Solidworks VBA Macro - Add Perpendicular Mate

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 we create and understand VBA macro of adding Perpendicular Mate in Assembly document of SOLIDWORKS CAD Software.

This method is most updated method, so use this method if you want to add Perpendicular Mate quickly.

Results We Can Get

After running our macro we successfully add Perpendicular Mate a Component in an Assembly as a result.

Below image shows the result we get.

We add Perpendicular Mate in following steps in general.

loop through each component in current assembly.
Loop through each face.
Get desired face from user confirmation.
Select required faces for mate.
Add Perpendicular Mate.
Final Work

To get the correct result please follow the steps correctly.

Macro Video

Below 🎬 video shows Adding Perpendicular Mate 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 Perpendicular Mate.

                        Option Explicit

' Variable for Solidworks Application
Dim swApp As SldWorks.SldWorks

' Variable for Solidworks document
Dim swDoc As SldWorks.ModelDoc2

' Variable for Solidworks Assembly
Dim swAssembly As SldWorks.AssemblyDoc

' Variable for Solidworks Component
Dim swComponent As SldWorks.Component2

' Variable for Solidworks Body
Dim swBody As SldWorks.Body2

' Variable for Solidworks Mate Feature
Dim swMateFeature As SldWorks.Feature

' Variable for Solidworks Face
Dim swFace As SldWorks.Face2

' Variable for Solidworks Face List
Dim vFaces(1 To 2) As SldWorks.Face2

' Program to add Perpendicular Mate
Sub main()
  
  ' Set Solidworks Application variable to current application
  Set swApp = Application.SldWorks
  
  ' 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."
    Exit Sub
  End If
  
  ' Set Solidworks Assembly document
  Set swAssembly = swDoc
  
  ' Variable for List of elements
  Dim vArray As Variant
  
  ' Get Components list in opened assembly
  vArray = swAssembly.GetComponents(True)
  
  ' Variable for component Index
  Dim componentIndex As Integer
  
  ' Loop Components List
  For componentIndex = 0 To UBound(vArray)
    
    ' Set Solidworks Component variable
    Set swComponent = vArray(componentIndex)
    
    ' Calling this function
    SelectFace swComponent, componentIndex
    
  Next
  
  ' Loop selected Face List
  For componentIndex = 1 To UBound(vFaces)
    
    ' Get and Set current Face
    Set swFace = vFaces(componentIndex)
    
    ' Select current Face
    swFace.Select True
    
  Next

  ' Add Perpendicular Mate
  Set swMateFeature = swAssembly.AddMate5(swMatePERPENDICULAR, swMateAlignALIGNED, False, 0, 0, 0, 0, 0, 0, 0, 0, False, False, 0, swAddMateError_ErrorUknown)

  ' Check if Mate is added or not
  If swMateFeature Is Nothing Then
    MsgBox "Failed to Add Mate."
    swDoc.ClearSelection2 True
    Exit Sub
  End If
  
  ' Clear all selection
  swDoc.ClearSelection2 True
  
  ' Zoom view to fit
  swDoc.ViewZoomtofit2
  
  ' Rebuild assembly
  swDoc.ForceRebuild3 True
  
End Sub

' Function to select required face for Perpendicular mate
Function SelectFace(component As SldWorks.Component2, componentIndex As Integer)
  
  ' Get body of current component
  Set swBody = component.GetBody
  
  ' Variable for Solidworks Select Data
  Dim swSelData As SldWorks.SelectData
  
  ' Set value of Solidworks Select Data variable
  Set swSelData = swDoc.SelectionManager.CreateSelectData
  
  ' Set Mark of Solidworks Select Data
  swSelData.Mark = 1
  
  ' Get First face
  Set swFace = swBody.GetFirstFace
  
  ' Variable to store Message Box result
  Dim resp As VbMsgBoxResult
  
  ' Loop through all Faces
  Do While Not swFace Is Nothing
    
    ' Select current face
    swFace.Select4 False, swSelData
    
    ' Ask user to confirm this selection
    resp = MsgBox("Is this correct Face?", vbYesNo, "Select Face")
    
    ' Check if user response if Yes
    If resp = vbYes Then
      ' Add current face to List of Faces
      Set vFaces(componentIndex + 1) = swFace
      Exit Function
    End If
    
    ' Get next face
    Set swFace = swFace.GetNextFace
    
  Loop
  
End Function

                      

Prerequisite

There are some prerequisite for this article.

