Hi Guys,
I need a help regarding drawing sheet format.
The situation is when I update my sheet format I want to update my drawings.
So what I do is reload my drawings.
The step are
1. Right-click the sheet
2. Select Properties.
3. Click Reload
3. Click OK.
So it takes four (4) clicks to reload the drawing.
It's fine if it is only one but what I have sometimes 7 drawings to update.
I think macro will do the trick just one click of a button.
Hope you have that kind of macro
Thanks guys.
Cheers,
Jeff,
I don't think API has codes for the reload button yet. So the workaround is to set the sheet format to none and then switching back to same sheet format. I've not tested this method and not sure if this would delete notes, etc. from the sheet format.
Please vote for SPRs #:330668
You probably just need to set the sheet properties using the existing values. This should reload the new template (I haven't tested this theory though.)
Check out this example from the help file: http://help.solidworks.com/2013/English/api/sldworksapi/Get_and_Set_Sheet_Properties_Example_VB.htm
Take out these lines:
' Switch projection property
bFirstAng = vSheetProps(4)
vSheetProps(4) = Not bFirstAng
That should get the existing sheet properties, and then reapply them but with an updated template.
Deepak,
Yeah I have that kind of process. I copied some codes.
So I have 2 macro button.
First macro setting the sheet format to none
Second macro reloading my updated sheet format.
Cheers,
Why don't you combine both of them OR share the codes/macro here and someone will help you out.
this is the first code
' **********************************************************************
' * PLEASE change the path/filename for the sheet templates (see below)
' **********************************************************************
' *
' * Macro changes the sheetformat (= the "paper" of your drawing) for
' * all sheets of the active drawing. You have to adjust the path and
' * the file names to the new sheet formats. After successfully changing
' * the sheetformat the drawing is saved with its current name.
' * ATTENTION: you CAN'T change the drawing template, this is not
' * possible. So with this macro you can't update document properties.
' * All sheet formats will be "userdefinied" after updating with this
' * macro. If you want to have the "standard" A-A0 formats and not
' * userdefinied you have to change the macro accordingly or use its
' * "compagnion" which reloads a standard sheettemplate
' *
' * This macro is intended to be used with PAC4SWX for batch reloading
' * of sheetformats, in case you changed you sheetformat with a new
' * company logo, new title block layout or similar. But it will also
' * word if fired from the GUI (taskplaner not tested, but should work;
' * but I would like to see you using PAC4SWX instead of taskplaner ;-))
' *
' * PAC4SWX - http://swtools.cad.de/prog_pac.htm
' *
' *
' * 17.12.2003 Stefan Berlitz
' * SolidWorks Solution Partner
' * Inoffizielle deutsche SolidWorks Hilfeseite
' *
' **********************************************************************
Sub ReloadSheetFormat()
Dim sheetformatpath(12) As String
Dim sheetformatdir As String
' ************ EDIT path and file name HERE ************************
' After editing the sheetformats delete the next line or comment it
'If MsgBox(msgtext(6), vbOKOnly, "Please Edit Macro") = vbOK Then End
' Path to directory with sheetformats
sheetformatdir = "C:\ProgramData\SolidWorks\SolidWorks 2013\lang\english\sheetformat\New Template\"
' path to the various sheet formats from A to A0, you may also use
' full pathnames, but if they are all in teh same subdir it's easier this way
sheetformatpath(0) = sheetformatdir & "temp_A.slddrt"
sheetformatpath(1) = sheetformatdir & "temp_av.slddrt"
sheetformatpath(2) = sheetformatdir & "temp_B.slddrt"
sheetformatpath(3) = sheetformatdir & "temp_c.slddrt"
sheetformatpath(4) = sheetformatdir & "temp_d.slddrt"
sheetformatpath(5) = sheetformatdir & "temp_e.slddrt"
sheetformatpath(6) = sheetformatdir & "temp_a4.slddrt"
sheetformatpath(7) = sheetformatdir & "temp_a4v.slddrt"
sheetformatpath(8) = sheetformatdir & "temp_a3.slddrt"
