Renaming and Line creation

[Alan Lowbands]

Hi Guys,
I'm trying to create a script to put a point in the centre of a hole then create a line from that relative to a planer face.
I have found some code that creates the first point and I've managed to alter it a little to send the point to a chosen geo set and also rename it.
I can't figure out how to get the rename to add a instance number like catia does when creating the points ie Point.1, Point.2 etc.
Does anyone know how to do this ?
After that I need to create a line.
I have found some commands from Automation V5 but how you put thim in to practice I don't know. I'm searching the web looking for a relative example.
Any help on either things would be really appreciated.

code below (whoever wrote that and shared, many thanks)

regards
Alan

---------------------------------------------------------------------------------------------------------------------------------------

Sub CATMain()

Set oDoc = CATIA.ActiveDocument
Set oPart = oDoc.Part

Dim reference1 'As Reference

Set oHSF = oPart.HybridShapeFactory

Dim InputObject(0)
InputObject(0) = "Edge"

Set oCentre = CATIA.ActiveDocument.Selection
Status = oCentre.SelectElement2(InputObject, "Select Circle", False)

Set oTemp = oCentre.Item(1)

Set oRef = oTemp.Reference

Set oPoint = oHSF.AddNewPointCenter(oRef)

'Set oHB = oPart.HybridBodies.Add() 'Will add a new Geometrical Set for each Point
Set oHB = oPart.HybridBodies.Item("Points") 'Sends to named Geo Set

oPoint.Name = "Hole Centre" &intIndex'+(oNo-1) ' Can't get this bit to rename in sequence

oPoint.Compute

oHB.AppendHybridShape oPoint

End Sub



' Found this in Automation V5

'Dim oSurface As Reference
'Set oSurface = LineNormal.Surface

'Dim oPoint As Reference
'Set oPoint = LineNormal.Point

'Dim oOrientation As long
'Set oOrientation = LineNormal.Orientation

'Dim oEnd As CATIALength
'Set oEnd = LineNormal.EndOffset

'Dim oStart As CATIALength
'Set oStart = LineNormal.BeginOffset

 

[tesak]

Hi Alan,
in your code you have a lot of undeclared variables, so no wonder it is not working properly. To get the next number in a sequence, just read the CATIA generated name of the current point, get the index and then change your name as you need. You can read the index only when the point already exists in the tree, so put the following code below this line:

...
oHB.AppendHybridShape oPoint

Dim nextIndex As Long
nextIndex = CLng(Split(oPoint.Name, ".")(1))
oPoint.Name = "Hole Centre." & nextIndex

Tesak

https://scripts4all.eu/play-tetris-in-catia-v5-drawing-vba/

- Play Tetris in CATIA V5 drawing

 

[Alan Lowbands]

Thanks tesak
really appreciated

 

[Alan Lowbands]

Hi again,
I have managed to get this Frankenstein code that I have botched together from other code to run in the way I wanted.
Run the script, select the edge of a hole then select the face.
I just creates a point and a line normal to the face 50mm long and renames the point and line.
Problem is that it only works at part level.
LWolf kindly gave me some code to do this for another macro.

Dim oPartProduct As Product
Dim oPartDocument As Document
Dim oPart As Part
For Each oPartProduct In product1.Products
Set oPartDocument = oPartProduct.ReferenceProduct.Parent
Set oPart = oPartDocument.Part

No mater how I apply it, it won't work on the script im working on.
Any help would be really welcome.

regards
Alan.

------------------------------------------------------------------------------------
Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument
Set part1 = partDocument1.Part
Set oPart = part1

Dim hybridShapeFactory1 'As Factory
Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim hybridBodies1 'As HybridBodies
Set hybridBodies1 = part1.HybridBodies

Dim hybridBody1 'As HybridBody
Set hybridBody1 = hybridBodies1.Item(1)

Dim hybridShapes1 'As HybridShapes
Set hybridShapes1 = hybridBody1.HybridShapes

Dim selection1 'As Selection
Set selection1 = partDocument1.Selection
selection1.Clear

Dim reference1 'As Reference
Dim oPart
Set oPart = part1

Dim oHSF
Set oHSF = oPart.HybridShapeFactory

Dim InputObject(0)
InputObject(0) = "Edge"

Dim oCentre
Set oCentre = CATIA.ActiveDocument.Selection
Status = oCentre.SelectElement2(InputObject, "Select Circle", False)

Dim oTemp
Set oTemp = oCentre.Item(1)

