Ilogic-How to choose plane and point iFeature (code)

[Anonymous]

I want insert iFeature into Part. But i don't know code choose Plane and Point. Please help me!!!

[Michael.Navara]

Here is good example how to insert standard iFeature

https://help.autodesk.com/view/INVNTOR/2020/ENU/?guid=GUID-8E822596-71C5-4C93-B935-7A6F04C7DE10

[Anonymous]

Thank you.

But it isn't " Pick Point" . I dont know define Point Refence iFeature. Can help me!!!

[Michael.Navara · Accepted solution]

Full example is in attachment

'Active part
Dim partDoc As PartDocument = ThisDoc.Document
Dim partDef As PartComponentDefinition = partDoc.ComponentDefinition

'Placement sources
Dim oSketch As PlanarSketch = partDef.Sketches("iFeatureTargetSketch")
Dim oFace As Face = oSketch.PlanarEntity
Dim oPoint As SketchPoint = oSketch.SketchPoints(1)

'iFeature creation
Dim iFeatureFileName As String = System.IO.Path.GetDirectoryName(partDoc.FullFileName) & "\Test.ide"
Dim iFeatureDef As iFeatureDefinition = partDef.Features.iFeatures.CreateiFeatureDefinition(iFeatureFileName)

For Each iFeaInput As iFeatureInput In iFeatureDef.iFeatureInputs
	
	'Explanation. See iLogic log window
	Logger.Debug("Expected entities for " & iFeaInput.Name & ": " & vbCrLf  & iFeaInput.EntityType.ToString("F").Replace(", ", vbCrLf))
	
	Select Case iFeaInput.Name
	Case "Plane"
		Dim planeInput As iFeatureSketchPlaneInput = iFeaInput 
		planeInput.PlaneInput = oFace
	Case "Point"
		Dim pointInput As iFeatureEntityInput = iFeaInput 
		pointInput.Entity = oPoint
	End Select
	
Next

partDef.Features.iFeatures.Add(iFeatureDef)

[Anonymous]

Thanks . I tried my best. But it's buggy, I don't fix them. I am using Inventor 2019 so I can't open your file. I send you my file. Can you check it out for me? Rules = iFeature

code

Dim oPartDoc As PartDocument
oPartDoc = ThisApplication.ActiveDocument

Dim oPartDef As PartComponentDefinition
oPartDef = oPartDoc.ComponentDefinition

Dim oPlane As WorkPlane = oPartDef.WorkPlanes.Item("YZ Plane")
Dim oPoint As WorkPoint = oPartDef.WorkPoints.Item("Center Point")
Dim oFeatures As PartFeatures
oFeatures = oPartDef.Features

Dim oiFeatureDef As iFeatureDefinition
oiFeatureDef = oFeatures.iFeatures.CreateiFeatureDefinition("C:\Users\Public\Documents\Autodesk\Inventor 2019\Catalog\TAVO\LINK PIPE\DN125SCH40.ide")
Dim oInput As iFeatureInput

For Each oInput In oiFeatureDef.iFeatureInputs
Dim oParamInput As iFeatureParameterInput
Select Case oInput.Name
Case "Plane1"
Dim oPlaneInput As iFeatureSketchPlaneInput=oInput
oPlaneInput.PlaneInput = oPlane
Case "Point1"
Dim pointInput As iFeatureEntityInput = oInput
pointInput.Entity = oPoint
Case "Angle_position"
oParamInput = oInput
oParamInput.Expression = "90 deg"
Case "Lenght_pipe"
oParamInput = oInput
oParamInput.Expression = "200 mm"
Case "Position_hold"
oParamInput = oInput
oParamInput.Expression = "500 mm"
Case "R_tank"
oParamInput = oInput
oParamInput.Expression = diameter/2
Case "Thick"
oParamInput = oInput
oParamInput.Expression = Thickness
End Select
Next
Dim oiFeature As iFeature
oiFeature = oFeatures.iFeatures.Add(oiFeatureDef)

[Michael.Navara]

You need to set appropriate variable type.

Here is the change

...
Select Case oInput.Name
    Case "Plane1"
        'This iFeatureInput is iFeatureWorkPlaneInput (NOT iFeatureSketchPlaneInput)
        Logger.Debug(oInput.Type.ToString("F"))
        Dim oPlaneInput As iFeatureWorkPlaneInput = oInput
        oPlaneInput.PlaneInput = oPlane
...     

The second bug is in setting .Expression. This must be a string (NOT double) and unit specifier is recomended

...
Case "R_tank"
    oParamInput = oInput
    oParamInput.Expression = string.format("{0} mm", diameter/2 *10) ' diameter

Case "Thick"
    oParamInput = oInput
    oParamInput.Expression =  string.format("{0} mm", Thickness *10) 'Thickness
...

[Anonymous]

That is a wonderful thing for me. Thank you very much. I have a question, I don't know if that variable exists. how do I know the variable name. While writing code on Inventor it does not show variable options. For example, I know the face I selected is Plane but I don't know the variable named iFeatureWorkPlaneInput. Can you share your experiences and materials? Once again thank you very much.

[Michael.Navara]

Documentation for Inventor API is available locally in SDK or online 

https://help.autodesk.com/view/INVNTOR/2020/ENU/?guid=GUID-6FD7AA08-1E43-43FC-971B-5F20E56C8846

I use VBA tools (Locals and Watch windows) for better understanding of object structure. This tools are very handy.

For general information for VB.NET I use standard sources (MSDN, StackOverflow,...)

But experience is not shareable 😐