Solidworks VBA Macro - Add Coincident 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 Coincident Mate in Assembly document of SOLIDWORKS CAD Software.

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

Results We Can Get

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

Below image shows the result we get.

unfix-component-final-result

We Coincident Mate in following steps in general.

  1. Get Assembly Name without extension.
  2. Loop through each plane.
  3. Get Plane names for selection.
  4. Select Both Planes.
  5. Add Coincident Mate.
  6. Final Work

To get the correct result please follow the steps correctly.

Macro Video

Below 🎬 video shows Adding Coincident 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 Coincident 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 Coincident 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 Coincident Mate
    Set swMateFeature = swAssembly.AddMate5(swMateCOINCIDENT, 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.

prerequisite

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:

  1. Create and Initialize required variables
  2. Get Assembly Title
  3. First Component and Plane List
  4. Get Plane names
  5. Select Planes
  6. Add Coincident Mate
  7. 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
' 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 Coincident Mate
Sub main()

End Sub
  • In above line, we create main Program to add Coincident 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
' 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 Coincident Mate

In this section, we add Coincident Mate.

' Add Coincident Mate
Set swMateFeature = swAssembly.AddMate5(swMateCOINCIDENT, 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 swMateCOINCIDENT
    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

' 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 Coincident 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 Coincident Mate as shown in below image.

unfix-component-final-result

Final work

In this section, after adding Coincident 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 !!!

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Hope this post helps you to Coincident Mate with SOLIDWORKS VBA Macros.

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