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Display part’s custom properties on drawing sheet by using Macro

Question asked by Xh Z on Jul 15, 2017
Latest reply on Jul 23, 2017 by Deepak Gupta

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I am trying to display a part’s custom properties on the drawing sheet using a macro but did not find exact the function to do it.

Here is my idea:

parts with one custom properties (DesignedBy) in the default configuration. We do not have other configurations.
Create 2d drawings.
Run the macro and the values of the above properties will be displayed on the sheet as one line.

Tried cusPropMgr.Get5, swModel.Extension.CustomPropertyManager() etc but seems cannot get it done.

i know we can link a text to that custom properties and it work well. but in this case, i just want to use a macro.

I am not familiar with SW API function. Any suggestions? Thank you.

Deepak Gupta Jul 16, 2017 1:09 PM

Correct Answer

Try these codes

Option Explicit
    Dim swApp           As SldWorks.SldWorks
    Dim swModel         As SldWorks.ModelDoc2
    Dim swDraw          As SldWorks.DrawingDoc
    Dim swView          As SldWorks.View
    Dim swCustProp      As CustomPropertyManager
    Dim Note            As SldWorks.Note
    Dim swAnn           As SldWorks.Annotation
    Dim valOut          As String
    Dim rValOut         As String
Sub main()


    Set swApp = Application.SldWorks
    Set swDraw = swApp.ActiveDoc
        
    Set swView = swDraw.GetFirstView
    Set swView = swView.GetNextView
    Set swModel = swView.ReferencedDocument
    Set swCustProp = swModel.Extension.CustomPropertyManager(swView.ReferencedConfiguration)
    
    swCustProp.Get2 "DesignedBy", valOut, rValOut 'Change the custom property name here
    Debug.Print "$PRP:" + Chr(34) + "DesignedBy" + Chr(34)
    Set Note = swDraw.InsertNote(rValOut) ' Use "$PRPSHEET:" + Chr(34) + "DesignedBy" + Chr(34)  in case you want to link to property
    Set swAnn = Note.GetAnnotation
    swAnn.SetPosition2 0, 0, 0 'Change note position here

End Sub

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Marshall Wilson Jul 15, 2017 3:59 PM

I'm not a fancy API guy, but this quick-n-dirty might work.

Create layers on the drawing template with notes on them. The notes could have references to the custom properties you want to show/hide.

By default they could be hidden and there's an easy macro for hiding / revealing layers.

Of course if I weren't so lazy I'm sure there's easy code for inserting a pre-determined note at coordinates (x,y).

Here's my code for a show/hide toogle of a layer that has an alignment grid on it.

Sub main()

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swLayerMgr As SldWorks.LayerMgr

Dim swLayer As SldWorks.Layer

Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swLayerMgr = swModel.GetLayerManager

Set swLayer = swLayerMgr.GetLayer("15 - GRID")

If swLayer.Visible = False Then

' Toggle layer on

swLayer.Visible = True

Debug.Assert True = swLayer.Visible

Else

' Toggle layer off

swLayer.Visible = False

Debug.Assert False = swLayer.Visible

End If

End Sub

'-----------------------------------

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Xh Z @ Marshall Wilson on Jul 16, 2017 12:08 PM

Hello Wilson,

thank you for the reply. your macro shows me another way to achieve it.

But i prefer to display the values directly using macro.

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Deepak Gupta Jul 16, 2017 3:27 AM

You need to display the property as linked OR want just the value?

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Xh Z @ Deepak Gupta on Jul 16, 2017 12:08 PM

Hello Deepak,

i just want to display the value of the custom property.

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Deepak Gupta @ Xh Z on Jul 16, 2017 1:09 PM

Try these codes

Option Explicit
    Dim swApp           As SldWorks.SldWorks
    Dim swModel         As SldWorks.ModelDoc2
    Dim swDraw          As SldWorks.DrawingDoc
    Dim swView          As SldWorks.View
    Dim swCustProp      As CustomPropertyManager
    Dim Note            As SldWorks.Note
    Dim swAnn           As SldWorks.Annotation
    Dim valOut          As String
    Dim rValOut         As String
Sub main()


    Set swApp = Application.SldWorks
    Set swDraw = swApp.ActiveDoc
        
    Set swView = swDraw.GetFirstView
    Set swView = swView.GetNextView
    Set swModel = swView.ReferencedDocument
    Set swCustProp = swModel.Extension.CustomPropertyManager(swView.ReferencedConfiguration)
    
    swCustProp.Get2 "DesignedBy", valOut, rValOut 'Change the custom property name here
    Debug.Print "$PRP:" + Chr(34) + "DesignedBy" + Chr(34)
    Set Note = swDraw.InsertNote(rValOut) ' Use "$PRPSHEET:" + Chr(34) + "DesignedBy" + Chr(34)  in case you want to link to property
    Set swAnn = Note.GetAnnotation
    swAnn.SetPosition2 0, 0, 0 'Change note position here

End Sub

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Xh Z @ Deepak Gupta on Jul 23, 2017 12:15 AM

Thank you Deepak,

it works well.

for read the custom properties from the default model (we do not have any other configurations in the part), i have changed the line as:

Set swCustProp = swModel.Extension.CustomPropertyManager("")

Thank you.

