===========
Operations_
===========

pushPull
========

.. autofunction:: hwx.inspire.core.geometry.pushPull

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   cylinder1 = model.createSolidCylinder(
      radius=1,
      height=6,
   )
   cylinder1.location = (-4, 0, 0)
   parts = model.parts
   featPlanar = parts[0].getFeatures(type='FeaturePlanar')[1]
   featPlanar.pushPull('1m')
   inspire.fitView()
   print("Cylinder1 is pushed to 1 meter without using variable.")
   inspire.orientView(direction="isometric")

   # Usage of variable to pushPull a feature.

   cylinder2 = model.createSolidCylinder(
      radius=1,
      height=6,
   )
   parts = model.parts
   featPlanar = parts[0].getFeatures(type='FeaturePlanar')[1]
   model.variables.add("depth", type="length", expression=0.8)
   featPlanar.pushPull("depth")
   inspire.fitView()
   print("Cylinder2 is pushed to 1 meter by using variable 'depth'.")
   inspire.orientView(direction="isometric")

   # Example to edit pushPull operation.
   pushPullCF = model.construction[-1]
   with pushPullCF.edit():
      pushPullCF.depth = 3
   inspire.fitView()
   print("Cylinder2 is pushed to 3 meter by editing cf.")
   inspire.orientView(direction="isometric")


extract
=======

.. autofunction:: hwx.inspire.core.geometry.extract

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.openTutorialFile("Structures/base.x_t")
   parts=model.parts
   featPlanar=model.parts[0].getFeatures(type='FeaturePlanar')[8]
   featPlanar.extract()
   print("Extracted part is created")
   inspire.orientView(direction="isometric")


mirror
======

.. autofunction:: hwx.inspire.core.geometry.mirror

**Example**

.. code-block::

   # There are two ways, user can create a mirrored part. One by calling
   # mirror method on the part, or else select a planar feature on which
   # the mirrored part will be created
   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()

   # First using the part
   box.mirror(planeOrigin=(0, 0, 1), planeNormal=(0, 0, 1))
   print("A new part has been mirrored")

   featurePlanar = box.getFeatures(type='FeaturePlanar')[1]
   featurePlanar.mirror()
   print("Another new part has been mirrored from the planar feature")
   inspire.orientView(direction="isometric")


patch
=====

.. autofunction:: hwx.inspire.core.geometry.patch

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   cyl = model.createSolidCylinder(radius=0.3)
   part = box.booleanSubtract(cyl)
   featCircular = part.getFeatures(type='FeatureCircular')[0]
   featCircular.patch()
   print("Patch is created on a cylindrical face ")

   featPlanar = part.getFeatures(type='FeaturePlanar')[2]
   featPlanar.deleteFaces()
   print("Deleted a planar face from the part ")
   inspire.orientView(direction="isometric")


rotate
======

.. autofunction:: hwx.inspire.core.geometry.rotate

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   cylinder1 = model.createSolidCylinder(
      radius=1,
      height=6,
      color='blue'
   )
   cylinder2 = model.createSolidCylinder(
      radius=1,
      height=6,
      color='red'
   )
   cylinder2.rotate('x', 45, degrees=True)
   inspire.fitView()


translate
=========

.. autofunction:: hwx.inspire.core.geometry.translate

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   cylinder1 = model.createSolidCylinder(
      radius=1,
      height=6,
      color='blue'
   )
   cylinder2 = model.createSolidCylinder(
      radius=1,
      height=6,
      color='red'
   )
   cylinder2.translate(x=10, y=0, z=0)
   inspire.fitView()


move
====

.. autofunction:: hwx.inspire.core.geometry.move

**Example**

.. code-block::

   from hwx import inspire
   from hwx.common.math import Matrix44

   model = inspire.newModel()
   cylinder1 = model.createSolidCylinder(
      radius=1,
      height=6,
      color='blue'
   )
   cylinder2 = model.createSolidCylinder(
      radius=1,
      height=6,
      color='red'
   )
   mat = Matrix44(origin=[1, 2, 3], angles=[30, 0, 0], degrees=True)
   cylinder2.move(mat)
   inspire.fitView()


