Reference Axis by Pycatia

[hosseintfr]

Hi. I want to create a plane with an angle about zx plane. But when I want to define the Z Axis of my part, I get an error. The macro that I do this is:

Language="VBSCRIPT"

Sub CATMain()

Set documents1 = CATIA.Documents

Set partDocument1 = documents1.Item("Winding_HV.CATPart")

Set part1 = partDocument1.Part

Set originElements1 = part1.OriginElements

Set hybridShapePlaneExplicit1 = originElements1.PlaneZX

Set reference1 = part1.CreateReferenceFromObject(hybridShapePlaneExplicit1)

Set bodies1 = part1.Bodies

Set body1 = bodies1.Item("PartBody")

Set hybridShapes1 = body1.HybridShapes

Set hybridShapeLineExplicit1 = hybridShapes1.Item("Z Axis")

Set reference2 = part1.CreateReferenceFromObject(hybridShapeLineExplicit1)

Set hybridShapeFactory1 = part1.HybridShapeFactory

Set hybridShapePlaneAngle1 = hybridShapeFactory1.AddNewPlaneAngle(reference1, reference2, -30.000000, False)

hybridShapePlaneAngle1.ProjectionMode = False

body1.InsertHybridShape hybridShapePlaneAngle1

part1.InWorkObject = hybridShapePlaneAngle1

part1.Update

End Sub

---

My python code is: ...

Winding_HV = documents.item("Winding_HV.CATPart") document = PartDocument(Winding_HV.com_object) part_HV = Part(document.part.com_object)

originElements1 = part_HV.origin_elements hybridShapePlaneExplicit1 = originElements1.plane_zx reference1 = part_HV.create_reference_from_object(hybridShapePlaneExplicit1) bodies1 = part_HV.bodies body1 = bodies1.item("PartBody") hybridShapes1 = body1.hybrid_shapes hybridShapeLineExplicit1 = hybridShapes1.item("Z Axis") reference2 = part_HV.create_reference_from_object(hybridShapeLineExplicit1) hybridShapeFactory1 = part_HV.hybrid_shape_factory hybridShapePlaneAngle1 = hybridShapeFactory1.add_new_plane_angle(reference1, reference2, -30.000000, False) hybridShapePlaneAngle1.projection_mode = False part_HV.in_work_object = hybridShapePlaneAngle1

part_HV.update()

[hosseintfr]

My other way for creating that plane is by defining the plane through 2 lines. The macro of this way works well without any error. But the pycatia method does not work. However, python does not have any error. But no plane is created!

Macro code: Language="VBSCRIPT"

Sub CATMain()

Dim documents1 As Documents Set documents1 = CATIA.Documents

Dim partDocument1 As Document Set partDocument1 = documents1.Item("Winding_HV.CATPart")

Dim part1 As Part Set part1 = partDocument1.Part

Dim hybridShapeFactory1 As Factory Set hybridShapeFactory1 = part1.HybridShapeFactory

Dim bodies1 As Bodies Set bodies1 = part1.Bodies

Dim body1 As Body Set body1 = bodies1.Item("PartBody")

Dim sketches1 As Sketches Set sketches1 = body1.Sketches

Dim sketch1 As Sketch Set sketch1 = sketches1.Item("sketch_line_b")

Dim reference1 As Reference Set reference1 = part1.CreateReferenceFromObject(sketch1)

Dim sketch2 As Sketch Set sketch2 = sketches1.Item("sketch_line_a")

Dim reference2 As Reference Set reference2 = part1.CreateReferenceFromObject(sketch2)

Dim hybridShapePlane2Lines1 As HybridShapePlane2Lines Set hybridShapePlane2Lines1 = hybridShapeFactory1.AddNewPlane2Lines(reference1, reference2)

body1.InsertHybridShape hybridShapePlane2Lines1

part1.InWorkObject = hybridShapePlane2Lines1

part1.Update

End Sub

Pycatia code:

Winding_HV = documents.item("Winding_HV.CATPart") document = PartDocument(Winding_HV.com_object) part_HV = Part(document.part.com_object) hybridShapeFactory = part_HV.hybrid_shape_factory bodies = part_HV.bodies body = bodies.get_item_by_name("PartBody") sketches1 = body.sketches

sketch_line_a = sketches1.item("sketch_line_a") sketch_line_b = sketches1.item("sketch_line_b") reference1 = part_HV.create_reference_from_object(sketch_line_a) reference2 = part_HV.create_reference_from_object(sketch_line_b) Plane2Lines = hybridShapeFactory.add_new_plane2_lines(reference1, reference2)

part_HV.in_work_object = Plane2Lines part_HV.update()

[evereux]

In your second example you've omitted the equivalent of body1.InsertHybridShape hybridShapePlane2Lines1.

