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| Author |
Messages |
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CRAIG HELM
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| 19 May 2006 12:33 PM |
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Please feel free to enter any handy code snippets here for the use of the public.
ALSO, PLEASE CHANGE/EDIT YOUR MESSAGE TITLE TO REFLECT WHAT YOUR CODE DOES. This way users can click on the link to get to it quickly since we are starting to get a number of them.
Thanks in advance,
-craig
Currently listed are:
1) Message Boxes
2) Reading from / Accessing Excel
3) Write to a Text File
4) Hide / Show things
5) Change Color of Dimensions in a Drawing
6) Change Line Type in Drawing
7) Insert Existing Component at a Ponit
8) Move active excel sheet
9) Identify Components in a Product
10) A batch convert - CATPart to STP (Windows)
11) A batch convert - CATPart to STP (Unix)
12) Modify View Scale
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-craig helm
Catia V5 R16 | Windows XP SP2 | Intel P4 3.4GHz | 2GB RAM | ATI FireGL V3100 128 MB DDR |
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PKARKARE
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| 19 May 2006 12:43 PM |
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Message Boxes -
Language = "VBSCRIPT"
Sub CATMain()
' ====> Get INPUT FROM USER
Flag = 1
While (Flag = 1)
Inp1 = InputBox("VAR_Name","DialogHeader", "10")
' ===> Input validity condition.
if (Inp1 < 10) Then Flag = 0
Wend
' ===> Display the variable value to user
MsgBox "Your VAR_Name value = " + Inp1, 1, "DialogHeader: Ok Cancel"
MsgBox "Your VAR_Name value = " + Inp1, 2, "DialogHeader: Abort Retry Ignore"
MsgBox "Your VAR_Name value = " + Inp1, 3, "DialogHeader: Yes No Cancel"
MsgBox "Your VAR_Name value = " + Inp1, 4, "DialogHeader: Yes No"
MsgBox "Your VAR_Name value = " + Inp1, 5, "DialogHeader: RETRY Cancel"
' ===> Ask user to continue
IntMsgRtrn = MsgBox ("Do you want to Continue...", vbYesNo, "DialogHeader")
if IntMsgRtrn = vbNo Then
MsgBox "You selected NO"
Else
MsgBox "You selected YES"
End If
End Sub
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JOBY
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| 24 May 2006 10:24 AM |
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To read from Microsoft Excel:
Language: CATScript / VBScript / VBA
Sub CATMain()
On Error Resume Next
Set xl = GetObject(, "EXCEL.Application")
If err.Number <> 0 Then
Set xl = CreateObject("EXCEL.Application")
xl.Visible = True
End If
MsgBox xl.ActiveSheet.Range("A1").Value
End Sub |
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JOBY
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| 31 May 2006 03:55 PM |
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To Write to a text file:
Language: CATScript / VBScript / VBA
__________________________________________________________
Dim sFileOutput as String
Dim oFileOutput As File
Dim oStream As TextStream
sFileOutput = "C:\outputdir\outputfile.txt"
Set oFileOutput = CATIA.FileSystem.CreateFile(sFileOutput, True) 'Create the output file, at the location "sFileOutput"
'The "False" in the above command: Boolean value that is True if an existing file with the same name can be overwritten; False if it is not, and the creation doesn't take place.
Set oStream = oFileOutput.OpenAsTextStream("ForWriting") 'Opens the file for text writing.
oStream.Write "Anything put here will be written to the text file" & chr(10)
oStream.Write "To make a new line in the text file, use chr(10)" & chr(10) & "this text is on the next line"
oStream.Close
__________________________________________________________
~Joe |
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PKARKARE
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| 01 Jun 2006 07:46 AM |
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HIDE/SHOW STUFF :
Sub CATMain()
Set productDocument1 = CATIA.ActiveDocument
Set selection1 = productDocument1.Selection
'_______________________________________________________________
' HIDE all 'axis-systems'
CATIA.StatusBar = "Hidding axis-systems ..."
' ===> You can try to do a SEARCH manually before putting this string below "'Part Desig'.'Axis System', all".
' ===> Make use of Advance search menu under edit search.
selection1.Search "'Part Design'.'Axis System',all"
' ===> SetShow 1 = HIDE; 0 = SHOW.
selection1.VisProperties.SetShow 1
CATIA.StatusBar = "Done axis-systems ..."
