Solidworks Macro - Move/Copy Sketch Entities

12 minute read

Introduction

In this post, I tell you about how to Move/Copy Sketch Entities using Solidworks VBA Macros in a Sketch.

In this post, I explain about MoveOrCopy method from Solidworks ModelDoc2’s Extension object.

This method is most updated method, I found in Solidworks API Help.

So use this method if you want to MoveOrCopy Sketch Entities.

This post is similar to previous Solidworks Macro - Edit Circular Sketch Pattern post.

If you have not visited my previous Solidworks Macro - Edit Circular Sketch Pattern post, then please do check-it if you want to learn Editing Circular Sketch Patterns.

Video of Code on YouTube

Please see below video on how to Move/Copy Sketch Entities from Solidworks VBA Macros.


Please note that there are no explaination in the video.

Explaination of each line and why we write code this way is given in this post.

Code Sample

Below is the code sample to Move/Copy Sketch Entities.

Option Explicit

' Create variable for Solidworks application
Dim swApp As SldWorks.SldWorks

' Create variable for Solidworks document
Dim swDoc As SldWorks.ModelDoc2

' Boolean Variable
Dim BoolStatus As Boolean

' Create variable for Solidworks Sketch Manager
Dim swSketchManager As SldWorks.SketchManager

' Create Variable for Solidworks Sketch Segment
Dim swSketchSegment As SldWorks.SketchSegment

' Main function of our VBA program
Sub main()

  ' Set Solidworks variable to Solidworks application
  Set swApp = Application.SldWorks
  
  ' Create string type variable for storing default part location
  Dim defaultTemplate As String

  ' Set value of this string type variable to "Default part template"
  defaultTemplate = swApp.GetUserPreferenceStringValue(swUserPreferenceStringValue_e.swDefaultTemplatePart)

  ' Set Solidworks document to new part document
  Set swDoc = swApp.NewDocument(defaultTemplate, 0, 0, 0)
  
  '-----------------------UNIT CONVERSION----------------------------------------

  ' Local variables used as Conversion Factors
  Dim LengthConversionFactor As Double
  Dim AngleConversionFactor As Double
  
  ' Use a Select Case, to get the length of active Unit and set the different factors
  Select Case swDoc.GetUnits(0)       ' GetUnits function gives us, active unit
    
    Case swMETER    ' If length is in Meter
      LengthConversionFactor = 1
      AngleConversionFactor = 1
    
    Case swMM       ' If length is in MM
      LengthConversionFactor = 1 / 1000
      AngleConversionFactor = 1 * 0.01745329
    
    Case swCM       ' If length is in CM
      LengthConversionFactor = 1 / 100
      AngleConversionFactor = 1 * 0.01745329
    
    Case swINCHES   ' If length is in INCHES
      LengthConversionFactor = 1 * 0.0254
      AngleConversionFactor = 1 * 0.01745329
    
    Case swFEET     ' If length is in FEET
      LengthConversionFactor = 1 * (0.0254 * 12)
      AngleConversionFactor = 1 * 0.01745329
    
    Case swFEETINCHES     ' If length is in FEET & INCHES
      LengthConversionFactor = 1 * 0.0254  ' For length we use sama as Inch
      AngleConversionFactor = 1 * 0.01745329
    
    Case swANGSTROM        ' If length is in ANGSTROM
      LengthConversionFactor = 1 / 10000000000#
      AngleConversionFactor = 1 * 0.01745329
    
    Case swNANOMETER       ' If length is in NANOMETER
      LengthConversionFactor = 1 / 1000000000
      AngleConversionFactor = 1 * 0.01745329
    
    Case swMICRON       ' If length is in MICRON
      LengthConversionFactor = 1 / 1000000
      AngleConversionFactor = 1 * 0.01745329
  End Select

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

  ' Select Front Plane
  BoolStatus = swDoc.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, swSelectOption_e.swSelectOptionDefault)

  ' Set Sketch manager for our sketch
  Set swSketchManager = swDoc.SketchManager

  ' Insert a sketch into selected plane
  swSketchManager.InsertSketch True
  
  ' Circle Radius
  Dim circleRadius As Double
  circleRadius = 5 * LengthConversionFactor
  
  ' Set Sketch Segment value and Create a Circle
  Set swSketchSegment = swSketchManager.CreateCircleByRadius(0, 0, 0, circleRadius)
  
  ' Defining variables for Destination Co-ordinates
  Dim destinationCoOrdinateInXDir As Double, destinationCoOrdinateInYDir As Double
  
