Solidworks VBA Macro - Create Shell

13 minute read

This article has "Beginner ➡ Intermediate" level Macro program.
If you are following my articles then will not be an issue for you.
In this article we did not use 🚀 UserForm for taking inputs, instead we use 🚀 Input Box for value input and 🚀 Message Box to notify user.
I hope you will also like this type of tutorials.
Thank you for reading.

Objective

In this article I want to:

Create Shell feature
From VBA Macro
Without using Userforms.

This method is most updated method, so use this method if you want to create a new Shell Feature quickly.

Results We Can Get

After running our macro we successfully create Shell feature as a result.

Below image shows the result we get.

We create Shell Feature in following steps in general.

Ask user to select **Faces to Shell **.
Ask for Shell Thickness.

To get the correct result please follow the steps correctly.

Macro Video

Below 🎬 video shows Shell feature from SOLIDWORKS VBA Macros.

Above video is just for visualization and there are no explanation.

I have explained each and every line in this article.

It is advisable to watch video, since it help you to better understand the process.

VBA Macro

Below is the VBA macro for creating Shell Feature.

                        Option Explicit

' Variable for Solidworks Application
Dim swApp As SldWorks.SldWorks

' Variable for Solidworks document
Dim swDoc As SldWorks.ModelDoc2

' Variable for Solidworks Selection Manager
Dim swSelMgr As SldWorks.SelectionMgr

' Variable for Solidworks Select Data
Dim swSelData As SldWorks.SelectData

' Main program for Shell
Sub main()

  ' Set Solidworks Application variable to current application
  Set swApp = Application.SldWorks
  
  ' Check if Solidworks is opened or not
  If swApp Is Nothing Then
    MsgBox ("Solidworks is not opened")
    Exit Sub
  End If
  
  ' Set Solidworks document variable to currently opened document
  Set swDoc = swApp.ActiveDoc
  
  ' Check if Solidworks document is opened or not
  If swDoc Is Nothing Then
    MsgBox ("Solidworks document is not opened. Please open a document.")
    Exit Sub
  End If
  
  ' Set Solidworks Selection Manager variable
  Set swSelMgr = swDoc.SelectionManager
  
  ' Variable for Solidworks Entity
  Dim swObject As SldWorks.Entity
  
  ' Message to show user
  Dim messageToUser As String

  ' Update Messages
  messageToUser = "Please select a Face."

  ' Show message to user
  MsgBox messageToUser
  
  ' Loop until we complete our selection
  While swObject Is Nothing
      
    ' Local integer for loop
    Dim i As Integer
    
    ' Looping until we select
    For i = 1 To swSelMgr.GetSelectedObjectCount2(-1)
      
      ' If the selection type is face
      If swSelMgr.GetSelectedObjectType3(i, -1) = swSelectType_e.swSelFACES Then
          
        ' Set the Solidworks Entity object to feature
        Set swObject = swSelMgr.GetSelectedObject6(i, -1)
          
      Else

        ' Inform user to select a Face
        MsgBox "Please select a Face."

        ' Clear selection
        swDoc.ClearSelection2 True
      End If
    Next
    
    DoEvents
  Wend
    
  ' Clear previous selection
  swDoc.ClearSelection2 True
  
  ' Create Select data for this entity
  Set swSelData = swSelMgr.CreateSelectData
  
  ' For shell face, set mark to 1
  swSelData.Mark = 1

  ' Select the current entity
  swObject.Select4 True, swSelData
  
  ' 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
  
  ' Variable for Shell thickness
  Dim shellThickness As Double
  
  ' Getting Shell thickness from user.
  shellThickness = InputBox("Please select Shell Thickness.") * LengthConversionFactor
  
  ' Create Shell feature
  swDoc.InsertFeatureShell shellThickness, False
  
  ' View zoom to fit
  swDoc.ViewZoomtofit2
  
  ' Clear all selection
  swDoc.ClearSelection2 True

End Sub

                      

Prerequisite

There are some prerequisite for this macro.

Knowledge of VBA programming language is ❗required.
We are not creating feature from code but we use existing 🚀 Extrude feature to create Shell feature.

Below image shown prerequisite 3D model for our demo.

As shown in above image, there is one Extrude features in our part.

Base Feature : This is our Base Extrude feature.

If you want to create this Extrude features programmatically then please refer to below article.

🚀 SOLIDWORKS Macros - Create Extrude/Boss

We will apply checks in this article, so the code we write should be error free most of the time.

Steps To Follow

This Shell Feature VBA macro can be divided into following sections:

Creating Global Variables
Initializing required variables
Ask user to select faces
Mark selected entities
Get unit Conversion factors
Get Shell Thickness
Create Shell feature
Final work

Every section with each line is explained below.

I also give some links (see icon 🚀) so that you can go through them if there are anything I explained in previous articles.