deleteFaces
===========

.. autofunction:: hwx.inspire.core.geometry.deleteFaces
scale
=====

.. autofunction:: hwx.inspire.core.geometry.scale

**Example**

.. code-block::

   from hwx import inspire

   model=inspire.openTutorialFile("Structures/plate.x_t")
   part=model.parts[0]
   part.scale(2.0)
   print("Part is scaled by factor 2")
   inspire.fitView()


booleanCombine
==============

.. autofunction:: hwx.inspire.core.geometry.booleanCombine

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   sphere = model.createSolidSphere()
   box.booleanCombine(sphere)
   print("Box is combined with sphere")
   inspire.orientView(direction="isometric")


booleanSubtract
===============

.. autofunction:: hwx.inspire.core.geometry.booleanSubtract

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   sphere = model.createSolidSphere()
   sphere.booleanSubtract(box)
   print("Sphere is subtracted with box")
   inspire.orientView(direction="isometric")


booleanIntersect
================

.. autofunction:: hwx.inspire.core.geometry.booleanIntersect

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   sphere = model.createSolidSphere()
   sphere.booleanIntersect(box)
   print("Sphere is intersected with box")
   inspire.orientView(direction="isometric")


slice
=====

.. autofunction:: hwx.inspire.core.geometry.slice

**Example**

.. code-block::

   # There are two ways, user can create a slice part. One by calling
   # slice method on the part with cutNormal & cutOrigion and other by calling
   # slice method with surfaceFeature to slice out on surface mode.
   from hwx import inspire

   model = inspire.newModel()
   part = model.createSolidBlock(x=2, y=1, z=1, location=(0, 0, 0))
   history = model.history

   # First using the Plane Slice
   part.slice(cutOrigin=(0,0,0), cutNormal=(1,0,0))
   print("A new part has been sliced out from the existing part on Plane Mode "
         "with both cutNormal and cutOrigin")

   # Second using the Surface Slice
   box = model.createSolidBlock(location=(-1, 0.5, 0))
   feature = box.features[21]
   part.slice(surfaceFeature=feature, extendSurface=True)
   history.noteState()
   print("Another new part has been sliced out from the existing part on Surface Mode")
   inspire.orientView(direction="isometric")


simplifyImprints
================

.. autofunction:: hwx.inspire.core.geometry.simplifyImprints

**Example**

.. code-block::

   # There are two ways, user can remove an imprint from model. One by calling
   # simplifyImprints on the imprint feature or choose the part from which you
   # want to remove the imprints from.
   from hwx import inspire
   from hwx.inspire.demo import openDemoFile

   model = openDemoFile("Imprints.x_t")
   linearFeatures = model.getFeatures(type='FeatureLinear')
   # Removing Imprint feature
   linearFeatures[0].simplifyImprints()
   print("A line imprint has been removed from the part")

   # Removing Imprints from a part
   model.parts[0].simplifyImprints()
   print("All the line imprints has been removed from the part")
   inspire.orientView(direction="isometric")


simplifyRounds
==============

.. autofunction:: hwx.inspire.core.geometry.simplifyRounds

**Example**

.. code-block::

   # There are two ways, user can remove a round or fillets from model. One by calling
   # simplifyRounds on the feature or choose the part from which you
   # want to remove the rounds from.
   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   feats = box.getFeatures(type='FeatureLinear')[:4]
   inspire.geometry.edgeFillet(feats, radius='60mm')

   featCylindrical = model.parts[0].getFeatures(type='FeatureCylindrical')[3]
   # Removing the fillet feature
   featCylindrical.simplifyRounds()
   print("A Fillet has been removed from the part.")

