Best methods of linking parameters across files.

[cratesW8UTY]

I have been given access to Inventor to learn at work.  My goal is to use linked parameters to make constructing crates and conforming them (and their interior braces & panels) to the size and relevant contours in a more automatic way.  So far I have discovered 3 methods:

1) Linking files directly inside an assembly files between related parts files.

2) Using an linked empty parts file's parameters to govern the parameters of an assembly between related parts files.

3) Using a linked spreadsheet file to create parameters to govern the parameters of an assembly between related files.

Here is a simple example of what I am working with:

1/2" plywood with 1x4 trim piece.

The goal is to link the parameters of each trim piece so it changes size with the 1/2" plywood or abutting trim piece.

**DISCLAIMER: I am aware that another method of constructing the panel component is to make a series of solid bodies in a parts file.  I am working on becoming familiar with that way also.  I am exploring this method of making each part individually here.**

I would prefer to link parameters of the parts from the Assembly file. This article in Autodesk makes it seem simple to do:

However, the problem I have had with trying to do this is, the cells in the Fx parameters windows in the Assembly & Parts will only allow me to view the linked parameters I bring into them.

But I am unable to write an equation to command the labeled dimensions to conform to the other labeled dimensions.

Is there a way to link parameters across files in an Assembly file? 

Do I have to link the Parts files first?

Is Inventor just not set up to allow linking parameters to be done this way?

If so, which one works better: using a) the Empty Parts File, or b) a Spreadsheet, to govern linked parameters for an Assembly file.

Thank you, Inventor wizards! 

[kacper.suchomski · Accepted solution]

Hi

There is no best method.

The method may be optimal taking into account factors such as:\

• workflow and company standard
• size and complexity of the project
• expected performance and flexibility of the project (at the expense of prior investment of time and effort)
• experience of third parties (e.g. in handling data exchange)
• and many others

There are many connecting methods:

• Linking parameters of files in the parameters window
• Derive prarameters (use Derive tool and select only parameters in the dialog box)
• Base file with parameters
• MS Excel
• iLogic
• Adaptability

The last three are useful if you want to influence the parameters of the part from the assembly perspective.

[Frederick_Law · Accepted solution]

ModelState/iPart/iAssembly

Master Sketch/Skeleton

Derive can reuse parameters and sketch from one ipt.

[jtylerbc · Accepted solution]

---

@cratesW8UTY wrote:

But I am unable to write an equation to command the labeled dimensions to conform to the other labeled dimensions.

Is there a way to link parameters across files in an Assembly file? 

Do I have to link the Parts files first?

Is Inventor just not set up to allow linking parameters to be done this way?

---

What exactly do you mean by the bolded portion?  I ask because that's literally the solution.  You link the parameters (which it looks like you've already done), then write an equation.  

Although looking at your screenshot, it appears that you may have linked the parameters from your parts to your assembly file.  The assembly file does not control the geometry of any of your parts, so this doesn't help you at all if I'm interpreting your screenshots correctly.  Instead, you need to link parameters from one part to another.  Then you'll be able to write the equation as expected.

This would be true whether you link individually from main piece to trim, or have a "master" part holding all the parameters.  The links would be from one part file to another, not from part to assembly.  A key thing you may be misunderstanding is that the link is one-way.  So if you link to the assembly, you are providing a number to the assembly itself, not to any of the parts in that assembly.

[cratesW8UTY]

Thank you so much for your reply.  It  really covers a lot of ground.

I will look up all those key terms and practice using those tools. For now, ...

1) Can you explain how I can link parameters across files from the Fx window in the Assembly file (per the example with the 1/2" & trim)? 

  (Which of the methods you enumerated describes that approach to linking parameters? Or closest to it?)

2) Which one do you think would best apply to a series of shipping crate models? 

3) Do you, personally, have a preferred method?

[cratesW8UTY]

Thanks,

I will look up Derived Parameters. Perhaps a more specific tutorial will come up for it. But that looks like it is what I am trying to do, currently.

[cratesW8UTY]

Yes, you are correct in your comment about the bolded portion. I would think that just like you can double click on a part and edit it as if you were in that part's Part file while in Assembly that you could also make adjustments across files though Parameters/Fx. I thought that was essentially what linking parameters was supposed to be. But as you say in your second paragraph, that (apparently) is not how it works (sadly).

Maybe Autodesk could make that possible at some point? I think it would be super convenient.

As for linking across Parts Files, I'll try it again. The 1/2" plywood is the "main part", so I believe it would be best to link from Trim 1 to Side B?

To be clear, by "one way" you mean if I link Trim 1 to Side B then I can only control parameters from the Side B file? And then, the results will show up in the shared Assembly file? If I have it wrong, please fill me in.

[jtylerbc · Accepted solution]

---

@cratesW8UTY wrote:
To be clear, by "one way" you mean if I link Trim 1 to Side B then I can only control parameters from the Side B file? And then, the results will show up in the shared Assembly file? If I have it wrong, please fill me in.

---

That's basically right.  I originally said that in the context of linking to an assembly file, so I'll explain in that context also.  What I meant was that if you link a parameter from a part to the assembly, the assembly doesn't gain the ability to control that parameter.  It just means that the assembly knows what the value of that part parameter is.  The assembly can use that parameter (for example, you can have an constraint offset defined as being half the length of your trim piece).  But the assembly can't change the value of the parameter or force another part to match it.

The same would be true if the link was between two part files.  If Part B has a linked parameter from Part A, then Part B can use that value, and thus can automatically adapt to changes that are made to Part A.  But Part B can't edit the value of that parameter in Part A.  Any parameters in Part B that don't come from a link can be changed from Part B, but any that came from a link must be edited in the source file.

