Solidworks Macro - Add dimension to Sketch Entities

20 minute read

Introduction

In this post, I tell you about how to Add dimension to Sketch Entities using Solidworks VBA Macros in a Sketch.

In this post, I explain about 2 different methods from which are listed below.

  1. From ModelDoc2 object

  2. From ModelDocExtension object

Methods from these objects are updated methods, hence use any one of them for adding dimension.

Method From ModelDoc2 object

Below is the code sample to Add dimension to Sketch Entities using ModelDoc2 object’s AddDimension2 method.

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
  
  ' Create a circle of diameter 10
  Set swSketchSegment = swSketchManager.CreateCircle(0, 0, 0, 10 * LengthConversionFactor, 0, 0)
  
  ' Disable dimension input box before adding dimension
  swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
  
  ' Add dimension to circle
  swDoc.AddDimension2 10 * LengthConversionFactor, 10 * LengthConversionFactor, 0
  
  ' Enable dimension input box after adding dimension
  swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True
  
  ' De-select all 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 ModelDoc2 object method

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.

' Create a circle of diameter 10
Set swSketchSegment = swSketchManager.CreateCircle(0, 0, 0, 10 * LengthConversionFactor, 0, 0)

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

This CreateCircle method creates a Circle between “2 given point distance as diameter”.

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

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

In above line, we create a Circle with:

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

  • Circle Diameter : 10 unit length

' Disable dimension input box before adding dimension
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False

In above line of code, we Disable dimension input box before adding dimension. 

' Add dimension to circle
swDoc.AddDimension2 10 * LengthConversionFactor, 10 * LengthConversionFactor, 0

For “adding dimension” to an sketch entity, we need AddDimension2 method from Solidworks ModelDoc2 object.

This AddDimension2 method takes following parameters as explained:

  • X : X coordinate of Dimension text location in meters.

  • Y : y coordinate of Dimension text location in meters.

  • Z : z coordinate of Dimension text location in meters.

After the function complete following are the results:

Return Value:

  • IDisplayDimension: Newly created dimension.

In our code, I have used following values:

  • X : X coordinate of Dimension text location = 10 * LengthConversionFactor.

  • Y : y coordinate of Dimension text location = 10 * LengthConversionFactor.

  • Z : z coordinate of Dimension text location = 0.

Below image shows before and after Circular Sketch Pattern.

Before Circular Sketch Pattern

before-add-dimension

After Circular Sketch Pattern

after-add-dimension

' Enable dimension input box after adding dimension
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True

In above line of code, we Enable dimension input box after adding dimension.

' De-select the Sketch after creation
swDoc.ClearSelection2 True

In the above line of code, we deselect the Sketch after the Linear Sketch Pattern operation.

For de-selecting, we use ClearSelection2 method from our Solidworks document name swDoc.

' Show Front View after Linear Sketch Pattern
swDoc.ShowNamedView2 "", swStandardViews_e.swFrontView

In the above line of code, we update the view orientation to Front View.

In my machine, after inserting a sketch view orientation does not changed.

Because of this I have to update the view to Front view.

For showing Front View we used ShowNamedView2 method from our Solidworks document name swDoc.

This method takes 2 parameter described as follows:

  • VName : Name of the view to display or an empty string to use ViewId instead

  • ViewId : ID of the view to display as defined by swStandardViews_e or -1 to use the VName argument instead.

NOTE: If you specify both VName and ViewId, then ViewId takes precedence if the two arguments do not resolve to the same view.

swStandardViews_e has following Standard View Types:

  • swBackView

  • swBottomView

  • swDimetricView

  • swFrontView

  • swIsometricView

  • swLeftView

  • swRightView

  • swTopView

  • swExtendetricView

In our code, we did not use VName instead I used empty string in form of ”“ symbol.

I used ViewId value to specify view and used swStandardViews_e.swFrontView value to use Standard Front View.

' Zoom to fit screen in Solidworks Window
swDoc.ViewZoomtofit

In this last line we use zoom to fit command.

For Zoom to fit, we use ViewZoomtofit method from our Solidworks document variable swDoc.