   # Removing all the fillet features from the part
   model.parts[0].simplifyRounds()
   print("All the fillets has been removed from the part.")
   inspire.orientView(direction="isometric")

   # Removing all fillet by passing Model.
   model = inspire.newModel()
   box2 = model.createSolidBlock()
   feats2 = box2.getFeatures(type='FeatureLinear')[:4]
   inspire.geometry.edgeFillet(feats2, radius='60mm')

   model.simplifyRounds()
   print("All the fillets has been removed from the model.")
   inspire.orientView(direction="isometric")


simplifyHoles
=============

.. autofunction:: hwx.inspire.core.geometry.simplifyHoles

**Example**

.. code-block::

   # There are two ways, user can remove a hole from model. One by calling
   # simplifyHoles on the hole feature or choose the part from which you
   # want to remove the holes from.
   from hwx import inspire

   model = inspire.openTutorialFile("Structures/bracket.x_t")
   featCylindrical = model.parts[0].getFeatures(type='FeatureCylindrical')[2]
   # Removing the hole feature
   featCylindrical.simplifyHoles()
   print("A Hole has been removed from the part.")

   # Removing holes feature from the part
   model.parts[0].simplifyHoles()
   print("All the holes has been removed from the part.")
   inspire.orientView(direction="isometric")


simplifyPlugs
=============

.. autofunction:: hwx.inspire.core.geometry.simplifyPlugs

**Example**

.. code-block::

   # There are two ways, user can plug holes from model. One by calling
   # simplifyPlugs on the hole feature or choose the part from which you
   # want to plug the holes from.
   from hwx import inspire

   model = inspire.openTutorialFile("Structures/bracket.x_t")
   featCylindrical = model.parts[0].getFeatures(type='FeatureCylindrical')[2]
   # Plug the hole feature
   featCylindrical.simplifyPlugs()
   print("A Hole has been plugged with new part.")

   # Plug all the holes in the part
   model.parts[0].simplifyPlugs()
   print("All the holes has been with new part.")
   inspire.orientView(direction="isometric")


partition
=========

.. autofunction:: hwx.inspire.core.geometry.partition

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.openTutorialFile("Structures/bracket.x_t")
   featCircular = model.parts[0].getFeatures(type='FeatureCylindrical')[2]
   featCircular.partition(thickness="3 mm")
   print("Partition part is created with thickness of 3mm")
   inspire.orientView(direction="isometric")


midSurface
==========

.. autofunction:: hwx.inspire.core.geometry.midSurface

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   part = model.createSolidBlock()
   part.midSurface(surfaceOptions='Left')
   print("A Surface has been extracted from part {0}", part)
   inspire.orientView(direction="isometric")


chamferByAngle
==============

.. autofunction:: hwx.inspire.core.geometry.chamferByAngle

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   featPlane1, featPlane2 = box.getFeatures(type='FeaturePlanar')[0:2]

   # Chamfer by angle
   featPlane1.chamferByAngle(angle=45, dist=0.05)

   print("New chamfers is created.")
   inspire.orientView(direction="isometric")


chamferByDistance
=================

.. autofunction:: hwx.inspire.core.geometry.chamferByDistance

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   featPlane1, featPlane2 = box.getFeatures(type='FeaturePlanar')[0:2]

   # Chamfer by distance
   featPlane2.chamferByDistance(dist1=0.06, dist2=0.06)

   print("New chamfer is created.")
   inspire.orientView(direction="isometric")


shell
=====

.. autofunction:: hwx.inspire.core.geometry.shell

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.openTutorialFile("Structures/base.x_t")
   parts=model.parts
   featPlanar=model.parts[0].getFeatures(type='FeaturePlanar')[9]
   featPlanar.shell(thickness=.5)
   print("Shell is created on base part with the thickness of 0.5mm")
   inspire.orientView(direction="isometric")


extrude
=======

.. autofunction:: hwx.inspire.core.geometry.extrude

**Example**

.. code-block::