The result of the link would then show up in the assembly, as you mentioned.  But the assembly itself does not interact with the link in any way other than showing the result.  The link is between the part files, and would work identically even if the assembly didn't exist.

[johnsonshiue · Accepted solution]

Hi! I think it depends on how this part will leveraged in the future. If this is a specialized part for this particular assembly or this type of assemblies, I will use Derive/Excel Link workflow (skeletal modeling) to link the parameters. If this is a common part and it may be used in different assemblies in different context, I will use an iLogic rule in the hosting assembly to drive the parameters. The parts themselves do not know such relationship.

Many thanks! 

[cratesW8UTY]

Thank you all for your contribution to this complex subject.  I will be studying all of your replies so that I can most fully understand linking parameters.  It seems a bit more complex than I initially thought it would be.  But, I am sure once I achieve proficiency the reasons for the limitations and various methods will make sense.

Much thanks to each of you!  If you have any other thoughts to add, they are welcome.

[cratesW8UTY]

I have been trying to apply what has already been posted here by starting from the beginning.  I now understand that the Fx in the Assembly File is "read only", but that each part can be edited in their own Parts File by double clicking or selecting "edit".  Once, back inside that part's Part File, then the Fx can be accessed for linking parameters between Parts Files; in this case Trim 1 to Side Panel A.

I want to make Side Panel A the Base.  So, I linked the relevant trim dimension:

This Part to Part File link should work (?).  I should be able to define TR1_hor_Height's equation.  I want it to be:

<TR1_hor_Length = SDA_hor_Length>

so that the length of the trim equals the length of the panel.  Then it should show up in the Assembly File.

I have to missing something simple because I simply cannot edit the equation cell.  What's up, wizards?

[kacper.suchomski · Accepted solution]

As my previous speakers mentioned, the linked parameters are for reading and use in equations; however, they cannot be defined.

If you want to use a parameter from file A in file B:

1. Open file B
2. Open the parameters window. Link the parameter from file A
3. Use the linked parameter in the parameter equation of file B that needs to depend on it.

[bradeneuropeArthur · Accepted solution]

Have a look at this link:

https://help.autodesk.com/view/INVNTOR/2024/ENU/?guid=GUID-456388EE-9B7F-442E-B917-B76BDE016FD2

[cratesW8UTY]

Ok, what I have learned is that if I want TR-1 to follow the size changes in Side A then I need to link the parameter from the Side A Part File inside the TR-1 Part File.  I have been doing it the other way around.

In the future, I will explain it to others that there is a Commanding/Base Part and a Responsive/Attaching Part in a linked parameter relationship.  And that the command to define the relationship has to reside in the Fx - parameter's window inside the Responsive/Attaching Part, using clear labels for the desired dimensions.

Also, that this must be done from within each Part File just like any change to the part's sketch, not from the Fx - parameter window of the Assembly itself because it is merely a menu of the parameters it contains from all the Parts Files inside it.

[kacper.suchomski · Accepted solution]

You can also create user parameters in an assembly file and link them to individual part files for use in those parts.

[cratesW8UTY]

That is more what I was more the kind of solution I was asking for at the beginning of my post - how to link parameters from Assembly.  I came across something yesterday that referred to User Parameters and kind of thought that might mean I could program equations to effect an assembly of parts from the Assembly File.  Now you have confirmed it.

I am having trouble finding tutorials on the exact techniques related to User Parameters.  So, any explanation or reference is much appreciated.

I have learned a lot exploring all these methods, though.  Right now I am dialed in on Derived Parts/Model State/Linking Parameters.  But, the User Parameters information would probably be more useful for my immediate goals.

[kacper.suchomski]

https://help.autodesk.com/view/INVNTOR/2024/PLK/?guid=GUID-595F9D8E-9EEA-4446-91AB-830E5BAE548E

[BDCollett]

---

@cratesW8UTY wrote:

That is more what I was more the kind of solution I was asking for at the beginning of my post - how to link parameters from Assembly.  I came across something yesterday that referred to User Parameters and kind of thought that might mean I could program equations to effect an assembly of parts from the Assembly File.  Now you have confirmed it.

I have learned a lot exploring all these methods, though.  Right now I am dialed in on Derived Parts/Model State/Linking Parameters.  But, the User Parameters information would probably be more useful for my immediate goals.

---

Looking at what you are trying to do. Multibody that you use to create your parts. Add the multibody to your assembly hidden so it makes controlling parameters as simple as pushing them from Assembly-Multibody. All the single parts will update.

It works quite well.

[jtylerbc]

---

@cratesW8UTY wrote:

Ok, what I have learned is that if I want TR-1 to follow the size changes in Side A then I need to link the parameter from the Side A Part File inside the TR-1 Part File.  I have been doing it the other way around.

In the future, I will explain it to others that there is a Commanding/Base Part and a Responsive/Attaching Part in a linked parameter relationship.  And that the command to define the relationship has to reside in the Fx - parameter's window inside the Responsive/Attaching Part, using clear labels for the desired dimensions.

---

This is correct.  When you were still having trouble, it was because you had the link created between the correct files, but in the wrong direction.  The way you had it set up, the "Trim" piece would have been controlling, and the "Side A" part would have been following.

Also, good observation on the parameter naming.  When linking parameters between parts, it can be very helpful to give the parameters reasonable names, so you don't have to try to figure out what "d127" is and why you linked it.  It is even more useful if others will need to work in your files later.  You might forget why you linked it, but they never knew.