topic Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop in Inventor Programming Forum

FaceProxy - Select Face from Assembly and Take the EdgeLoop

florian_wenzel — Mon, 20 Jun 2022 07:15:09 GMT

Hi;

Invnentor 2022

API: VB.NET VisualStudio

i try to Select a Face in Assembly Enviroment,

then i want to take the Insides EdgeLoop.

And from every Inside EdgeLoop take the CenterPoint, Create WorkAxis, WorkPlane, PlanarSketch and Extrude Negative, CutOperation - Make Holes.

The Problem is that this is Face in Other Part in Other Assembly.

This is my Code:

Public Sub CommandFunctionfweButton_07() Dim oAsmDoc As AssemblyDocument = g_inventorApplication.ActiveDocument Dim oAsmCompDef As AssemblyComponentDefinition = oAsmDoc.ComponentDefinition Dim oTO As TransientObjects = g_inventorApplication.TransientObjects Dim oTG As TransientGeometry = g_inventorApplication.TransientGeometry 'Create Matrix Dim oMatrix As Matrix oMatrix = oTG.CreateMatrix 'Create New Part in Main Assembly Dim oNameFile As String = InputBox("text") Dim oPartB As PartDocument = g_inventorApplication.Documents.Add(DocumentTypeEnum.kPartDocumentObject) oPartB.SaveAs("C:\InventorAPI\1780-007\Part_B_" & oNameFile & ".ipt", False) 'Create NewOccurrence, PartComponentDefinition Dim oOccPartB As ComponentOccurrence oOccPartB = oAsmCompDef.Occurrences.AddByComponentDefinition(oPartB.ComponentDefinition, oMatrix) oPartB.Close() Dim oPartB_Def As PartComponentDefinition = oOccPartB.Definition 'Create New Sketch and Profile and Extrude Dim oSketchPartB As PlanarSketch = oPartB_Def.Sketches.Add(oPartB_Def.WorkPlanes.Item(3), False) Dim oRectangleLines As SketchEntitiesEnumerator oRectangleLines = oSketchPartB.SketchLines.AddAsTwoPointRectangle(oTG.CreatePoint2d(0, 0), oTG.CreatePoint2d(40, 40)) Dim oProfile As Profile oProfile = oSketchPartB.Profiles.AddForSolid Dim oExtrudeDef As ExtrudeDefinition oExtrudeDef = oPartB_Def.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, PartFeatureOperationEnum.kJoinOperation) Call oExtrudeDef.SetDistanceExtent(1, PartFeatureExtentDirectionEnum.kPositiveExtentDirection) Dim oExtrude1 As ExtrudeFeature oExtrude1 = oPartB_Def.Features.ExtrudeFeatures.Add(oExtrudeDef) 'Select face form Other part in Other Assembly Dim oFace As Face = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick a Face") Dim oOcc1 As ComponentOccurrence = oFace.Parent.Parent 'Create faceProxy Dim oFaceProxy As FaceProxy Call oOcc1.CreateGeometryProxy(oFace, oFaceProxy) 'Create Loop and Select every InsideEdgeLoop, create a CenterPoint, Axis, Plane, Sketch, Circle and Extrude. If oFace IsNot Nothing Then For Each oEdgeloop As EdgeLoop In oFace.EdgeLoops If Not oEdgeloop.IsOuterEdgeLoop Then Dim oEdgeColl As EdgeCollection = oTO.CreateEdgeCollection For Each oEdge In oEdgeloop.Edges oEdgeColl.Add(oEdge) Next Dim oWorkpoint As WorkPoint = oPartB_Def.WorkPoints.AddAtCentroid(oEdgeColl) Dim oWorkAxis As WorkAxis = oPartB_Def.WorkAxes.AddByNormalToSurface(oFace, oWorkpoint, False) Dim oWorkPlane As WorkPlane = oPartB_Def.WorkPlanes.AddByNormalToCurve(oWorkAxis, oWorkpoint, False) Dim oWorkSketch As PlanarSketch = oPartB_Def.Sketches.AddWithOrientation(oWorkPlane, oWorkAxis, True, True, oWorkpoint, True) Dim oPointCenters As SketchPoint oPointCenters = oWorkSketch.SketchPoints.Add(oTG.CreatePoint2d(0, 0), True) Dim oCircle As SketchCircle oCircle = oWorkSketch.SketchCircles.AddByCenterRadius(oPointCenters, 2) Dim oProfile01 As Profile oProfile01 = oWorkSketch.Profiles.AddForSolid Dim oExtrudeDef02 As ExtrudeDefinition oExtrudeDef02 = oPartB_Def.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile01, PartFeatureOperationEnum.kCutOperation) Call oExtrudeDef02.SetThroughAllExtent(PartFeatureExtentDirectionEnum.kSymmetricExtentDirection) Dim oExtrude2 As ExtrudeFeature oExtrude2 = oPartB_Def.Features.ExtrudeFeatures.Add(oExtrudeDef02) End If Next End If End Sub