Dim oRef
Set oRef = oTemp.Reference

Dim oPoint
Set oPoint = oHSF.AddNewPointCenter(oRef)

Dim oHB
'Set oHB = oPart.HybridBodies.Add() 'Will add a new Geometrical Set for each Point
Set oHB = oPart.HybridBodies.Item("Points")

oPoint.Compute

oHB.AppendHybridShape oPoint

Dim nextIndex
nextIndex = CLng(Split(oPoint.Name, ".")(1))
oPoint.Name = "Hole Centre." & nextIndex

Set reference1 = oPoint

selection1.Clear

Dim InputObjectType(0), Status1
InputObjectType(0)="Face"
Status1=selection1.SelectElement2(InputObjectType,"Select Face",false)
If Status1 = "Cancel" Then selection1.Clear: Exit Sub

Dim reference2 'As Reference
Set reference2 = selection1.Item(1).Reference

Dim hybridShapeLineNormal
Set hybridShapeLineNormal = hybridShapeFactory1.AddNewLineNormal(reference2, reference1, 0.000000, 50.000000, True)

hybridBody1.AppendHybridShape hybridShapeLineNormal

part1.InWorkObject = hybridShapeLineNormal

Dim nextIndex1
nextIndex1 = CLng(Split(hybridShapeLineNormal.Name, ".")(1))
hybridShapeLineNormal.Name = "Vector." & nextIndex

part1.Update

End Sub
----------------------------------------------------------------

 

[LWolf]

Alan... this really is a FrankenCode...

I did not bother changing it too much, just made it work for you. However:
it only takes in a straight part-structure, i.e. a product with a bunch of parts right under.
AND it only does ONE hole in each part
(this will be your homework to make it more general, both in terms of number of holes, AND a more nested part/sub-assy structure)
you also assume there is a geometrical set called Points right under part-node.

have fun!

Sub CATMain()
Dim product1 As Product
Set product1 = CATIA.ActiveDocument.Product
Dim oPartProduct As Product
Dim oPartDocument As Document
Dim part1 As Part

For Each oPartProduct In product1.Products

Set oPartDocument = oPartProduct.ReferenceProduct.Parent
Set part1 = oPartDocument.Part

Dim hybridBodies1 'As HybridBodies
Set hybridBodies1 = part1.HybridBodies
Dim hybridBody1 'As HybridBody
Set hybridBody1 = hybridBodies1.item(1)
Dim hybridShapes1 'As HybridShapes
Set hybridShapes1 = hybridBody1.HybridShapes

Dim oHSF
Set oHSF = part1.HybridShapeFactory
Dim InputObject(0)
InputObject(0) = "Edge"
Dim mySel
Set mySel = CATIA.ActiveDocument.Selection
Status = mySel.SelectElement2(InputObject, "Select Circle", False)

Dim oTemp
Set oTemp = mySel.item(1)

Dim oRef
Set oRef = oTemp.Reference

Dim oPoint
Set oPoint = oHSF.AddNewPointCenter(oRef)

Dim oHB

Set oHB = part1.HybridBodies.item("Points")

oPoint.Compute

oHB.AppendHybridShape oPoint

Dim nextIndex
nextIndex = CLng(Split(oPoint.name, ".")(1))
oPoint.name = "Hole Centre." & nextIndex

Set reference1 = oPoint

mySel.Clear

Dim InputObjectType(0), Status1
InputObjectType(0) = "Face"
Status1 = mySel.SelectElement2(InputObjectType, "Select Face", False)
If Status1 = "Cancel" Then mySel.Clear: Exit Sub

Dim reference2 'As Reference
Set reference2 = mySel.item(1).Reference

Dim hybridShapeLineNormal
Set hybridShapeLineNormal = oHSF.AddNewLineNormal(reference2, reference1, 0#, 50#, True)

hybridBody1.AppendHybridShape hybridShapeLineNormal

part1.InWorkObject = hybridShapeLineNormal

Dim nextIndex1
nextIndex1 = CLng(Split(hybridShapeLineNormal.name, ".")(1))
hybridShapeLineNormal.name = "Vector." & nextIndex

part1.Update
​

Next

End Sub



regards,
LWolf

 

[Alan Lowbands]

Thanks LWolf,
I shall have a go at tidying it up over the weekend and try and work out how to get multiple holes and more nested structure.
I know it is a botch up but when I swapped around the references on line-
Set hybridShapeLineNormal = oHSF.AddNewLineNormal(reference2, reference1, 0#, 50#, True)
and the line popped up, I was jumping about like an idiot

