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creating a sketch on a new plane

Question asked by M. Doga Dogan on Jul 5, 2017
Latest reply on Mar 28, 2018 by Matthew Davey

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Hello,

I would like to write a macro that creates a new plane with a given distance dynamically, and then starts a 2D sketch on it. Therefore I need to select the newly created plane before I start the sketch. I couldn't understand how to choose a newly created plane.

My current code looks like this:

Dim myRefPlane As Object

Distance = Distance / 1000

Set myRefPlane = Part.FeatureManager.InsertRefPlane(8, Distance, 0, 0, 0, 0)

Part.ClearSelection2 True

boolstatus = Part.Extension.SelectByID2("Plane1", "PLANE", 0, 0, 0, False, 0, Nothing, 0)

Part.SketchManager.InsertSketch True

The code above just assumes that the new plane is called Plane1, however, this might not be the case. Any ideas?

Thank you

Andreas Killer Jul 6, 2017 3:26 AM

Correct Answer

Get the last added feature from the ModelDocExtension object.

Andreas.

Option Explicit

Sub Main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swExt As SldWorks.ModelDocExtension
Dim Distance

'Refer to the current model
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swExt = swModel.Extension

'Be sure a plane is selected
Dim swSelMgr As SldWorks.SelectionMgr
Set swSelMgr = swModel.SelectionManager
With swSelMgr
    If .GetSelectedObjectCount2(-1) = 0 Then
      MsgBox "Select a plane and try again"
    End If
    If .GetSelectedObjectType3(1, -1) <> swSelectType_e.swSelDATUMPLANES Then
      MsgBox "Select a plane and try again"
    End If
End With

'Ask for the distance
Distance = InputBox("Distance in mm:")
'Abort?
If Not IsNumeric(Distance) Then Exit Sub
'Change to meters
Distance = Distance / 1000

'Insert the new plane
Dim myRefPlane As SldWorks.RefPlane
Set myRefPlane = swModel.FeatureManager.InsertRefPlane(swRefPlaneReferenceConstraints_e.swRefPlaneReferenceConstraint_Distance, Distance, 0, 0, 0, 0)

'Get the last feature
Dim swFeature As SldWorks.Feature
Set swFeature = swExt.GetLastFeatureAdded
'Select it
swFeature.Select2 False, -1
'Insert a sketch
swModel.SketchManager.InsertSketch True
End Sub

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Abilash V. Jul 5, 2017 2:29 PM

Dim swApp As SldWorks.SldWorks

Dim swmodel As SldWorks.ModelDoc2

Dim swfeat As SldWorks.Feature

Dim var As Variant

Dim swfeatmgr As SldWorks.FeatureManager

Dim n As Integer

Dim plan As Variant

Dim swplan As SldWorks.Feature

Dim bool As Boolean

Sub main()

Set swApp = Application.SldWorks

Set swmodel = swApp.ActiveDoc

Set swfeatmgr = swmodel.FeatureManager

var = swfeatmgr.GetFeatures(False)

For i = 0 To UBound(var)

Set swfeat = var(i)

If swfeat.GetTypeName2 = "RefPlane" Then

n = i

Debug.Print swfeat.Name & " " & swfeat.GetTypeName2

End If

bool = var(n).Select2(False, 0)

End Sub

'This would automatically select the last created plane.

'Hope it helps.

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M. Doga Dogan @ Abilash V. on Jul 5, 2017 6:01 PM

Thank you so much, Abilash! works like a charm.

But could you please briefly explain what each line does?

Best,

Doga

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Dave Bear @ M. Doga Dogan on Jul 6, 2017 12:24 AM

You're basically asking Abilash to teach you coding.......

Dave.

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Andreas Killer Jul 6, 2017 3:26 AM

Get the last added feature from the ModelDocExtension object.

Andreas.

Option Explicit

Sub Main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swExt As SldWorks.ModelDocExtension
Dim Distance

Actions

Simon Turner @ Andreas Killer on Jul 6, 2017 3:40 AM

Even simpler, you can just Set swFeature = myRefPlane

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Andreas Killer @ Simon Turner on Jul 6, 2017 3:53 AM

Correct! Not easy to find objects inherited from another object in the Solidworks API.

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M. Doga Dogan @ Simon Turner on Jul 6, 2017 11:10 AM

Thanks guys! It looks like a shorter solution.

I would like to ask another question similar to this one. I want to dynamically select the first point of the last added sketch (not feature). Is there a short way to accomplish this?

For example, if the last added sketch is Sketch2, then I could write:

boolstatus = Part.Extension.SelectByID2("Point1@Sketch2", "EXTSKETCHPOINT", 0, 0, 0, True, 0, Nothing, 0)

Best regards,

Doga

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Matthew Davey @ Andreas Killer on Mar 28, 2018 8:42 AM

Andreas - This is great!

I needed a macro to easily set up a number of new offset reference planes, so I was really glad to see this can be done!

