Adding A Dimension from a point or Sketch entity to an edge of a face

[cencinaNB2ET]

I have gone through the API help page on Inventor 2018 and i cant find any examples there nor in the forum.

Basically You select a face, you place a point and you can make that point a hole, that is fine.

But that centre-point is not constrained with dimensions towards the edges of that particular face.

how can I just add a dimension by code, either by ilogic or VBA?

The API help page talks about geometric constraints but a not adding a dimension.

You can see the point is unconstrained ( green)

I want to add to dimensions towards the referenced edges of that face.

pretty simple right?

Please see that attached part with Rule 1 in ilogic.

[YuhanZhang · Accepted solution]

Below is a VBA sample for your specific data to create the dimensions for the hole center, open the data, and run below code to see the result:

Sub CreateOffsetDimConstraintSample()
    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument
    
    Dim oSk As PlanarSketch
    Set oSk = oDoc.ComponentDefinition.Sketches("My New Sketch")
    
    Dim oFace As Face
    Set oFace = oDoc.ComponentDefinition.Features.ExtrudeFeatures(1).SideFaces(1)
    
    Dim oHoleCenter As SketchPoint
    Set oHoleCenter = oSk.SketchPoints(1)
    oDoc.SelectSet.Select oHoleCenter
    
    oSk.Edit
    oSk.AddByProjectingEntity oFace.Edges(2)
    oSk.AddByProjectingEntity oFace.Edges(5)
    
    Call oSk.DimensionConstraints.AddOffset(oSk.SketchLines(1), oHoleCenter, ThisApplication.TransientGeometry.CreatePoint2d(2, 2), False)
    Call oSk.DimensionConstraints.AddOffset(oSk.SketchLines(2), oHoleCenter, ThisApplication.TransientGeometry.CreatePoint2d(-2, 0), False)
    
    oSk.ExitEdit
End Sub

Please let me if it works for you.

[cencinaNB2ET]

That is great!

Thank you.

Now I need to identify the consumed by parameter ( This new sketch name ) in order to change the access the dimension since i dont know that dimension name being added.

So i can access this dimension and give it some value as soon as its created.

Thanks again.