3d curve macro recording not working in catia vba

[Hadiza Hamza]

i have been trying to record the creation of a 3d curve using control points in catia using the macro recorder but it refuses to record anything except part.update. I even tried it in both Freestyle workbench and Digitized shape editor workbench, but both have same result. please could someone explain to me how to do it or atleast where i could find such macro.

 

[itsmyjob]

you should check the v5automation.chm, the answer is there.

Eric N.
indocti discant et ament meminisse periti ​

 

[Hadiza Hamza]

Thanks for the reply. I did as as you advised and checked the file, however, i couldn't find anything. It might also be that i dont kow the exact words to search for. But i did search and check every result that had to with 3D Curve, 3D Spline, Record Macro as well as NURBS creation. However i couldn't find any useful information on them. Do you know any or did you find any? Please i would appreciate the help.

 

[itsmyjob]

if not in v5automation.chm file then it is not available. Freestyle API are not open... if you need them, talk to DS. This is not free, DS will ask for $$$ to make it available to you.

Eric N.
indocti discant et ament meminisse periti ​

 

[drewmumaw]

@Hadiza Hamza
Have you tried removing the points and re-adding them? Also in your specific scenario could you just recreate the 3D curve?

Drew Mumaw

http://www.textsketcher.com

http://www.drewmumaw.com

 

[Hadiza Hamza]

@drewmumaw

I am not trying to create a normal 2D spline which one can use the addNewSpline method for, but the 3D Curve which uses control points to guide its path. I have checked the object browser and it is not part of the index. I was told that when it is not in the Object browser that it could not be automated. I have also seen it being discussed as one of the features of catia that could only be automated using CAA RADE.

 

[itsmyjob]

i know that some freestyle function do not have API available, even in CAA. That's why some people are using non catia libraries (

http://www.smlib.com/nlib.html)

and import geometry in catia.

Eric N.
indocti discant et ament meminisse periti ​

 

[drewmumaw]

@Hadiza Hamza
AddNewSpline() can create a 3D curve if you use non-planar points. See code below that uses 3 points to create a 3D curve (in this example I already created 3 points in a geometrical set in CATIA, but you could create them in your own script to make it fully automated).

Sub CATMain()

Dim partDocument1 As PartDocument
Set partDocument1 = CATIA.ActiveDocument

Dim part1 As Part
Set part1 = partDocument1.Part

Dim hybridShapeFactory1 As HybridShapeFactory
Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim hybridShapeSpline1 As HybridShapeSpline
Set hybridShapeSpline1 = hybridShapeFactory1.AddNewSpline()

hybridShapeSpline1.SetSplineType 0

hybridShapeSpline1.SetClosing 0

Dim hybridBodies1 As HybridBodies
Set hybridBodies1 = part1.HybridBodies

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

Dim hybridShapes1 As HybridShapes
Set hybridShapes1 = hybridBody1.HybridShapes

Dim hybridShapePointCoord1 As HybridShapePointCoord
Set hybridShapePointCoord1 = hybridShapes1.Item("Point.1")

Dim reference1 As Reference
Set reference1 = part1.CreateReferenceFromObject(hybridShapePointCoord1)

hybridShapeSpline1.AddPointWithConstraintExplicit reference1, Nothing, -1#, 1, Nothing, 0#

Dim hybridShapePointCoord2 As HybridShapePointCoord
Set hybridShapePointCoord2 = hybridShapes1.Item("Point.2")

Dim reference2 As Reference
Set reference2 = part1.CreateReferenceFromObject(hybridShapePointCoord2)

hybridShapeSpline1.AddPointWithConstraintExplicit reference2, Nothing, -1#, 1, Nothing, 0#

Dim hybridShapePointCoord3 As HybridShapePointCoord
Set hybridShapePointCoord3 = hybridShapes1.Item("Point.3")

Dim reference3 As Reference
Set reference3 = part1.CreateReferenceFromObject(hybridShapePointCoord3)

hybridShapeSpline1.AddPointWithConstraintExplicit reference3, Nothing, -1#, 1, Nothing, 0#

hybridBody1.AppendHybridShape hybridShapeSpline1

part1.InWorkObject = hybridShapeSpline1

part1.Update

End Sub

Drew Mumaw

http://www.textsketcher.com

http://www.drewmumaw.com