   from hwx import inspire

   # Extrude As Solid
   model = inspire.newModel()
   s = inspire.core.Sketch()
   s.addRectangle2Vertex((0, 0), (2, 2))
   s.realize()
   sketch_part = model.getAllChildren('SketchPart')[0]
   inspire.geometry.extrude(sketch_part.getFeatures(type=inspire.FeatureArea),
                           "SINGLE", "NEW_PART", extrudeTo1=0.1)

   s = inspire.core.Sketch()
   s.addCircleCenterRadius((1, 1), 0.3)
   s.realize()
   sketch_part = model.getAllChildren('SketchPart')[1]
   sketch_part.position
   p = model.parts[0]
   faces = p.getFeatures('FeaturePlanar')
   inspire.geometry.extrude(sketch_part.getFeatures(type=inspire.FeatureArea),
                           "SINGLE", "SUBTRACT", extrudeTo1=faces[4])

   # Extrude As Sheet
   s = inspire.core.Sketch()
   s.addRectangle2Vertex((0, 0), (2, 2))
   s.realize()
   sketch_part = model.getAllChildren('SketchPart')[0]
   inspire.geometry.extrude(sketch_part.getFeatures(type=inspire.FeatureArea),
                           "SYMMETRY", "NEW_PART", extrudeTo1=0.1, angle1=45, extrudeAsSolid=False,
                           reference=(0, 0, 1), extrusionEndCaps="BOTH")

   inspire.orientView(direction="isometric")


offset
======

.. autofunction:: hwx.inspire.core.geometry.offset

**Example**

.. code-block::

   from hwx import inspire

   # Creating a solid box and applying offset of value 3.0 in face feature and value 0.2 to part
   model = inspire.newModel()
   box = model.createSolidBlock()

   featFace = box.getFeatures(type="FeaturePlanar")
   inspire.core.geometry.offset(featFace, value=3.0)
   inspire.core.geometry.offset(box, value=0.2)

   print("Offset has been applied to feature and part")
   inspire.orientView(direction="isometric")


thicken
=======

.. autofunction:: hwx.inspire.core.geometry.thicken

**Example**

.. code-block::

   from hwx import inspire

   # Creating a solid box and applying thicken of value 0.2
   model = inspire.newModel()
   box = model.createSolidBlock()
   inspire.core.geometry.thicken(box, value=0.2)

   print("Thicken has been applied to a part")
   inspire.orientView(direction="isometric")


linearPattern
=============

.. autofunction:: hwx.inspire.core.geometry.linearPattern

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()

   # Creating a linear pattern of box.
   box.linearPattern(direction1=box.getFeatures(type="FeatureCurve")[0],
                     spacing1=2, count1=5, symmetry1=True)

   print("Linear pattern has been created for Box")
   inspire.orientView(direction="isometric")


createPipe
==========

.. autofunction:: hwx.inspire.core.geometry.createPipe

**Example**

.. code-block::

   from hwx import inspire

   # Creating a sketch of line segment.
   model = inspire.newModel()
   s = inspire.core.Sketch()
   point1 = s.addPoint(0, 0)
   start = s.addPoint(0, 5)
   s.addLineSegment(point1, start)
   s.realize()
   sketch_part = model.getAllChildren(inspire.SketchPart)[0]
   features = sketch_part.getFeatures(type=inspire.FeatureLinear)

   # Creating a circular pipe.
   inspire.core.geometry.createPipe(features, section="CIRCLE",
                                    resultType="NEW_PART", thickness=1, size=5)

   print("Circular Pipe has been created for given feature path")
   inspire.orientView(direction="isometric")


moveFaces
=========

.. autofunction:: hwx.inspire.core.geometry.moveFaces

**Example**

.. code-block::

   from hwx import inspire

   # Creating a solid block with a hole in it.
   model = inspire.newModel()
   box = model.createSolidBlock()
   cyl = model.createSolidCylinder(radius=0.03)
   part = box.booleanSubtract(cyl)
   part.location = (0, 0, 0)
   feature = model.getFeatures(type="FeatureCylindrical")[0]
   location1 = inspire.math.Matrix44(origin=[0.31, 0.30, 1])