'_______________________________________________________________
'_______________________________________________________________
' ===> COPY PASTE the above block to hide/show another set of entity type (search).
'_______________________________________________________________
' ===> Set the Status bar back to default.
CATIA.StatusBar = "Select an Object or a command"
End Sub
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FERDO
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| 29 Jun 2006 01:34 PM |
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Change collor of dimensions in drawing...
Language="VBSCRIPT"
Sub CATMain()
Dim drawingDocument1 As Document
Set drawingDocument1 = CATIA.ActiveDocument
'~ ******* select all dimensions in drawing
Dim selection1 As Selection
Set selection1 = drawingDocument1.Selection
selection1.Search "CATDrwSearch.DrwDimension,all"
'~ ******* change the color of selection (in this case will be magenta -RGB code 255,0,255)
Set visPropertySet1 = selection1.VisProperties
visPropertySet1.SetRealColor 255,0,255,0
selection1.Clear
'~ *******
End Sub |
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Best Regards
Fernando |
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COE-FORUM-USER
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| 30 Jun 2006 05:05 AM |
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Search forbidden chars in strings.
I use this procedure to scan in CATIA V5, components, bodies, etc. (ie: NAMECHECKER(PartBody.Name) )
Sub NAMECHECKER(kString)
' Allowed Characters (Airbus allowed chars in this case)
'-------------------------
' . Chr(46)
' - Chr(45)
' _ Chr(95)
' Numbers range Chr(48) to Chr(57)
' Upper case letters Chr(65) to Chr(90)
' Lower case letters Chr(97) to Chr(122)
' char by char...
For i = 1 To Len(kString)
' Extracts ascii code
kAscii = Asc(Mid(kString,i,1))
' Comparison with allowed chars
Select Case kAscii
Case 45
Case 46
Case 95
Case 48 To 57
Case 65 To 90
Case 97 To 122
Case Else
MsgBox "Warning - String: " & kString & " Character: " & Chr(kAscii)
End Select
Next
End Sub
----------------------
Kike |
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FERDO
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| 10 Jul 2006 12:30 PM |
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Change Line Type in all views or in few selected views
Language="VBSCRIPT"
Sub CATMain()
Dim drawingDocument1 As Document
Set drawingDocument1 = CATIA.ActiveDocument
'-------------- generated items
Dim selection4 As Selection
Set selection4 = drawingDocument1.Selection
selection4.Search "CATDrwSearch.CATEarlyGenItem,all"
Set visProperties1 = CATIA.ActiveDocument.Selection.VisProperties
visProperties1.SetRealLineType 1,0.2 '-----------change line type
Set visProperties1 = CATIA.ActiveDocument.Selection.VisProperties
visProperties1.SetRealWidth 1,0.2 '-----------change width
End Sub
If you want to change only a selected view you have to change the line
selection4.Search "CATDrwSearch.CATEarlyGenItem,all"
with
selection4.Search "CATDrwSearch.CATEarlyGenItem,sel"
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Best Regards
Fernando |
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tjs4689
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| 11 Jul 2006 03:08 PM |
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To promote easily ready code I would recommend that we adopt a format to use to create well documented scripts like:
Option Explicit
' COPYRIGTH COE 2006
' ***********************************************************************
' Purpose: Creates constraints between assembly Parts using Publications
' Assumptions: Looks for xxxxx.CATProduct in the DocView
' Author:
' Languages: VBScript
' Locales: English
' CATIA Level: V5R6
' ***********************************************************************
Sub CATMain()
End Sub
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Timothy J. Suhr
COE EME DPC Co-Chair
Technical Product Designer
The Boeing Company
P.O. Box 3707 M/S 42-54
Seattle, WA 98124-2207 |