Could you point me in the direction of any material that explains some of the main the functions etc.
I have the V5 scripting course but find some of it doesn't go into detail on why things are done in a certain way.
I also find the V5 Automation hard to follow and to find things.
I'm not looking for freebies, this is something I need to learn and not having a programming background I'm starting from scratch.

anyway,
thanks again
Alan

 

[Alan Lowbands]

LWolf,
I couldn't get that code to run. I'm probably doing something totally wrong lol
I think I have messed up from the start though.
My idea was to have an assembly open, create a part called Data or something and create a geo set in there called Points.
I then wanted to run the macro at assembly level to create the points and vectors in the Data.part/Points Geo-set.
If I save my assembly as an AllCatPart it works a treat and I can copy the Data.Part back into my original assembly. so at a pinch it's usable on small assemblies.
Anyway I've tried to clean it up a bit and renamed some items to try and get my head around what there doing.

thanks
Alan

---------------------------------------------------------------------------------------------------

Sub CATMain()

Dim part1
Set partDocument1 = CATIA.ActiveDocument
Set part1 = partDocument1.Part

Dim hybridShapeFactory1 'As Factory
Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim hybridBodies1 'As HybridBodies
Set hybridBodies1 = part1.HybridBodies

Dim hybridBody1 'As HybridBody
Set hybridBody1 = hybridBodies1.Item(1)

Dim hybridShapes1 'As HybridShapes
Set hybridShapes1 = hybridBody1.HybridShapes

Dim selection1 'As Selection
Set selection1 = partDocument1.Selection

'------------------------------Select Hole Centre & Create Point---------------------
Dim InputObject1(0)
InputObject1(0) = "Edge"
Dim oCentreSelection
Set oCentreSelection = CATIA.ActiveDocument.Selection
Status = oCentreSelection.SelectElement2(InputObject1, "Select Circle", False)
Dim oCentreItem
Set oCentreItem = oCentreSelection.Item(1)
Dim oCentreRef
Set oCentreRef = oCentreItem.Reference
Dim oCentrePoint
Set oCentrePoint = hybridShapeFactory1.AddNewPointCenter(oCentreRef)
hybridBody1.AppendHybridShape oCentrePoint

'-----------------------------Select Face & Create Vector----------------------------
Dim InputObject2(0)
InputObject2(0)= "Face"
Dim oFaceSelection
Set oFaceSelection = CATIA.ActiveDocument.Selection
Status=oFaceSelection.SelectElement2(InputObject2,"Select Face",false)
Dim oFaceItem
Set oFaceItem = oFaceSelection.Item(1)
Dim oFaceRef
Set oFaceRef = oFaceItem.Reference
Dim oVector
Set oVector = hybridShapeFactory1.AddNewLineNormal(oFaceRef, oCentrePoint, 0.000000, 50.000000, True)
hybridBody1.AppendHybridShape oVector

'----------------------------Rename-------------------------------------------------
Dim nextIndex
nextIndex = CLng(Split(oCentrePoint.Name, ".")(1))
oCentrePoint.Name = "Hole Centre." & nextIndex

Dim nextIndex1
nextIndex1 = CLng(Split(oVector.Name, ".")(1))
oVector.Name = "Vector." & nextIndex

selection1.Clear
part1.Update

End Sub

 

[Alan Lowbands]

Hi guys
Could anyone help me with this last problem.
I have got the code to run a product level but the part wont update due to no reference element being created when the point is.
It creates the point and line in a an active part (first geo-set)

any help on this would be really appreciated as I can't find anything relevant on line.

regards
Alan

'-----------------------------------------------------------------------------------------------

Sub CATMain()

Dim InputObject1(0)
Dim oCentreSelection
Dim oCentreItem
Dim oCentreRef
Dim oCentrePoint
Dim InputObject2(0)
Dim oFaceSelection
Dim oFaceItem
Dim oFaceRef
Dim oVector

'Do

Dim part1
Set partDocument1 = CATIA.ActiveDocument.Product.Products.Item(1).ReferenceProduct.Parent

Set part1 = partDocument1.Part

Dim hybridShapeFactory1 'As Factory
Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim hybridBodies1 'As HybridBodies
Set hybridBodies1 = part1.HybridBodies

Dim hybridBody1 'As HybridBody
Set hybridBody1 = hybridBodies1.Item(1)

Dim hybridShapes1 'As HybridShapes
Set hybridShapes1 = hybridBody1.HybridShapes

Dim selection1 'As Selection
Set selection1 = partDocument1.Selection

'------------------------------Select Hole Edge & Create Point---------------------