Creating Global Variables

Option Explicit

Purpose: Above line forces us to define every variable we are going to use.
Reference: 🚀 SOLIDWORKS Macros - Open new Part document article.

                        ' Variable for Solidworks application
Dim swApp As SldWorks.SldWorks

Purpose: In above line, we create a variable for Solidworks application.
Variable Name: swApp
Type: SldWorks.SldWorks
Reference: Please visit 🚀 online SOLIDWORKS API Help.

                        ' Variable for Solidworks document
Dim swDoc As SldWorks.ModelDoc2

Purpose: In above line, we create a variable for Solidworks document.
Variable Name: swDoc
Type: SldWorks.ModelDoc2
Reference: Please visit 🚀 online SOLIDWORKS API Help.

                        ' Variable for Solidworks Selection Manager
Dim swSelMgr As SldWorks.SelectionMgr

Purpose: In above line, we create a variable for Solidworks Selection Manager.
Variable Name: swSelMgr
Type: SldWorks.SelectionMgr.
Reference: Please visit 🚀 online SOLIDWORKS API Help.

                        ' Variable for Solidworks Select Data
Dim swSelData As SldWorks.SelectData

Purpose: In above line, we create a variable for Marking of Solidworks Select Data.
Variable Name: swSelData
Type: SldWorks.SelectData
Reference: Please visit 🚀 online SOLIDWORKS API Help.

These all are our global variables.

They are SOLIDWORKS API Objects.

                        ' Main program for Shell
Sub main()

End Sub

In above line, we create main program for Shell Feature.
This is a Sub procedure which has name of main.
This procedure hold all the statements (instructions) we give to computer.
Reference: Detailed information 🚀 VBA Sub and Function Procedures article of this website.

Initializing Required Variables

Inside this section we initialize required variables.

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

In above line, we set value of swApp variable.
This value is currently opened Solidworks application.

                        ' Check if Solidworks is opened or not
If swApp Is Nothing Then  
  MsgBox ("SOLIDWORKS is not opened")  
  Exit Sub
End If

                      

In above code block, we check if we successfully set the value of swApp variable.
We use 🚀 IF statement for checking.
Condition: swApp Is Nothing
When this condition is True,
- We show and 🚀 message window to user.
- Message: SOLIDWORKS is not opened
- Then we stop our macro here.

                        ' Set Solidworks document variable to currently opened document
Set swDoc = swApp.ActiveDoc

In above line, we set value of swDoc variable.
This value is currently opened part document.

                        ' Check if Solidworks document is opened or not
If swDoc Is Nothing Then
  MsgBox ("Solidworks document is not opened. Please open a document.")
  Exit Sub
End If

                      

In above code block, we check if we successfully set the value of swDoc variable.
We use 🚀 IF statement for checking.
Condition: swDoc Is Nothing
When this condition is True,
- We show and 🚀 message window to user.
- Message: SOLIDWORKS document is not opened. Please open a document.
- Then we stop our macro here.

                        ' Set Solidworks Selection Manager variable
Set swSelMgr = swDoc.SelectionManager

In above line, we set value of swSelMgr variable.
This value is current document’s Selection Manager.

                        ' Variable for Solidworks Entity
Dim swObjects As SldWorks.Entity

Purpose: In above line, we create a variable for selection and marking of Solidworks Entity.
Variable Name: swObject
Type: SldWorks.Entity
Reference: Please visit 🚀 online SOLIDWORKS API Help.

Ask user to select face

In this section, we ask user to select face for Shell feature.

                        ' Message to show user
Dim messageToUser As String

In above line, we create a variable to show a messages we want to show before selection.
Variable Name: messageToUser
Type: String

                        ' Update Messages
messageToUser = "Please select a Faces."

In above code block, we set value of messageToUser variable.
We set messageToUser to "Please select a Faces."

                        ' Show message to user
MsgBox messageToUser

In above line, we show the message to user.
Below image shows the message for Face selection to the user.

                        ' Loop until we complete our selection
While swObject Is Nothing    

Wend

In above line, we create another While loop.
This loops continues to run until we select the our Face for Shell feature.
Reference: 🚀 VBA Looping article from this website.

                        ' Local integer for loop
Dim i As Integer

In above line, we create a variable as a counter.
Variable Name: i
Type: Integer

                        ' Loop until we select
For i = 1 To swSelMgr.GetSelectedObjectCount2(-1)

Next

In above line, we create a For loop.
This loops start from i = 1 to number of objects we select.

                        ' If the selection type is face
If swSelMgr.GetSelectedObjectType3(i, -1) = swSelectType_e.swSelFACES Then

  ' Set the Solidworks Entity object to feature
  Set swObjects(selectItems) = swSelMgr.GetSelectedObject6(i, -1)

Else

	' Inform user to select a Face
	MsgBox "Please select a Face."

