Solidworks Macro - Offset Sketch Entities

13 minute read

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

Video of Code on YouTube

Please see below video how visually we Offset Sketch Entities in Solidworks VBA macro.

Please note that there are no explaination given in the video.

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

For Experience Macro Developer

If you are an experience Solidworks Macro developer, then you are looking for a specific code sample.

Below is the code for Offset Sketch Entities from Solidworks VBA Macro.

                        ' Boolean Variable
Dim BoolStatus As Boolean

' Select Line 1
BoolStatus = swDoc.Extension.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, swSelectOption_e.swSelectOptionDefault)

' Select Line 2
BoolStatus = swDoc.Extension.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, swSelectOption_e.swSelectOptionDefault)

' Offset Solidworks Sketch segment by "SketchOffset2" method from Solidworks sketch manager
BoolStatus = swSketchManager.SketchOffset2(0.5, False, False, swSkOffsetCapEndType_e.swSkOffsetNoCaps, swSkOffsetMakeConstructionType_e.swSkOffsetDontMakeConstruction, True)

                      

Method Name: SketchOffset2

Description: Offsets the selected sketch entities.

For Offset Solidworks Sketch entities, first you need to Create a variable of Boolean type.

After creating variable, you need to set the value of this Boolean variable.

For this you used SketchOffset2 method from Solidworks Sketch Manager.

This SketchOffset2 method set the value of Boolean type variable.

If Offset is successful then SketchOffset2 method return True value otherwise SketchOffset2 returns False value.

This SketchOffset2 method takes following parameters as explained:

Offset : Offset value; negative value offsets the sketch entities in the opposite direction

BothDirections : True to offset the sketch entities in both directions, false to offset the sketch entities in one direction

Chain : True to offset the chain of sketch entities, false to offset only the selected sketch entities

CapEnds : Cap the ends as defined by swSkOffsetCapEndType_e

swSkOffsetCapEndType_e enum defines following different End cap types constants:

swSkOffsetArcCaps
swSkOffsetLineCaps
swSkOffsetNoCaps

MakeConstruction : Convert original and offset sketch entities to construction sketch entities as defined by swSkOffsetMakeConstructionType_e

swSkOffsetMakeConstructionType_e enum defines following different Construction Types constants:

swSkOffsetDontMakeConstruction
swSkOffsetMakeBothConstruction
swSkOffsetMakeOffsConstruction
swSkOffsetMakeOrigConstruction

AddDimensions : True to add the dimension to the offset, false if not want to add the dimension to the offset.

If you want more detailed explaination then please read further otherwise this will help you to Offset Sketch Entities From VBA Macro.

For Beginners Macro Developers

In this post, I tell you about SketchOffset2 method from Solidworks SketchManager object.

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

So use this method if you want to Offset Sketches.

Below is the code sample for Offset Sketches.

                        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)

  ' 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
  
  ' Set Sketch Segment value and Create Line 1
  Set swSketchSegment = swSketchManager.CreateLine(-0.5, 0.75, 0, -0.25, -0.5, 0)
  
  ' Set Sketch Segment value and Create Line 2
  Set swSketchSegment = swSketchManager.CreateLine(-0.75, -1.25, 0, 0.5, -1.25, 0)
  
  ' De-select the lines after creation
  swDoc.ClearSelection2 True
  
  ' Select Line 1
  BoolStatus = swDoc.Extension.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, swSelectOption_e.swSelectOptionDefault)

  ' Select Line 2
  BoolStatus = swDoc.Extension.SelectByID2("Line2", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, swSelectOption_e.swSelectOptionDefault)

  ' Offset selected Sketch Segments by "SketchOffset2" method from Solidworks sketch manager
  BoolStatus = swSketchManager.SketchOffset2(0.5, False, False, swSkOffsetCapEndType_e.swSkOffsetNoCaps, swSkOffsetMakeConstructionType_e.swSkOffsetDontMakeConstruction, True)

  ' De-select the Sketch Segment after Offset
  swDoc.ClearSelection2 True
  
  ' Show Front View after Offset Sketch Segments
  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.

                        ' 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.

                        ' Set Sketch Segment value and Create Line 1
Set swSketchSegment = swSketchManager.CreateLine(-0.5, 0.75, 0, -0.25, -0.5, 0)

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

This CreateLine method creates Lines between 2 given points.

For more information about CreateLine method, you can read my Solidworks Sketch Macros - Create Line post.

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

In above line, we create a Line between point (-0.5, 0.75, 0) and point (-0.25, -0.5, 0).

This line is not parallel to any axis.

This line is at an angle to Vertical axis.

                        ' Set Sketch Segment value and Create Line 2
Set swSketchSegment = swSketchManager.CreateLine(-0.75, -1.25, 0, 0.5, -1.25, 0)

In above line we create Line 2 by using same CreateLine method from Solidworks Sketch Manager.

In above code, we create our 2nd line between point (-0.75, -1.25, 0) and point (0.5, -1.25, 0).

This line is parallel to X-axis.

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

After creating both lines we de-select those lines.

We don’t need to de-select the lines for Offset operation as we will select those lines agains in next 2 lines. I just want to show you how to select a Sketch Segment with SelectById Menthod in next line of code.

                        ' Select Line 1
BoolStatus = swDoc.Extension.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, False, 0, Nothing, swSelectOption_e.swSelectOptionDefault)

In above line of code, we select Line 1.

