ilogic code to capatilize text in title block

[patrick3HNXX]

I am just trying to capitalize the material text in my title block. I have tried using the iproperties and UCase functions to do this, but I am apparently missing something.  

[snappyjazz]

Can you post an example of your code?

[bradeneuropeArthur]

Use.

Property.item("yourname").value =Property.item("yourname").value.toupper

[Ralf_Krieg]

Hello

I would suggest the following:

- Create an iLogic Rule in your Part with following code and run it.

iProperties.Value("Custom", "Mat")=iProperties.Material.ToUpper

 - Add your rule to the event trigger "material change".

- Edit your titleblock definition and add a textbox with your user defined iprop "Mat".

[patrick3HNXX]

iProperties.Value("Design Tracking Properties", "Material") = iProperties.Material.ToUpper

iLogicVb.UpdateWhenDone = True

It's not a custom value; it's the default material being pulled from the part. Just won't change.

[Ralf_Krieg]

Hello

I would not write in an internal iProp, but that's another story. Your code converts the prop value to upper case as expected. What do you mean with "won't change"? If you change material, prop value is not updated automatically or ...?

[patrick3HNXX]

I don't need the material to change. I just need to take the existing material which is in lower case and convert it to uppercase.

[Ralf_Krieg]

Hello

That's exactly what

iProperties.Value("Design Tracking Properties", "Material") = iProperties.Material.ToUpper

does. If I assign the material "Steel" to my part and run this code, the value of iProp Material in the Design Tracking Propertyset is "STEEL". If I edit my titleblock definition in my drawing and insert a textblock with iProp Material, I get a titleblock with the text "STEEL".

If I change the material to Rubber, the titleblock shows "Rubber". I had to run the code again. Or, if don't want to remember running the code manually every time the material changed, I add this rule to the event trigger "material change". After that, I can change material to Rubber and my titleblock shows  ..... RUBBER.

[patrick3HNXX]

Ok I finally got it working. Is there a way to do this without adding a rule to the part file? I have hundreds of parts to go through. I would have open each part and add this rule. I am unclear as to why I can't do this inside the .idw. I have other rules that pull info directly from the title block and modify it, but the material seems to be different for some reason.

[Ralf_Krieg · Accepted solution]

Hello

Create an external rule, instead of an internal. So you don't have to create that rule in every existing part document. Create it once and link it to the event trigger for material change. Every part document will update the iProp if you change material.

You can also create an external rule running from the drawing (see below). The problem here is, you must use the event trigger e.g before save.

iLogicVb.UpdateWhenDone=True

Dim oDrawDoc As DrawingDocument=ThisDrawing.Document

Dim oPartDoc As Inventor.PartDocument 
Dim oPropSet As PropertySet
Dim oView As DrawingView
For Each oView In oDrawDoc.ActiveSheet.DrawingViews
	If oView.ViewType = DrawingViewTypeEnum.kStandardDrawingViewType Then
		If oView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kPartDocumentObject Then
			oPartDoc = DirectCast(oView.ReferencedDocumentDescriptor.ReferencedDocument ,Inventor.PartDocument)
			oPropSet = oPartDoc.PropertySets.Item("{32853F0F-3444-11D1-9E93-0060B03C1CA6}")
			oPropSet.Item("Material").Value = oPartDoc.ActiveMaterial.DisplayName.ToUpper
		End If
	End If
Next

[patrick3HNXX]

Thank you very much.

Works perfectly.

You are a gentleman and scholar.

[patrick3HNXX]

How were you able to get the properties identifier? "

"{32853F0F-3444-11D1-9E93-0060B03C1CA6}"

Do you have code to generate a list?

[Ralf_Krieg · Accepted solution]

Hello

Enabel the iLogic Protocol tab in the iLogic browser. There you can copy'n paste the output. According to the active document open, the output differs.

You can get propertyset internal names/names and all property names/ displaynames like:

Dim oDoc As Document = ThisDoc.Document
For Each oPropset As PropertySet In oDoc.PropertySets
	Logger.Info(vbcrlf & "Name: " & oPropset.Name & vbCrLf & "InternalName: " & oPropset.InternalName)
	'comment the next three lines to not display property names
	For i = 1 To oPropset.Count 
		Logger.Info("Name: " & oPropset.Item(i).Name & vbCrLf & "DisplayName: " & oPropset.Item(i).DisplayName )	
	Next
Next