InputObject1(0) = "Edge"
Set oCentreSelection = CATIA.ActiveDocument.Selection
Status = oCentreSelection.SelectElement2(InputObject1, "Select Circle", False)
Set oCentreItem = oCentreSelection.Item(1)
Set oCentreRef = oCentreItem.Reference
Set oCentrePoint = hybridShapeFactory1.AddNewPointCenter(oCentreRef)
hybridBody1.AppendHybridShape oCentrePoint

'-----------------------------Select Face & Create Vector----------------------------

InputObject2(0)= "Face"

Set oFaceSelection = CATIA.ActiveDocument.Selection
Status=oFaceSelection.SelectElement2(InputObject2,"Select Face",false)
Set oFaceItem = oFaceSelection.Item(1)
Set oFaceRef = oFaceItem.Reference
Set oVector = hybridShapeFactory1.AddNewLineNormal(oFaceRef, oCentrePoint, 0.000000, 50.000000, True)
hybridBody1.AppendHybridShape oVector

selection1.Clear

part1.Update

'Loop (will sort this later)

End Sub

 

[LWolf]

here you go. works as script and in vba. commented what I removed...

Sub CATMain()

Dim InputObject1(0)
Dim oCentreSelection
Dim oCentreItem
'Dim oCentreRef 'LWolf removed
Dim oCentrePoint
Dim InputObject2(0)
Dim oFaceSelection
Dim oFaceItem
'Dim oFaceRef 'LWolf removed
Dim oVector

'Do

Dim part1
Set partDocument1 = CATIA.ActiveDocument.Product.Products.item(1).ReferenceProduct.Parent

Set part1 = partDocument1.Part

Dim hybridShapeFactory1 'As Factory
Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim hybridBodies1 'As HybridBodies
Set hybridBodies1 = part1.HybridBodies

Dim hybridBody1 'As HybridBody
Set hybridBody1 = hybridBodies1.item(1)

Dim hybridShapes1 'As HybridShapes
Set hybridShapes1 = hybridBody1.HybridShapes

'------------------------------Select Hole Edge & Create Point---------------------

InputObject1(0) = "Edge"
Set oCentreSelection = CATIA.ActiveDocument.Selection
Status = oCentreSelection.SelectElement2(InputObject1, "Select Circle", False)
Set oCentreItem = oCentreSelection.item(1).value 'LWolf added .value
'Set oCentreRef = oCentreItem.Reference 'LWolf removed
Set oCentrePoint = hybridShapeFactory1.AddNewPointCenter(oCentreItem)
hybridBody1.AppendHybridShape oCentrePoint

'-----------------------------Select Face & Create Vector----------------------------

InputObject2(0) = "Face"

Set oFaceSelection = CATIA.ActiveDocument.Selection
Status = oFaceSelection.SelectElement2(InputObject2, "Select Face", False)
Set oFaceItem = oFaceSelection.item(1).value 'LWolf added .value
'Set oFaceRef = oFaceItem.Reference 'LWolf removed
Set oVector = hybridShapeFactory1.AddNewLineNormal(oFaceItem, oCentrePoint, 0, 50, True)
hybridBody1.AppendHybridShape oVector

part1.Update

'Loop (will sort this later)

End Sub


regards,
LWolf

 

[LWolf]

Alan, just curious, what do you want the point and line for?... you ask for two inputs, if you go with axis, you just ask for one...

regards,
LWolf

 

[Alan Lowbands]

Hi LWolf,
The code is to add a vector from the hole centre 50mm long. On the line are 2 points one at 25 and one at 50.
These points are named OTP and will be used for laser tracking.
This is something that I usually have to do one at a time and can be a real pain.
I have used the same steps to create it in a macro as I would do manually so there could well be an easier option.
Another bit of code I got a while back searches the geo-set for OTP and renames them in order 1, 2, 3 etc
Some companies have a macro that then add them point positions to a table on a drawing. Unfortuanely I haven't got that as it only runs on a machine that it has been installed on.
If I can get this to work my next project is a table macro?
I have removed the naming for the first point and line as it wasn't really needed.
I need a way to get the support elements into the collector geo-set so it will update, I can then have a go at the loop.

cheers
Alan

ps Is the line
Set partDocument1 = CATIA.ActiveDocument.Product.Products.Item(1).ReferenceProduct.Parent
the correct way to work at product level ?