                        ' Select Line 2
BoolStatus = swDoc.Extension.SelectByID2("Line1", "SKETCHSEGMENT", 0, 0, 0, True, 0, Nothing, swSelectOption_e.swSelectOptionDefault)

In above line of code, we select Line 2 and add Line 2 to selection list.

                        ' Offset selected Sketch Segments by "SketchOffset2" method from Solidworks sketch manager
BoolStatus = swSketchManager.SketchOffset2(0.5, False, False, swSkOffsetCapEndType_e.swSkOffsetNoCaps, swSkOffsetMakeConstructionType_e.swSkOffsetDontMakeConstruction, True)

In above line, we Offset selected Lines by SketchOffset2 method from Solidworks sketch manager.

This SketchOffset2 method takes following parameters as explained:

Offset : Offset value; negative value offsets the sketch entities in the opposite direction

BothDirections : True to offset the sketch entities in both directions, false to offset the sketch entities in one direction

Chain : True to offset the chain of sketch entities, false to offset only the selected sketch entities

CapEnds : Cap the ends as defined by swSkOffsetCapEndType_e

swSkOffsetCapEndType_e enum defines following different End cap types constants:

swSkOffsetArcCaps
swSkOffsetLineCaps
swSkOffsetNoCaps

MakeConstruction : Convert original and offset sketch entities to construction sketch entities as defined by swSkOffsetMakeConstructionType_e

swSkOffsetMakeConstructionType_e enum defines following different constants:

swSkOffsetDontMakeConstruction
swSkOffsetMakeBothConstruction
swSkOffsetMakeOffsConstruction
swSkOffsetMakeOrigConstruction

AddDimensions : True to add the dimension to the offset, false if not want to add the dimension to the offset.

Return Value:

True: If Extend operation is Success.
False: If Extend operation is Fail.

In our code, I have used following values:

Offset : I have used 0.5 value for Offset.

BothDirections : I have used False value for BothDirections.

Chain : I have used False value for Chain.

CapEnds : I have used swSkOffsetCapEndType_e.swSkOffsetNoCaps value for CapEnds.

MakeConstruction : I have used swSkOffsetMakeConstructionType_e.swSkOffsetDontMakeConstruction value for MakeConstruction.

AddDimensions : I have used True value for AddDimensions.

Below image shows before and after Offset operation on the sketch.

Before Offset Operation

before-offset

After Offset Operation

after-offset

Now let us modify some values and look for the changes:

BothDirections : Let us change the value to True value for BothDirections and see the result:

offset-both-side

CapEnds : Now we change the value of End cap.

Please see below for both Line and Arc option for End cap:

If we change CapEnds value to swSkOffsetLineCaps and then the result would be:

end-cap-is-line-type

If we change CapEnds value to swSkOffsetArcCaps and then the result would be:

end-cap-is-arc-type

These 2 covers all option available in Cap End.

MakeConstruction : Now we change the value of MakeConstruction.

Please see below for all MakeConstruction options:

If we change MakeConstruction value to swSkOffsetMakeOrigConstruction and then the result would be:

make-original-entities-construction

If we change MakeConstruction value to swSkOffsetMakeOffsConstruction and then the result would be:

make-offset-entities-construction

If we change MakeConstruction value to swSkOffsetMakeBothConstruction and then the result would be:

original-and-offset-entities-are-construction

This covers all options in SketchOffset2 method.

NOTE

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 Sketch after creation
swDoc.ClearSelection2 True

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

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

                        ' Show Front View after Sketch Offset
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 !!!

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

VBA Language feature used in this post

In this post used some features of VBA programming language.

This section of post, has some brief information about the VBA programming language specific features.

We use Option Explicit for capturing un-declared variables. If you want to read more about Option Explicit then please visit Declaring and Scoping of Variables.
Then we create variable for different data types. If you know in detail about the Variables, then please visit Variables and Data-types posts of this blog. It will help you to understand what Variables are and how to use them.
Then we create main Sub procedure for our macro. If you know in detail about the Sub procedure, then I suggest you to visit VBA Sub and Function Procedures and Executing Sub and Function Procedures posts of this blog. It will help you to understand what Procedures are and how to use them.
In most part we create some variables and set their values. We set those values by using some functions provided from objects. If you don’t know about the functions, then you should visit VBA Functions and VBA Functions that do more posts of this blog. It will help you to understand what functions are and how to use them.

Solidworks API Objects

In this post of Sketch Offset, we use Solidworks API objects and their methods.

This section contains the list of all Solidworks Objects used in this post.

I have also attached links of these Solidworks API Objects in API Help website.

If you want to explore those objects, you can use these links.

These Solidworks API Objects are listed below:

Solidworks Application Object

If you want explore Properties and Methods/Functions of Solidworks Application Object object you can visit this link.
Solidworks Document Object

If you want explore Properties and Methods/Functions of Solidworks Document Object object you can visit this link.
Solidworks Sketch Manager Object

If you want explore Properties and Methods/Functions of Solidworks Sketch Manager Object you can visit this link.
Solidworks Sketch Segment Object

If you want explore Properties and Methods/Functions of Solidworks Sketch Segment Object you can visit this link.

Hope this post helps you to Offset Sketch Entities with Solidworks VBA Macros.

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

Till then, Happy learning!!!