   # Moving hole to other location
   inspire.geometry.moveFaces(feature, location1)

   print("Hole is moved from origin to location1 in solid box")
   inspire.orientView(direction="isometric")


intersect
=========

.. autofunction:: hwx.inspire.core.geometry.intersect

**Example**

.. code-block::

   from hwx import inspire

   # Creating a model to show intersect tool.
   model = inspire.newModel()
   part1 = model.createSheetPolygon(radius=3)
   part2 = model.createSheetRectangle(x=4, y=2)
   part3 = model.createSolidCylinder()

   # Intersecting all part from model
   inspire.geometry.intersect([part1, part2, part3], createSolids=True)

   print("All parts in a model are intersected and a new part is created")
   inspire.orientView(direction="isometric")


convertToMass
=============

.. autofunction:: hwx.inspire.core.geometry.convertToMass

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   cyl = model.createSolidCylinder()
   sph = model.createSolidSphere()

   # Replace part with ConcentratedMass
   cm1 = box.convertToMass()

   # Replace multiple parts with ConcentratedMass
   cm2 = inspire.geometry.convertToMass([cyl, sph])

   print("Parts have been replaced with concentrated masses : ", cm1, cm2)
   inspire.orientView(direction="isometric")


replaceFromFile
===============

.. autofunction:: hwx.inspire.core.geometry.replaceFromFile

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   filePath = str(inspire.demo.getDemoFilePath('M01_FourBar.x_b'))
   part = inspire.geometry.replaceFromFile(box, filePath)

   print("Box is replaced with the file: M01_FourBar.x_b")
   inspire.orientView(direction="isometric")


replaceFromPart
===============

.. autofunction:: hwx.inspire.core.geometry.replaceFromPart

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock(x=2, y=2, z=0.5)
   cyl = model.createSolidCylinder()
   inspire.geometry.replaceFromPart(box, cyl)

   print("Box is replaced with Cylinder")
   inspire.orientView(direction="isometric")


circularPattern
===============

.. autofunction:: hwx.inspire.core.geometry.circularPattern

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   feature = model.getFeatures(type="FeatureLinear")[0]

   # Creating a circular pattern of box.
   box.circularPattern(axis=feature, angle=60, count=6, symmetry=True)

   print("Circular pattern has been created for Box")
   inspire.orientView(direction="isometric")


draft
=====

.. autofunction:: hwx.inspire.core.geometry.draft

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   model.createSolidBlock(x=0.01, y=0.01, z=0.08)
   feature = model.getFeatures(type="FeaturePlanar")[1]
   neutralPlane = model.getFeatures(type="FeaturePlanar")[0]

   # Creating a draft in Single direction with 20-degree angle.
   feature.draft("SINGLE", neutralPlane, angle1=20)

   print("Draft has been created in single direction with 20 degree angle")
   inspire.orientView(direction="isometric")


convertBodiesToParts
====================

.. autofunction:: hwx.inspire.core.geometry.convertBodiesToParts

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   model.createSolidBlock()
   features = model.getFeatures(type="FeaturePlanar")
   m1 = inspire.math.Matrix44(origin=[3, 0, 0])
   inspire.geometry.moveFaces(features, m1, duplicate=True)
   parts = inspire.geometry.convertBodiesToParts(model.parts[0])

   print(" Converted Parts: ", parts)
   inspire.orientView(direction="isometric")


breakInstance
=============

.. autofunction:: hwx.inspire.core.geometry.breakInstance

**Example**

.. code-block::

   from hwx import inspire
   from hwx.inspire.demo import openDemoFile

   model = openDemoFile("BreakInstance.stmod")
   inspire.geometry.breakInstance([model.parts[0], model.parts[1]])

   print("Break Instance has been applied to both parts.")
   inspire.orientView(direction="isometric")


