Stopping iLogic to add additional sketches and features
Accepted solution
Hi @sam ,
There are likely several ways you can do this.... sometimes I just check for the feature and delete it first if it exists, and that way the code can run without issue... in this example the code looks for a feature named "cutout" and deletes it if found, and then after it's created it names it "cutout" so that it can be found by the rule next time:
' Create a new part document, using the default part template.
Dim oDoc As PartDocument
oDoc = ThisApplication.ActiveDocument
' a reference to the component definition.
Dim oCompDef As PartComponentDefinition
oCompDef = oDoc.ComponentDefinition
' a reference to the transient geometry object.
Dim oTransGeom As TransientGeometry
oTransGeom = ThisApplication.TransientGeometry
Try
oCompDef.Features.ExtrudeFeatures.Item("Cutout").Delete
Catch
End Try
Dim oExtrude As ExtrudeFeature
oExtrude = oCompDef.Features.ExtrudeFeatures.Item(1)
' Get the top face of the extrusion to use for creating the new sketch.
Dim oFrontFace As Face
oFrontFace = oExtrude.StartFaces.Item(1)
' Create a new sketch on this face, but use the method that allows you to
' control the orientation and orgin of the new sketch.
oSketch = oCompDef.Sketches.AddWithOrientation(oFrontFace, _
oCompDef.WorkAxes.Item(1), True, True, oCompDef.WorkPoints(1))
' Determine where in sketch space the point (0.5,0.5,0) is.
Dim oCorner As Point2d
oCorner = oSketch.ModelToSketchSpace(oTransGeom.CreatePoint(0.5, 0.5, 0))
' Create the interior 3cm x 2cm rectangle for the pocket.
oRectangleLines = oSketch.SketchLines.AddAsTwoPointRectangle( _
oCorner, oTransGeom.CreatePoint2d(oCorner.X + 3, oCorner.Y + 2))
' Create a profile.
oProfile = oSketch.Profiles.AddForSolid
' Create a pocket .25 cm deep.
oExtrudeDef = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kCutOperation)
Call oExtrudeDef.SetDistanceExtent(0.25, kNegativeExtentDirection)
oExtrude = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)
oExtrude.Name = "Cutout"
or you can look for the feature or sketch by name and exit the rule if it is found, again you'll want to have the code name the thing being looked for a predictable name as it is created so it can find it next time, in this example it's looking for a sketch called "Cutout_sketch" and if found the rule won't continue running.
' Create a new part document, using the default part template.
Dim oDoc As PartDocument
oDoc = ThisApplication.ActiveDocument
' a reference to the component definition.
Dim oCompDef As PartComponentDefinition
oCompDef = oDoc.ComponentDefinition
' a reference to the transient geometry object.
Dim oTransGeom As TransientGeometry
oTransGeom = ThisApplication.TransientGeometry
Try
oTest = oCompDef.Sketches.Item("Cutout_Sketch")
'found sketch so exit rule
Return
Catch
End Try
Dim oExtrude As ExtrudeFeature
oExtrude = oCompDef.Features.ExtrudeFeatures.Item(1)
' Get the top face of the extrusion to use for creating the new sketch.
Dim oFrontFace As Face
oFrontFace = oExtrude.StartFaces.Item(1)
' Create a new sketch on this face, but use the method that allows you to
' control the orientation and orgin of the new sketch.
oSketch = oCompDef.Sketches.AddWithOrientation(oFrontFace, _
oCompDef.WorkAxes.Item(1), True, True, oCompDef.WorkPoints(1))
oSketch.Name = "Cutout_Sketch"
' Determine where in sketch space the point (0.5,0.5,0) is.
Dim oCorner As Point2d
oCorner = oSketch.ModelToSketchSpace(oTransGeom.CreatePoint(0.5, 0.5, 0))
' Create the interior 3cm x 2cm rectangle for the pocket.
oRectangleLines = oSketch.SketchLines.AddAsTwoPointRectangle( _
oCorner, oTransGeom.CreatePoint2d(oCorner.X + 3, oCorner.Y + 2))
' Create a profile.
oProfile = oSketch.Profiles.AddForSolid
' Create a pocket .25 cm deep.
oExtrudeDef = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kCutOperation)
Call oExtrudeDef.SetDistanceExtent(0.25, kNegativeExtentDirection)
oExtrude = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)
oExtrude.Name = "Cutout"
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Accepted solution
Hi @sam ,
You might have already figured it out, but just in case I just reordered some things in your code and then it worked well.
' Set a reference to the part component definition.
' This assumes that a part document is active.
Dim oCompDef As PartComponentDefinition
oCompDef = ThisApplication.ActiveDocument.ComponentDefinition
''Set a reference To the transient geometry Object.
Dim oTransGeom As TransientGeometry
oTransGeom = ThisApplication.TransientGeometry
'' Create face With the origin defined By
'' the center Point. (The first WorkPoint In the Collection Is the center
'' Point work Point.) In this Case, no Sketch Geometry will be created
'' since the final argument has been Left Out And it defaults To False.
oFace = oCompDef.SurfaceBodies.Item(1).Faces.Item(3)
oEdge = oFace.Edges.Item(1)
'check for existing sketch
Try
oTest = oCompDef.Sketches.Item("EndDetailsFeaureLeft")
'found sketch so exit rule
Return
Catch
End Try
'add sketch
oSketch = oCompDef.Sketches.AddWithOrientation _
(oFace, oEdge, True, True, oCompDef.WorkPoints.Item(1))
'Change the name.
oSketch.Name = "EndDetailsFeaureLeft"
Dim oXAxis2 As SketchEntity
oXAxis2 = oSketch.AddByProjectingEntity(oCompDef.WorkAxes.Item(3))
'the rest of the code here......
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