	' Clear selection
	swDoc.ClearSelection2 True
End If

                      

In above code block, we use 🚀 IF/ElseIf statement with conditions.
The 🚀 IF statement is True when selected object is type of SOLIDWORKS Face.
If selected object is not type of SOLIDWORKS Face then 🚀 Else statement code runs.

When we select Model view, then selected object is SOLIDWORKS Face.
When we select from Feature Tree, then select object is SOLIDWORKS Body Feature.

                        ' Set the Solidworks Entity object to feature
Set swObjects(selectItems) = swSelMgr.GetSelectedObject6(i, -1)

When 🚀 IF statement is True we run above line.
In above line, we set the object inside array.
- Array of SOLIDWORKS Entities = swObjects
- Indexed Entity Object = swObjects[selectItems]
Indexed Entity Object value set by GetSelectedObject6() method.
- GetSelectedObject6() method is part of SOLIDWORKS Selection Manager.
- Reference: Please visit 🚀 online Solidworks API Help.

                        ' Inform user to select a Face
MsgBox "Please select a Face."

' Clear selection
swDoc.ClearSelection2 True

When 🚀 Else statement is True we execute run above lines.
1st Line: We show a message to user to select Feature from Feature Tree.
2nd Line: After that we clear our selection.

DoEvents

After For loop end, we have a call for DoEvents function.
This function repeats the While loop until we complete Face selection.

                        ' Clear previous selection
swDoc.ClearSelection2 True

In above line. we clear previous selection.

Mark selected Entities

In previous section, we complete our selection.

In this section, we complete Select and Mark entities correctly our Face.

                        ' Create Select data for this entity
Set swSelData = swSelMgr.CreateSelectData

In above line, we create SOLIDWORKS Select Data for current SOLIDWORKS Entity object.

                        ' For shell face, set mark to 1  
swSelData.Mark = 1

In above lines, we set Mark to 1.
For Shell feature, Mark values will be 1.
Reference: Please visit 🚀 InsertFeatureShell Method in SOLIDWORS API Help.

                        ' Select the current entity
swObject.Select4 True, swSelData

In above line, we select the object.
We select it by using Select4 method of SOLIDWORKS Entity object.
This method takes 2 arguments.
- Append - True appends the entity to the selection list, False replaces the selection list with this entity.
- Data - Pointer to the ISelectData object.
We use following values as parameter.
- Append - True
- Data - swSelData

Get unit Conversion factors

In this section we get unit Conversion factors.

                        ' 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

                      

I have already explained about this in previous 🚀 Solidworks Macro - Fix Unit Issue article in this website.
Please visit 🚀 Solidworks Macro - Fix Unit Issue article for more details.

Get Shell Thickness

In this section, we get get the Shell Thickness from user.

                        ' Variable to Shell thickness
Dim shellThickness As String

In above line, we create a variable as a counter.
Variable Name: shellThickness
Type: String

                        ' Getting Shell thickness from user
shellThickness = InputBox("Please select Shell Thickness.") * LengthConversionFactor

In above line of code we are doing 3 steps in one line.

Those 3 steps are explained below.

Step 1 - Getting Shell Thickness from user. Below image shows the message for Shell Thickness to the user.

Step 2 - Convert input spacing as per document unit system.
Step 3 - Assigned converted value to shellThickness property.

Create Shell feature

In this section, we create Shell feature.

                        ' Create Shell feature
swDoc.InsertFeatureShell shellThickness, False

In above line of code we create Shel Feature by InsertFeatureShell method.
InsertFeatureShell method is part of swDoc variable i.e. ModelDoc2 object.
This InsertFeatureShell method takes following parameters as explained:
- Thickness - Shell thickness in meters.
- Outward - True for outside, False for inside.
Return Value : This InsertFeatureShell method did not return any value.

In our code, I have used following values:

Parameter Name	Value Used
Thickness	`shellThickness`
Outward	`False`

Reference: For more details about InsertFeatureShell Method: 🚀 online Solidworks API Help for InsertFeatureShell Method.

Final work

In this section, after creating Shell Feature, we have to do some cleaning work so that we can use this macro frequently.

                        ' View zoom to fit
swDoc.ViewZoomtofit2

In above line, we make our view zoom to fit the model.
For this we use ViewZoomtofit2 method which is part of SOLIDWORKS Document variable i.e swDoc variable.

                        ' Clear all selection
swDoc.ClearSelection2 True

In above line, we clear all previous selection.
For this we use ClearSelection2 method which is part of SOLIDWORKS Document variable i.e swDoc variable.

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 Shell Feature with SOLIDWORKS VBA Macros.

For more such tutorials on SOLIDWORKS VBA Macro, do come to this website after sometime.

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

Till then, Happy learning!!!