Error:

Unknow Error

What i need to do with Proxy?

FaceProxy

EdgeLoopProxy

etc..

Thanks For Any Suggestion

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

florian_wenzel — Sun, 19 Jun 2022 22:52:36 GMT

Hi,

i would be very grateful, if Someone could tell me:

What are the Rules, when i want to take Geometry (Face) from other Assembly?

and then use for example the Inside EdgeLoop to Create a CenterPoint of Each EdgeLoop.

I know, that when i what for Example Project a Curve from One Assembly to other Assembly, then i Create for Each Sketch a Proxy, and The Proxy need to be at the same Level.

But what i need to do with Face or FaceProxy.

How to use the Geometry in other Assembly, in other Part?

Is this Possible in API?

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

florian_wenzel — Mon, 20 Jun 2022 07:30:27 GMT

Hi Again.

i have still Question about Taking Geometry from Face in Assembly Enviroment.

When i Pick a Face in Assembly Context, than this should be a Face or FaceProxy:

Dim oFace As Face = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick a Face")

Dim oFace As FaceProxy = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick a Face")

What are the Rules?

Then for EdgeLoop, i use the Face or FaceProxy ?

Or Face.NativeObject ?

From a FaceProxy when i want to take the EdgeLoop, i will Create EdgeLoop or EdgeLoopProxy?

In HelpDesk are info, that i Create From FaceProxy a normal EdgeLoop.

Inventor 2022 Help | FaceProxy.EdgeLoops Property | Autodesk

Than the Question, when i Create a EdgeLoopProxy ??? when from a FaceProxy i Create a Normal EdgeLoop?

If i want Create in a my PartB: WorkPoint, WorkAxis and so on.

Then i Need to Create Proxy for Everything?

FaceProxy -- EdgeLoopProxy --EdgeProxy etc... ?

Is this Possible in Inventor API?

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

JhoelForshav — Mon, 20 Jun 2022 08:14:49 GMT

Hi @florian_wenzel

I did some experimenting with the files you sent me last week, and my recommendation is to just copy the surface with the holes as a nonparametricbasefeature, then handle everything else within the part.

To quickly test the code I wrote it as an iLogic rule. In the example you sent me, you can run it after PartA is created and first select the curved surface in Assembly_Elements, then the surface to copy the holes to in PartA 🙂

In the example files attached here, just pick the surface with the holes first and then a surface parallel to that surface in your other part.

I hope this helps! 🙂

Dim oAsm As AssemblyDocument = ThisDoc.Document
Dim oTransaction As Transaction = ThisApplication.TransactionManager.StartTransaction(oAsm, "Create slots")
Dim oFace As FaceProxy = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick Face with original holes")
Dim oFaceOcc As ComponentOccurrence = oFace.ContainingOccurrence
Dim aFace As FaceProxy = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick Face to create holes on")
Dim aFaceRefKey(-1) As Byte
Dim aFaceKeyContext As Integer = oAsm.ReferenceKeyManager.CreateKeyContext
aFace.GetReferenceKey(aFaceRefKey, aFaceKeyContext)
Dim aOcc As ComponentOccurrence = aFace.ContainingOccurrence
Dim aDef As PartComponentDefinition = aOcc.Definition
Dim NPBFdef As NonParametricBaseFeatureDefinition = aDef.Features.NonParametricBaseFeatures.CreateDefinition
Dim oCol As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection
oCol.Add(oFace)
NPBFdef.BRepEntities = oCol
NPBFdef.OutputType = kSurfaceOutputType
NPBFdef.TargetOccurrence = aOcc
NPBFdef.IsAssociative = True