 

[Alan Lowbands]

Sorry
Forgot to add the code

Sub CATMain()

Dim InputObject1(0)
Dim oCentreSelection
Dim oCentreItem
Dim oCentreRef
Dim oCentrePoint
Dim InputObject2(0)
Dim oFaceSelection
Dim oFaceItem
Dim oFaceRef
Dim oVector


Do


Dim part1
'Set partDocument1 = CATIA.ActiveDocument 'Part Level
Set partDocument1 = CATIA.ActiveDocument.Product.Products.Item(1).ReferenceProduct.Parent 'Product Level

Set part1 = partDocument1.Part

Dim hybridShapeFactory1 'As Factory
Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim hybridBodies1 'As HybridBodies
Set hybridBodies1 = part1.HybridBodies

Dim hybridBody1 'As HybridBody
Set hybridBody1 = hybridBodies1.Item(1)

Dim hybridShapes1 'As HybridShapes
Set hybridShapes1 = hybridBody1.HybridShapes

Dim selection1 'As Selection
Set selection1 = partDocument1.Selection

'------------------------------Select Hole Centre & Create Point---------------------
'Dim InputObject1(0)
InputObject1(0) = "Edge"
'Dim oCentreSelection
Set oCentreSelection = CATIA.ActiveDocument.Selection
Status = oCentreSelection.SelectElement2(InputObject1, "Select Circle", False)
'Dim oCentreItem
Set oCentreItem = oCentreSelection.Item(1)
'Dim oCentreRef
Set oCentreRef = oCentreItem.Reference
'Dim oCentrePoint
Set oCentrePoint = hybridShapeFactory1.AddNewPointCenter(oCentreRef)
hybridBody1.AppendHybridShape oCentrePoint

'-----------------------------Select Face & Create Vector----------------------------
'Dim InputObject2(0)
InputObject2(0)= "Face"
'Dim oFaceSelection
Set oFaceSelection = CATIA.ActiveDocument.Selection
Status=oFaceSelection.SelectElement2(InputObject2,"Select Face",false)
'Dim oFaceItem
Set oFaceItem = oFaceSelection.Item(1)
'Dim oFaceRef
Set oFaceRef = oFaceItem.Reference
'Dim oVector
Set oVector = hybridShapeFactory1.AddNewLineNormal(oFaceRef, oCentrePoint, 0.000000, 50.000000, True)
hybridBody1.AppendHybridShape oVector

Set oPoint25 = hybridShapeFactory1.AddNewPointOnCurveFromDistance(oVector, 25.000000, False) 'Point at 25mm
oPoint25.DistanceType = 1
hybridBody1.AppendHybridShape oPoint25

Set oPoint50 = hybridShapeFactory1.AddNewPointOnCurveFromDistance(oVector, 0.000000, False) 'Point at 50mm - end of Vector
oPoint50.DistanceType = 1
hybridBody1.AppendHybridShape oPoint50

'----------------------------Rename-------------------------------------------------

oPoint25.Name = "OTP"

oPoint50.Name = "OTP"

selection1.Clear

part1.Update

Loop

End Sub

 

[LWolf]

Alan, this was fun... here, try this:
just copy the code and run on your assy...
see if you can figure it out, perhaps you need some tweaking to get your 50mm lines

Sub CATMain()

Dim oManuName
oManuName = 3 'InputBox("Enter Screw size M?")

Dim holeDia
Dim holeHDAngle
Dim holeHDDepth
Dim holeName
If oManuName = 3 Then holeDia = 3.5
If oManuName = 3 Then holeHDAngle = 90
If oManuName = 3 Then holeHDDepth = 1.86
If oManuName = 3 Then holeName = "C/Sunk Hole for M3 CSHS"

Dim product1 As Product
Set product1 = CATIA.ActiveDocument.Product
Dim oSelection
Set oSelection = CATIA.ActiveDocument.Selection
oSelection.Clear

Dim oPart As Part
oSelection.Clear
oSelection.Search "Type=Hole,all"

Dim hole1 As Object

For i = 1 To oSelection.count
Set hole1 = oSelection.item(i).Value
reDim myAxisCoordinate(8)
hole1.Sketch.GetAbsoluteAxisData myAxisCoordinate
OriginX = myAxisCoordinate(0)
OriginY = myAxisCoordinate(1)
OriginZ = myAxisCoordinate(2)
HorizontalX = myAxisCoordinate(3)
HorizontalY = myAxisCoordinate(4)
HorizontalZ = myAxisCoordinate(5)
VerticalX = myAxisCoordinate(6)
VerticalY = myAxisCoordinate(7)
VerticalZ = myAxisCoordinate(8)
reDim H(2) 'As Double
reDim V(2) 'As Double
H(0) = HorizontalX
H(1) = HorizontalY
H(2) = HorizontalZ
V(0) = VerticalX
V(1) = VerticalY
V(2) = VerticalZ
Dim zAxis
zAxis = CrossProd(H, V)

