Contour Flange offset direction

[breinkemeyer]

Is there a method or property in the contour flange feature or definition that controls the offset side of the flange?  I see it when I manually edit the flange, but don't see it in the API.

[blandb]

May want to try this in the iLogic forum, may get better results there?

[blandb]

scratch that wrong post, my apologies lol

[JelteDeJong · Accepted solution]

I think you are looking for the "ExtentDirection" property. As an example run the following iLogic rule. Select the Contour Flange feature. And check that it's changing.

Dim f As ContourFlangeFeature = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFeatureFilter, "")

If (f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kNegativeExtentDirection) Then
    f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kPositiveExtentDirection
Else
    f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kNegativeExtentDirection
End If 

[breinkemeyer]

That did the trick, thanks!

[Curtis_Waguespack · Accepted solution]

@kacper.suchomski , see example for this without the Pick selection. 

hope that helps, Curtis

Dim oDoc As PartDocument = ThisDoc.Document
Dim f As ContourFlangeFeature 

f = oDoc.ComponentDefinition.Features.Item("Contour Flange1")

If (f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kNegativeExtentDirection) Then
    f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kPositiveExtentDirection
Else
    f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kNegativeExtentDirection
End If 

[kacper.suchomski]

Wow! Thanks!

I slightly modified the code because I wanted it to be dependent on the text parameter - Size - "Outer" / "Inner" / "Middle"

Dim oDoc As PartDocument = ThisDoc.Document
Dim f As ContourFlangeFeature

f = oDoc.ComponentDefinition.Features.Item("Contour Flange1")

If Size = "Out" Then
	f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kPositiveExtentDirection
Else If Size = "Inn" Then
	f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kNegativeExtentDirection
Else
	f.Definition.ExtentDirection = PartFeatureExtentDirectionEnum.kSymmetricExtentDirection

End If 

This is to define how the handle size will be oriented in relation to the dimensions.