doc/gui/examples/tutorial.py

   1 # -*- coding: utf-8 -*-
   2
   3 from SketchAPI import *
   4
   5 from salome.shaper import model
   6
   7 model.begin()
   8 partSet = model.moduleDocument()
   9 Part_1 = model.addPart(partSet)
  10 Part_1_doc = Part_1.document()
  11
  12 # Step1. Sketch.
  13 Sketch_1 = model.addSketch(Part_1_doc, model.defaultPlane("XOY"))
  14 SketchLine_1 = Sketch_1.addLine(-57.7, 99.93933159672423, 57.7, 99.93933159672423)
  15 SketchLine_2 = Sketch_1.addLine(57.7, 99.93933159672423, 0, 0)
  16 SketchLine_2.setAuxiliary(True)
  17 SketchConstraintCoincidence_1 = Sketch_1.setCoincident(SketchLine_1.endPoint(), SketchLine_2.startPoint())
  18 SketchLine_3 = Sketch_1.addLine(0, 0, -57.7, 99.93933159672423)
  19 SketchLine_3.setAuxiliary(True)
  20 SketchConstraintCoincidence_2 = Sketch_1.setCoincident(SketchLine_2.endPoint(), SketchLine_3.startPoint())
  21 SketchConstraintCoincidence_3 = Sketch_1.setCoincident(SketchLine_1.startPoint(), SketchLine_3.endPoint())
  22 SketchProjection_1 = Sketch_1.addProjection(model.selection("VERTEX", "PartSet/Origin"), False)
  23 SketchPoint_1 = SketchProjection_1.createdFeature()
  24 SketchConstraintCoincidence_4 = Sketch_1.setCoincident(SketchLine_3.startPoint(), SketchAPI_Point(SketchPoint_1).coordinates())
  25 SketchProjection_2 = Sketch_1.addProjection(model.selection("EDGE", "PartSet/OY"), False)
  26 SketchLine_4 = SketchProjection_2.createdFeature()
  27 SketchConstraintPerpendicular_1 = Sketch_1.setPerpendicular(SketchLine_4.result(), SketchLine_1.result())
  28 SketchConstraintEqual_1 = Sketch_1.setEqual(SketchLine_3.result(), SketchLine_1.result())
  29 SketchConstraintEqual_2 = Sketch_1.setEqual(SketchLine_2.result(), SketchLine_1.result())
  30 SketchMultiRotation_1 = Sketch_1.addRotation([SketchLine_1.result()], SketchAPI_Line(SketchLine_4).startPoint(), 360, 6, True)
  31 [SketchLine_5, SketchLine_6, SketchLine_7, SketchLine_8, SketchLine_9] = SketchMultiRotation_1.rotated()
  32 SketchConstraintLength_1 = Sketch_1.setLength(SketchLine_1.result(), 115.4)
  33 model.do()
  34
  35 # Step2. Polyline.
  36 Point_2 = model.addPoint(Part_1_doc, 50, 0, 0)
  37 Point_2.result().setColor(0, 0, 255)
  38 Point_3 = model.addPoint(Part_1_doc, 80, 0, 0)
  39 Point_3.result().setColor(0, 0, 255)
  40 Point_4 = model.addPoint(Part_1_doc, 112, 0, 13)
  41 Point_4.result().setColor(0, 0, 255)
  42 Point_5 = model.addPoint(Part_1_doc, 112, 0, 48)
  43 Point_5.result().setColor(0, 0, 255)
  44 Point_6 = model.addPoint(Part_1_doc, 80, 0, 63)
  45 Point_6.result().setColor(0, 0, 255)
  46 Point_7 = model.addPoint(Part_1_doc, 80, 0, 90)
  47 Point_7.result().setColor(0, 0, 255)
  48 Point_8 = model.addPoint(Part_1_doc, 50, 0, 90)
  49 Point_8.result().setColor(0, 0, 255)
  50
  51 Polyline_1_objects = [model.selection("VERTEX", "Point_1"), model.selection("VERTEX", "Point_2"),
  52                       model.selection("VERTEX", "Point_3"), model.selection("VERTEX", "Point_4"),
  53                       model.selection("VERTEX", "Point_5"), model.selection("VERTEX", "Point_6"),
  54                       model.selection("VERTEX", "Point_7")]
  55 Polyline_1 = model.addPolyline3D(Part_1_doc, Polyline_1_objects, True)
  56
  57 # Step3. Face.
  58 Face_1 = model.addFace(Part_1_doc, [model.selection("WIRE", "Polyline_1_1")])
  59
  60 # Step4. Revolution.
  61 Revolution_1 = model.addRevolution(Part_1_doc, [model.selection("FACE", "Face_1_1")], model.selection("EDGE", "PartSet/OZ"), 360, 0)
  62
  63 # Step5. Extrusion.
  64 Wire_Name = "Sketch_1/Wire-SketchLine_1r-SketchLine_5r-SketchLine_6r-SketchLine_7r-SketchLine_8r-SketchLine_9r"
  65 Extrusion_1 = model.addExtrusion(Part_1_doc, [model.selection("WIRE", Wire_Name)], model.selection("EDGE", "PartSet/OZ"), 100, 0)
  66
  67 # Step6. Common.
  68 Common_1 = model.addCommon(Part_1_doc, [model.selection("SOLID", "Revolution_1_1"), model.selection("SOLID", "Extrusion_1_1")])
  69
  70 # Step7. Fillet.
  71 Fillet_1 = model.addFillet(Part_1_doc, [model.selection("EDGE", "Revolution_1_1/Generated_Face_5&Common_1_1/Modified_Face_10")], 10)
  72
  73 # Step8. Box.
  74 Box_1 = model.addBox(Part_1_doc, 20, 120, 20)
  75
  76 # Step9. Translation.
  77 Translation_1 = model.addTranslation(Part_1_doc, [model.selection("SOLID", "Box_1_1")], -10, 20, 70)
  78
  79 # Step10. Angular Copy.
  80 AngularCopy_1 = model.addMultiRotation(Part_1_doc, [model.selection("SOLID", "Translation_1_1")], model.selection("EDGE", "PartSet/OZ"), 6)
  81
  82 # Step11. Cut.
  83 Cut_1 = model.addCut(Part_1_doc, [model.selection("SOLID", "Fillet_1_1")], [model.selection("COMPOUND", "AngularCopy_1_1")])
  84 Cut_1.result().setColor(255, 214, 0)
  85
  86 model.do()
  87 model.end()