  ' Setting the values of Destination Co-ordinates in X & Y directions for Move
  destinationCoOrdinateInXDir = 10 * LengthConversionFactor
  destinationCoOrdinateInYDir = 10 * LengthConversionFactor
  
  ' Move circle
  swDoc.Extension.MoveOrCopy False, 1, False, 0, 0, 0, destinationCoOrdinateInXDir, destinationCoOrdinateInYDir, 0
  
  ' Setting the values of Destination Co-ordinates in X & Y directions for Copy
  destinationCoOrdinateInXDir = 15 * LengthConversionFactor
  destinationCoOrdinateInYDir = 15 * LengthConversionFactor
  
  ' Copy circle
  swDoc.Extension.MoveOrCopy True, 3, True, 0, 0, 0, destinationCoOrdinateInXDir, destinationCoOrdinateInYDir, 0
  
  ' De-select the lines after creation
  swDoc.ClearSelection2 True
  
  ' Show Front View after Circular Sketch Pattern
  swDoc.ShowNamedView2 "", swStandardViews_e.swFrontView
  
  ' Zoom to fit screen in Solidworks Window
  swDoc.ViewZoomtofit2
  
End Sub

Understanding the Code

Now let us walk through each line in the above code, and understand the meaning and purpose of every line.

I also give some link so that you can go through them if there are anything I explained in previous posts.

Option Explicit

This line forces us to define every variable we are going to use.

For more information please visit Solidworks Macros - Open new Part document post.

' Create variable for Solidworks application
Dim swApp As SldWorks.SldWorks

In this line, we create a variable which we named as swApp and the type of this swApp variable is SldWorks.SldWorks.

' Create variable for Solidworks document
Dim swDoc As SldWorks.ModelDoc2

In this line, we create a variable which we named as swDoc and the type of this swDoc variable is SldWorks.ModelDoc2.

' Boolean Variable
Dim BoolStatus As Boolean

In this line, we create a variable named BoolStatus as Boolean object type.

' Create variable for Solidworks Sketch Manager
Dim swSketchManager As SldWorks.SketchManager

In above line, we create variable swSketchManager for Solidworks Sketch Manager.

As the name suggested, a Sketch Manager holds variours methods and properties to manage Sketches.

To see methods and properties related to SketchManager object, please visit this page of Solidworks API Help

' Create variable for Solidworks Sketch Segment
Dim swSketchSegment As SldWorks.SketchSegment

In this line, we Create a variable which we named as swSketchSegment and the type of this swSketchSegment variable is SldWorks.SketchSegment.

We create variable swSketchSegment for Solidworks Sketch Segments.

To see methods and properties related to swSketchSegment object, please visit this page of Solidworks API Help

These all are our global variables.

As you can see in code sample, they are Solidworks API Objects.

So basically I group all the Solidworks API Objects in one place.

I have also place boolean type object at top also, because after certain point we will need this variable frequently.

Thus, I have started placing it here.

Next is our Sub procedure which has name of main.

This procedure hold all the statements (instructions) we give to computer.

' Set Solidworks variable to Solidworks application
Set swApp = Application.SldWorks

In this line, we set the value of our Solidworks variable swApp; which we define earlier; to Solidworks application.

' Create string type variable for storing default part location
Dim defaultTemplate As String
' Set value of this string type variable to "Default part template"
defaultTemplate = swApp.GetUserPreferenceStringValue(swUserPreferenceStringValue_e.swDefaultTemplatePart)

In 1st statement of above example, we are defining a variable of string type and named it as defaultTemplate.

This variable defaultTemplate, hold the location the location of Default Part Template.

In 2nd line of above example. we assign value to our newly define defaultTemplate variable.

We assign the value by using a Method named GetUserPreferenceStringValue().

This GetUserPreferenceStringValue() method is a part of our main Solidworks variable swApp.

' Set Solidworks document to new part document
Set swDoc = swApp.NewDocument(defaultTemplate, 0, 0, 0)

In this line, we set the value of our swDoc variable to new document.

For detailed information about these lines please visit Solidworks Macros - Open new Part document post.

I have discussed them thoroghly in Solidworks Macros - Open new Part document post, so do checkout that post if you want to understand above code in more detail.