trimAndSplit
============

.. autofunction:: hwx.inspire.core.geometry.trimAndSplit

**Example**

.. code-block::

   from hwx import inspire

   # Creating a model to show project and split tool.
   model = inspire.newModel()
   part = model.createSolidBlock(x=2, y=1, z=1, location=(0, 0, 0))
   box = model.createSolidBlock(location=(-1, 0.5, 0))
   feature = box.features[21]
   part.slice(surfaceFeature=feature, extendSurface=False)
   part.slice(surfaceFeature=feature, extendSurface=True)
   tool = model.getFeatures(type="FeatureLinear")[31]
   target = model.parts[1]

   inspire.core.geometry.trimAndSplit(target, tool, "Y", trim=False)
   print("A linear feature has been projected on part and also divided it "
         "into two parts")
   inspire.orientView(direction="isometric")


revolve2
========

.. autofunction:: hwx.inspire.core.geometry.revolve2

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   rectangle = model.createSheetRectangle()
   feat = rectangle.getFeatures(inspire.FeaturePlanar)[0]
   feat2 = rectangle.getFeatures(inspire.FeatureLinear)[2]
   inspire.geometry.revolve2(feat, feat2, "SINGLE", "NEW_PART", angle1=200)

   print("Rectangular sheet has been revolved on linear axis for 200 degree")
   inspire.fitView()


edgeFillet
==========

.. autofunction:: hwx.inspire.core.geometry.edgeFillet

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   edge = box.getFeatures(type='FeatureLinear')[0]
   edge.edgeFillet(radius='60mm')
   print('Fillet is created on a edge with radius "60mm"')
   inspire.orientView(direction="isometric")


sweep
=====

.. autofunction:: hwx.inspire.core.geometry.sweep

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   sketch1 = inspire.Sketch()
   sketch1.addRegularPolygon((0, 0), (1, 0), 7)
   sketch2 = inspire.Sketch("Global Y")
   sketch2.addLineSegment((0, -2), (0, 5))
   sketch2.realize()
   sketch1.realize()
   sks = model.sketches
   path = sks[0].getFeatures(inspire.core.FeatureCurve)
   profile = sks[1].getFeatures(inspire.core.FeatureArea)
   inspire.geometry.sweep(profile, path, pathDirection="BOTH", twistType="NO_OF_TURNS",
                  twistTurns=1, twistTurnsDir2=2, resultType="NEW_PART")

   print("Sweep has been created in both direction of profile.")
   inspire.orientView(direction="isometric")


nurbsCurve
==========

.. autofunction:: hwx.inspire.core.geometry.nurbsCurve

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   model.createSolidBlock()
   point1 = model.getFeatures(type="FeaturePoint")[0]
   point2 = model.getFeatures(type="FeaturePoint")[1]
   point3 = model.getFeatures(type="FeaturePoint")[3]
   inspire.geometry.nurbsCurve([point1, point2, point3])

   print("NURBS Curve has been created with given control points.")
   inspire.orientView(direction="isometric")


patternAlongPath
================

.. autofunction:: hwx.inspire.core.geometry.patternAlongPath

**Example**

.. code-block::

   from hwx import inspire

   model = inspire.newModel()
   box = model.createSolidBlock()
   path = box.getFeatures(type=inspire.FeatureCurve)[0]

   # Creating a box pattern along the path.
   box.patternAlongPath(path=path, count=3, spacing=1)

   print("Pattern along the path has been created for Box")
   inspire.orientView(direction="isometric")


