Solidworks Macro - Create Extrude/Boss

11 minute read

In this post, I tell you about how to create Extrude/Boss through Solidworks VBA Macros in a sketch.

In this post, I tell you about FeatureExtrusion3 method from Solidworks FeatureManager object.

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

So use this method if you want to create a new Corner Extrude/Boss.

Code Sample

Below is the code sample for creating Corner Rectangle.

                        Option Explicit

' Creating variable for Solidworks application
Dim swApp As SldWorks.SldWorks
' Creating variable for Solidworks document
Dim swDoc As SldWorks.ModelDoc2
' Boolean Variable
Dim BoolStatus As Boolean
' Creating variable for Solidworks Sketch Manager
Dim swSketchManager As SldWorks.SketchManager
' Creating variable for Solidworks Feature
Dim swFeature As SldWorks.Feature

' Main function of our VBA program
Sub main()

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

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

  ' Selecting Front Plane
  BoolStatus = swDoc.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, False, 0, Nothing, swSelectOption_e.swSelectOptionDefault)
  
  ' Setting Sketch manager for our sketch
  Set swSketchManager = swDoc.SketchManager
  
  ' Inserting a sketch into selected plane
  swSketchManager.InsertSketch True
  
  ' Creating a "Variant" Variable which holds the values return by "CreateCornerRectangle" method
  Dim vSketchLines As Variant
  
  ' Creating a Corner Rectangle
  vSketchLines = swSketchManager.CreateCornerRectangle(0, 1, 0, 1, 0, 0)
  
  ' De-select the lines after creation
  swDoc.ClearSelection2 True
  
  ' Zoom to fit screen in Solidworks Window
  swDoc.ViewZoomtofit2
  
  ' Exit the Sketch
  swSketchManager.InsertSketch True

  ' Create Extrude Feature
  Set swFeature = swDoc.FeatureManager.FeatureExtrusion3(True, False, False, swEndConditions_e.swEndCondBlind, swEndConditions_e.swEndCondBlind, 2, 0, False, False, False, True, 0, 0, False, False, False, False, True, False, True, swEndConditions_e.swEndCondBlind, 0, False)

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

                        ' Creating variable for Solidworks Feature
Dim swFeature As SldWorks.Feature

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

We create variable swFeature for Solidworks Feature.

To see methods and properties related to Feature 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.

                        ' 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.

                        ' Creating a "Variant" Variable which holds the values return by "CreateCornerRectangle" method
Dim vSketchLines As Variant
    
' Creating a Corner Rectangle
vSketchLines = swSketchManager.CreateCornerRectangle(0, 1, 0, 1, 0, 0)

In above sample code, we 1st create a variable named vSketchLines of type Variant.

A Variant type variable can hold any type of value depends upon the use of variable.

In 2nd line, we set the value of variable vSketchLines.

In the above code sample I have used (0, 1, 0) Upper-left point in Y-direction.

For Lower-right point I used (1, 0, 0) which is 1 point distance in X-direction.

This CreateCornerRectangle method returns an array of sketch segments that represent the edges created for this corner rectangle.

For more information about Create Corner Rectangle please visit Solidworks Macros - Selection Methods post.

It is very important to remember that, when you give distance or any other numeric value in Solidworks API, Solidworks takes that numeric value in Meter only.
Solidworks API does not care about your application’s Unit systems.
For example, I works in ANSI system means inches for distance.
But when I used Solidworks API through VBA macros or C#, I need to use converted numeric values.
Because Solidworks API output the distance in Meter which is not my requirement.

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

In the this line of code, we deselect the Corner rectangle we have created.

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

                        ' Zoom to fit screen in Solidworks Window
swDoc.ViewZoomtofit2

In this last line we use zoom to fit command.

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

                        ' Exit the Sketch
swSketchManager.InsertSketch True

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

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

                        ' Create Extrude Feature
Set swFeature = swDoc.FeatureManager.FeatureExtrusion3(True, False, False, swEndConditions_e.swEndCondBlind, swEndConditions_e.swEndCondBlind, 2, 0, False, False, False, True, 0, 0, False, False, False, False, True, True, True, swEndConditions_e.swEndCondBlind, 0, False)

In above line of code we set the value of variable swFeature by FeatureExtrusion3 method.

FeatureExtrusion3 method is part of FeatureManager object.

This FeatureManager is again part of swDoc variable i.e. ModelDoc2 object.

Method Parameters Details

This FeatureExtrusion3 method takes following parameters as explained:

Sd - True for single ended, False for double ended.
Flip - True to flip the side to cut

This option activate when we select feature “Extruded Cut”.
Dir - True to flip the direction of extrusion.
T1 - Termination type for first end of the extrusion as defined in swEndConditions_e.

