Macro help

Anyone have a macro that inserts a block into a drawing at a specified X,Y
location in the sheet format?

I have tried to record a macro to do this, but no sucess. I looked up the
help in api for insterting a bloack but I cannot seem to decipher the notes
on this.

Ben

 

I use this to insert a revision block we use and it sets all of it's
annotations to and empty string.
It determines the location by the name of the template so you will have to
handle that according to your own system.

Regards
Corey


Function insertBlock() As SldWorks.BlockDefinition

Dim x As Double
Dim y As Double
Dim Bscale As Double
Dim RevLev As Object
Dim RLX As Double
Dim RLY As Double
Dim RLHeight As Double
Dim RevLevTxt As String
Dim SheetSize As String
Dim blockDef As SldWorks.BlockDefinition
Dim MyBlock As SldWorks.BlockInstance

SheetSize = LCase(Right(sheet.GetTemplateName, 8))

Select Case SheetSize
Case "a.slddrt"
x = 4.33 * 0.0254 'dimension in inches comvert to metric
y = 0.2 * 0.0254
Bscale = 1
RLX = 10.36 * 0.0254
RLY = 8.05 * 0.0254
RLHeight = 0.187 * 0.0254
Case "b.slddrt"
x = 8 * 0.0254 'dimension in inches comvert to metric
y = 0.25 * 0.0254
Bscale = 1
RLX = 13.81 * 0.0254
RLY = 10.7 * 0.0254
RLHeight = 0.187 * 0.0254
Case "c.slddrt"
x = 8.66 * 0.0254 'dimension in inches comvert to metric
y = 0.4 * 0.0254
Bscale = 2
RLX = 10.36 * 2 * 0.0254
RLY = 8.05 * 2 * 0.0254
RLHeight = 0.187 * 2 * 0.0254
Case Else
x = 0 * 0.0254 'dimension in inches comvert to metric
y = 0 * 0.0254
Bscale = 1
RLX = 10.36 * 0.0254
RLY = 8.05 * 0.0254
RLHeight = 0.187 * 0.0254
End Select
dwgdoc.EditTemplate
PathName = swApp.GetCurrentMacroPathName
PathOnly = Mid(PathName, 1, InStr(1, PathName, "A CHANGE.swp") - 2)
'dwgdoc.InsertNewNote2 RevLev, "", True, False, swNO_ARROWHEAD,
swLS_SMART, 0#, swBS_None, swBF_Tightest, 0, 0
If RevLev Is Nothing Then
RevLevTxt = ""
Set RevLev = dwgdoc.CreateText2(RevLevTxt, RLX, RLY, 0, RLHeight, 0)
RevLev.SetName "Revision Level"
End If

Set MyBlock = dwgdoc.insertBlock(PathOnly + "\A Change.SLDBLK", x, y,
0#, Bscale)

MyBlock.SetAttributeValue "TOP LETTER", ""
MyBlock.SetAttributeValue "TOP DESC", ""
MyBlock.SetAttributeValue "TOP DATE", ""
MyBlock.SetAttributeValue "MID LETTER", ""
MyBlock.SetAttributeValue "MID DESC", ""
MyBlock.SetAttributeValue "MID DATE", ""
MyBlock.SetAttributeValue "BOT LETTER", ""
MyBlock.SetAttributeValue "BOT DESC", ""
MyBlock.SetAttributeValue "BOT DATE", ""

Set blockDef = dwgdoc.GetBlockDefinition("A CHANGE")
dwgdoc.EditSheet

If blockDef Is Nothing Then
MsgBox "There was a problem finding the block." &
VBA.Chr(vbKeyReturn) & _
"Make sure " & VBA.Chr(34) & "A Change.SLDBLK" & VBA.Chr(34)
& "is in the same directory as this macro."
End
End If
Set insertBlock = blockDef

End Function

 

If the block already exists in the drawing, you can insert it using this
code:

DrawingDoc.InsertBlock("BlockName", 1 * 25.4 / 1000, 1 * 25.4 / 1000, 0, 1)

where the 1*25.4/1000 are the coordinates (in meters) where you want it.

Evan