sheetformatpath(9) = sheetformatdir & "temp_a2.slddrt"
sheetformatpath(10) = sheetformatdir & "temp_a1.slddrt"
sheetformatpath(11) = sheetformatdir & "temp_a0.slddrt"
' already user defined
sheetformatpath(12) = sheetformatdir & "WS-A3.slddrt"
' ************************* EDIT END *******************************
Dim swApp As Object
Dim DrawingDoc As Object
Dim Sheet As Object
Dim Titel As String
Dim Datei As String
Dim temp As String
Dim pfad As String
Dim msgtxt As String
Dim Name As String
Dim paperSize As Long
Dim templateIn As Long
Dim scale1 As Double
Dim scale2 As Double
Dim firstAngle As Boolean
Dim templateName As String
Dim Width As Double
Dim Height As Double
Dim propertyViewName As String
Dim i As Long
Dim MySheetCount As Long
Dim SheetNames As Variant
Dim SheetProperties As Variant
Const swDocDRAWING = 3
Const swDwgTemplateCustom = 12
Const swDwgTemplateNone = 13
' attach to SolidWorks
Set swApp = CreateObject("SldWorks.Application")
Set DrawingDoc = swApp.ActiveDoc
If DrawingDoc Is Nothing Then
' check if document is open
MsgBox "No Drawing Open"
Exit Sub
End If
If (DrawingDoc.GetType <> swDocDRAWING) Then
' check if document is a drawing
MsgBox "No Drawing Open"
Exit Sub
End If
' get sheet count and traverse all sheets to reload sheetfromat
'
MySheetCount = DrawingDoc.GetSheetCount
SheetNames = DrawingDoc.GetSheetNames
' reset error messages
msgtxt = ""
For i = 0 To MySheetCount - 1
' activate next sheet
If DrawingDoc.ActivateSheet(SheetNames(i)) Then
' attach to sheet object
Set Sheet = DrawingDoc.GetCurrentSheet
SheetProperties = Sheet.GetProperties
' first we have to set the sheet to use "no sheetformat", for SolidWorks
' wont reload a sheetformat if it is the same name as before
Name = Sheet.GetName
paperSize = SheetProperties(0)
' set NO SHEETFORMAT
templateIn = swDwgTemplateNone
scale1 = SheetProperties(2)
scale2 = SheetProperties(3)
firstAngle = CBool(SheetProperties(4))
' no sheetformat = no path
templateName = ""
' but we need the sheet size
Width = SheetProperties(5)
Height = SheetProperties(6)
propertyViewName = Sheet.CustomPropertyView
retval = DrawingDoc.SetupSheet5( _
Name, _
paperSize, _
templateIn, _
scale1, _
scale2, _
firstAngle, _
templateName, _
Width, _
Height, _
propertyViewName, _
True)
If retval = False Then
msgtxt = "Error" & vbCrLf
Else
' and now we set the new sheetformat; it is necessary to set
' USER DEFINIED sheetformat for SolidWorks will look for the
' standard templates temp_??.slddrt in your spefified folder
' if using the standard sheet sizes.
templateIn = swDwgTemplateCustom
' get correct sheetformat for this size depending on the
' papersize, this will allow aleady userdefined sheetformats
' to properly be reloaded
paperSize = GetSheetSizeFromPaperSize(Width, Height)
templateName = sheetformatpath(paperSize)
retval = DrawingDoc.SetupSheet5( _
Name, _
paperSize, _
templateIn, _
scale1, _
scale2, _
firstAngle, _
templateName, _
Width, _
Height, _
propertyViewName, _
True)
If retval = False Then
' ERROR : can't load new sheetformat
msgtxt = "Can't Load" & templateName & vbCrLf
Else
' everything worked fine, no message here for automation
' save the document without backup
'If DrawingDoc.Save2(True) > 0 Then
' error saving file
' Fehler beim Speichern
' msgtxt = msgtxt & msgtext(5) & vbCrLf
'End If
End If
End If
Else
msgtxt = "Something" & Name & vbCrLf
End If
Next i
'SetDraftingStandard
'SetCurrentLayer
'If Len(msgtxt) Then
' MsgBox msgtxt
'End If
DrawingDoc.ViewZoomtofit2
DrawingDoc.ForceRebuild3 False
End Sub
Function GetSheetSizeFromPaperSize(SheetWidth, SheetHeight)
' Function returns the SheetSize constant based on the width and heigth
' useful for userdefined sheetformats
Const swDwgPaperAsize = 0
Const swDwgPaperAsizeVertical = 1
Const swDwgPaperBsize = 2
Const swDwgPaperCsize = 3
Const swDwgPaperDsize = 4
Const swDwgPaperEsize = 5
Const swDwgPaperA4size = 6
Const swDwgPaperA4sizeVertical = 7
Const swDwgPaperA3size = 8
Const swDwgPaperA2size = 9
Const swDwgPaperA1size = 10
Const swDwgPaperA0size = 11
Const swDwgPapersUserDefined = 12
If (Round(SheetWidth, 4) = 0.2794) And (Round(SheetHeight, 4) = 0.2159) Then
