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Sunday, April 14, 2013

Linking Parameters from One Part to Another in Autodesk Inventor

“New links must be forged as old ones rust”
Jane Howard

Last week, I was asked "Can you link parameters from one part to another in Inventor?" 

I had to think back a bit.  It's been several years since I had used this method, but in short, yes it can be done, and this is how to do it.

First, I have two parts, a shaft, and a base that contains a bore shown in an assembly file.  The shaft has a dimension that may vary, but I know the corresponding bore has to be .025 larger than the shaft.  I'm purposefully keeping the clearance large so the change is easier to see.

 Looking at the image below, it's easy to tell that the clearance is far larger than .025.  I'll use parameters to like the diameter of the bore to the diameter of the shaft.


The shaft and bore.  The dimensions are unlinked.

The first step to perform is to edit the shaft part, and rename the parameters that define the shaft diameter.  This step isn't really necessary, but it does make the parameters easier to work with.  I'm also going to check the "Export Parameter" check box.

Parameters are located on the "Manage" tab. 

Preparing the Parameter for use.
With the shaft parameters prepared, finish editing the shaft, and start editing the base.   Edit the parameters for this component as well.  Note that the parameter for the hole diameter has already been given a unique name.

Showing the parameters for the bore.
The first step to linking the two files together is to click on the "Link" button.

The "Link" button is in the lower left of the parameters box.
This will cause the Open dialog box to appear.  Change the file type from Excel files, to Inventor files.  I'll select the Shaft.ipt part, and click "Open".

Opening the file to link.

The Link Parameters dialog appears, this is where the parameters to be linked can be selected.  Although multiple parameters can be selected, in this case, only the parameter Shaft_Dia needs to be selected.  Click on the icon so a yellow "+" symbol appears.




Selecting the parameters to link

Clicking "OK", the parameter will be linked into the file containing the bore.  The parameter will appear in gray, at the bottom of the parameters dialog box.



The parameters are added.

Now, an equation can be built using this parameter, adding the clearance of .025 inches.  The image below shows the equation created in the parameters dialog box.

The equation created.

 Closing the dialog box will reveal that the bore as already sized according to the new equation that's been added.  In the image below, the assembly has been sectioned, and the shaft made flush with the bore to make the gap more visible.

The gap added.
The real strength of this method, is when the shaft is re-sized.  Since the shaft and bore diameters are linked, the dimension of the shaft will change the diameter of the bore, while maintaining the clearance!

First changing the size of the shaft.

Changing the parameter. The shaft has already updated.
Finishing the component edit will reveal that the bore has updated while maintaining the clearance.

The bore re-sized.

This application can be very helpful in dynamic designs where component dimensions are going to change often, and a little bit of "light automation" can be helpful. 

Where is that case to be found?  That's up to you! 

For a video showing the steps used above, look below! In my video, I used .015 inches for the clearance.  But the ideas are still the same!




16 comments:

  1. Anonymous11:26 PM

    Clear and clever explanation. Thank you!

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  2. I tried to link a parameter from the assemblie in a part file (it's OK) and then insert the part in the same assemblie, but I got a error "cyclic reference". I want to drive the dimension in the part from a positional relationship in the assemblie, is it possible?

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  3. I tried to link a parameter from the assembly in a part file (it's OK) and then I inserted the part in the same assembly , but I got a error: "cyclic reference". I want to drive a dimension in the part from a positional relationship in the assembly, is it possible?

    ReplyDelete
    Replies
    1. Fernando, it might be trying to recreate the same parameters in the same place, which would explain the cyclical dependency.

      One thought might be using a separate *.ipt file to drive the parameters into the parts, or possibly an Excel spreadsheet.

      Delete
  4. hello sir very nice blog really helped .. i need some help sir
    i need to link excel sheet for sheet metal part but the parameters which i mention in excel is not linking .. can i know wt should i mention the excel spreadsheet so dat my data ll link to fx .. i gave flange length . but it only recongnising bend radius n so .... plzzzzzzzzzzz help

    ReplyDelete
    Replies
    1. Thanks for the comments!

      I'm afraid I don't know what could be causing it "sight unseen", but you might try this blog post here: It's got some nice instructions that might help locate the error.

      http://inventortutorials.blogspot.com/2011/08/using-and-understanding-linked.html

      My first thought is perhaps the starting cell isn't correct, or maybe there's a problem in the formatting of that particular field. You might look for a unit error, or perhaps a special character causing a problem in the field.

      Delete
  5. Hi Jonathan,

    I have successfully been linking parts to make dynamic assemblies for a while now. Do you know how to break the link between parts? The reason I want to do this is because I want to use one of my parts in another assembly but when I do the part looks for the reference part from the previous assembly. you can skip this but the the part shows up as unresolved in the new assembly.

    ReplyDelete
    Replies
    1. Shaun, in the part you derived into, have you tried right clicking on the browser name and choosing "break link". That should do it. You may have to click on the node under the name. I'm afraid I'm not in front of my computer, so I'm recalling this from memory.

      Delete
  6. None of the parts are derived. They are standard sheet metal parts that are linked to parameters of one part in an assembly. I want to copy a flange from the original assembly to another assembly and link it to another part. The reason I want to use this flange and not create a new one is because I have some useful i-logic embedded in it. When I link it to a part in the new assembly it works fine but the flange is unresolved in the browser.

    ReplyDelete
    Replies
    1. Shaun, I assume the flange is part and not a feature with the Inventor flange tool? Making sure. Wrong assumptions can be easy to make.

      I'm not sure I completely have my head around it (it's 4am in L.A.). But it are you trying to link one part using iLogic from another, different part? I'll try peeling back a layer at a time.

      First, when you state "When I link to another part in a new assembly, it works fine, but the flange is unresolved in the browser." How are you linking the part? Placed Component? Linked parameters? Is there even a chance your project file needs tweaking.

      One other (perhaps random) thought, have you considered making your iLogic rule external? It might make sharing the rule a little easier.

      Delete
  7. Thank you very much for a very helpful video.
    The explanation was wonderful.
    Thanks again

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  8. Is it possible to get this to work for 2 parts that have configurations in them?

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    Replies
    1. Yes. It is possible, although if you change the "parent" part, both children will change to match the new values.

      Delete
  9. Is it possible to get this to work for 2 parts that have configurations in them?

    ReplyDelete