Using "User Parameters" in BOM.

[Anonymous]

Good day,

Not sure if this is the right forum to ask this question, but here goes...

I am creating an assembly of a movable hopper with a mixture of part types, i.e. platework (not sheetmetal), structural steel sections, mechanical components (shafts, spindles, etc.), fasteners (custom ipt parts, not content centre parts) and vendor parts (mainly imported step files converted to IV and shrinkwrapped where needed).

With all these different types of parts in my assemblies and sub-assemblies, I created a User Parameter in the Parameters function at part level, with multiple options covering these different types.  The user then as part of the part modelling, selects the correct type and save the part.

I would like to add this "User Parameter" to my Bill of Material in either my 3D assembly or in my drawings that we create for fabrication and construction.  Google and searching here have not been much help and the "User Parameter" do not have an "Export" function as the "Model Parameters" have.

Anyone that can point me in the right direction please?  I will be most grateful.

Regards

Kobus

Inventor 2018 / AutoCAD 2018

[clutsa]

I would recommend using an iProperty instead of a user parameter (maybe even the category) those are easily added to the parts list or BOM. 

[omartin]

Where are you trying to export the parameter? going into the fxParamters, user parameters do have the option to export

[Anonymous]

I tried but one can only Export numerical User Parameters, and I need to use multiple values like Mechanical, Structural, Platework, Fasteners, etc.

Thanks for your reply anyway.

Regards

[Anonymous]

OK, accepted.....however please humor me, I have kids that are millennials.  Can you tell me how to use the iProperty to set this up and get it into my BOM.  I have created custom iProperties in the Custom tab, but somehow am missing the boat to get it into my BOM.

Regards

Kobus

[clutsa]

In the model "BOM" if you right click on the headers there's a "Runtime Column Customization" but I don't see any custom iProperties in there... I'll look into this if you want, let me know if that's what you need.

For the "parts list" (often called the BOM) on the drawing  double click the list and in the top left corner click on "Column Chooser". If your iProperty isn't listed click the "New Property" button below the list and type in the name of your custom iProperty. Click "OK" until you're back at your print and you should see a new column with your data.

[Anonymous]

Thanks again for your quick reply, I am going to try this and see what the results are.  Will let you know what I got right (or not) tomorrow.

Regards

[JelteDeJong]

it is possible to export a string parameter value to a custom iProperty by using an iLogic rule.

like this:

iProperties.Value("Custom", "MyPropertyName") = MyMultiValueParameterName

[bshbsh]

https://cadsetterout.com/inventor-tutorials/autodesk-inventor-creating-coordinated-bom-for-large-ass...

[Anonymous]

I ran into the same issue (you cannot export a text user parameters like you can numerical user parameters). The solution that worked for me was a single line of iLogic code, like "hjalte79" suggested. This allows you to flip your text parameter into a custom iProperty. After the custom iProperty is created by the iLogic rule, it can be used in other iProperties or even exported into other files just like any other iProperty.