End Conditions has following enumeration values:
- swEndCondBlind or 0
- swEndCondMidPlane or 6
- swEndCondOffsetFromSurface or 5
- swEndCondThroughAll or 1
- swEndCondThroughAllBoth or 9
- swEndCondThroughNext or 2
- swEndCondUpToBody or 7
- swEndCondUpToNext or 11
- swEndCondUpToSelection or 10
- swEndCondUpToSurface or 4 = Do not use; superseded by swEndCondUpToSelection
- swEndCondUpToVertex or 3 = Do not use; superseded by swEndCondUpToSelection
T2 - Termination type for second end of the extrusion as defined in swEndConditions_e.

End Conditions has enumeration values as described in T1.
D1 - Depth of extrusion for first end in meters; offset, if T1 is set to swEndConditions_e.swEndCondOffsetFromSurface
D2 - Depth of extrusion for second end in meters; offset, if T2 is set to swEndConditions_e.swEndCondOffsetFromSurface
Dchk1 - True to allow drafting in the first direction, False to not
Dchk2 - True to allow drafting in the second direction, False to not
Ddir1 - True for first draft angle to be inward, False to be outward; valid only if Dchk1 is true
Ddir2 - True for second draft angle to be inward, False to be outward; valid only if Dchk2 is true
Dang1 - Draft angle for first end; valid only if Dchk1 is true
Dang2 - Draft angle for second end; valid only if Dchk2 is true
OffsetReverse1 - True to offset the first end from another face or plane in a direction away from the sketch, False to offset in a direction toward the sketch; valid only if T1 is set to swEndConditions_e.swEndCondOffsetFromSurface
OffsetReverse2 - True to offset the second end from another face or plane in a direction away from the sketch, False to offset in a direction toward the sketch; valid only if T2 is set to swEndConditions_e.swEndCondOffsetFromSurface
TranslateSurface1 - True if the first end of the extrusion is a translation of the reference surface, False if it has a true offset; valid only if T1 is set to swEndConditions_e.swEndCondOffsetFromSurface
TranslateSurface2 - True if the second end of the extrusion is a translation of the reference surface, False if it has a true offset; valid only if T2 is set to swEndConditions_e.swEndCondOffsetFromSurface
Merge - True to merge the results in a multibody part, False to not

This option visible when we Extrude from existing feature/body.
UseFeatScope - True if the feature only affects selected bodies, False if the feature affects all bodies.
UseAutoSelect - True to automatically select all bodies and have the feature affect those bodies, False to select the bodies that the feature affects.
T0 - Start condition as defined in swStartConditions_e

Start Conditions has following enumeration values:
- swStartOffset or 3
- swStartSketchPlane or 0
- swStartSurface or 1
- swStartVertex or 2
StartOffset - Distance from the sketch plane to start the extrude; valid only if T0 is set to swStartConditions_e.swStartOffset
FlipStartOffset - True to flip the direction of the start offset, False to not; valid only if T0 is set to swStartConditions_e.swStartOffset

Return Value : This FeatureExtrusion3 method retun Feature object.

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

In our code, I have used following values:

Sd - I use True for single ended.
Flip - I use False to flip the side to cut
Dir - I use False to flip the direction of extrusion
T1 - *I use swEndConditions_e.swEndCondBlind of Termination type for first end of the extrusion *
T2 - *I use swEndConditions_e.swEndCondBlind of Termination type for second end of the extrusion *
D1 - I use 2 as *Depth of extrusion for first end in meters*
D2 - I use 0 as *Depth of extrusion for second end in meters*
Dchk1 - I use False to allow drafting in the first direction
Dchk2 - I use False to allow drafting in the second direction
Ddir1 - I use False for first draft angle to be inward
Ddir2 - I use True for second draft angle to be inward

Since Dchk2 is False, setting the value to True is invalid.
Dang1 - I use 0 for first end’s draft angle
Dang2 - I use 0 for second end’s draft angle
OffsetReverse1 - I use False to offset the first end from another face or plane in a direction away from the sketch
OffsetReverse2 - I use False to offset the second end from another face or plane in a direction away from the sketch
TranslateSurface1 - I use False to the first end of the extrusion is a translation of the reference surface
TranslateSurface2 - I use False to the second end of the extrusion is a translation of the reference surface
Merge - I use True to merge the results in a multibody part
UseFeatScope - I use False so that this feature affects to all bodies
UseAutoSelect - I use True to automatically select all bodies and have the feature affect those bodies
T0 - I use swEndConditions_e.swEndCondBlind as Start condition
StartOffset - I use 0 for distance from the sketch plane to start the extrude
FlipStartOffset - I use False to flip the direction of the start offset

After running macro we get extrude as shown in below image.

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 create Extrude/Boss 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!!!