CAD Forum

I've been looking for a macro to rename all sketches in feature tree to the name of the feature it belongs to + Sketch.
Something like :
- -
Does anyone know a macro that does something like this?

thanks.

There is a macro to hide all sketches in a model but I have not seen a one to rename them based on their feature name. This one will have to be made.

How would it work when sketches are shared?

josh wrote: ↑Wed Feb 07, 2024 7:42 am How would it work when sketches are shared?

We never use shared Sketches.
But for the sake of changes in our workflow in future, I prefer it be named with the first feature that use that sketch.
If it makes any problem, renaming it to the last feature is OK as well.


thanks.

Now that it seems what I need is not possible,
is it possible to rename only the selected sketch to --> the name of the feature it belongs to + SK?

thanks again.

Here is a quick (dirty) macro that does the job.

gupta9665 wrote: ↑Wed Feb 14, 2024 2:46 am Here is a quick (dirty) macro that does the jib.

Code: Select all

Sub Mian()

Dim swApp           As SldWorks.SldWorks
Dim swPart          As SldWorks.PartDoc
Dim swFeat          As SldWorks.Feature
Dim swSubFeature    As SldWorks.Feature
Dim FeatureName     As String
Dim i               As Integer


Set swApp = Application.SldWorks
Set swPart = swApp.ActiveDoc
Set swFeat = swPart.FirstFeature


While Not swFeat Is Nothing

  If swFeat.GetTypeName2 <> "ProfileFeature" Then
    Set swSubFeature = swFeat.GetFirstSubFeature
    While Not swSubFeature Is Nothing
    
     If swSubFeature.GetTypeName2 = "ProfileFeature" Then
    
     FeatureName = swFeat.Name & " Sketch"
     
     While False <> swPart.FeatureManager.IsNameUsed(swNameType_e.swFeatureName, FeatureName)
      i = i + 1
      FeatureName = swFeat.Name & " Sketch" & (i)
     Wend
     
     swSubFeature.Name = FeatureName
     
     End If
    
    Set swSubFeature = swSubFeature.GetNextSubFeature
    
    Wend
  End If

Set swFeat = swFeat.GetNextFeature

Wend

End Sub

Deepak still beeing the man

Thanks to both.
Will give it a try.

gupta9665 wrote: ↑Wed Feb 14, 2024 2:46 am Here is a quick (dirty) macro that does the job.

Code: Select all

Sub Mian()

Dim swApp           As SldWorks.SldWorks
Dim swPart          As SldWorks.PartDoc
Dim swFeat          As SldWorks.Feature
Dim swSubFeature    As SldWorks.Feature
Dim FeatureName     As String
Dim i               As Integer


Set swApp = Application.SldWorks
Set swPart = swApp.ActiveDoc
Set swFeat = swPart.FirstFeature


While Not swFeat Is Nothing

  If swFeat.GetTypeName2 <> "ProfileFeature" Then
    Set swSubFeature = swFeat.GetFirstSubFeature
    While Not swSubFeature Is Nothing
    
     If swSubFeature.GetTypeName2 = "ProfileFeature" Then
    
     FeatureName = swFeat.Name & " Sketch"
     
     While False <> swPart.FeatureManager.IsNameUsed(swNameType_e.swFeatureName, FeatureName)
      i = i + 1
      FeatureName = swFeat.Name & " Sketch" & (i)
     Wend
     
     swSubFeature.Name = FeatureName
     
     End If
    
    Set swSubFeature = swSubFeature.GetNextSubFeature
    
    Wend
  End If

Set swFeat = swFeat.GetNextFeature

Wend

End Sub

@gupta9665 Million thanks.
Works perfect.

I only had to add a If Left(swSubFeature.Name, 6) = "Sketch" Then to prevent renaming the sketches that have already been renamed manually, and add a i = 0 after GetNextFeature to reset the counter for each feature.

I really don't know how to appreciate this favor.
Thanks again.