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SKWOK
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| 02 Aug 2006 04:46 PM |
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Sub InsertExistingComponentAtPoint()
'VBA Code by Steven Kwok 08-02-06
'Insert Existing Component At A Point using SelectElement2
'For the exclusive use of COE members as a reference tool: Code Snippet
'Works with all licenses
'Written in CatiaV5R14
'Setting Variables
Dim partDocument1
Dim product1
Dim products1
Dim InputObjectType(1)
Dim Status
Dim SelectedPoints(999)
Dim MySelection
Dim HowManyParts As Integer
Dim Errer As Integer
Dim i As Integer
'Clear Error Codes
Errer = 0
'Reset Integer i
i = 0
'Set Active Document Information
Set partDocument1 = CATIA.ActiveDocument
Set product1 = partDocument1.Product
Set products1 = product1.Products
Set constraints1 = product1.Connections("CATIAConstraints")
'Select a file
fpath = CATIA.FileSelectionBox("Select an existing part!", "*.CATPart", CatFileSelectionModeOpen)
If fpath = "" Then
Errer = 1
GoTo ErrerCodes
End If
'Instantiate picked component
Dim arrayOfVariantOfBSTR1(0)
arrayOfVariantOfBSTR1(0) = fpath
products1.AddComponentsFromFiles arrayOfVariantOfBSTR1, "All"
Set MySelection = partDocument1.selection
'Choose an Object Type (Must be in this order Vertex=0, Point=1, no idea why)
'Select any non-geometric point from screen (ie: corner, sketch point, etc)
InputObjectType(0) = "Vertex"
'Select any geometric set point on screen or from tree
InputObjectType(1) = "Point"
'Clear Selection from memory so user can choose one
MySelection.Clear
Status = MySelection.SelectElement2(InputObjectType(), "Select a Point", False)
If (Status <> "Normal") Then
Errer = 2
GoTo ErrerCodes
End If
'Get reference name from selection
Set SelectedPoints(i) = MySelection.Item(1).Value
Set Part1Product = MySelection.FindObject("CATIAProduct")
Set Part1Assembly = Part1Product.Parent
'Get reference name from instantiated component
HowManyParts = products1.Count
Set Part2Product = products1.Item(HowManyParts)
'Create references and constrain them using a coincidence constraint
Set reference1 = product1.CreateReferenceFromName(Part1Assembly.Name & "/" & Part1Product.Name & "/!" & SelectedPoints(0).Name)
Set reference2 = product1.CreateReferenceFromName(Part1Assembly.Name & "/" & Part2Product.Name & "/!Origin")
'Moves instantiated component origin to selected point
'Switching reference1 and reference2 will do the opposite
Set constraint1 = constraints1.AddBiEltCst(catCstTypeOn, reference2, reference1)
product1.Update
ErrerCodes:
If (Errer = 1) Then
MsgBox "No file selected, program terminating."
End If
If (Errer = 2) Then
MsgBox "No point selected, program terminating."
End If
If (Errer = 0) Then
MsgBox "Code complete." & sLF & "Finished at " & Time
End If
End Sub
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Steven Kwok
PLM Solutions Consultant
CATIA V5 Instructor
CATIA V5 R16/17/18/19
CATVBA
VB 6.0
Visual Basic .NET 2003/2005 |
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COE-FORUM-USER
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| 04 Aug 2006 08:47 AM |
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R14 sp5 tested and works sample catia and excel file attached
1 .asks user for a excel sheet name
2. opens an excel process
3. moves the active sheet selected by user
4. saves the document
5. closes excel process
Sub CATMain()
Dim Excel As Object
Dim workbooks As workbooks
Dim workbook As workbook
Dim Sheets As Object
Dim Sheet As Object
Dim worksheet As Excel.worksheet
Err.Clear
On Error Resume Next
Set Excel = GetObject(, "EXCEL.Application")
If Err.Number <> 0 Then
Err.Clear
Set Excel = CreateObject("EXCEL.Application")
End If
Set workbooks = Excel.Application.workbooks
Set myworkbook = workbooks.Add("C:\Documents and Settings\mjeeves\Desktop\design table tests\MULTISHEET.xls")
Set myworksheet = ActiveWorkbook.Item(1)
''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''
'Asks for Name of the required Active Sheet
WhichSheet = inputBox ("Type Model year Ie 07,08,09,10,11....")