Method From ModelDocExtension object

Below is the code sample to Add dimension to Sketch Entities using ModelDocExtension object’s AddDimension method

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

' Create Variable for Solidworks Display Dimension
Dim swDisplayDim As SldWorks.DisplayDimension

' 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
  
  ' Create a circle of diameter 10
  Set swSketchSegment = swSketchManager.CreateCircle(0, 0, 0, 10 * LengthConversionFactor, 0, 0)
  
  ' Disable dimension input box before adding dimension
  swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False
  
  ' Add dimension to circle
  Set swDisplayDim = swDoc.Extension.AddDimension(0, 12 * LengthConversionFactor, 0, swSmartDimensionDirection_e.swSmartDimensionDirection_Right)
  
  ' Enable dimension input box after adding dimension
  swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True
  
  ' De-select all 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 ModelDocExtension object method

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

' Create Variable for Solidworks Display Dimension
Dim swDisplayDim As SldWorks.DisplayDimension

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

We create variable swDisplayDim for dimension we create.

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.

' Create a circle of diameter 10
Set swSketchSegment = swSketchManager.CreateCircle(0, 0, 0, 10 * LengthConversionFactor, 0, 0)

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

This CreateCircle method creates a Circle between “2 given point distance as diameter”.

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

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

In above line, we create a Circle with:

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

  • Circle Diameter : 10 unit length

' Disable dimension input box before adding dimension
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, False

In above line of code, we Disable dimension input box before adding dimension. 

' Add dimension to circle
Set swDisplayDim = swDoc.Extension.AddDimension(0, 12 * LengthConversionFactor, 0, swSmartDimensionDirection_e.swSmartDimensionDirection_Right)

For “adding dimension” to an sketch entity, we need AddDimension method from Solidworks ModelDocExtension object.

This AddDimension method takes following parameters as explained:

  • X : X coordinate of Dimension text location in meters.

  • Y : y coordinate of Dimension text location in meters.

  • Z : z coordinate of Dimension text location in meters.

  • Direction : Direction of dimensioning extension line or rapid dimensioning quadrant as defined in swSmartDimensionDirection_e.

There are 4 values we can use from swSmartDimensionDirection_e enum.

They are as follows:

  • swSmartDimensionDirection_Down

  • swSmartDimensionDirection_Left

  • swSmartDimensionDirection_Right

  • swSmartDimensionDirection_Up

After the function complete following are the results:

Return Value:

  • IDisplayDimension: Newly created dimension.

In our code, I have used following values:

  • X : X coordinate of Dimension text location = 0.

  • Y : y coordinate of Dimension text location = 12 * LengthConversionFactor.

  • Z : z coordinate of Dimension text location = 0.

  • Direction : Direction of dimensioning extension line or rapid dimensioning quadrant = swSmartDimensionDirection_e.swSmartDimensionDirection_Right.

Below image shows before and after Circular Sketch Pattern.

Before Circular Sketch Pattern

before-add-dimension

After Circular Sketch Pattern

after-add-dimension

' Enable dimension input box after adding dimension
swApp.SetUserPreferenceToggle swUserPreferenceToggle_e.swInputDimValOnCreate, True

In above line of code, we Enable dimension input box after adding dimension.

' De-select the Sketch after creation
swDoc.ClearSelection2 True

In the above line of code, we deselect the Sketch after the Linear Sketch Pattern operation.

For de-selecting, we use ClearSelection2 method from our Solidworks document name swDoc.

' Show Front View after Linear Sketch Pattern
swDoc.ShowNamedView2 "", swStandardViews_e.swFrontView

In the above line of code, we update the view orientation to Front View.

In my machine, after inserting a sketch view orientation does not changed.

Because of this I have to update the view to Front view.

For showing Front View we used ShowNamedView2 method from our Solidworks document name swDoc.

This method takes 2 parameter described as follows:

  • VName : Name of the view to display or an empty string to use ViewId instead

  • ViewId : ID of the view to display as defined by swStandardViews_e or -1 to use the VName argument instead.

NOTE: If you specify both VName and ViewId, then ViewId takes precedence if the two arguments do not resolve to the same view.

swStandardViews_e has following Standard View Types:

  • swBackView

  • swBottomView

  • swDimetricView

  • swFrontView

  • swIsometricView

  • swLeftView

  • swRightView

  • swTopView

  • swExtendetricView

In our code, we did not use VName instead I used empty string in form of ”“ symbol.

I used ViewId value to specify view and used swStandardViews_e.swFrontView value to use Standard Front View.

' Zoom to fit screen in Solidworks Window
swDoc.ViewZoomtofit

In this last line we use zoom to fit command.

For Zoom to fit, we use ViewZoomtofit method from our Solidworks document variable swDoc.

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 Add dimension to 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!!!

Updated: