Custom iProperty in idw STYLES

[cadman777]

Hi All,

This is a long-standing question I've had since 2010.

I'd be grateful for an answer.

Can a macro be made to input a Custom iProperty here in my DRAWING TEMPLATE?:

Manage>Styles and Standards>Standard>(click on the name of your standard)>View Preferences>Display>Edit View Label (the Pencil icon)>Type (dropdown) - no Custom iProperty is available there. I want to insert the Custom iProperty into the Text Editor as a line-item. See here:

Much obliged!

[pball]

If you're referring to custom iProperties from models I've only figured out one way to do that. If you insert a model into your template file and add the custom iProperties from that model you want, the model can then be deleted and the template saved. When you create a new drawing and insert a model that property will relink with the new model.

If you edit the template that custom iProperty value won't be editable unless you insert a model again.

[cadman777]

Hi Pball,

Thanx for your reply.

I did do that many years ago, and didn't get any results.

So I must be missing something in the process.

Would you please show me where you "add the custom iProperties from that model"?
I don't know what you mean by that.

Thanx!

[rhasell]

Hi

I don't think you can do that in the styles editor.

Play around with the following code, I extracted a small section from my code, it should help you on your way.

My label format is different to yours, but I left some of the formatting etc for you to get an idea of how it works.

But the main thing is your custom iProperty entry of "SIZE" that should work for you.

Sub Main oView
Dim oSSet As SelectSet = ThisDoc.Document.SelectSet
If oSSet.Count = 0 Then
oView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select a View") 'Added Rev2
oSSet.Select(oView)
End If
oLabel()
End Sub

Sub oLabel
Dim oSSet As SelectSet = ThisDoc.Document.SelectSet
Dim oView As DrawingView= TryCast(oSSet.Item(1), DrawingView)
oModel = ThisDoc.ModelDocument
If oView IsNot Nothing Then
oView.ShowLabel = True

o_iPropID_SIZE = oModel.PropertySets.Item("User Defined Properties").Item("SIZE").PropId

	 oStringSIZE = "<StyleOverride Underline='True' FontSize='0.5' Bold='True'><Property Document='model' PropertySet='User Defined Properties' Property='customPropertyName' FormatID='{D5CDD505-2E9C-101B-9397-08002B2CF9AE}' PropertyID='" _
	 & o_iPropID_SIZE & "'>customPropertyName </Property></StyleOverride>"
 
	oStringTXT = "<StyleOverride Underline='True' FontSize='0.5' Bold='False'> OFF - AS SHOWN - MARK AS - </StyleOverride>"
	oStringScale = "<Br/><StyleOverride FontSize='0.25'>SCALE <DrawingViewScale/></StyleOverride>"

'add to the view label
oView.Label.FormattedText =  oStringTXT & oStringSIZE & oStringScale
Else
	MessageBox.Show("The selected object is not a drawing view", "iLogic")
End If
End Sub

[pball]

@cadman777 

When a model view is added to a drawing the Custom Properties - Model option appears. Then it's possible to add those to your text. The model view can then be removed and the drawing saved as a template file. Next time a model view is added those properties will show that models info.

[cadman777]

Pball,

Thanx for your input.

I really don't understand what you're saying, b/c that's not how it works with my Inventor software.

What Inventor version do you have?
I'm using 2010.

I don't know of any way to make the Custom Model iProperties get into the view label AUTOMATICALLY unless they are setup in your Styles and Standards. Inventor 2010 doesn't allow Custom Model iProperties to be inserted into the Styles and Standards view labels. And if it's not in the Style, then it ain't gonna be in the label when you place a Base View.

So how in the world does your Inventor version allow this?

You got me curious!

[pball]

I guess the way I'm doing it isn't available in 2010. I've been using this method since at least 2014 so I'm not sure when things might have changed. Sorry I can't be of any help since I don't have 2010.

[rhasell]

Hi Chris

It does not work in the Styles and Standards. I tested it in 2020, the option is not available.

It does however work when you edit an exiting label. (Admittedly, I do not know about 2010)

Try the code, but I am not sure if it works in 2010.

[cadman777]

Thanx Reg,

Let me see if I can hack my way through your code to do something with it.

I got help in another thread on a similar issue from another kind gentleman in this forum.

Hopefully, between the two of you and all the other bits and pieces I've gathered in here, I can cobble together something to suit my needs.

Cheers ...

[cadman777]

Thanx for the confirmation.

This is something Autodesk SHOULD HAVE added to Inventor many moons ago.

Same with using iProperties in Parts List titles.

It's just a simple matter of DATA MANAGEMENT consistent throughout the software.

Cheers ...