API Problem - Get thickness from Sheet metal part

I am trying to get the thickness from a sheet metal part. When I run
the code, I get a Run-time error 424. Object required.

Here is the code:

START CODE
-------------------------------
Dim swApp As Object
Dim Thickness As Double
Dim model As ModelDoc2

Sub main()

Set swApp = Application.SldWorks
Set model = swApp.ActiveDoc
Thickness = SheetMetalFeatureData.Thickness


End Sub

 

Hello SW Monkey,

I have a code that gets this value, although I cannot check it right
now. I will look for the code next week.

What you have to do is iterate the features and get the sheetmetal
feature type (could be named differently). Then set the sheetmetal
featuredata object and you can get the info.

Kind regards,

JJ
www.studiozwaard.nl


SW Monkey schreef:

 

Dim swsheetmetal As SldWorks.SheetMetalFeatureData

Dim swapp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2


sub main()
Set swapp=createobject("Sldworks.application")
Set swmodel=swapp.activedoc
Set swfeat = swModel.FirstFeature
While Not swfeat Is Nothing
'Debug.Print swfeat.Name & " - " & swfeat.GetTypeName

If swfeat.GetTypeName = "SheetMetal" Then
Set swsheetmetal = swfeat.GetDefinition
Thickness = swsheetmetal.Thickness

End If

Set swfeat = swfeat.GetNextFeature

Wend
end sub

 

Thanks, that works.

Im trying to get the thickness and also the volume so I can calculate
the sq area in feet for the sheetmetal part. This is used in our MRP
system for material qty. I tried to convert the thickness value to
inches, but how can I display only 3 decimal places (it currently shows
6)

Next up, figuring out how to get the volume of the part.

 

Hello SW Monkey,

You can get the volume using API, or you can iterate all faces and get
the largest face.

The first one is the easiest.

Else: this one is from the API help

Option Explicit

Sub main()

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swModDocExt As SldWorks.ModelDocExtension

Dim swMass As SldWorks.MassProperty

Dim vCofG As Variant

Dim vXaxis As Variant

Dim vYAxis As Variant

Dim vZAxis As Variant

Dim swSkCofG As SldWorks.SketchPoint

Dim swSkXaxis As SldWorks.SketchLine

Dim swSkYaxis As SldWorks.SketchLine

Dim swSkSegXaxis As SldWorks.SketchSegment

Dim swSkSegYaxis As SldWorks.SketchSegment

Dim swSelMgr As SldWorks.SelectionMgr

Dim swSelData As SldWorks.SelectData

Dim bRet As Boolean



Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swSelMgr = swModel.SelectionManager

Set swSelData = swSelMgr.CreateSelectData

Set swModDocExt = swModel.Extension

Set swMass = swModDocExt.CreateMassProperty



vCofG = swMass.CenterOfMass

vXaxis = swMass.PrincipleAxesOfInertia(0)

vYAxis = swMass.PrincipleAxesOfInertia(1)

vZAxis = swMass.PrincipleAxesOfInertia(2)



Debug.Print "File = " & swModel.GetPathName

Debug.Print " Mass = " & swMass.Mass * 1000# & " g"

Debug.Print " Surface Area = " & swMass.SurfaceArea * 1000000#
& " mm^2"

Debug.Print " Volume = " & swMass.Volume * 1000000000# &
" mm^3"

Debug.Print " Density = " & swMass.Density & " kg/m^3"

Debug.Print " CenterOfMass = (" & vCofG(0) * 1000# & ", " &
vCofG(1) * 1000# & ", " & vCofG(2) * 1000# & ") mm"

Debug.Print " X axis = (" & vXaxis(0) & ", " & vXaxis(1)
& ", " & vXaxis(2) & ")"

Debug.Print " Y axis = (" & vYAxis(0) & ", " & vYAxis(1)
& ", " & vYAxis(2) & ")"

Debug.Print " Z axis = (" & vZAxis(0) & ", " & vZAxis(1)
& ", " & vZAxis(2) & ")"



swModel.Insert3DSketch2 False

swModel.SetAddToDB True



Set swSkCofG = swModel.CreatePoint2(vCofG(0), vCofG(1), vCofG(2))

Set swSkXaxis = swModel.CreateLine2( _

vCofG(0), vCofG(1), vCofG(2), _

vCofG(0) + vXaxis(0), vCofG(1) + vXaxis(1),
vCofG(2) + vXaxis(2))

Set swSkYaxis = swModel.CreateLine2( _

vCofG(0), vCofG(1), vCofG(2), _

vCofG(0) + vYAxis(0), vCofG(1) + vYAxis(1),
vCofG(2) + vYAxis(2))



Set swSkSegXaxis = swSkXaxis

Set swSkSegYaxis = swSkYaxis

swModel.SetAddToDB False

swModel.Insert3DSketch2 True



swModel.ClearSelection2 True



swSelData.mark = 1

bRet = swSkCofG.Select4(True, swSelData): Debug.Assert bRet

swSelData.mark = 2

bRet = swSkSegXaxis.Select4(True, swSelData): Debug.Assert bRet

swSelData.mark = 4

bRet = swSkSegYaxis.Select4(True, swSelData): Debug.Assert bRet



bRet = swModel.InsertCoordinateSystem(False, False, False):
Debug.Assert bRet

End Sub

Kind regards,

JJ
www.studiozwaard.nl

 

JJ,

I would rather use

retval = MassProperty.Volume (VB Get property)

but I cant seem to get it to work correctly. I know that I can create
a custom property called VOLUME, and the value is
"". This will show the volume of the part in
a custom property. How do I get this in my API?

So far here is my code to get the thickness and show it in a message
box.

Dim swsheetmetal As SldWorks.SheetMetalFeatureData
Dim swapp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim conv As Double
Sub main()
Set swapp = CreateObject("Sldworks.application")
Set swModel = swapp.ActiveDoc
Set swfeat = swModel.FirstFeature
While Not swfeat Is Nothing
'Debug.Print swfeat.Name & " - " & swfeat.GetTypeName
If swfeat.GetTypeName = "SheetMetal" Then
Set swsheetmetal = swfeat.GetDefinition
Thickness = swsheetmetal.Thickness
End If
Set swfeat = swfeat.GetNextFeature
Wend
conv = 39.37 'metric conversion factor
Thickness = Thickness * conv
Thickness = FormatNumber(Thickness, 3)
MsgBox ("Thickness is" & Chr(13) & Thickness)
End Sub