'-----------------------UNIT CONVERSION----------------------------------------

' Local variables used as Conversion Factors
Dim LengthConversionFactor As Double
Dim AngleConversionFactor As Double

' Use a Select Case, to get the length of active Unit and set the different factors
Select Case swDoc.GetUnits(0)       ' GetUnits function gives us, active unit
  
  Case swMETER    ' If length is in Meter
    LengthConversionFactor = 1
    AngleConversionFactor = 1
  
  Case swMM       ' If length is in MM
    LengthConversionFactor = 1 / 1000
    AngleConversionFactor = 1 * 0.01745329
  
  Case swCM       ' If length is in CM
    LengthConversionFactor = 1 / 100
    AngleConversionFactor = 1 * 0.01745329
  
  Case swINCHES   ' If length is in INCHES
    LengthConversionFactor = 1 * 0.0254
    AngleConversionFactor = 1 * 0.01745329
  
  Case swFEET     ' If length is in FEET
    LengthConversionFactor = 1 * (0.0254 * 12)
    AngleConversionFactor = 1 * 0.01745329
  
  Case swFEETINCHES     ' If length is in FEET & INCHES
    LengthConversionFactor = 1 * 0.0254  ' For length we use sama as Inch
    AngleConversionFactor = 1 * 0.01745329
  
  Case swANGSTROM        ' If length is in ANGSTROM
    LengthConversionFactor = 1 / 10000000000#
    AngleConversionFactor = 1 * 0.01745329
  
  Case swNANOMETER       ' If length is in NANOMETER
    LengthConversionFactor = 1 / 1000000000
    AngleConversionFactor = 1 * 0.01745329
  
  Case swMICRON       ' If length is in MICRON
    LengthConversionFactor = 1 / 1000000
    AngleConversionFactor = 1 * 0.01745329
End Select

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

Above code sample shows how to fix Solidworks API Unit issue.

We 1st get the current unit of the part and apply the switch statements to update our Length and Angle Conversion factors.

I have already explained in detail about Fixing Solidworks API Unit Issue in General - Fix Unit Issue blog post.

Do checkout above post for Fixing Solidworks API Issue.

' Select Front Plane
BoolStatus = swDoc.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, swSelectOption_e.swSelectOptionDefault)

In above line, we select the front plane by using SelectByID2 method from Extension object.

For more information about selection method please visit Solidworks Macros - Selection Methods post.

' Set Sketch manager for our sketch
Set swSketchManager = swDoc.SketchManager

In above line, we set the Sketch manager variable to current document’s sketch manager.

' Insert a sketch into selected plane
swSketchManager.InsertSketch True

In above line, we use InsertSketch method of SketchManager and give True value.

This method allows us to insert a sketch in selected plane.

' Circle Radius
Dim circleRadius As Double
circleRadius = 5 * LengthConversionFactor

In above code sample, we do following:

  1. Create a local variable named circleRadius, which is Double type.

  2. In 2nd line, we assign a value of 5 to our circleRadius variable, also we multiple with our LengthConversionFactor variable.

Since I am using IPS unit system, I want to create a circle of Radius 5 inch. 

' Set Sketch Segment value and Create a Circle
Set swSketchSegment = swSketchManager.CreateCircleByRadius(0, 0, 0, circleRadius)

In above line, we set the value of Solidworks Sketch Segment variable swSketchSegment by CreateCircleByRadius method from Solidworks Sketch Manager.

This CreateCircleByRadius method creates a Circle at given point with radius.

For more information about CreateCircleByRadius method, you can read my Solidworks Macro - Create Circle By Radius post.

That post describe all the parameters we need for this CreateCircleByRadius method in details.

In above line, we create a Circle with:

  • Circle Centerpoint : At origin i.e. (0, 0, 0)

  • Circle Radius : circleRadius

' Defining variables for Destination Co-ordinates
Dim destinationCoOrdinateInXDir As Double, destinationCoOrdinateInYDir As Double

In above line of code, we create two variables of double type in one single line.

These variables we use for defining Destination Co-ordinates.

Variables Name:

  • destinationCoOrdinateInXDir

  • destinationCoOrdinateInYDir

' Setting the values of Destination Co-ordinates in X & Y directions for Move
destinationCoOrdinateInXDir = 10 * LengthConversionFactor
destinationCoOrdinateInYDir = 10 * LengthConversionFactor

In above line of code, we set the values of Destination Co-ordinates in X & Y directions for Move selected circle.

Variables Values:

  • destinationCoOrdinateInXDir = 10 * LengthConversionFactor

    10” in X direction.

  • destinationCoOrdinateInYDir = 10 * LengthConversionFactor

    10” in Y direction.