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Deepak Gupta @ Xh Z on Jul 23, 2017 3:18 AM

Since you said configuration in the first post, I used configuration properties. Glad to know that you got it working

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Xh Z @ Deepak Gupta on Jul 23, 2017 5:51 AM

Thank you again.

is there any method to automatically run this macro when i open a drawing (or upon rebuild, or upon save)?

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Deepak Gupta @ Xh Z on Jul 23, 2017 6:28 AM

Yes it is possible using event. Check this example: Fire Notification When Activating a Sheet Example (VBA)

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9 Replies

Marshall Wilson Jul 15, 2017 3:59 PM
Mark Correct
Correct Answer
I'm not a fancy API guy, but this quick-n-dirty might work.

Create layers on the drawing template with notes on them. The notes could have references to the custom properties you want to show/hide.
By default they could be hidden and there's an easy macro for hiding / revealing layers.

Of course if I weren't so lazy I'm sure there's easy code for inserting a pre-determined note at coordinates (x,y).

Here's my code for a show/hide toogle of a layer that has an alignment grid on it.
Sub main()
    Dim swApp                      As SldWorks.SldWorks
    Dim swModel                    As SldWorks.ModelDoc2
    Dim swLayerMgr                  As SldWorks.LayerMgr
    Dim swLayer                    As SldWorks.Layer

    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swLayerMgr = swModel.GetLayerManager
    Set swLayer = swLayerMgr.GetLayer("15 - GRID")

    If swLayer.Visible = False Then
        ' Toggle layer on
        swLayer.Visible = True
        Debug.Assert True = swLayer.Visible
    Else
        ' Toggle layer off
        swLayer.Visible = False
        Debug.Assert False = swLayer.Visible
    End If
End Sub
'-----------------------------------
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- Xh Z @ Marshall Wilson on Jul 16, 2017 12:08 PM
  Mark Correct
  Correct Answer
  Hello Wilson,
  
  thank you for the reply. your macro shows me another way to achieve it.
  But i prefer to display the values directly using macro.
  Like • Show 0 Likes0
  Actions
Deepak Gupta Jul 16, 2017 3:27 AM
Mark Correct
Correct Answer
You need to display the property as linked OR want just the value?
Like • Show 2 Likes2
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- Xh Z @ Deepak Gupta on Jul 16, 2017 12:08 PM
  Mark Correct
  Correct Answer
  Hello Deepak,
  i just want to display the value of the custom property.
  Like • Show 0 Likes0
  Actions
  - Deepak Gupta @ Xh Z on Jul 16, 2017 1:09 PM
    Unmark Correct
    Correct Answer
    Try these codes
    
    Option Explicit Dim swApp As SldWorks.SldWorks Dim swModel As SldWorks.ModelDoc2 Dim swDraw As SldWorks.DrawingDoc Dim swView As SldWorks.View Dim swCustProp As CustomPropertyManager Dim Note As SldWorks.Note Dim swAnn As SldWorks.Annotation Dim valOut As String Dim rValOut As String Sub main() Set swApp = Application.SldWorks Set swDraw = swApp.ActiveDoc Set swView = swDraw.GetFirstView Set swView = swView.GetNextView Set swModel = swView.ReferencedDocument Set swCustProp = swModel.Extension.CustomPropertyManager(swView.ReferencedConfiguration) swCustProp.Get2 "DesignedBy", valOut, rValOut 'Change the custom property name here Debug.Print "$PRP:" + Chr(34) + "DesignedBy" + Chr(34) Set Note = swDraw.InsertNote(rValOut) ' Use "$PRPSHEET:" + Chr(34) + "DesignedBy" + Chr(34) in case you want to link to property Set swAnn = Note.GetAnnotation swAnn.SetPosition2 0, 0, 0 'Change note position here End Sub
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    - Xh Z @ Deepak Gupta on Jul 23, 2017 12:15 AM
      Mark Correct
      Correct Answer
      Thank you Deepak,
      
      it works well.
      for read the custom properties from the default model (we do not have any other configurations in the part), i have changed the line as:
      Set swCustProp = swModel.Extension.CustomPropertyManager("")
      
      Thank you.
      Like • Show 0 Likes0
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      - Deepak Gupta @ Xh Z on Jul 23, 2017 3:18 AM
        Mark Correct
        Correct Answer
        Since you said configuration in the first post, I used configuration properties. Glad to know that you got it working
        Like • Show 0 Likes0
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        Xh Z @ Deepak Gupta on Jul 23, 2017 5:51 AM
        Mark Correct
        Correct Answer
        Thank you again.
        is there any method to automatically run this macro when i open a drawing (or upon rebuild, or upon save)?
        Like • Show 0 Likes0
        Actions
        Deepak Gupta @ Xh Z on Jul 23, 2017 6:28 AM
        Mark Correct
        Correct Answer
        Yes it is possible using event. Check this example: Fire Notification When Activating a Sheet Example (VBA)
        Like • Show 0 Likes0
        Actions

Display part’s custom properties on drawing sheet by using Macro

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