I understand that work axes at assembly level are either fixed (in space) or constrained.
I know how to constrain parts to each other in an assembly, but how do I programmatically create and constrain a work axis in an assembly to, for example a hole in a part? I can do it manually, so there must be a sequence of API calls to do it!
TIA
Here is an example iLogic rule that will create a work axis within an assembly that coincides with the center axis of a hole in a part within. My test assembly had two parts in it. Both parts had holes in them, but the target part only had one hole in it, that was made using a hole feature, instead of just an extruded cut feature. So, if I want to specify that cylindrical face of that hole in the part without manually selecting it, I must navigate to that cylindrical face within the part. Once I've got that face, I create a FaceProxy object from it, which brings its geometry over into the context of the assembly's 3D space, instead of that parts 3D space. Then I extract the Cylinder geometry from that cylindrical face, and extract the needed Point and UnitVector objects/data needed from that. Then I use the WorkAxes.AddFixed() method, supply those last two objects to it, and there you go.
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
MsgBox("An Assembly Document must be active for this rule to work. Exiting.",vbOKOnly+vbCritical, "WRONG DOCUMENT TYPE")
Exit Sub
End If
Dim oADoc As AssemblyDocument = ThisApplication.ActiveDocument
Dim oADef As AssemblyComponentDefinition = oADoc.ComponentDefinition
Dim oComp As ComponentOccurrence = oADef.Occurrences.ItemByName("TestPart1:1")
Dim oPDoc As PartDocument = oComp.Definition.Document
Dim oPDef As PartComponentDefinition = oPDoc.ComponentDefinition
Dim oHole As HoleFeature = oPDef.Features.HoleFeatures.Item(1)
'oHole.HoleCenterPoints 'could likely use these too
Dim oCylFace As Face = oHole.SideFaces.Item(1)
If oCylFace.SurfaceType = SurfaceTypeEnum.kCylinderSurface Then
Dim oCylFaceProxy As FaceProxy
oComp.CreateGeometryProxy(oCylFace, oCylFaceProxy)
oCyl = oCylFaceProxy.Geometry
Dim oPoint As Inventor.Point = oCyl.BasePoint
Dim oAxis As UnitVector = oCyl.AxisVector
oADef.WorkAxes.AddFixed(oPoint, oAxis, False)
Else
MsgBox("Hole's first side face was not a Cylinder. Exiting.", , "")
Exit Sub
End If
You could likely condense this code a bit more if you wanted, but the process of how to do what you wanted should be fairly easy for you to follow. The key in this process is creating the FaceProxy, as you may have guessed.
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Wesley Crihfield
(Not an Autodesk Employee)
I guess I wasn't sure about that part of the request. OK, that's doable too.
I have updated that code to constrain the axis to the parts hole, after it is created.
I just added a variable name in front of the line that creates the work axis, then I use that variable within the line to constrain it. Then the line to constrain it (it's a long line of code, so you could wrap it to another line if needed).
Try this:
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
MsgBox("An Assembly Document must be active for this rule to work. Exiting.",vbOKOnly+vbCritical, "WRONG DOCUMENT TYPE")
Exit Sub
End If
Dim oADoc As AssemblyDocument = ThisApplication.ActiveDocument
Dim oADef As AssemblyComponentDefinition = oADoc.ComponentDefinition
Dim oComp As ComponentOccurrence = oADef.Occurrences.ItemByName("TestPart1:1")
Dim oPDoc As PartDocument = oComp.Definition.Document
Dim oPDef As PartComponentDefinition = oPDoc.ComponentDefinition
Dim oHole As HoleFeature = oPDef.Features.HoleFeatures.Item(1)
'oHole.HoleCenterPoints 'could likely use these too
Dim oCylFace As Face = oHole.SideFaces.Item(1)
If oCylFace.SurfaceType = SurfaceTypeEnum.kCylinderSurface Then
Dim oCylFaceProxy As FaceProxy
oComp.CreateGeometryProxy(oCylFace, oCylFaceProxy)
oCyl = oCylFaceProxy.Geometry
Dim oPoint As Inventor.Point = oCyl.BasePoint
Dim oAxis As UnitVector = oCyl.AxisVector
oWAxis = oADef.WorkAxes.AddFixed(oPoint, oAxis, False)
Dim oMConst1 As MateConstraint = oADef.Constraints.AddMateConstraint2(oWAxis, oCylFaceProxy,0,InferredTypeEnum.kInferredLine,InferredTypeEnum.kInferredLine, MateConstraintSolutionTypeEnum.kAlignedSolutionType)
Else
MsgBox("Hole's first side face was not a Cylinder. Exiting.", , "")
Exit Sub
End If
If this solved your problem, or answered your question, please click ACCEPT SOLUTION.
Or, if this helped you, please click (LIKE or KUDOS) 👍.
If you want and have time, I would appreciate your Vote(s) for My IDEAS 💡or you can Explore My CONTRIBUTIONS
Wesley Crihfield
(Not an Autodesk Employee)
Apparently I didn't declare the Type of the oCyl variable in my original code, but it was intended to be a 'Cylinder' object (Transient mathematical geometry), not a FaceProxy or Face. It is the underlying geometry object that makes up that specific FaceProxy object (because the face was cylindrical shaped in my example).
Wesley Crihfield
(Not an Autodesk Employee)
Also if oADef.Occurrences.Item(1) doesn't work for you, and you would rather supply the component's name (as you hinted at in your later posted code comment), then you could use this instead:
Dim oComp As ComponentOccurrence = oADef.Occurrences.ItemByName("Bent-Part-With-Hole:1")
I just used Item(1) in my example, because it was simple and generic, and just happened to be the right component in my test assembly.
Wesley Crihfield
(Not an Autodesk Employee)