multiSweep
==========

.. autofunction:: hwx.inspire.core.geometry.multiSweep

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   model.createSolidBlock(z=2)
   feature = model.getFeatures(type=inspire.FeaturePlanar)[0]
   inspire.geometry.Plane(feature, "OFFSET", offset=0.05)
   systems = model.getAllChildren(type=inspire.geometry.Plane)[-1]
   sketch1 = inspire.Sketch()
   sketch3 = inspire.Sketch(systems)
   sketch1.addRegularPolygon((0, 0), (1, 0), 7)
   sketch3.addRegularPolygon((0, 0), (1, 1), 7)
   sketch2 = inspire.Sketch("Global Y")
   sketch2.addLineSegment((0, -3), (0, 1))
   sketch2.realize()
   sketch1.realize()
   sketch3.realize()
   sks = model.sketches
   path = sks[0].getFeatures(inspire.core.FeatureCurve)
   profile1 = sks[1].getFeatures(inspire.core.FeatureArea)[0]
   profile2 = sks[2].getFeatures(inspire.core.FeatureArea)[0]
   systems.destroy()
   model.parts[0].destroy()
   inspire.geometry.multiSweep([profile1, profile2], path, resultType="NEW_PART")

   print("Multi Sweep has been created with profile1 and profile2.")
   inspire.orientView(direction="isometric")


loft
====

.. autofunction:: hwx.inspire.core.geometry.loft

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   model.createSolidBlock(z=2)
   feature = model.getFeatures(type=inspire.FeaturePlanar)[0]
   inspire.geometry.Plane(feature, "OFFSET", offset=0.05)
   systems = model.getAllChildren(type=inspire.geometry.Plane)[-1]
   sketch1 = inspire.Sketch()
   sketch3 = inspire.Sketch(systems)
   sketch1.addRegularPolygon((0, 0), (1, 0), 7)
   sketch3.addRegularPolygon((0, 0), (1, 1), 7)
   sketch2 = inspire.Sketch("Global Y")
   sketch2.addLineSegment((0, -3), (0, 1))
   sketch2.realize()
   sketch1.realize()
   sketch3.realize()
   sks = model.sketches
   path = sks[0].getFeatures(inspire.core.FeatureCurve)
   profile1 = sks[1].getFeatures(inspire.core.FeatureArea)[0]
   profile2 = sks[2].getFeatures(inspire.core.FeatureArea)[0]
   systems.destroy()
   model.parts[0].destroy()
   inspire.geometry.loft([profile1, profile2], resultType="NEW_PART")

   print("Loft has been created with profile1 and profile2.")
   inspire.orientView(direction="isometric")


helixCurve
==========

.. autofunction:: hwx.inspire.core.geometry.helixCurve

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   sketch1 = inspire.Sketch()
   sketch1.addCircleCenterRadius((0, 0), 7)
   sketch1.realize()
   sks = model.sketches
   profile = sks[0].getFeatures(inspire.core.FeatureCircular)[0]
   inspire.geometry.helixCurve(profile, startAngle=30)
   inspire.fitView()

   print("Helix Curve has been created with profile.")
   inspire.orientView(direction="isometric")


divideCurve
===========

.. autofunction:: hwx.inspire.core.geometry.divideCurve

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   sketch1 = inspire.Sketch()
   sketch1.addCircleCenterRadius((0, 0), 7)
   sketch1.realize()
   sks = model.sketches
   profile = sks[0].getFeatures(inspire.core.FeatureCircular)[0]
   curve = inspire.geometry.helixCurve(profile, startAngle=10, numTurns=10)
   inspire.geometry.divideCurve(curve.features[-1], [[0.2, 0.6]])
   inspire.fitView()

   print("Curve has been divided in to 3 parts.")
   inspire.orientView(direction="isometric")


extendCurve
===========

.. autofunction:: hwx.inspire.core.geometry.extendCurve

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   sketch1 = inspire.Sketch()
   sketch1.addLineSegment((0, 0), (0, 1))
   sketch1.realize()
   sks = model.sketches
   curve = sks[0].getFeatures(inspire.core.FeatureLinear)[0]
   inspire.geometry.extract(curve)
   curve = model.parts[0].getFeatures(inspire.core.FeatureLinear)[0]
   inspire.geometry.extendCurve(curve, ["EXTENSION_DISTANCE", 1],
                                 extendAsNewPart=True)
   inspire.fitView()