'Setting The Active Sheet
Set myWorkSheet = myWorkbook.Worksheets.Item(WhichSheet)
myWorkSheet.Activate
Set lastSheet = myWorkbook.Worksheets(myWorkbook.Worksheets.Count)
call myWorkSheet.Select
call myWorkSheet.Move ( ,lastSheet)
call myWorkSheet.SaveAs("C:\Documents and Settings\mjeeves\Desktop\design table tests\MULTISHEET.xls")
''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''
'close routine:
Application.DisplayAlerts = False
workbook.Close
Excel.Quit
Set workbook = Nothing
Set workbooks = Nothing
Set Excel = Nothing
Application.DisplayAlerts = True
End Sub
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COE-FORUM-USER
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| 16 Oct 2006 06:59 AM |
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- Identify components in a product -
Language="VBSCRIPT"
Sub CATMain()
Set productDocument1 = CATIA.ActiveDocument
Set product1 = productDocument1.Product
Set products1 = product1.Products
For i = 1 To products1.Count
NameOfProdPart = products1.Item(i).ReferenceProduct.Parent.Name
If Right(NameOfProdPart,7) = "CATPart" Then
Msgbox "Part! " & NameOfProdPart
Elseif Right(NameOfProdPart,7) = "Product" Then
If NameOfProdPart = product1.Name & ".CATProduct" Then
Msgbox "Component! " & NameOfProdPart
Else
Msgbox "Product! " & NameOfProdPart
End If
End If
Next
End Sub
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FERDO
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| 16 Oct 2006 02:07 PM |
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A batch convert - CATPart to STP (Windows)
Language="VBSCRIPT"
Sub CATMain()
folderinput = InputBox ("Take your files from here","Input","C:\tempin\",2000,4000)
folderoutput = InputBox ("Put your files here","Output","C:\tempout\",2000,4000)
Dim fs, f, f1, fc, s
Set fs = CreateObject("Scripting.FileSystemObject")
Set f = fs.GetFolder(folderinput)Set fc = f.Files
For Each f1 in fc
Dim PartDocument1 'As Document
Set documents1 = CATIA.Documents
Dim document1 'As Document
INTRARE = folderinput & f1.name
Set PartDocument1 = CATIA.Documents.Open(INTRARE)
IESIRE = folderoutput & f1.name & ".stp"
PartDocument1.ExportData IESIRE, "stp"
s = s & f1.name
s = s & vbCrLf
CATIA.ActiveDocument.Close
Next
End Sub
Of course you can do a lot of combinations just replacing stp with something else sopported by ExportData or combination like CATDrawing (instead of CATPart) to pdf (instead of stp). Just be careful to create the necessary folders.... |
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Best Regards
Fernando |
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FERDO
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| 16 Oct 2006 02:10 PM |
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Same batch convert but here is the UNIX version - CATPart to STP
Language="VBSCRIPT"
Sub CATMain()
folderinput = InputBox ("Take your files from here","Input","/home/tempin/",2000,4000)
folderoutput = InputBox ("Put your files here","Output","/home/tempout/",2000,4000)
Dim fs, f, f1, fc, s As FileSystem
Set fs = CATIA.FileSystemSet f = fs.
GetFolder(folderinput)Set fc = f.Files
For Each f1 in fc
Dim PartDocument1 'As Document
Set documents1 = CATIA.Documents
Dim document1 'As Document
INTRARE = folderinput & f1.name
Set PartDocument1 = CATIA.Documents.Open(INTRARE)
IESIRE = folderoutput & f1.name & ".stp"
PartDocument1.ExportData IESIRE, "stp"
s = s & f1.name
s = s & vbCrLf
CATIA.ActiveDocument.Close
Next
End Sub |
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Best Regards
Fernando |
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FERDO
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| 18 Oct 2006 01:44 PM |
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Modifying view scale (UNIX)
A CATScript which will modify views scale. The macro will skip the views which are not created and will do the job in the order specified in the message box.
Sub CATMain()
MsgBox "First 2 inputs are for Main View Scale and Background View Scale: Even if you will modify these 2 scales, you will not notice any modifications, that's why implicit value is 1. 1st value is for Main, 2nd for Background, 3rd for Front, 4th for Top, 5th for Up, 6th for Left, 7th for Right, 8th for ISO. Use only double value, do NOT use 1:2 or 1/2 (for example) "
Dim theDrawing As DrawingDocument
Set theDrawing = CATIA.ActiveDocument
Dim aSheet As DrawingSheet
Dim aView As DrawingView
Dim i As Integer, j As Integer
For i = 1 To theDrawing.Sheets.count
Set aSheet = theDrawing.Sheets.Item(i)
For j = 1 To aSheet.Views.count
Set aView = aSheet.Views.Item(j)
' Retrieve the drawing components collection of the target drawing view
Dim o2DComponents As DrawingComponents
Set o2DComponents = aView.Components
'Gets the View Scale;
aView.Scale = InputBox("Enter drawing scale", "scale", "1")
If aView.Scale = "" Then
MsgBox "The Macro has been aborted."
Exit Sub
End If
Next
Next
End Sub |
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Best Regards
Fernando |
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