9 Replies Latest reply on Jul 23, 2017 6:28 AM by Deepak Gupta

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

Xh Z Jul 15, 2017 3:26 PM

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.

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

Marshall Wilson Jul 15, 2017 3:59 PM (in response to Xh Z)

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
'-----------------------------------
Like Show 2 Likes(2)

Actions
- Re: Display part’s custom properties on drawing sheet by using Macro
  
  Xh Z Jul 16, 2017 12:08 PM (in response to Marshall Wilson)
  
  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 Likes(0)
  
  Actions
Re: Display part’s custom properties on drawing sheet by using Macro

Deepak Gupta Jul 16, 2017 3:27 AM (in response to Xh Z)

You need to display the property as linked OR want just the value?
Like Show 2 Likes(2)

Actions
- Re: Display part’s custom properties on drawing sheet by using Macro
  
  Xh Z Jul 16, 2017 12:08 PM (in response to Deepak Gupta)
  
  Hello Deepak,
  i just want to display the value of the custom property.
  
  Like Show 0 Likes(0)
  
  Actions
  - Re: Display part’s custom properties on drawing sheet by using Macro
    
    Deepak Gupta Jul 16, 2017 1:09 PM (in response to Xh Z)
    
    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
    
    Like Show 0 Likes(0)
    
    Actions
    - Re: Display part’s custom properties on drawing sheet by using Macro
      
      Xh Z Jul 23, 2017 12:15 AM (in response to Deepak Gupta)
      
      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 Likes(0)
      
      Actions
      - Re: Display part’s custom properties on drawing sheet by using Macro
        
        Deepak Gupta Jul 23, 2017 3:18 AM (in response to Xh Z)
        
        Since you said configuration in the first post, I used configuration properties. Glad to know that you got it working
        
        Like Show 0 Likes(0)
        
        Actions
        
        Re: Display part’s custom properties on drawing sheet by using Macro
        
        Xh Z Jul 23, 2017 5:51 AM (in response to Deepak Gupta)
        
        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 Likes(0)
        
        Actions
        
        Re: Display part’s custom properties on drawing sheet by using Macro
        
        Deepak Gupta Jul 23, 2017 6:28 AM (in response to Xh Z)
        
        Yes it is possible using event. Check this example: Fire Notification When Activating a Sheet Example (VBA)
        
        Like Show 0 Likes(0)
        
        Actions

Go to original post