User Defined Functions In Parameter Expressions

[bradeneuropeArthur]

Is this not longer supported in Inventor 2022?

[bradeneuropeArthur]

@johnsonshiue do you have any ideas?

[WCrihfield]

I remember seeing that documentation before, and used it in a few test/sample documents, but never used it widely or heavily.  It is referring to a very specific situation and only applies to VBA.  Basically, as it says, when you have some documents open, and you have the VBA Editor open, you will see document projects listed below the application project.  Within the 'Modules' folder under each of those document projects are two items.  One specifically called Functions, and an empty regular Module named "Module1" (by default).  Apparently the only thing the one called Functions is used for, is to let you define custom logical/mathematical functions that will be made available for use within the Equation box of the parameters in the Parameters dialog of that document.  And there doesn't seem to be a global/external 'Functions' module for an Application Project yet, that would allow shared use across multiple documents.  It's a bit restrictive, but can be useful in odd/complicated situations.

I'm still using Inventor Pro 2021 right now, with plans to update to 2022 very soon, but it seems like this has been there for a while now.  Just not very popular, apparently.  As far I know, the other VBA modules will continue to work as normal, but the other modules just are not exposed for use within the Equation box of the Parameters dialog, like this one is.

[TLoberto]

I am also finding that this no longer works in 2022 (currently running 2022.2.1). However, I did a quick test in 2021.3.3 and found that the behavior works as expected. It would be nice to hear back from an Autodesk employee, indicating if this was intentionally removed or if there's a bug we can expect a fix for.

[Ralf_Krieg]

Hello

Stumbled across this too in 2022.2.2

@johnsonshiue

Can Autodesk please tell if it's no longer supported or how to restore functionality?

[MjDeck]

Sorry about not responding sooner. This has been disabled by default in Inventor 2022 and later, but you can set an environment variable to enable it. It looks like we haven't documented this anywhere.

Create an environment variable named InventorEnableParameterMacros and set it to 1.

You can follow the steps on this page. But use InventorEnableParameterMacros for the variable name and 1 for the value. Then restart Inventor.

[MjDeck]

Note that there's a separate problem with VBA parameter functions in Inventor 2022 and later. A function won't work if it has more than one argument. There is no error message, but you get the wrong result. This is issue number INVGEN-61047. We should be able to fix it soon.

[MjDeck]

INVGEN-61047 was fixed in Inventor 2023.1.

[victoria_ulvangGXUXJ]

Hi, I have Inventor Pro 2023.4 and VBA 7.1.

I'm trying to access the test function from the parameters part (.ipt). It works as expected from the macro but not from the part parameters. Tried both with prefix "VBA:" and without

Any help would be much appreciated

[bradeneuropeArthur]

Have you read this?

https://forums.autodesk.com/t5/inventor-programming-ilogic/user-defined-functions-in-parameter-expre...

[victoria_ulvangGXUXJ]

Yes, but as I understand error INVGEN-61047 is already fixed.

[MjDeck]

Hi @victoria_ulvangGXUXJ , please make sure you have set the environment variable

set InventorEnableParameterMacros=1

The VBA parameter formulas won't work without that.

Also, it looks like you might have problems with the units in your expression. Often you need units conversion to get the correct results. However, the expression should be able to parse without an error as long as the units are recognized.
For more info on units, see the help.

[bill.jiang]

Thank you very much

[bill.jiang]

Another 2 issues must be careful:

1, The parmeter used in the function must be double, not single

2, If the parmeter have been used in the ilogic, the Function also will have problem.