Solidworks VBA Macro - Add Parallel Mate

12 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 Parallel Mate in Assembly document of SOLIDWORKS CAD Software.

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

Results We Can Get

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

Below image shows the result we get.

We Parallel Mate in following steps in general.

Get Assembly Name without extension.
Loop through each plane.
Get Plane names for selection.
Select Both Planes.
Add Parallel Mate.
Final Work

To get the correct result please follow the steps correctly.

Macro Video

Below 🎬 video shows Adding Parallel 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 Parallel 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 Mate Feature
Dim swMateFeature As SldWorks.Feature

' Boolean Variable
Dim boolStatus As Boolean

' Program to add Parallel 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 Assembly Title
  Dim assemblyTitle As String
  
  ' Get assembly title
  assemblyTitle = swDoc.GetTitle
  
  ' Variable for List of elements
  Dim vArray As Variant
  
  ' Using this variable for getting Assembly name without extension
  vArray = Split(assemblyTitle, ".")
  
  ' Update Assembly Title
  assemblyTitle = vArray(0)
  
  ' Get Components list in opened assembly
  vArray = swAssembly.GetComponents(True)
  
  ' Set Solidworks Component variable
  Set swComponent = vArray(0)
  
  ' Redefine array variable
  ReDim vArray(1 To 3) As String
  
  ' Update Array list
  vArray(1) = "Front Plane"
  vArray(2) = "Right Plane"
  vArray(3) = "Top Plane"
  
  ' Variable for loop
  Dim i As Integer
  
  ' Loop Plane List
  For i = 1 To UBound(vArray)
    
    ' Variable for Current Plane
    Dim currentPlane As String
    
    ' Set current plane
    currentPlane = vArray(i)
    
    ' Variable for First Plane name
    Dim firstSelection As String
    
    ' Set First Plane Name
    firstSelection = currentPlane + "@" + assemblyTitle
    
    ' Variable for Second Plane name
    Dim secondSelection As String
    
    ' Set Second Plane name
    secondSelection = currentPlane + "@" + swComponent.Name + "@" + assemblyTitle
    
    ' Select First Plane
    boolStatus = swDoc.Extension.SelectByID2(firstSelection, "PLANE", 0, 0, 0, False, 1, Nothing, swSelectOptionDefault)
    
    ' Select Second Plane
    boolStatus = swDoc.Extension.SelectByID2(secondSelection, "PLANE", 0, 0, 0, True, 1, Nothing, swSelectOptionDefault)
  
    ' Add Parallel Mate
    Set swMateFeature = swAssembly.AddMate5(swMatePARALLEL, 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
    
  Next
  
  ' Rebuild assembly
  swDoc.ForceRebuild3 True
  
  ' Zoom to fit
  swDoc.ViewZoomtofit2
  
End Sub

                      

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 Assembly Title
First Component and Plane List
Get Plane names
Select Planes
Add Parallel 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 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.

                        ' Boolean Variable
Dim boolStatus As Boolean

Purpose: In above line, we create a variable for Boolean selection.
Variable Name: boolStatus
Type: Boolean

These all are our global variables.

They are SOLIDWORKS API Objects.

                        ' Program to add Parallel Mate
Sub main()

End Sub

In above line, we create main Program to add Parallel 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 Assembly Title

In this section, we Get Assembly Title without extension.

                        ' variable for Assembly Title
Dim assemblyTitle As String

Purpose: In above line, we create a variable for Assembly Title.
Variable Name: assemblyTitle
Type: String

                        ' Get assembly title
assemblyTitle = swDoc.GetTitle

In above line, we set the value of assemblyTitle variable.
We set value by GetTitle method of swDoc variable.

                        ' 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

                        ' Using this variable for getting Assembly name without extension
vArray = Split(assemblyTitle, ".")

In above line, we set the value of vArray variable.
We set value by Split method.
Split method takes 2 arguments.
1. Input String which we want to split.
2. Delimiter, by which we want to split the Input String.

                        ' Update Assembly Title
assemblyTitle = vArray(0)

In above line, we set the value of assemblyTitle variable.
We set value to First instance vArray variable.

First Component and Plane List

In this section, we Get First Component and update Plane List.

                        ' 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.

                        ' Set Solidworks Component variable
Set swComponent = vArray(0)

In above line, we set value of swComponent variable.
This value is First component inside vArray variable.
We get current component by Indexing vArray variable.

                        ' Redefine array variable
ReDim vArray(1 To 3) As String

In above line, we Redefine 🚀 Array of String.
Variable Name: vArray
Type: String
Length of Array: (1 To 3)
Reference: Please visit
- For Arrays in VBA : 🚀 Array on this website.

                        ' Update Array list
vArray(1) = "Front Plane"
vArray(2) = "Right Plane"
vArray(3) = "Top Plane"

                      

In above code, we update Array list by adding Plane names.

                        ' Variable for loop
Dim i As Integer

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

                        ' Loop Plane List
For i = 1 To UBound(vArray)

Next

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

Get Plane names

In this section, we Get Plane names.

                        ' Variable for Current Plane
Dim currentPlane As String

In above line, we create a variable for Current Plane.
Variable Name: currentPlane
Type: String

                        ' Set current plane
currentPlane = vArray(i)

In above line, we set value of currentPlane variable.
This value is plane inside vArray variable.
We get current component by Indexing vArray variable.

                        ' Variable for First Plane name
Dim firstSelection As String

In above line, we create a variable for First Plane name.
Variable Name: firstSelection
Type: String

                        ' Set First Plane Name
firstSelection = currentPlane + "@" + assemblyTitle

In above line, we set value of firstSelection variable.
This value is combinations of currentPlane & assemblyTitle variables.

                        ' Variable for Second Plane name
Dim secondSelection As String

In above line, we create a variable for Second Plane name.
Variable Name: secondSelection
Type: String

                        ' Set Second Plane name
secondSelection = currentPlane + "@" + swComponent.Name + "@" + assemblyTitle

In above line, we set value of secondSelection variable.
This value is combinations of currentPlane, swComponent.Name & assemblyTitle variables.

Select Planes

In this section, we Select Planes.

                        ' Select First Plane
boolStatus = swDoc.Extension.SelectByID2(firstSelection, "PLANE", 0, 0, 0, False, 1, Nothing, swSelectOptionDefault)

In above line, we select First Plane.

                        ' Select Second Plane
boolStatus = swDoc.Extension.SelectByID2(secondSelection, "PLANE", 0, 0, 0, True, 1, Nothing, swSelectOptionDefault)

In above line, we select Second Plane.

Add Parallel Mate

In this section, we add Parallel Mate.

                        ' Add Parallel Mate
Set swMateFeature = swAssembly.AddMate5(swMatePARALLEL, 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	`swMatePARALLEL`
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 Parallel 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 Parallel Mate as shown in below image.

Final work

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

                        ' 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.

                        ' 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.

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.

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