ilogic to convert circles to holes

[FProcp]

Does anyone know of an iLogic code that can convert circles to holes?

We receive plate models from others and the holes are drawn as circles and then extruded as through cuts.

I would like to be able to convert all circles in the plate (possibly under a certain diameter) to proper holes.

Has anyone done this before?

[FProcp]

Thank you so much. This works perfectly 

Please keep me informed on your feasibility study.

[chandra.shekar.g · Accepted solution]

Hi @FProcp,

Its working with Part document and posted the iLogic code as well.

Dim oDoc As PartDocument
oDoc = ThisDoc.Document
Dim oSK As PlanarSketch
oSK = oDoc.ComponentDefinition.Sketches(1)
Dim objCol As ObjectCollection
objCol = ThisApplication.TransientObjects.CreateObjectCollection

For Each oskarc In oSK.SketchArcs
    objCol.Add(oskarc)
Next
For Each oskline In oSK.SketchLines
    objCol.Add (oskline)
Next

Dim oRadiusList As ArrayList = New ArrayList 
Dim oCircle As SketchCircle
For Each oCircle In oSK.SketchCircles	
	If oRadiusList.Contains(Math.Round(oCircle.Radius, 3)) = False Then		
		oRadiusList.Add(Math.Round(oCircle.Radius, 3))
	End If	
Next

Dim oCircleCol(oRadiusList.Count) As ObjectCollection
For i = 0 To oRadiusList.Count 
    oCircleCol(i) = ThisApplication.TransientObjects.CreateObjectCollection
Next

For j = 0 To oRadiusList.Count - 1
	For Each oCircle In oSK.SketchCircles 
		If Math.Round(oCircle.Radius, 3).ToString = oRadiusList.Item(j).ToString Then
			oCircleCol(j).Add(oCircle)
		End If
	Next
Next 

Dim oP1 As Profile
oP1 = oSK.Profiles.AddForSolid(False, objCol)
oD1 = oDoc.ComponentDefinition.Features.ExtrudeFeatures.CreateExtrudeDefinition(oP1, kNewBodyOperation)
oD1.SetDistanceExtent("6 mm", kSymmetricExtentDirection)
oF2 = oDoc.ComponentDefinition.Features.ExtrudeFeatures.Add(oD1)


'Create hole feature for the rest center point of the circles
Dim oTempCol As ObjectCollection
oTempCol = ThisApplication.TransientObjects.CreateObjectCollection
Dim oPD As HolePlacementDefinition
For i = 0 To oRadiusList.Count - 1
    oTempCol.Clear
    Dim dDiameter As Double
    For Each oCircle In oCircleCol(i)
        oTempCol.Add (oCircle.CenterSketchPoint)
    Next
	
    dDiameter = oCircleCol(i).Item(1).Radius * 2
	dDiameter = Math.Round(dDiameter, 1)
    oPD = oDoc.ComponentDefinition.Features.HoleFeatures.CreateSketchPlacementDefinition(oTempCol)
    Dim oHole As HoleFeature
	oHole = oDoc.ComponentDefinition.Features.HoleFeatures.AddDrilledByThroughAllExtent(oPD, dDiameter, kSymmetricExtentDirection)		
	dDiameter = dDiameter * 10
	oHole.Name = "HoleD" + dDiameter.ToString
Next

Thanks and regards,

[GeorgK]

Hello Chandra,

thats a realy great tool. Is it possible to check for several diameter with the same origin and use only the inner diameter?

Thank you

Georg

[FProcp]

We sometimes have drawings with two holes located at the same place, one is larger than the other. These represent counterbored or countersunk holes.
It would be good if it could turn double holes into counterbored holes of any depth. I could then go back and edit them later.
There usually aren't many of those so it's a minor issue.

[GeorgK]

The counterbored holes could use the standard hole depth.

[Anonymous]

Can you try this for me Chandra? I can't seem to get this to work. It adds an extrusion instead of a hole? Simple piece of 10mm plate with two extruded circular features

Thanks for your time with this....

[chandra.shekar.g · Accepted solution]

Hi @Anonymous,

To work with below iLogic code for part document, only sketch is enough. The modified part is attached with this post.