Set oPart = GetPartFromObject(hole1)
Dim hybridShapeFactory1 As HybridShapeFactory
Set hybridShapeFactory1 = oPart.HybridShapeFactory
Dim hybridShapeDirection1 As HybridShapeDirection
Set hybridShapeDirection1 = hybridShapeFactory1.AddNewDirectionByCoord(zAxis(0), zAxis(1), zAxis(2))
Dim hybridShapeLinePtDir1 As HybridShapeLinePtDir
Set hybridShapeLinePtDir1 = hybridShapeFactory1.AddNewLinePtDir(hole1.Sketch.AbsoluteAxis.Origin, hybridShapeDirection1, -0, 20, False)

Dim hybridBodies1 As HybridBodies
Set hybridBodies1 = oPart.HybridBodies

Dim hybridBody1 As HybridBody
Set hybridBody1 = hybridBodies1.item(1)

hybridBody1.AppendHybridShape hybridShapeLinePtDir1
hole1.name = holeName & "." & i
oPart.Update
Next

oSelection.Clear

End Sub

Public Function CrossProd(V1, V2) 'As Double()
Dim Res() 'As Double
ReDim Res(2)
Res(0) = V1(1) * V2(2) - V1(2) * V2(1)
Res(1) = V1(2) * V2(0) - V1(0) * V2(2)
Res(2) = V1(0) * V2(1) - V1(1) * V2(0)
CrossProd = Res
Erase Res
End Function

Private Function GetPartFromObject(ByRef iObject As Object) As Part
Dim strTypeName As String
strTypeName = TypeName(iObject)

If strTypeName = "Part" Then
Set GetPartFromObject = iObject
Exit Function
ElseIf strType = TypeName(iObject.Parent) Then
Set GetPartFromObject = Nothing
Exit Function
Else
Set GetPartFromObject = GetPartFromObject(iObject.Parent)
End If
End Function


regards,
LWolf

 

[Alan Lowbands]

Wow, is that what it should have looked like.
I thought I was doing so well lolz
It’s a big learning curve.

Really have appreciated your help

Regards
Alan

 

[Alan Lowbands]

Hi LWolf,
I couldn't get the code to run but I think I see what you mean.
Using your method give the point a reference where my approach didn't.
It would have been nice to have it all linked to the selected hole in case anything was moved. An update request would make me check everything was ok.
I might try and create a curve on the hole edge to help spot if anything has moved. Would stand out more than just the line and points.
Couldn't find a way to isolate the point and tried AddPointDatum but couldn't get either to work
I shall have a go with what you sent.

and it isn't fun lol

thanks & best regards
Alan

 

[LWolf]

I tried the code as CATScript and inserted in VBA, both worked without any mishaps...
I have an assy with 3parts containing pads with random holes...
how is it not working?... anybody out there, could you pls. try to run the code?

regards,
LWolf

 

[Alan Lowbands]

Hi,
I have tried it again this morning on my work machine and it still drops out at
Private Function GetPartFromObject(ByRef iObject As Object) As Part

cheers
Alan

 

[Alan Lowbands]

Used the dodgy part level code this morning.
Made an AllCatPart of the assy, Battered of 40 plus points and copied them back over to the original assy.
Renamed and made the table.
Took about 20 min. Would have took 1 or 2 hours before so happy as a pig in ****.
Lost all links but it still counts as a win
Quite like these macro'y things lol

cheers LWolf & tesak

 

[Alan Lowbands]

Hi Guys,

Tried to get the code to run by trying to get the coordinates but got nowhere.
This line just wont work and I keep getting errors " hole1.Sketch.GetAbsoluteAxisData myAxisCoordinate "

Can anyone tell me how I can isolate the points in my original code so it will work in a product ?
Getting desperate lol

cheers
Alan

 

[tesak]

I would perhaps try to change the line

reDim myAxisCoordinate(8)

to

Dim myAxisCoordinate(8)

First one returns a dynamic array, a second one static array, which could make a difference in the end.

Tesak

https://scripts4all.eu/play-tetris-in-catia-v5-drawing-vba/

- Play Tetris in CATIA V5 drawing