 | | How to Set Part Density and Custom PropertiesTutorial Level = Intermediate by Greg Jankowski, SolidWorks Corporation This VB (Visual Basic) application sets the part density and custom properties based on values entered in a spreadsheet. This eliminates the need for multiple part templates for each material type. This application consists of two parts: a module (PartDensity1) which defines and reads the density and custom property information, and UserForm1 which provides the UI (User Interface) and sets the new values. Features: - Read density value and custom property (Material).
- Automatically add the custom properties if they do not exist (Material).
- Works for any unit of measure.
Requirements: - Only set the density for a part. Warn the user if it's a drawing or assembly.
- Work with different units of measure. Only change the density if it is supported within the application.
- Check to see if the user selected a value and entered a number for the density, if required. It is a good programming practice to check to see if the user entered a valid value. Otherwise, when you try to set the density to "ABC," the application will have a problem.
Challenges: - All values for density are in kg/m^3. So the macro needs to convert the default value in the current unit of measure.
- Set the material type from a pull-down menu. If the property existed, use that name.
Key:
Text = Comments
Text = Reserved VB Words
Text = Non-reserved words PartDensity1
' ****************************************************************
' Name: SetPartDensity.swp Ver: 1.0
' Created By: gjankowski@solidworks.com
' SolidWorks Ver: 2001 Plus
' Description: This macro will set the part density based on
' user input.
' ****************************************************************
Dim swApp As Object 'SldWorks object
Dim Part As Object 'ModelDoc object
Public pDensity, materialName
Public cUnits As Long
'Consistent with type names defined in swconst.bas
Const swDocPART = 1
Const swMaterialPropertyDensity = 7
Sub main()
'Get the active session
Set swApp = CreateObject("SldWorks.Application")
'Get handle to the active SolidWorks part
Set Part = swApp.ActiveDoc
'Set the message box props
Dim Msg, Style, Title, Help, Ctxt, Response, MyString
Title = "Set Part Density" ' Define the title
'If not a part, then exit
If (Part.GetType <> swDocPART) Then
'Define the message
Msg = "Current document is not a part. Density is only set on a part."
'Display the message box
Response = MsgBox(Msg, 0, Title)
Exit Sub
End If
'Get the current UOM
cUnits = Part.LengthUnit
'Get the current part density in (kg/meter^3)
pDensity = Part.GetUserPreferenceDoubleValue(swMaterialPropertyDensity)
'Convert the UOM if it is not Meters. The current application only supports
'the listed UOM's. Additional UOM's can be added
If cUnits = 0 Then 'mm
'Sets the value from the default value and converts the UOM
pDensity = pDensity / 1000000
'Set the text value for the UOM
UserForm1.txtUOM.Caption = "gram/mm^3"
ElseIf cUnits = 1 Then 'cm
pDensity = pDensity / 1000
UserForm1.txtUOM.Caption = "gram/cm^3"
ElseIf cUnits = 2 Then 'm
pDensity = pDensity / 1
UserForm1.txtUOM.Caption = "gram/m^3"
ElseIf cUnits = 3 Then 'in
pDensity = pDensity / 27679.9125177614
UserForm1.txtUOM.Caption = "lb/in^3"
ElseIf cUnits = 4 Then 'ft
pDensity = pDensity / 16.0184678922231
UserForm1.txtUOM.Caption = "lb/in^3"
ElseIf cUnits = 5 Then 'ft-in
pDensity = pDensity / 27679.9125177614
UserForm1.txtUOM.Caption = "lb/in^3"
Else
'If the current UOM is not supported, do not set the value and exit
Msg = "The current UOM is not supported!" 'Set the message
Response = MsgBox(Msg, 0, Title) 'Display the message box
End
End If
'This section defines the material pull-down list
'When adding to this list, the corresponding values must
'be added to the UserForm1 module where the density is set.