Knowledge of VBA programming language is ❗required.
We use an existing part in Assembly document.
This component is Float as shown in below image.

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

Steps To Follow

This VBA macro can be divided into following sections:

Create and Initialize required variables
Get Components and Loop through them
Get desired face
Select faces
Add Perpendicular Mate
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.

Create and Initialize required 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 Assembly
Dim swAssembly As SldWorks.AssemblyDoc

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

                        ' Variable for Solidworks Component
Dim swComponent As SldWorks.Component2

Purpose: In above line, we create a variable for Solidworks Component.
Variable Name: swComponent
Type: SldWorks.Component2.
Reference: Please visit 🚀 online SOLIDWORKS API Help.

                        ' Variable for Solidworks Body
Dim swBody As SldWorks.Body2

Purpose: In above line, we create a variable for Solidworks Component.
Variable Name: swBody
Type: SldWorks.Body2.
Reference: Please visit 🚀 online SOLIDWORKS API Help.

                        ' Variable for Solidworks Mate Feature
Dim swMateFeature As SldWorks.Feature

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

                        ' Variable for Solidworks Face
Dim swFace As SldWorks.Face2

Purpose: In above line, we create a variable for Solidworks Face.
Variable Name: swFace
Type: SldWorks.Face2.
Reference: Please visit 🚀 online SOLIDWORKS API Help.

                        ' Variable for Solidworks Face List
Dim vFaces(1 To 2) As SldWorks.Face2

Purpose: Define 🚀 Array of Face2.
Variable Name: vFaces
Type: Face2
Length of Array: (1 To 2)
Reference: Please visit
- For Arrays in VBA : 🚀 Array on this website.

These all are our global variables.

They are SOLIDWORKS API Objects.

                        ' Program to add Perpendicular Mate
Sub main()

End Sub

In above line, we create main Program to add Perpendicular Mate in assembly.
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.

                        ' 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.

                        ' 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.")
  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.
- Then we stop our macro here.

                        ' Set Solidworks Assembly document
Set swAssembly = swDoc

In above line, we set value of swAssembly variable.
This value is swDoc variable.

Get Components and Loop through them

In this section, we Get Components and Loop through them.

                        ' Variable for List of elements
Dim vArray As Variant

Purpose: In above line, we create a variable for List of elements.
Variable Name: vArray
Type: Variant

                        ' Get Components list in opened assembly
vArray = swAssembly.GetComponents(True)

In above line, we set the value of vArray variable.
We set value by GetComponents method of swAssembly variable.

                        ' Variable for component Index
Dim componentIndex As Integer

In above line, we create a variable for component Index as a counter.
Variable Name: componentIndex
Type: Integer

                        ' Loop Components List
For componentIndex = 0 To UBound(vArray)
  
Next

In above line, we create a For loop.
This loops start from i = 0 to maximum of vArray we select.

                        ' Set Solidworks Component variable
Set swComponent = vArray(componentIndex)

In above line, we set value of swComponent variable.
This value is current value of array vArray.

Get desired face

In this section we get desired face for Perpendicular mate.

                        ' Calling this function
SelectFace swComponent, componentIndex

In above line, we call a function.
Function Name: SelectFace
Function Parameters: They are
- swComponent
- componentIndex

                        ' Function to select required face for Perpendicular mate
Function SelectFace(component As SldWorks.Component2, componentIndex As Integer)
  
End Function

In above line, we create a Function to select required face for Perpendicular mate.
This is a Function procedure which has name of SelectFace.
This procedure hold all the statements (instructions) for select required face for Perpendicular mate.
Reference: Detailed information 🚀 VBA Sub and Function Procedures article of this website.

This function has 2 parameters as follows:

component As SldWorks.Component2
componentIndex As Integer

                        ' Get body of current component
Set swBody = component.GetBody

In above line, we set value of swBody variable.
Value of swBody variable is set by GetBody method of component variable.

