one iPart member to an iAssembly member accordingly.

Please let me know if it works for you.

Thanks!