Create Project Geometry, Offset and Extrude using ilogic

[murugasubi]

Hi Dear,

I have a part, I want to create project geometry on edges and offset the edges to 1 inch and extrude the sketch. Please refer to the attached image A and B. I want to create image B.

I used the below codes, but could not complete the code. Please help.

Sub Main
    Dim oPartDoc As PartDocument
    oPartDoc = ThisApplication.ActiveDocument
                    
    Dim oCompDef As PartComponentDefinition
    oCompDef = oPartDoc.ComponentDefinition
    
     Dim oSketches As PlanarSketches = ThisApplication.ActiveEditDocument.ComponentDefinition.Sketches
	
     Dim oSketch1 As PlanarSketch
    oSketch1 = oSketches("Sketch1") 'I have used the existing sketch to extrude

    Dim oProfile As Profile
    oProfile = oSketch1.Profiles.AddForSolid
    
    ' Create a base extrusion 1 inch thick.
    Dim oExtrudeDef As ExtrudeDefinition
    oExtrudeDef = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kJoinOperation)
    Call oExtrudeDef.SetDistanceExtent(1, kNegativeExtentDirection)
    Dim oExtrude As ExtrudeFeature
    oExtrude = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)
	
	Dim oFrontFace As Face
    oFrontFace = oExtrude.StartFaces.Item(1)
	
'Code not working from here
	Dim oSketch2 As PlanarSketch
    oSketch2 = oCompDef.Sketches.Add(oFrontFace)
		
	Dim featEdge As Edge
	 For Each featEdge In oFrontFace.Edges
		 Call oSketch2.AddByProjectingEntity(featEdge)
	 Next 
end sub

[Michael.Navara · Accepted solution]

Your code works as expected.

I just recommend you to modify this line of code to the following form. Avoid to use active document multiple times, because it may be changed.

...
Dim oSketches As PlanarSketches = oCompDef.Sketches
...

and then you can use this for rest of your task. Here is used simpler version for projecting all face edges.

...

'Code not working from here
Dim oSketch2 As PlanarSketch

If False Then
    oSketch2 = oCompDef.Sketches.Add(oFrontFace)

    Dim featEdge As Edge
    For Each featEdge In oFrontFace.Edges
        Call oSketch2.AddByProjectingEntity(featEdge)
    Next
Else
    'Simpler version
    oSketch2 = oCompDef.Sketches.Add(oFrontFace, True)
End If

Dim entitiesForOffset As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection()
entitiesForOffset.Add(oSketch2.SketchLines(1))

Dim offsetDistance As Double = 1
Dim offsetDirection As Boolean = True
Dim offsetedEntities = oSketch2.OffsetSketchEntitiesUsingDistance(entitiesForOffset, offsetDistance, offsetDirection, True, True)

Dim profile2 = oSketch2.Profiles.AddForSolid(True)
Dim oExtrudeDef2 = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(profile2, PartFeatureOperationEnum.kJoinOperation)
Dim oExtrude2 = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef2)

[murugasubi]

Thanks a lot Michael. Navara

Code working well.. I really appreciate your help and respect your opinion..