UserForm1.frmMatName.AddItem "ALUMINUM 2024-T3"
UserForm1.frmMatName.AddItem "ALUMINUM 3003"
UserForm1.frmMatName.AddItem "ALUMINUM 6061-T6"
UserForm1.frmMatName.AddItem "ALUMINUM 7079-T6"
UserForm1.frmMatName.AddItem "COPPER - PURE"
UserForm1.frmMatName.AddItem "IRON"
UserForm1.frmMatName.AddItem "NICKEL -PURE"
UserForm1.frmMatName.AddItem "NYLON"
UserForm1.frmMatName.AddItem "POLYCARBONATE"
UserForm1.frmMatName.AddItem "POLYETHYLENE"
UserForm1.frmMatName.AddItem "PTFE"
UserForm1.frmMatName.AddItem "STEEL AISI 304"
UserForm1.frmMatName.AddItem "STEEL AISI 4130"
UserForm1.frmMatName.AddItem "STEEL AISI C1020"
UserForm1.frmMatName.AddItem "TITANIUM B 120VCA"
'Populate the dialog box density value field
UserForm1.frmDValue.Value = pDensity
'Get the property "MATERIAL"" exists
materialName = Part.CustomInfo("MATERIAL")
'if the material prop does not exist, prompt the user to select one
If materialName = "" Then
materialName = "Select a material from the list"
End If
'Use this value for the material name in the
UserForm dialog boxUserForm1.frmMatName = materialName
'Set the focus on the input dialog box, and select text field so the
'user can just enter the number
UserForm1.frmDValue.SetFocus
UserForm1.frmDValue.SelStart = 0
UserForm1.frmDValue.SelLength = 90
'Show the input dialog box
UserForm1.Show
End Sub
UserForm1
' ****************************************************************
' Name: SetPartDensity.swp Ver: 1.0
Sub btnCancel_Click()
'Exit the application if the cancel button is pressed
End
End Sub
Sub btnOK_Click()
'Consistent with type names defined in swconst.bas
Const swMaterialPropertyDensity = 7
Const swCustomInfoText = 30
'Declare the other variable names
Dim wasSet, retVal As Boolean
Set swApp2 = CreateObject("SldWorks.Application")
Set part2 = swApp2.ActiveDoc
'Get the value from the density value field
pDensity = UserForm1.frmDValue.Value
'If the value was not a number warn the user and make them enter a number
If Not IsNumeric(pDensity) Then 'it a number
Msg = "The density value must be a number"
'Display message.
Response = MsgBox(Msg, 0, Title)
End
End If
'If a new material was selected, re-set the density value
'Only do this if the material has changed.
If PartDensity1.materialName <> UserForm1.frmMatName Then
'All values in kg/m^3
'When adding to this list, the corresponding values must
'be added to the PartDensity1 module where the material pull-down
'list is defined.
If UserForm1.frmMatName = "ALUMINUM 2024-T3" Then
pDensity = 2770
ElseIf UserForm1.frmMatName = "ALUMINUM 3003" Then
pDensity = 2700
ElseIf UserForm1.frmMatName = "ALUMINUM 6061-T6" Then
pDensity = 2700
ElseIf UserForm1.frmMatName = "ALUMINUM 7079-T6" Then
pDensity = 2740
ElseIf UserForm1.frmMatName = "COPPER - PURE" Then
pDensity = 8900
ElseIf UserForm1.frmMatName = "IRON" Then
pDensity = 7830
ElseIf UserForm1.frmMatName = "NICKEL -PURE" Then
pDensity = 8900
ElseIf UserForm1.frmMatName = "NYLON" Then
pDensity = 1700
ElseIf UserForm1.frmMatName = "POLYCARBONATE" Then
pDensity = 1300
ElseIf UserForm1.frmMatName = "POLYETHYLENE" Then
pDensity = 2300
ElseIf UserForm1.frmMatName = "PTFE" Then
pDensity = 1200
ElseIf UserForm1.frmMatName = "STEEL AISI 304" Then
pDensity = 8030
ElseIf UserForm1.frmMatName = "STEEL AISI C1020" Then
pDensity = 7850
ElseIf UserForm1.frmMatName = "TITANIUM B 120VCA" Then
pDensity = 4850
'If the user does not select a value, pick Not Defined and use
'the value shown
ElseIf UserForm1.frmMatName = "Select a material from the list" Then
UserForm1.frmMatName = "NOT DEFINED"
pDensity = UserForm1.frmDValue
Else
'If the user does not select a new material, use the density
'value shown
'This allows to the user to enter a different density value
'that the default
pDensity = UserForm1.frmDValue
End If
End If
'Remove and re-apply the property
retVal = part2.DeleteCustomInfo("MATERIAL")
retVal = part2.AddCustomInfo2("MATERIAL", swCustomInfoText, UserForm1.frmMatName)
'Convert the UOM back to grams/m^3. Do not have to check for unsupported
'UOMs because it was checked already
If cUnits = 0 Then 'mm
pDensity = pDensity * 1000000
ElseIf cUnits = 1 Then 'cm
pDensity = pDensity * 1000
ElseIf cUnits = 2 Then 'm
pDensity = pDensity * 1
ElseIf cUnits = 3 Then 'in
pDensity = pDensity * 27679.9125177614
ElseIf cUnits = 4 Then 'ft
pDensity = pDensity * 16.0184678922231
ElseIf cUnits = 5 Then 'ft-in
pDensity = pDensity * 27679.9125177614
End If
'Set the density in the SolidWorks part. This method will return true
'if the value was set correctly
wasSet = part2.SetUserPreferenceDoubleValue(swMaterialPropertyDensity, CDbl(pDensity))
'Turn off the user form
UserForm1.Hide
'Define the message and format the density value and display the system
'unit of measure
If wasSet Then 'If the value was set ok
Msg = "Part Density has been set to -> " & Format(pDensity) & " kg/cubic meter"
Else
Msg = "There was a problem setting the density value"
End If
'Display message.
Response = MsgBox(Msg, 0, Title)
'Release the objects
Set Part = Nothing
Set part2 = Nothing
Set swApp = Nothing
Set swApp2 = Nothing
'After the value has been set, exit the app
End
End Sub
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