Model states, Engraved text, drawing views

[terry.nicholls]

Hi, 

I have an ID plate I wanted to use model states to create the iterations of ID plates. Its the same design to be engraved with different details. Problem is you can't use text user parameters that change between model states. So I had to create a custom property that writes to a parameter which is used in the text.

I have got it to change text with the model state change using a basic rule that just has user parameter = custom property. On event trigger model state change.

To get it to update I had to create a second rule the runs after on  model state change to force the model to update. It works in the model and changing states updates the engraved text.

But when the model is inserted into a drawing view they just show the active view in the model not the text for the model state selected.

In the drawing the iProperties have updated for the part with model state but the geometry hasn't.

Any idea how to get this to work?

[pcrawley]

It looks like one of those (increasingly rare) cases where "iPart" beats "Model States".

I think I read somewhere that Model States don't yet support text parameters.  And that's a shame in this case!

I wrote this iLogic rule (trigger it on "Model State Changed as you did previously) which writes the name of the current Model State into the text parameter called "Label".  You never know, it might be useful in the future!

Dim oModelStateName= ThisDoc.Document.ModelStateName
Label = oModelStateName
iLogicVb.UpdateWhenDone = True

[mcgyvr]

Maybe I'm just a simple man but why can't each different version of the text just be a new sketch/emboss feature and you suppress all the others in each model state? 

No need for ilogic or any other hoops to jump through..

[terry.nicholls]

Thanks for that. "iLogicVb.UpdatedWhenDone = True" simplifies things a bit and does away with needing a second rule just to update the model.

[terry.nicholls]

Thanks for the suggestion, I was trying to avoid having multiple sketches and features to keep the model simple. The model gets heavy very quickly when you add a lot of engraved text. There is potential for this model to contain 50+ iterations of serial numbers so I wanted to be able to use the model states table. I would also make it easy to add new iterations. I might just have to convert it to an iPart and do it that way instead.

[pcrawley]

A new sketch/emboss feature works, but if the OP needs 100 labels - or 1000? 

1000 features is a very long model tree.

Alternative questions might be:

• Why do Model States only support numeric parameters?  iParts support all types.
• Why can't you insert iProperties into model sketch text?  You can in sketches on drawings.

They're frustratingly difficult to discover inconsistencies.  I empathize with the OP because I've had to do the same thing with 15,000 parts embossed with a unique number.  That was solved by using iLogic to directly update the Emboss feature's sketch text.  Might have to look that up if the OP doesn't find an alternative solution.

[terry.nicholls]

Thanks @pcrawley 

Either of those questions would solve the problem. I'm running into similar problems with iParts, I can't get it to pull user text parameters, and you can't export text parameters to custom properties or insert iproperties into text in parts.

I have spent to much time trying to get this work so I will just do save as for each iteration in this case. It has come up a couple of times in our office that someone has wanted to do this.

There is an Ideas station post for adding text parameters to models states already. 

Model States: Capture Text parameters in the Model States table - Autodesk Community

And for and adding iProperties to model sketch text

In Sketch: Access to iproperties of parts and rotation, in text dialog box. - Autodesk Community

[pcrawley]

@terry.nicholls - Your mouse-clicking muscles will get a good workout!

You can copy and paste from an Excel column into Inventor's multi-value parameter editor box to simplify the data entry.

If you need a model of every label, use "Place iLogic Component" (hidden under "Place") to place the label part into an assembly.  "Place iLogic Component" creates unique instances of the part and prevents many "Save Copy As" functions.  You also get to pick the multi-value parameter at the time of placement.

[johnsonshiue]

Hi! Folks,

Let me clarify one thing. iPart, iAssembly, and Model States as of 2022 do not support text parameters on the table. You will need to leverage custom iProperties and iLogic to facilitate the text configuration.

This is an enhancement on our radar. We are working on a solution but it is not available on any currently released products. Please sign up Inventor Feedback Community (https://autode.sk/InventorBeta) and try out the latest internal build.

Many thanks!

[pcrawley · Accepted solution]

Happy Monday @terry.nicholls 

New in Inventor 2023:  https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-3434F58E-26A3-42DA-933C-C8984FE8F6E7

And...

 Mark Command, a new feature command for standard and sheet metal parts.

• Use sketch text or geometry to add marking features to your models.
• Use Mark Styles to control the modeling and export properties of Mark features. Use the Styles and Standards editor to manage Mark Styles.
• Export to specific layers in DXF or DWG files.

[terry.nicholls]

Morning Peter,

That's great news. Thanks for following it up.