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

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

                        ' Set value of Solidworks Select Data variable
Set swSelData = swDoc.SelectionManager.CreateSelectData

In above line, we set value of swSelData variable.
Value of swSelData variable is set by CreateSelectData, which is part of SelectionManager. This SelectionManager is part of swDoc variable.

                        ' Set Mark of Solidworks Select Data
swSelData.Mark = 1

In above line, we set Mark of swSelData variable to 1.

                        ' Get First face
Set swFace = swBody.GetFirstFace

In above line, we set value of swFace variable.
Value of swFace variable is set by GetFirstFace, which is part of swBody variable.

                        ' Variable to store Message Box result
Dim resp As VbMsgBoxResult

Purpose: In above line, we create a variable to store Message Box result.
Variable Name: resp
Type: VbMsgBoxResult

                        ' Loop through all Faces
Do While Not swFace Is Nothing
  
Loop

In above line, we loop through all Faces.

                        ' Select current face
swFace.Select4 False, swSelData

In above line, we select current face.

                        ' Ask user to confirm this selection
resp = MsgBox("Is this correct Face?", vbYesNo, "Select Face")

In above line, we ask user to confirm this selection.
We do this in following steps.
1. Show a Message Box to user as shown below.
1. Store user response in resp variable.

                        ' Check if user response if Yes
If resp = vbYes Then

End If

In above code block, we check if user response if Yes.
We use 🚀 IF statement for checking.
Condition: resp = vbYes

                        ' Add current face to List of Faces
Set vFaces(componentIndex + 1) = swFace
Exit Function

                      

When user response if Yes, then above code execute.
In above line, 1st we add current face to List of Faces.
2nd, we exit this SelectFace function.

                        ' Get next face
Set swFace = swFace.GetNextFace

In above line, we set the value of swFace variable.
This is done by GetNextFace method of swFace variable.

Select Faces

In this section, we Select Faces.

                        ' Loop selected Face List
For componentIndex = 1 To UBound(vFaces)
  
Next

In above line, we Loop selected Face List.

                        ' Get and Set current Face
Set swFace = vFaces(componentIndex)

In above line, we set the value of swFace variable to current face of list.

                        ' Select current Face
swFace.Select True

In above line, we select current Face.

Add Perpendicular Mate

In this section, we add Perpendicular Mate.

                        ' Add Perpendicular Mate
Set swMateFeature = swAssembly.AddMate5(swMatePERPENDICULAR, swMateAlignALIGNED, False, 0, 0, 0, 0, 0, 0, 0, 0, False, False, 0, swAddMateError_ErrorUknown)

In above line, we set the value of variable swMateFeature by AddMate5 method.

This AddMate5 method takes following parameters as explained:

MateTypeFromEnum - Type of mate as defined in swMateType_e:

Member	Description
`swMateANGLE`	6
`swMateCAMFOLLOWER`	9
`swMateCOINCIDENT`	0
`swMateCONCENTRIC`	1
`swMateCOORDINATE`	20
`swMateDISTANCE`	5
`swMateGEAR`	10
`swMateHINGE`	22
`swMateLINEARCOUPLER`	18
`swMateLOCK`	16
`swMateLOCKTOSKETCH`	12
`swMateMAGNETIC`	25
`swMateMAXMATES`	14
`swMatePARALLEL`	3
`swMatePATH`	15
`swMatePERPENDICULAR`	2
`swMatePROFILECENTER`	24
`swMateRACKPINION`	13
`swMateSCREW`	17
`swMateSLIDER`	23
`swMateSLOT`	21
`swMateSYMMETRIC`	8
`swMateTANGENT`	4
`swMateUNIVERSALJOINT`	19
`swMateUNKNOWN`	7
`swMateWIDTH`	11

AlignFromEnum - Type of mate as defined in swMateAlign_e:

Member	Description
`swAlignAGAINST`	Obsolete. Do not use.
`swAlignNONE`	Obsolete. Do not use.
`swAlignSAME`	Obsolete. Do not use.
`swMateAlignALIGNED`	0
`swMateAlignANTI_ALIGNED`	1
`swMateAlignCLOSEST`	2