' Move circle
swDoc.Extension.MoveOrCopy False, 1, False, 0, 0, 0, destinationCoOrdinateInXDir, destinationCoOrdinateInYDir, 0

For “Moving” a sketch entity, we need MoveOrCopy method from Solidworks ModelDoc2’s Extension object.

This MoveOrCopy method takes following parameters as explained:

  • Copy : True to copy the sketch entities, False to not.

  • NumCopies : Number of copies you want to create.

  • KeepRelations : True to keep sketch relations after Move or Copy operation, False to not.

  • BaseX : X coordinate of the base point from which to move the sketch entities.

  • BaseY : Y coordinate of the base point from which to move the sketch entities.

  • BaseZ : Z coordinate of the base point from which to move the sketch entities.

  • DestX : X coordinate of the destination point from which to move the sketch entities.

  • DestY : Y coordinate of the destination point from which to move the sketch entities.

  • DestZ : Z coordinate of the destination point from which to move the sketch entities.

NOTE: There are no return value after this function.

Cases

In this section, we will go through different cases by

  • Modifying different parameters

  • See images, before and after parameter modification

CASE 1 : Move Sketch Entities

In our code, if we want to Move Sketch Entities, then we need to use code sample as given below:

' Defining variables for Destination Co-ordinates
Dim destinationCoOrdinateInXDir As Double, destinationCoOrdinateInYDir As Double

' Setting the values of Destination Co-ordinates in X & Y directions for Move
destinationCoOrdinateInXDir = 10 * LengthConversionFactor
destinationCoOrdinateInYDir = 10 * LengthConversionFactor

' Move circle
swDoc.Extension.MoveOrCopy False, 1, False, 0, 0, 0, destinationCoOrdinateInXDir, destinationCoOrdinateInYDir, 0

In above line we Move Sketch Entities to new position i.e. 10” in X-Direction and 10” in Y-Direction.

In above code we need to set following parameters:

  • Copy : False to not create a copy.

  • NumCopies : Number of copies you want to create to 1 which is itself.

  • KeepRelations : True to keep sketch relations after Move or Copy operation.

  • BaseX : X coordinate of the base point = 0

  • BaseY : Y coordinate of the base point = 0

  • BaseZ : Z coordinate of the base point = 0

  • DestX : X coordinate of the destination = 10”

  • DestY : Y coordinate of the destination point = 10”

  • DestZ : Z coordinate of the destination point = 0

Example Images:

Below image shows before and after we Move Sketch Entitny.

Before Move Sketch Entitny

before-move-copy

After Move Sketch Entitny

after-move

CASE 2 : Copy Sketch Entities

In our code, if we want to Copy Sketch Entities, then we need to use code sample as given below:

' Defining variables for Destination Co-ordinates
Dim destinationCoOrdinateInXDir As Double, destinationCoOrdinateInYDir As Double

' Setting the values of Destination Co-ordinates in X & Y directions for Move
destinationCoOrdinateInXDir = 15 * LengthConversionFactor
destinationCoOrdinateInYDir = 15 * LengthConversionFactor

' Copy circle
swDoc.Extension.MoveOrCopy True, 3, True, 0, 0, 0, destinationCoOrdinateInXDir, destinationCoOrdinateInYDir, 0

In above line we Copy Sketch Entities to new position i.e. 15” in X-Direction and 15” in Y-Direction for every copy of sketch.

This will more clear in below images when you scroll down.

In above code we need to set following parameters:

  • Copy : True to create a copy.

  • NumCopies : Number of copies we want to create: 3

  • KeepRelations : True to keep sketch relations after Move or Copy operation.

  • BaseX : X coordinate of the base point = 0

  • BaseY : Y coordinate of the base point = 0

  • BaseZ : Z coordinate of the base point = 0

  • DestX : X coordinate of the destination = 15”

  • DestY : Y coordinate of the destination point = 15”

  • DestZ : Z coordinate of the destination point = 0

Example Images:

Below image shows before and after we Copy Sketch Entitny.

Before Copy Sketch Entitny

before-move-copy

After Copy Sketch Entitny

after-copy

This is it !!!

I hope my efforts will helpful to someone!

If you found anything to add or update, please let me know on my e-mail.

Hope this post helps you to Move/Copy Sketch Entities with Solidworks VBA Macros.

For more such tutorials on Solidworks VBA Macro, do come to this blog after sometime.

If you like the post then please share it with your friends also.

Do let me know by you like this post or not!

Till then, Happy learning!!!

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