GetSheetSizeFromPaperSize = swDwgPaperAsize
ElseIf (Round(SheetWidth, 4) = 0.2159) And (Round(SheetHeight, 4) = 0.2794) Then
GetSheetSizeFromPaperSize = swDwgPaperAsizeVertical
ElseIf (Round(SheetWidth, 4) = 0.4318) And (Round(SheetHeight, 4) = 0.2794) Then
GetSheetSizeFromPaperSize = swDwgPaperBsize
ElseIf (Round(SheetWidth, 4) = 0.5588) And (Round(SheetHeight, 4) = 0.4318) Then
GetSheetSizeFromPaperSize = swDwgPaperCsize
ElseIf (Round(SheetWidth, 4) = 0.8636) And (Round(SheetHeight, 4) = 0.5588) Then
GetSheetSizeFromPaperSize = swDwgPaperDsize
ElseIf (Round(SheetWidth, 4) = 1.1176) And (Round(SheetHeight, 4) = 0.8636) Then
GetSheetSizeFromPaperSize = swDwgPaperEsize
ElseIf (Round(SheetWidth, 4) = 0.297) And (Round(SheetHeight, 4) = 0.21) Then
GetSheetSizeFromPaperSize = swDwgPaperA4size
ElseIf (Round(SheetWidth, 4) = 0.21) And (Round(SheetHeight, 4) = 0.297) Then
GetSheetSizeFromPaperSize = swDwgPaperA4sizeVertical
ElseIf (Round(SheetWidth, 4) = 0.42) And (Round(SheetHeight, 4) = 0.297) Then
GetSheetSizeFromPaperSize = swDwgPaperA3size
ElseIf (Round(SheetWidth, 4) = 0.594) And (Round(SheetHeight, 4) = 0.42) Then
GetSheetSizeFromPaperSize = swDwgPaperA2size
ElseIf (Round(SheetWidth, 4) = 0.841) And (Round(SheetHeight, 4) = 0.594) Then
GetSheetSizeFromPaperSize = swDwgPaperA1size
ElseIf (Round(SheetWidth, 4) = 1.189) And (Round(SheetHeight, 4) = 0.841) Then
GetSheetSizeFromPaperSize = swDwgPaperA0size
Else
GetSheetSizeFromPaperSize = swDwgPapersUserDefined
End If
End Function
this is the second code
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim Part As Object
Sub main()
Set swApp = New SldWorks.SldWorks
Set Part = swApp.ActiveDoc
Part.SetupSheet4 "Sheet1", 6, 12, 1, 1, False, _
"C:\ProgramData\SolidWorks\SolidWorks 2013\lang\english\sheetformat\New Template\WS-A3.slddrt", _
0.297, 0.21, "Default"
Part.EditSketch
End Sub
There is an error with that code.
I dont know why.
Cheers
I think " we want to do manually", Macro will not suitable for this
The best would be to set the template to NONE and then reapply the same format. I just tested it out and it seems to work.
What is location of your template and template name so that I can incorporate them in the macro for you.
Really?It works on your PC.
The location is C:\ProgramData\SolidWorks\SolidWorks 2013\lang\english\sheetformat\New Template
And the file name is WS-A3.slddrt
I already replace the path in the code but what happens is when I click the macro button for that
the template is set to NONE afterwards nothing happens.
So I have the second macro to reload my new template.
I'll wait for the reply
Thanks
Jeff,
Try this macro. Please try it on sample files first.
This has been tested on SW2014 SP3 Win 7 x64. So in case you've lower version of SW, you may need to fix the reference libraries in the macro.
Deepak,
I got error in in this part
Sub main()
Dim swApp As SldWorks.SldWorks
I dont know why. I am using SolidWorks 2013 SP3
Cheers,
Here is the one fixed for SW2013, can you try it out.
Was a typo, fixed that.
Hey Deepak,
Finally, it works!!
Thank you very much for the help.
Till next time
Cheers,
How can we get it to also update additional sheets?
If i go to sheet 2 and use the macro, it takes me back to the first sheet.
Do you want to change all sheets OR only second sheet?
Just the active sheet if that's possible.
Try the attached one. Make sure you've changed the sheet format path and name. Don't forget to add \ at the end of the sheet format path.
P.S. I've added version for SW2013 and SW2014.
Deepak, you rock!
I might just have to find some more roller coasters to take you on, as a thank you :-)
Hello Deepak,
I tried your macro and it works great for sheet one but it won't reload the sheet format of sheet 2 and so on. Even if I goto sheet 2 and run the macro it jumps back to sheet 1 and reloads the format for that sheet only.
Garret
Hey Deepak,
How to change the codes so that I could change all sheets in the drawing?
Thanks
Jeffrey
Deepak,
I think that version is for 2014.
I'm getting an error for it.
How do you change it for 2013 version.
Cheers
Here is the one fixed for SW2013, can you try it out.
Was a typo, fixed that.