The only improvement for me would be to have a dialogue box appear after the dimension has been input to re-name the plane (with user input text). I do not need to start a sketch on the plane so have removed this bit of code, instead I should like to simply move on to defining the next plane offset distance and its name.....

Do you know if this can this be done please?

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8 Replies

Abilash V. Jul 5, 2017 2:29 PM
Mark Correct
Correct Answer
Dim swApp As SldWorks.SldWorks
Dim swmodel As SldWorks.ModelDoc2
Dim swfeat As SldWorks.Feature
Dim var As Variant
Dim swfeatmgr As SldWorks.FeatureManager
Dim n As Integer
Dim plan As Variant
Dim swplan As SldWorks.Feature
Dim bool As Boolean
Sub main()
Set swApp = Application.SldWorks
Set swmodel = swApp.ActiveDoc
Set swfeatmgr = swmodel.FeatureManager
var = swfeatmgr.GetFeatures(False)
For i = 0 To UBound(var)
Set swfeat = var(i)
If swfeat.GetTypeName2 = "RefPlane" Then
n = i
Debug.Print swfeat.Name & " " & swfeat.GetTypeName2
End If
Next
bool = var(n).Select2(False, 0)
End Sub

'This would automatically select the last created plane.
'Hope it helps.
Like • Show 2 Likes2
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- M. Doga Dogan @ Abilash V. on Jul 5, 2017 6:01 PM
  Mark Correct
  Correct Answer
  Thank you so much, Abilash! works like a charm.
  But could you please briefly explain what each line does?
  
  Best,
  Doga
  Like • Show 1 Like1
  Actions
  - Dave Bear @ M. Doga Dogan on Jul 6, 2017 12:24 AM
    Mark Correct
    Correct Answer
    You're basically asking Abilash to teach you coding.......
    
    Dave.
    Like • Show 0 Likes0
    Actions
Andreas Killer Jul 6, 2017 3:26 AM
Unmark Correct
Correct Answer
Get the last added feature from the ModelDocExtension object.

Andreas.

Option Explicit

Sub Main()
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swExt As SldWorks.ModelDocExtension
Dim Distance

'Refer to the current model
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swExt = swModel.Extension

'Be sure a plane is selected
Dim swSelMgr As SldWorks.SelectionMgr
Set swSelMgr = swModel.SelectionManager
With swSelMgr
    If .GetSelectedObjectCount2(-1) = 0 Then
      MsgBox "Select a plane and try again"
    End If
    If .GetSelectedObjectType3(1, -1) <> swSelectType_e.swSelDATUMPLANES Then
      MsgBox "Select a plane and try again"
    End If
End With

'Ask for the distance
Distance = InputBox("Distance in mm:")
'Abort?
If Not IsNumeric(Distance) Then Exit Sub
'Change to meters
Distance = Distance / 1000

'Insert the new plane
Dim myRefPlane As SldWorks.RefPlane
Set myRefPlane = swModel.FeatureManager.InsertRefPlane(swRefPlaneReferenceConstraints_e.swRefPlaneReferenceConstraint_Distance, Distance, 0, 0, 0, 0)

'Get the last feature
Dim swFeature As SldWorks.Feature
Set swFeature = swExt.GetLastFeatureAdded
'Select it
swFeature.Select2 False, -1
'Insert a sketch
swModel.SketchManager.InsertSketch True
End Sub
Like • Show 2 Likes2
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- Simon Turner @ Andreas Killer on Jul 6, 2017 3:40 AM
  Mark Correct
  Correct Answer
  Even simpler, you can just Set swFeature = myRefPlane
  Like • Show 2 Likes2
  Actions
  - Andreas Killer @ Simon Turner on Jul 6, 2017 3:53 AM
    Mark Correct
    Correct Answer
    Correct! Not easy to find objects inherited from another object in the Solidworks API.
    Like • Show 2 Likes2
    Actions
  - M. Doga Dogan @ Simon Turner on Jul 6, 2017 11:10 AM
    Mark Correct
    Correct Answer
    Thanks guys! It looks like a shorter solution.
    I would like to ask another question similar to this one. I want to dynamically select the first point of the last added sketch (not feature). Is there a short way to accomplish this?
    
    For example, if the last added sketch is Sketch2, then I could write:
    boolstatus = Part.Extension.SelectByID2("Point1@Sketch2", "EXTSKETCHPOINT", 0, 0, 0, True, 0, Nothing, 0)
    
    Best regards,
    Doga
    Like • Show 1 Like1
    Actions
- Matthew Davey @ Andreas Killer on Mar 28, 2018 8:42 AM
  Mark Correct
  Correct Answer
  Andreas - This is great!
  
  I needed a macro to easily set up a number of new offset reference planes, so I was really glad to see this can be done!
  
  The only improvement for me would be to have a dialogue box appear after the dimension has been input to re-name the plane (with user input text). I do not need to start a sketch on the plane so have removed this bit of code, instead I should like to simply move on to defining the next plane offset distance and its name.....
  
  Do you know if this can this be done please?
  Like • Show 1 Like1
  Actions

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