Open bgbsww opened 1 month ago
bgbsww
commented
1 month ago Does not immediately replicate with Additive Cylinder or Additive Box used instead of Additive Cone. But there's essentially no code in Additive Cone, and zooming in on the original broken case shows the geometry of the intersecting Pipes is messed up. So strongly points at PD pipes.
mwganson
commented
1 month ago This is likely an upstream OCCT issue. It is often grouped within a class of issues known as "coplanar issues". Typically, the workaround for the overlapped seams is to rotate one of the parts slightly. Here you can set the attachment offset rotation angle of the 2nd profile sketch to 91 degrees (from 90).
Your code modified to run as a macro, with the workaround added near the bottom:
import TestSketcherApp
class Test:
def __init__(self):
self.Doc = FreeCAD.ActiveDocument
def testCrossedAdditivePipesWithConeCase(self):
App.KeepTestDoc = True
self.Body = self.Doc.addObject('PartDesign::Body','Body')
self.ProfileSketch = self.Doc.addObject('Sketcher::SketchObject', 'ProfileSketch')
self.Body.addObject(self.ProfileSketch)
TestSketcherApp.CreateCircleSketch(self.ProfileSketch, (0, 0), 1)
self.Doc.recompute()
self.SpineSketch = self.Doc.addObject('Sketcher::SketchObject', 'SpineSketch')
self.Body.addObject(self.SpineSketch)
self.SpineSketch.MapMode = 'FlatFace'
self.SpineSketch.AttachmentSupport = (self.Doc.XZ_Plane, [''])
self.Doc.recompute()
self.SpineSketch.addGeometry(Part.LineSegment(App.Vector(0.0,-10,0),App.Vector(0,10,0)),False)
self.SpineSketch.addConstraint(Sketcher.Constraint('PointOnObject',0,2,-2))
self.SpineSketch.addConstraint(Sketcher.Constraint('PointOnObject',0,1,-2))
self.SpineSketch.addConstraint(Sketcher.Constraint('DistanceY',0,1,0,2,20))
self.SpineSketch.addConstraint(Sketcher.Constraint('DistanceY',0,1,-1,1,10))
self.Doc.recompute()
self.ProfileSketch2 = self.Doc.addObject('Sketcher::SketchObject', 'ProfileSketch2')
self.ProfileSketch2.MapMode = 'FlatFace'
self.ProfileSketch2.AttachmentSupport = (self.Doc.YZ_Plane, [''])
# put the "seam" on the "side" to trigger bug
self.ProfileSketch2.AttachmentOffset = App.Placement(App.Vector(0,0,0),App.Rotation(App.Vector(0,0,1),90))
self.Body.addObject(self.ProfileSketch2)
TestSketcherApp.CreateCircleSketch(self.ProfileSketch2, (0, 0), 1)
self.SpineSketch2 = self.Doc.addObject('Sketcher::SketchObject', 'SpineSketch2')
self.Body.addObject(self.SpineSketch2)
self.SpineSketch2.MapMode = 'FlatFace'
self.SpineSketch2.AttachmentSupport = (self.Doc.XZ_Plane, [''])
self.Doc.recompute()
self.SpineSketch2.addGeometry(Part.LineSegment(App.Vector(-10,0,0),App.Vector(10,0,0)),False)
self.SpineSketch2.addConstraint(Sketcher.Constraint('PointOnObject',0,2,-1))
self.SpineSketch2.addConstraint(Sketcher.Constraint('PointOnObject',0,1,-1))
self.SpineSketch2.addConstraint(Sketcher.Constraint('DistanceX',0,1,0,2,20))
self.SpineSketch2.addConstraint(Sketcher.Constraint('DistanceX',0,1,-1,1,10))
self.Doc.recompute()
self.AdditivePipe = self.Doc.addObject("PartDesign::AdditivePipe","AdditivePipe")
self.Body.addObject(self.AdditivePipe)
self.AdditivePipe.Profile = self.ProfileSketch
self.AdditivePipe.Spine = self.SpineSketch
self.Doc.recompute()
# self.assertAlmostEqual(self.AdditivePipe.Shape.Volume, math.pi * 1 * 1 * 20)
self.AdditivePipe2 = self.Doc.addObject("PartDesign::AdditivePipe","AdditivePipe2")
self.Body.addObject(self.AdditivePipe2)
self.AdditivePipe2.Profile = self.ProfileSketch2
self.AdditivePipe2.Spine = self.SpineSketch2
self.Doc.recompute()
# self.assertAlmostEqual(self.AdditivePipe2.Shape.Volume, math.pi * 1 * 1 * 36 + (16*1*1*1)/3 )
self.AdditiveCone = self.Doc.addObject("PartDesign::AdditiveCone","AdditiveCone")
self.Body.addObject(self.AdditiveCone)
self.AdditiveCone.Radius1 = 1.5
self.AdditiveCone.Radius2 = 3
self.AdditiveCone.Height = 4
self.AdditiveCone.AttachmentSupport = [(self.Doc.getObject('XZ_Plane'),'')]
self.AdditiveCone.MapMode = 'FlatFace'
self.Doc.recompute()
# self.assertTrue(self.AdditiveCone.isValid())
self.ProfileSketch2.AttachmentOffset.Rotation.Angle = 91
self.Doc.recompute()
t = Test()
t.testCrossedAdditivePipesWithConeCase()I do not believe this is limited to PartDesign::AdditivePipe, but would also affect Part::Sweep and objects generated with python scripting.
adrianinsaval
commented
1 month ago yeah it's just strange that this particular case used to work but now doesn't
Is there an existing issue for this?
Problem description
Found while investigating various issues in #16634; this is a simplification of a problem that causes significant breakage in the larger multi file model. Test below shows that is you create two intersecting AdditivePipes, ensuring that the "seams" on the pipes are on the side, then if you try to place an AdditiveCone such that a face lands exactly at the pipe seams ( at the halfway depth of the pipes ), the cone starts to fail to build. I think this is probably an AdditivePipes issue, but can't be sure.
Full version info
Subproject(s) affected?
PartDesign
Anything else?
This test shows the issue:
Code of Conduct