In your first example the same thing is missing but you say you're getting an error. What is the error you're getting? How do I need to set-up my CATIA part to run your code?

[hosseintfr]

There is no command equivalent with body1.InsertHybridShape in Pycatia. Where is inserhybridshape command?!

In my first code my error is this: (it seems that the Z axis is not defined in Catia)

[2024-01-20 16:36:43,944] INFO in documents: Creating a new "Product". Traceback (most recent call last): File "C:\Users\u6790\PycharmProjects\pythonProject\Pycatia_Winding.py", line 798, in hybridShapeLineExplicit1 = hybridShapes1.item("Z Axis") ^^^^^^^^^^^^^^^^^^^^^^^^^^^^ File "C:\Users\u6790\PycharmProjects\pythonProject\venv\Lib\site-packages\pycatia\mec_mod_interfaces\hybrid_shapes.py", line 103, in item return HybridShape(self.hybrid_shapes.Item(i_index)) ^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^ File "<COMObject >", line 2, in Item pywintypes.com_error: (-2147352567, 'Exception occurred.', (0, 'CATIAHybridShapes', 'The method Item failed', None, 0, -2147352573), None)

[hosseintfr]

Can you please create a plane by pycatia that is equivalent of one of three main planes with an angle about it? I can just create a plane that is offset of one of three main planes. The other ways for creating plane is not working. Can you please write an example that create a plane other than offset method? Like angle with a plane, or crossing three points or by crossing two lines?

[evereux]

There is no command equivalent with body1.InsertHybridShape in Pycatia. Where is inserhybridshape command?!

https://pycatia.readthedocs.io/en/latest/api/pycatia/mec_mod_interfaces/body.html#pycatia.mec_mod_interfaces.body.Body.insert_hybrid_shape !?

https://github.com/evereux/pycatia/blob/7263c27b248e3d2fd107dfd395943625a5410315/pycatia/mec_mod_interfaces/body.py#L200 !?

You need to provide me information so I may reproduce your problem then point you in the right direction. I don't know what my part needs in order reproduce your error.

[evereux]

Can you please create a plane by pycatia that is equivalent of one of three main planes with an angle about it? I can just create a plane that is offset of one of three main planes. The other ways for creating plane is not working. Can you please write an example that create a plane other than offset method? Like angle with a plane, or crossing three points or by crossing two lines?

Maybe in the future. I don't have the time right now. Maybe someone else can.

[hosseintfr]

Thanks a lot. I found my problem. I did not import HybridShapes in the first of my code. I added this: from pycatia.mec_mod_interfaces.body import Body, HybridShape, HybridBodies, Shapes

But yet I don't know how to define the 3 major axis (x, y, and z axis) to pycatia.

[evereux]

Here is a working example.

requires:

• CATPart open
• Geometrical set named "Geometrical Set.1"
• Inside "Geometrical Set.1" a line named "Line.1" which is drawn normal to the XY plane.

from pycatia import catia
from pycatia.mec_mod_interfaces.part import Part

caa = catia()
application = caa.application
part_document = application.active_document
part = Part(part_document.part.com_object)

bodies = part.bodies
hybrid_bodies = part.hybrid_bodies
hsf = part.hybrid_shape_factory

geom_set = hybrid_bodies.get_item_by_name("Geometrical Set.1")
hybrid_shapes = geom_set.hybrid_shapes
line = hybrid_shapes.get_item("Line.1")

origin_elements = part.origin_elements
plane_zx = origin_elements.plane_zx

ref_line = part.create_reference_from_object(line)
ref_plane_zx = part.create_reference_from_object(plane_zx)

new_plane = hsf.add_new_plane_angle(ref_plane_zx, ref_line, 45, True)
geom_set.append_hybrid_shape(new_plane)

part.update()