Dim oDoc As PartDocument
oDoc = ThisDoc.Document
Dim oSK As PlanarSketch
oSK = oDoc.ComponentDefinition.Sketches(1)
Dim objCol As ObjectCollection
objCol = ThisApplication.TransientObjects.CreateObjectCollection

For Each oskarc In oSK.SketchArcs
    objCol.Add(oskarc)
Next
For Each oskline In oSK.SketchLines
    objCol.Add (oskline)
Next

Dim oRadiusList As ArrayList = New ArrayList 
Dim oCircle As SketchCircle
For Each oCircle In oSK.SketchCircles	
	If oRadiusList.Contains(Math.Round(oCircle.Radius, 3)) = False Then		
		oRadiusList.Add(Math.Round(oCircle.Radius, 3))
	End If	
Next

Dim oCircleCol(oRadiusList.Count) As ObjectCollection
For i = 0 To oRadiusList.Count 
    oCircleCol(i) = ThisApplication.TransientObjects.CreateObjectCollection
Next

For j = 0 To oRadiusList.Count - 1
	For Each oCircle In oSK.SketchCircles 
		If Math.Round(oCircle.Radius, 3).ToString = oRadiusList.Item(j).ToString Then
			oCircleCol(j).Add(oCircle)
		End If
	Next
Next 

Dim oP1 As Profile
oP1 = oSK.Profiles.AddForSolid(False, objCol)
oD1 = oDoc.ComponentDefinition.Features.ExtrudeFeatures.CreateExtrudeDefinition(oP1, kNewBodyOperation)
oD1.SetDistanceExtent("6 mm", kSymmetricExtentDirection)
oF2 = oDoc.ComponentDefinition.Features.ExtrudeFeatures.Add(oD1)


'Create hole feature for the rest center point of the circles
Dim oTempCol As ObjectCollection
oTempCol = ThisApplication.TransientObjects.CreateObjectCollection
Dim oPD As HolePlacementDefinition
For i = 0 To oRadiusList.Count - 1
    oTempCol.Clear
    Dim dDiameter As Double
    For Each oCircle In oCircleCol(i)
        oTempCol.Add (oCircle.CenterSketchPoint)
    Next
	
    dDiameter = oCircleCol(i).Item(1).Radius * 2
	dDiameter = Math.Round(dDiameter, 2)
    oPD = oDoc.ComponentDefinition.Features.HoleFeatures.CreateSketchPlacementDefinition(oTempCol)
    Dim oHole As HoleFeature
	oHole = oDoc.ComponentDefinition.Features.HoleFeatures.AddDrilledByThroughAllExtent(oPD, dDiameter, kSymmetricExtentDirection)		
	dDiameter = dDiameter * 10
	oHole.Name = "HoleD" + dDiameter.ToString
Next

Thanks and regards,

[Anonymous]

thanks Chandra

I am on v2017 so cant open. Is it a part with only one sketch or multiple sketches... ie one sketch for the plate , one sketch for a hole and another sketch for 2 holes?

or is it all in one sketch...or something else?

[chandra.shekar.g]

Hi @Anonymous,

Everything should be in one sketch.

Thanks and regards,

[GeorgK]

Hello @chandra.shekar.g,

is it possible to add the countersunk hole function?

Thank you very much

Georg

[chandra.shekar.g]

Hi @GeorgK,

To create Countersunk hole, Collecting a concentric circles from sketch looks challenging task.

Thanks and regards,

[FProcp]

Of course it's possible. It's just a matter of investing the time in working out a method.
I hope Chandra will take on this challenge.

[GeorgK]

to get the table 🙂 :

http://esss.de/LBP_Werkstatt-Computer/Tabellenbuch-Auszuege/Senkungen-Zylinderkopfschrauben.pdf

https://schraube-mutter.de/bohrtabelle-fuer-zylinderschrauben/

[smilinger]

CounterSink or CounterBore holes are also doable, just a little complicated:

Imports System.Linq
Imports Inventor

Dim doc As PartDocument = ThisDoc.Document
Dim comp As PartComponentDefinition = doc.ComponentDefinition

'Assuming the 2nd sketch is for holes
Dim sketch1 As PlanarSketch = doc.ComponentDefinition.Sketches(2)

'Group circles by position
Dim circleGroups = sketch1.SketchCircles.Cast(Of SketchCircle)().GroupBy(
	Function(c)
		Dim point = c.CenterSketchPoint.Geometry
		Return Round(point.X, 3) & ", " & Round(point.Y, 3)
	End Function
)

'Group single circles by diameter
Dim drilledCircleGroups = circleGroups.Where(Function(g) g.Count() = 1).Select(Function(g) g.Single()).GroupBy(Function(c) Round(c.Geometry.Radius * 2, 3))

'Group pairs of circles by diameters
Dim counterBoreCirclesGroups = circleGroups.Where(Function(g) g.Count() = 2).Select(
	Function(g)
		Dim o = g.OrderBy(Function(c) c.Radius)
		Return New With {.Center = g.First().CenterSketchPoint, .InnerDiameter = Round(o(0).Radius*2, 3), .OuterDiameter = Round(o(1).Radius*2, 3)}
	End Function
).GroupBy(Function(item) item.InnerDiameter*10 & "x" & item.OuterDiameter*10)

