Chamfer to all edge on selected body

[kresh.bell]

Hi,

is it possible create iLogic for add chamfer to all edge on selected body?

[Michael.Navara]

This is the easiest way. This code adds chamfer to all edges, but be careful because you can't run it twice on body or it fails when the chamfer on some edge can't be created.

Sub Main
	Dim part As PartDocument = ThisDoc.Document
	Dim body As SurfaceBody = part.ComponentDefinition.SurfaceBodies(1)
	Dim distance As Double = 0.05

	Dim edges As EdgeCollection = ThisApplication.TransientObjects.CreateEdgeCollection()
	For Each edge As Edge In body.Edges
		edges.Add(Edge)
	Next

	part.ComponentDefinition.Features.ChamferFeatures.AddUsingDistance(edges, distance)
End Sub

[kresh.bell]

Thanks,

I work with multibody part. Is it possible, when I run rule, that I need select body for chamfer and field for chamfer value?

[Michael.Navara]

Yes, you can use Pick Method for selecting body and InputBox for input distance value.

Sub Main
	Dim part As PartDocument = ThisDoc.Document
	Dim body As SurfaceBody = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartBodyFilter, "Select part") ' part.ComponentDefinition.SurfaceBodies(1)
	Dim distance As Double =  Double.Parse(InputBox("Chamfer distance", "iLogic", 0.05)) ' 0.05

	Dim edges As EdgeCollection = ThisApplication.TransientObjects.CreateEdgeCollection()
	For Each edge As Edge In body.Edges
		edges.Add(Edge)
	Next

	part.ComponentDefinition.Features.ChamferFeatures.AddUsingDistance(edges, distance)
End Sub

[kresh.bell]

Perfect,

but I think that iLogic have minor bug. If I want chamfer 2, in field must be 0,2

[FINET_Laurent · Accepted solution]

Hi @kresh.bell,

Inventor internaly uses centimeters. If you create a double with a value of 1, it will read 1cm what ever the document unit is. If you want your distance to be 1mm, you'll need to convert it by dividing the input value by 10 :

Dim distance As Double =  (Double.Parse(InputBox("Chamfer distance", "iLogic", 0.05))) /10 ' 0.05

Kind regards,

FINET L.

[Michael.Navara]

This is because Inventor's internal units are [cm]. You need to convert input string to appropriate numeric value in required units. 

[kresh.bell]

Thanks, it works perfect

[kresh.bell]

Is it big problem add option multibody select?

[FINET_Laurent]

@kresh.bell,

I'm not sure to understand correctly your request ? What would be the workflow? 
To be able to select one or more solid bodies by click? 

Kind regards,

FINET L.

[kresh.bell]

yes

[FINET_Laurent · Accepted solution]

Hi @kresh.bell,

Note you can mark multiple replies as solutions for your topic. Here is a code that let you pick multiples surfacebodies. When you are done selecting, simply press "esc" to create the chamfers : 

Sub Main
	Dim doc As Inventor.PartDocument = ThisApplication.ActiveDocument
	Dim partdef As Inventor.PartComponentDefinition = doc.ComponentDefinition
	Dim bodyCol As Inventor.ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection
	
	For i As Integer = 1 To partdef.SurfaceBodies.Count
		Dim body As SurfaceBody = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartBodyFilter, "Select part")
		If body Is Nothing Then Exit For
		If check(body, bodyCol) = False Then  bodyCol.Add(body)
		
	Next

	Dim distance As Double = (Double.Parse(InputBox("Chamfer distance", "iLogic", 0.05))) / 10 ' 0.05
	Dim edges As EdgeCollection = ThisApplication.TransientObjects.CreateEdgeCollection()
	
	For Each body As Inventor.SurfaceBody In bodyCol
		For Each edge As Edge In body.Edges
			edges.Add(Edge)
			
		Next
	Next
	
	partdef.Features.ChamferFeatures.AddUsingDistance(Edges, distance)
End Sub

Private Function check(input As Object, col As Inventor.ObjectCollection)
	If col.Count = 0 Then Return False
		
	For Each obj As Object In col
		If obj is input Then Return True
		
	Next
	
	Return False
End Function

Does this suits your needs ?

Kind regards,

FINET L.

[kresh.bell]

Perfect, thanks

[kresh.bell]

iLogic works perfect. Is it possible, when I select bodies, that selected bodies be highlights