Toggle Hole Types with iLogic

[STVand]

Hello, I am trying to write a snippet of code to do something which I thought would be simple: toggle a hole feature to be either drilled or countersunk based on user input.  However, I am getting a very vague "The parameter is incorrect." error when I try to execute this iLogic rule.  I'm guessing that I am not using the SetCSink method correctly but I have no idea how to fix the problem.  I have checked and all of the variables I am using are already initialized to positive values. Code is posted below, any help would be greatly appreciated!

Dim odoc As PartDocument
odoc = ThisApplication.ActiveDocument

Dim oHole As HoleFeature
oHole = odoc.ComponentDefinition.Features.HoleFeatures.Item(1)

Select Case ANCHOR_HOLE_SIZE
    Case = .25
    CSinkDia = .53125
    Case = .3125
    CSinkDia = .65625
    Case = .375
    CSinkDia = .78125
    Case = .4375
    CSinkDia = .84375
    Case = .5
    CSinkDia = .9375
    Case = .625
    CSinkDia = 1.1875
    Case = .75
    CSinkDia = 1.4375
End Select

If HOLE_TYPE = "THRU"
oHole.SetDrilled()
ElseIf HOLE_TYPE = "COUNTERSUNK"
oHole.SetCSink(CSinkDia, CSinkAng)
End If

[Curtis_Waguespack · Accepted solution]

Hi STVand,

I'm not seeing the error when I (quickly) pasted in your code and ran it, but here is a quick iLogic example that I had on hand that sets a hole feature named Hole1 to a countersink or counterbore based on user input.

After posting and re-reading  your question, I realize that I've not addressed the right issue. But I'll try to have a look again tomorrow if I can.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

oInput = InputRadioBox _
("Select one:", "Make Countersink.", "Make Counterbore", True, “iLogic")

Dim oHole As HoleFeature
oHole = ThisDoc.Document.ComponentDefinition.Features.Item("Hole1")

If oInput = True Then
oHole.SetCSink(1 mm, 82*(PI/180)) '82 degrees
Else
oHole.SetCBore(2 mm, 1 mm) 
End If

[STVand]

Curtis, thanks for the reply.  I tried making a new part from scratch with just an extrusion and a hole feature named "Hole1" and running your iLogic rule, and I am still getting the same vague "The Parameter is Incorrect" error on running it, regardless of whether I choose countersunk or counterbored.  I have read the help docs on the API and the syntax should be correct for the SetCSink/SetCBore methods, so now I am absolutely puzzled. 

[STVand]

Solved it! After fooling around a bit with your code, I changed your "mm" to "in" (the native units of the part document) and it worked.

I thought i remember reading that if the object passed into the SetCSink() method didn't have units it would default to the native units, but it seems that isn't true.  The correct syntax for it is SetCSink( ### in, ###).  Without having in (or mm, or whatever unit) it errors out.  Thanks for the help!