For Each circleGroup In drilledCircleGroups
	Dim points As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection()
	For Each Circle In circleGroup
		points.Add(Circle.CenterSketchPoint)
	Next
	Dim placementDef As HolePlacementDefinition = comp.Features.HoleFeatures.CreateSketchPlacementDefinition(points)
	
	'Create drilled holes according to different diameters
	If circleGroup.Key = 1 Then
		comp.Features.HoleFeatures.AddDrilledByDistanceExtent(placementDef, circleGroup.Key, 5, PartFeatureExtentDirectionEnum.kPositiveExtentDirection)
	Else If circleGroup.Key = 1.6 Then
		comp.Features.HoleFeatures.AddDrilledByDistanceExtent(placementDef, circleGroup.Key, 7.2, PartFeatureExtentDirectionEnum.kPositiveExtentDirection)
	Else
		comp.Features.HoleFeatures.AddDrilledByThroughAllExtent(placementDef, circleGroup.Key, PartFeatureExtentDirectionEnum.kPositiveExtentDirection)
	End If
Next

For Each circlesGroup In counterBoreCirclesGroups
	Dim points As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection()
	For Each counterBoreCircles In circlesGroup
		points.Add(counterBoreCircles.Center)
	Next
	Dim placementDef As HolePlacementDefinition = comp.Features.HoleFeatures.CreateSketchPlacementDefinition(points)
	
	'Create countersink or counterbore holes according to different diameters
	If circlesGroup.Key = "6x14" Then
		comp.Features.HoleFeatures.AddCSinkByDistanceExtent(placementDef, circlesGroup.First().InnerDiameter, 8, PartFeatureExtentDirectionEnum.kPositiveExtentDirection, circlesGroup.First().OuterDiameter, 90)
	Else If circlesGroup.Key = "8x20" Then
		comp.Features.HoleFeatures.AddCSinkByDistanceExtent(placementDef, circlesGroup.First().InnerDiameter, 12, PartFeatureExtentDirectionEnum.kPositiveExtentDirection, circlesGroup.First().OuterDiameter, 90)
	Else
		comp.Features.HoleFeatures.AddCBoreByThroughAllExtent(placementDef, circlesGroup.First().InnerDiameter, PartFeatureExtentDirectionEnum.kPositiveExtentDirection, circlesGroup.First().OuterDiameter, 0.2)
	End If
Next

[GeorgK]

I think it is better to write an add-in an store the data in DataTables. It's much easier to sort and filter the data.

[FProcp]

One of the issues with Chandra's routine is that it extrudes the plate up (towards you) and it should extrude down (away from you).

If you are looking at the top view of the plate, you would see the counter-bored or counter-sunk holes on the top plane of the plate and going down into the plate.

To convert some of the holes to countersunk holes I currently have to go to the first face extrusion and switch it to extrude in the opposite direction and then edit some holes to become countersunk.

It would be nicer if it did this originally.

[smilinger · Accepted solution]

This code should suffice in most cases, including sheet metal, countersink or counterbore holes:

Imports System.Linq
Imports Inventor

Dim doc As PartDocument = ThisDoc.Document
Dim comp As PartComponentDefinition = doc.ComponentDefinition

Dim IsSheetMetal As Boolean = comp.Type = ObjectTypeEnum.kSheetMetalComponentDefinitionObject

Dim sketch1 As PlanarSketch = doc.ComponentDefinition.Sketches(1)
Dim profile As profile = sketch1.Profiles.AddForSolid(False)
If IsSheetMetal Then
	Dim faceDef As FaceFeatureDefinition = comp.Features.FaceFeatures.CreateFaceFeatureDefinition(profile)
	faceDef.Direction = PartFeatureExtentDirectionEnum.kNegativeExtentDirection
	comp.Features.FaceFeatures.Add(faceDef)
Else
	'Change the thickness for non-Sheetmetal parts here.
	Dim thickness = "6 mm"
	Dim extrudeDef = comp.Features.ExtrudeFeatures.CreateExtrudeDefinition(profile, PartFeatureOperationEnum.kNewBodyOperation)
	extrudeDef.SetDistanceExtent(thickness, PartFeatureExtentDirectionEnum.kNegativeExtentDirection)
	comp.Features.ExtrudeFeatures.Add(extrudeDef)
End If

'Group circles by position
Dim circleGroups = sketch1.SketchCircles.Cast(Of SketchCircle)().GroupBy(
	Function(c)
		Dim point = c.CenterSketchPoint.Geometry
		Return Round(point.X, 3) & ", " & Round(point.Y, 3)
	End Function
)