Flip - True to flip the mate entities, False to not; valid only if MateTypeFromEnum is swMatetype_e.swMateDISTANCE.
Distance - Distance value; valid only if MateTypeFromEnum is swMateType_e.swMateDISTANCE.
DistanceAbsUpperLimit - Absolute maximum distance value; valid only if MateTypeFromEnum is swMateType_e.swMateDISTANCE.
DistanceAbsLowerLimit - Absolute minimum distance value; valid only if MateTypeFromEnum is swMateType_e.swMateDISTANCE.
GearRatioNumerator - Gear ratio numerator value; valid only if MateTypeFromEnum is swMateType_e.swMateGEAR.
GearRatioDenominator - Gear ratio denominator value; valid only if MateTypeFromEnum is swMateType_e.swMateGEAR.
Angle - Angle value; valid only if MateTypeFromEnum is swMateType_e.swMateANGLE.
AngleAbsUpperLimit - Absolute maximum angle value; valid only if MateTypeFromEnum is swMateType_e.swMateANGLE.
AngleAbsLowerLimit - Absolute minimum angle value; valid only if MateTypeFromEnum is swMateType_e.swMateANGLE.
ForPositioningOnly - True to only position the components according to the mating relationship and not return a mate, False to return a mate.
LockRotation - True to lock component rotation, False to not.

WidthMateOption - Width mate options as defined in swMateWidthOptions_e; valid only if MateTypeFromEnum is swMateType_e.swMateWIDTH.

Member	Description
`swMateWidth_Centered`	0
`swMateWidth_Dimension`	2
`swMateWidth_Free`	1
`swMateWidth_Percent`	3

ErrorStatus - Success or error as defined by swAddMateError_e as follows.

Member	Description
`swAddMateError_ErrorUknown`	0
`swAddMateError_IncorrectAlignment`	3
`swAddMateError_IncorrectGearRatios`	6
`swAddMateError_IncorrectMateType`	2
`swAddMateError_IncorrectSelections`	4
`swAddMateError_NoError`	1
`swAddMateError_OverDefinedAssembly`	5

Return Value : This AddMate5 method return 👉 Mate2 data object.

In our code, I have used following values:

Parameter Name	Value Used
MateTypeFromEnum	`swMatePERPENDICULAR`
AlignFromEnum	`swMateAlignALIGNED`
Flip	`false`
Distance	`0`
DistanceAbsUpperLimit	`0`
DistanceAbsLowerLimit	`0`
GearRatioNumerator	`0`
GearRatioDenominator	`0`
Angle	`0`
AngleAbsUpperLimit	`0`
AngleAbsLowerLimit	`0`
ForPositioningOnly	`False`
LockRotation	`False`
WidthMateOption	`0`
ErrorStatus	`swAddMateError_ErrorUknown`

Reference: For more details about

Solidworks AssemblyDoc details: 🚀 online Solidworks API Help for Solidworks Feature Manager.
AddMate5 Method: 🚀 online Solidworks API Help for AddMate5 Method.

                        ' Check if Mate is added or not
If swMateFeature Is Nothing Then
  MsgBox "Failed to Add Mate."
  swDoc.ClearSelection2 True
  Exit Sub
End If

                      

In above code block, we check if we successfully added Perpendicular Mate or not.
We use 🚀 IF statement for checking.
Condition: swMateFeature Is Nothing
When this condition is True,
- We show and 🚀 message window to user.
- Message: *Failed to Add Mate.
- After that we clear the selection.
- Then we stop our macro here.

Now we run the macro and after running macro we get Perpendicular Mate as shown in below image.

Final work

In this section, after adding Perpendicular Mate, we have to do some cleaning work so that we can use this macro frequently.

                        ' Clear all selection
swDoc.ClearSelection2 True

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

                        ' 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.

                        ' Rebuild assembly
swDoc.ForceRebuild3 True

In above line, we Rebuild assembly.
For this we use ForceRebuild3 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 Perpendicular Mate with SOLIDWORKS VBA Macros.

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