Saturday, October 29, 2011

Linking Parameters Between Parts and Assemblies in Autodesk Inventor

Platform: Autodesk Inventor Professional 2011
Level of difficulty: Intermediate

Author: Ndianabasi Udonkang
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This lesson was written as a response to a question asked by an anonymous reader in the lesson: Using and Understanding Linked Parameter in Autodesk Inventor. I hope this answers your question.
At a time in your design workflow, we might want to link an existing parameter in a part file to another part or assembly. This way, changes to the parameter will reflect in the other part or assembly. In this lesson, we are going learn to link an existing parameter in a part to another part or assembly.


For this lesson, I have uploaded the dataset: to a public file server. Download the zip file, and extract the files to the directory of your active project.

  1. Open linking_parameters_shaft_part.ipt.
  2. Go to the Manage tab > Parameters panel and click on Parameters. Examine the existing parameters. The parameters are consumed in the model.
  3. Open linking_parameters_hole_part.ipt.
  4. Go to the Manage tab > Parameters panel and click on Parameters. Examine the existing parameters. The parameters are also consumed in the model.
  5. Our aim is link the Shaft_Dia parameter in the linking_parameters_shaft_part.ipt to the Hole_Dia parameter in the linking_parameters_hole_part.ipt. So that if the Shaft_Dia parameter is changed, the Hole_Dia parameter will update accordingly.
  6. Switch to linking_parameters_hole_part.ipt. Go to the Manage tab > Parameters panel and click on Parameters. On the Parameters dialog box, click Link at the bottom of the dialog box.
  7. On the Open dialog box, change the Files of type to Inventor file (*.ipt, *.iam). Select linking_parameters_shaft_part.ipt and click Open.
  8. On the Link Parameter box, double click the Shaft_Dia to add it to the parameters that would be linked from linking_parameters_shaft_part.ipt to linking_parameters_hole_part.ipt. Click Ok
  9. The Shaft_Dia has been linked to the active part.
  10. On the row for Hole_Dia, click the equation 100 mm and then click the arrow. Click List Parameters and select Shaft_Dia. Click Done to close the Parameters dialog box. Save the file.
  11. The Hole_Dia parameter has been equated to the Shaft_Dia parameter.
  12. Open linking_parameters_shaft_part.ipt. Change the Shaft_Dia parameter to 200mm. Save the file. Open linking_parameters_hole_part.ipt. Click Local Update on the Quick Access Toolbar. The Hole feature updates accordingly.

This method can be used for linking parameters between parts and assemblies and vice versa. I hope this tutorial was useful. Drop a comment you liked this or ask any questions. Have a lovely day.


  1. This is pretty good. It pointed out some capabilities that I was never taught.

    i was wondering, though, if there can be another layer of abstraction here. For instance, I am making a nameplate for a pressure vessel. This nameplate can be used on any number of vessels, so the serial number, the tag number, the number of plates, etc changes for each assembly.

    I would like to be able to place this nameplate model on an arbitrary assembly (which already has all of these parameters defined) and have the nameplate reflect the values stored in the assembly.

    The difference here is that the method described above links to a specific model. If I have to redefine the link for all 30 parameters each time I use the nameplate, I might as well do the data entry manually. It would be great if I could link to "the immediate parent in the assembly", no matter which assembly I use.

    Can this be done? Is ilogic an option?

    1. Hello,
      Thanks for writing. Just saw your comment. I'll give you a full reply soonest. Have a lovely weekend.

  2. Your tutorial was exactly what I wanted.
    But I still ran into a problem.
    I have two parts coupled with parameters as in the tutorial.
    Now I have one part made to a iPart ​​to the width and length to make flexible.
    I have both parts placed in an assy.
    If I change the iPart the other part then it is not updated.
    Am I doing something wrong?

  3. Hello Heijden.
    Your challenge has gone beyond the realm of parameters. You have to use iLogic to solve it. I'm working on the problem, and will reply you when I'm done. Thanks for writing.

    1. Hello,
      It's not necessery to use iLogic, you can simply combine iPart and iAssembly.
      Give some usefull names to dimmensions you want to change in iPart [I'm expecting you've done this already but for sure]. Open your assembly, transform it into iAssembly [same way for iPart], now you have to prepare table of rules, make new line and put there all parametrs you need to determinate part as it should be [length, width, diametr,name of part, description and so on] when you are finished make another line[s] for new variations.
      PS There is only one "problem" Inventor will make one sub folder for all parts you described. In my opinion it doesn't metter. I'm using this way and have no bad experiance with it.
      Hopefully it will help you.

    2. Thank you for the input, Tom.

  4. I was designing a storage cabinet and using multiple parts. Often had to change the parameters and then had to update all the parts! This thought was enough to make me go hunting for solutions and this one is just perfect for me. Thanks for posting this.

  5. can i know why i have a resolving problem when i start to link the excel file to inventor ??
    thanks for help.

    1. Tony. I'm glad that you are learning fast. The "resolve link" problem you are experiencing is caused by the fact that the Excel file is not in the same folder as your project folder. Copy or cut the Excel file into the current Project folder, i.e., the folder where you have your Inventor part/assembly files for your current project. Once the Excel file is in the same folder as your part/assembly files, the "resolving problem" will stop. I hope this helps. If you still have problems don't hesitate to post a comment. Cheers!!

    Now the problem is solve.
    can u show me the step for update the new dimension of drawing with use excel file.coz i not so understand the step?

    1. You are welcome brother. Now, when you make changes to the parameters in the Excel file, save and close the file. Then, return to Inventor. Inventor will detect the changes. On the quick access toolbar at the top of Inventor, you will see Update. Click Update and the Inventor file will update with new parameters that were set in the Excel file. Let me know if this helped. Thanks.

    2. thanks.bro
      and further more,
      how to save the drawing as dxf file???
      thanks you very much bro.

    3. Hello. Could you remind of this later? I'm not with my PC now. Thanks.

  7. ok
    ]how to save the drawing as dxf file???
    thanks you very much bro.

    1. Hello Tony,

      There is no direct way of exporting Inventor files to DXF format. But there is a walkaround. So you have to first, export the file to AutoCAD DWG, then from DWG to DXF. Follow these steps:
      1. In Inventor, go to Menu Browser (the big "I" at the upper-left corner of Inventor), then click Export > Export to DWG.
      2. Save the file to DWG format. Note the folder where the DWG file was saved.
      3. Go to AutoCAD and open the saved DWG.
      3. In AutoCAD, go to Menu Browser > Save As > Other Formats.
      5. On the Save Drawing As dialog, change "Files of type" to AutoCAD 20**/LT20**(*.dxf).
      6. Save the file. It is now exported to DXF.


  8. thanks very much
    u are my teacher now,haha

    1. LOL. Thank you very much. I'm glad that I was of help :)

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