'Group single circles by diameter
Dim drilledCircleGroups = circleGroups.Where(Function(g) g.Count() = 1).Select(Function(g) g.Single()).GroupBy(Function(c) Round(c.Geometry.Radius * 2 * 10, 3))

'Group pairs of circles by diameters
Dim counterBoreCirclesGroups = circleGroups.Where(Function(g) g.Count() = 2).Select(
	Function(g)
		Dim o = g.OrderBy(Function(c) c.Radius)
		Return New With {.Center = g.First().CenterSketchPoint, .InnerDiameter = Round(o(0).Radius*2, 3), .OuterDiameter = Round(o(1).Radius*2, 3)}
	End Function
).GroupBy(Function(item) item.InnerDiameter*10 & "x" & item.OuterDiameter*10)

For Each circleGroup In drilledCircleGroups
	Dim points As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection()
	For Each Circle In circleGroup
		points.Add(Circle.CenterSketchPoint)
	Next
	Dim placementDef As HolePlacementDefinition = comp.Features.HoleFeatures.CreateSketchPlacementDefinition(points)
	
	Dim depth As Double	'Unit: mm
	Dim thread As String
	If IsSheetMetal Then depth = comp.Thickness.Value * 10

	'Create drilled holes according to different diameters
	Dim hole As HoleFeature
	Dim direction = PartFeatureExtentDirectionEnum.kPositiveExtentDirection
	
	'Uncomment and change these case statements to adapt to your need
	Select Case circleGroup.Key	'Diameter, Unit: mm
'		Case 6	'Unit: mm
'			depth = 35
			
'			'Change thread definition here if needed
'			thread = "M6x1"
			
'			'Create threaded hole
'			Dim tapinfo = comp.Features.HoleFeatures.CreateTapInfo(True, "ISO Metric profile", thread, "6H", True)
'			comp.Features.HoleFeatures.AddDrilledByDistanceExtent(placementDef, tapinfo, depth/10, direction)
'		Case 10, 12
'			depth = 50
'			comp.Features.HoleFeatures.AddDrilledByDistanceExtent(placementDef, circleGroup.Key/10, depth/10, direction)
'		Case 16
'			depth = 75
'			comp.Features.HoleFeatures.AddDrilledByDistanceExtent(placementDef, circleGroup.Key/10, depth/10, direction)
		Case Else
			comp.Features.HoleFeatures.AddDrilledByThroughAllExtent(placementDef, circleGroup.Key/10, direction)
	End Select
Next

For Each circlesGroup In counterBoreCirclesGroups
	Dim points As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection()
	For Each counterBoreCircles In circlesGroup
		points.Add(counterBoreCircles.Center)
	Next
	Dim placementDef As HolePlacementDefinition = comp.Features.HoleFeatures.CreateSketchPlacementDefinition(points)
	
	Dim id As Double = circlesGroup.First().InnerDiameter
	Dim od As Double = circlesGroup.First().OuterDiameter
	Dim depth As Double	'Unit: mm
	Dim sinkDepth As Double	'Unit: mm
	Dim angle As Double = 100	'Unit: degree
	
	If IsSheetMetal Then depth = comp.Thickness.Value * 10

	'Create countersink or counterbore holes according to different diameters
	Dim hole As HoleFeature
	Dim direction = PartFeatureExtentDirectionEnum.kPositiveExtentDirection
	
	'Uncomment and change these case statements to adapt to your need
	Select Case circlesGroup.Key	'<Hole Diameter>x<CounterSink Diameter>, Unit: mm
'		Case "6x14"
'			depth = 40
'			comp.Features.HoleFeatures.AddCSinkByDistanceExtent(placementDef, id, depth/10, direction, od, angle)
'		Case "8x20"
'			depth = 50
'			comp.Features.HoleFeatures.AddCSinkByDistanceExtent(placementDef, id, depth/10, direction, od, angle)
'		Case "12x35"
'			sinkDepth = 2
'			comp.Features.HoleFeatures.AddSpotFaceByThroughAllExtent(placementDef, id, direction, od, sinkDepth/10)
		Case Else
			sinkDepth = 3
			comp.Features.HoleFeatures.AddCBoreByThroughAllExtent(placementDef, id, direction, od, sinkDepth/10)
	End Select
Next

[FProcp]

Hi

smilinger,

How difficult would it be to place the hole diameter in the name of the hole feature to one decimal place?

For example re-name a Ø14.3 hole to "HoleD14.3".

This would make this code perfect 

[smilinger · Accepted solution]

Can be complicated for countersink holes, I suggest turn on the inventor option to show the infomation automatically.

[FProcp]

Yes, this is excellent