Dim planeInput As New List(Of KeyValuePair(Of WorkPoint, WorkAxis))

Dim cpySurf As NonParametricBaseFeature
cpySurf = aDef.Features.NonParametricBaseFeatures.AddByDefinition(NPBFdef)
For Each oLoop As EdgeLoop In cpySurf.Faces(1).EdgeLoops
	If oLoop.IsOuterEdgeLoop = False
		Dim oPoint As WorkPoint = aDef.WorkPoints.AddAtCentroid(oLoop)
		Dim oAxis As WorkAxis = aDef.WorkAxes.AddByNormalToSurface(oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject, oPoint)
		planeInput.Add(New KeyValuePair(Of WorkPoint, WorkAxis)(oPoint, oAxis))
	End If
Next
cpySurf.SurfaceBodies(1).Visible = False
For Each oPair As KeyValuePair(Of WorkPoint, WorkAxis) In planeInput
	Dim oPlane As WorkPlane = aDef.WorkPlanes.AddByNormalToCurve(oPair.Value, oPair.Key)
	Dim oSketch As PlanarSketch = aDef.Sketches.Add(oPlane)
	Dim oCP As SketchPoint = oSketch.AddByProjectingEntity(oPair.Key)
	Dim oEP As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oCP.Geometry.X + 1.5 / 2, oCP.Geometry.Y)
	Dim oSlot As SketchEntitiesEnumerator = oSketch.AddStraightSlotBySlotCenter(oCP, oEP, 0.8)
	Dim oLine As SketchLine = oSlot.OfType(Of SketchLine).FirstOrDefault(Function(x As SketchLine) x.Construction = True)
	oSketch.GeometricConstraints.AddHorizontal(oLine)
	oSketch.DimensionConstraints.AddTwoPointDistance(oLine.StartSketchPoint, oLine.EndSketchPoint, DimensionOrientationEnum.kHorizontalDim, oCP.Geometry)
	Dim oLines = oSlot.OfType(Of SketchLine).Where(Function(x As SketchLine) x.Construction = False)
	Dim oLine1 As SketchLine = oLines(0)
	Dim oLine2 As SketchLine = oLines(1)
	oSketch.DimensionConstraints.AddOffset(oLine1, oLine2, oCP.Geometry, False)
	Dim oProfile As Profile = oSketch.Profiles.AddForSolid
	aDef.Features.EmbossFeatures.AddEngraveFromFace(oProfile, 2, PartFeatureExtentDirectionEnum.kNegativeExtentDirection, , oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject)
	oSketch.Visible = False
	oPlane.Visible = False
	oPair.Key.Visible = False
	oPair.Value.Visible = False
Next
oAsm.Update
oTransaction.End

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

florian_wenzel — Mon, 20 Jun 2022 09:35:52 GMT

Hi @JhoelForshav

Thanks.

Yes it works with the PartA.

Now i need to Translate this to VB.NET

I think is Possible.

I see this is more complicated than I thought.

My idea was with FaceProxy and EdgeLoop.

Thanks for the Solution!

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

JhoelForshav — Mon, 20 Jun 2022 12:48:07 GMT

@florian_wenzel

It seems like using proxys as the geometry to add workgeometry doesn't work. For example using a proxy as the argument for a method like WorkPoints.AddAtCentroid will give an error.

iLogic is based on VB.NET so there isn't really anything to translate. Just replace ThisApplication with your Application object (g_inventorApplication) and replace ThisDoc.Document with g_inventorApplication.ActiveDocument and you're all set 🙂

