Chamfer

The Chamfer declaration can be used to add a straight cut to edges on a shape. There's several different types of chamfer operations that can be performed so let's cover each.

Chamfer Operations

The screenshot above demonstrates the following chamfer operations:

  • Chamfering all edges of a shape with a the same distance and optional distance2 (shown in orange)
  • Chamfering only faces given in the operations list with the same distance and optional distance2 attribute (shown in red)
  • Chamfering specific sets of faces with specific dstances by defining them in the operations list (shown in purple)
  • Chamfering specific sets of edges and faces pairs by defining them in the operations list (shown in blue)
  • Chamfering any combination of the above by setting them in the in the operations list (shown in green)

The code for the chamfer example is as follows:

""" This example shows how to use chamfer operations

See https://dev.opencascade.org/doc/overview/html/occt_user_guides__modeling_algos.html#occt_modalg_6
for more on how this works.

"""

from declaracad.occ.api import Part, Box, Chamfer


enamldef Assembly(Part):
    name = "Chamfer Operations"

    Chamfer:
        # If no operations are given it applies to all faces
        distance = 20
        Box:
            position = (-300, 0, 0)
            dx = 200
            dy = 200
            dz = 200

    Chamfer:
        # Or you can supply which faces to apply the chamfer to
        # and you can change the slope by specifying distance2
        color = 'red'
        distance = 20
        distance2 = 40
        attr top_face = self.children[0].topology.faces[5]
        attr bottom_face = self.children[0].topology.faces[4]
        operations = [top_face, bottom_face]
        Box:
            position = (300, 0, 0)
            dx = 200
            dy = 200
            dz = 200

    Chamfer:
        # You also supply specify different chamfer distances for each chamfer
        color = 'purple'
        operations = [
            (20, self.children[0].topology.faces[5]),
            (50, self.children[0].topology.faces[4]),
        ]
        Box:
            dx = 200
            dy = 200
            dz = 200

    Chamfer:
        # You can supply a tuple of (edge, face) to define which edges of a
        # given face should be chamfered
        color = 'blue'
        distance = 20
        attr top_face = self.children[0].topology.faces[5]
        attr top_edges = self.children[0].topology.edges_from_face(top_face)
        operations = [
            (top_edges[0], top_face),
            (top_edges[2], top_face)
        ]
        Box:
            position = (0, -300, 0)
            dx = 200
            dy = 200
            dz = 200

    Chamfer:
        # You also supply the chamfer distances for these as well
        color = 'green'
        attr top_face = self.children[0].topology.faces[5]
        attr bottom_face = self.children[0].topology.faces[4]
        attr top_edges = self.children[0].topology.edges_from_face(top_face)
        operations = [
            (70, 20, top_edges[0], top_face),
            (50, top_edges[2], top_face),
            (50, bottom_face)
        ]
        Box:
            position = (0, 300, 0)
            dx = 200
            dy = 200
            dz = 200

Variable width chamfer

DeclaraCAD can now also perform a chamfer with variable widths. To use it provide a list of parametric values and widths in the operations list along with the edge.

Variable width chamfer

enamldef CylinderEdge(Part):
    attr h = 4
    Chamfer:
        material = 'aluminium'
        color = 'slategray'
        attr edges = plate.topology.edges
        attr profile_edges = (58, 130, 163)
        attr top_edges = (46, 50, 54, 58, 71, 130, 137, 141, 145, 154, 158, 162, 163, 170, 174, 178, 182, 186)
        attr profile = [
            (0, 0.5),
            (0.2, 1),
            (0.5, 1.2),
            (0.8, 1),
            (1, 0.5),
        ]
        operations = [
            (profile if i in profile_edges else 0.5, edges[i])
            for i in top_edges
        ]
        Cut: plate:
            Fillet:
                radius = 5
                attr edges = self.children[0].topology.edges
                operations = [
                    edges[i] for i in ( 24, 26, 28, 33, 38, 42, 46, 50, 54)
                ]
                Fuse:
                    Cylinder:
                        radius = 20
                        height = h
                    Extrude:
                        vector = (0, 0, h)
                        Face:
                            Polygon:
                                radius = 30
                                co unt = 3
            Cylinder: # Center hole
                radius = 14
                height = h

            Looper: # Bolt holes
                iterable = [0, 120, -120]
                Cylinder:
                    attr r = 20
                    attr a = radians(loop.item)
                    position = (r*cos(a), r*sin(a))
                    radius = 2
                    height = h

Note: At the moment it requires a patch to OCCT.