   print("Part 1 has been extended to Part 2.")
   inspire.orientView(direction="isometric")


blendCurve
==========

.. autofunction:: hwx.inspire.core.geometry.blendCurve

**Example**

.. code-block::

   from hwx import inspire
   from hwx.common import math
   inspire.newModel()
   points = [[math.Point(1, 1, 0)], [math.Point(1, 2, 0)]]
   inspire.geometry.blendCurve(points)
   inspire.fitView()

   print("Blend curve has been created between two given points.")
   inspire.orientView(direction="isometric")


faceCurve
=========

.. autofunction:: hwx.inspire.core.geometry.faceCurve

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   model.createSolidBlock()
   face = model.getFeatures(type=inspire.FeaturePlanar)[0]
   vertex = model.getFeatures(type=inspire.FeaturePoint)[0]
   inspire.geometry.faceCurve(face, vertexFeature=vertex)
   inspire.fitView()

   print("Face curves has been extracted from the face of solid block as Part 1"
         " and Part 2.")
   inspire.orientView(direction="isometric")


offsetCurves
============

.. autofunction:: hwx.inspire.core.geometry.offsetCurves

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   sketch1 = inspire.Sketch()
   sketch1.addLineSegment((0, 0), (0, 0.5))
   sketch1.realize()
   sks = model.sketches
   curve = sks[0].getFeatures(inspire.core.FeatureLinear)[0]
   inspire.geometry.extract(curve)
   curve = model.parts[0].getFeatures(inspire.core.FeatureLinear)[0]
   inspire.geometry.offsetCurves(curve, 0.02,  extensionType="LINEAR",
                                 endOptions='CLOSED_AND_ROUNDED',
                                 symmetry=True)
   inspire.fitView()

   print("Offset Curves has been created for given line.")
   inspire.orientView(direction="isometric")


extendSurface
=============

.. autofunction:: hwx.inspire.core.geometry.extendSurface

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   rectangleSheet = model.createSheetRectangle()
   inspire.geometry.extendSurface(
   rectangleSheet.getFeatures(inspire.core.FeatureLinear), distance=0.3,
   createNewPart=True)
   inspire.fitView()

   print("Extend Surface has been created as a new part around the rectangular"
         "sheet.")
   inspire.orientView(direction="isometric")



intersectCurve
==============

.. autofunction:: hwx.inspire.core.geometry.intersectCurve

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   sketch1 = inspire.Sketch()
   sketch2 = inspire.Sketch()
   sketch1.addLineSegment((0, -1), (0, 1))
   sketch2.addLineSegment((-1, 0), (1, 0))
   sketch1.realize()
   sketch2.realize()
   sks = model.sketches
   inspire.geometry.extract(sks[0].getFeatures(inspire.core.FeatureLinear)[0])
   inspire.geometry.extract(sks[1].getFeatures(inspire.core.FeatureLinear)[0])
   part1 = model.parts[0]
   part2 = model.parts[1]
   inspire.geometry.intersectCurve(part1, part2)
   inspire.fitView()

   print("Curves are intersected using intersectCurve tool and a new curve "
         "as a part has been created.")
   inspire.orientView(direction="isometric")


rib
===

.. autofunction:: hwx.inspire.core.geometry.rib

**Example**

.. code-block::

   from hwx import inspire
   model = inspire.newModel()
   box = model.createSolidBlock()
   featPlane = box.getFeatures(type="FeaturePlanar")[0]
   featPlane.shell(thickness=0.01)
   sketch1 = inspire.Sketch("Global Y")
   sketch1.addLineSegment((0.2, -0.5), (0, -0.5))
   sketch1.realize()
   sks = model.sketches
   profile = sks[0]
   inspire.geometry.rib(profile, box, draftAngle=30)
   inspire.fitView()

   print("Rib has been created in the shell.")
   inspire.orientView(direction="isometric")



.. toctree::
	:maxdepth: 2

	Reference_/Reference_.rst