Dim oAsm As AssemblyDocument = g_inventorApplication.ActiveDocument
Dim oTransaction As Transaction = g_inventorApplication.TransactionManager.StartTransaction(oAsm, "Create slots")
Dim oFace As FaceProxy = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick Face with original holes")
Dim oFaceOcc As ComponentOccurrence = oFace.ContainingOccurrence
Dim aFace As FaceProxy = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick Face to create holes on")
Dim aFaceRefKey(-1) As Byte
Dim aFaceKeyContext As Integer = oAsm.ReferenceKeyManager.CreateKeyContext
aFace.GetReferenceKey(aFaceRefKey, aFaceKeyContext)
Dim aOcc As ComponentOccurrence = aFace.ContainingOccurrence
Dim aDef As PartComponentDefinition = aOcc.Definition
Dim NPBFdef As NonParametricBaseFeatureDefinition = aDef.Features.NonParametricBaseFeatures.CreateDefinition
Dim oCol As ObjectCollection = g_inventorApplication.TransientObjects.CreateObjectCollection
oCol.Add(oFace)
NPBFdef.BRepEntities = oCol
NPBFdef.OutputType = kSurfaceOutputType
NPBFdef.TargetOccurrence = aOcc
NPBFdef.IsAssociative = True

Dim planeInput As New List(Of KeyValuePair(Of WorkPoint, WorkAxis))

Dim cpySurf As NonParametricBaseFeature
cpySurf = aDef.Features.NonParametricBaseFeatures.AddByDefinition(NPBFdef)
For Each oLoop As EdgeLoop In cpySurf.Faces(1).EdgeLoops
	If oLoop.IsOuterEdgeLoop = False
		Dim oPoint As WorkPoint = aDef.WorkPoints.AddAtCentroid(oLoop)
		Dim oAxis As WorkAxis = aDef.WorkAxes.AddByNormalToSurface(oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject, oPoint)
		planeInput.Add(New KeyValuePair(Of WorkPoint, WorkAxis)(oPoint, oAxis))
	End If
Next
cpySurf.SurfaceBodies(1).Visible = False
For Each oPair As KeyValuePair(Of WorkPoint, WorkAxis) In planeInput
	Dim oPlane As WorkPlane = aDef.WorkPlanes.AddByNormalToCurve(oPair.Value, oPair.Key)
	Dim oSketch As PlanarSketch = aDef.Sketches.Add(oPlane)
	Dim oCP As SketchPoint = oSketch.AddByProjectingEntity(oPair.Key)
	Dim oEP As Point2d = g_inventorApplication.TransientGeometry.CreatePoint2d(oCP.Geometry.X + 1.5 / 2, oCP.Geometry.Y)
	Dim oSlot As SketchEntitiesEnumerator = oSketch.AddStraightSlotBySlotCenter(oCP, oEP, 0.8)
	Dim oLine As SketchLine = oSlot.OfType(Of SketchLine).FirstOrDefault(Function(x As SketchLine) x.Construction = True)
	oSketch.GeometricConstraints.AddHorizontal(oLine)
	oSketch.DimensionConstraints.AddTwoPointDistance(oLine.StartSketchPoint, oLine.EndSketchPoint, DimensionOrientationEnum.kHorizontalDim, oCP.Geometry)
	Dim oLines = oSlot.OfType(Of SketchLine).Where(Function(x As SketchLine) x.Construction = False)
	Dim oLine1 As SketchLine = oLines(0)
	Dim oLine2 As SketchLine = oLines(1)
	oSketch.DimensionConstraints.AddOffset(oLine1, oLine2, oCP.Geometry, False)
	Dim oProfile As Profile = oSketch.Profiles.AddForSolid
	aDef.Features.EmbossFeatures.AddEngraveFromFace(oProfile, 2, PartFeatureExtentDirectionEnum.kNegativeExtentDirection, , oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject)
	oSketch.Visible = False
	oPlane.Visible = False
	oPair.Key.Visible = False
	oPair.Value.Visible = False
Next
oAsm.Update
oTransaction.End

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

florian_wenzel — Mon, 20 Jun 2022 13:12:12 GMT

Thanks @JhoelForshav

dont know with:

153 kSurfaceOutputType

Error: kSurfaceOutputType not Declare

NPBFdef.OutputType = kSurfaceOutputType = Nothing ?? - Not Working also

158 Dim planeInput As New List(Of KeyValuePair(Of WorkPoint, WorkAxis))

Error: not define Variable and List

I need to write: Dim KeyValuePair As String ?

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

JhoelForshav — Mon, 20 Jun 2022 13:47:44 GMT

Hi @florian_wenzel

When it comes to kSurfaceOutputType, change it to BaseFeatureOutputTypeEnum.kSurfaceOutputType.

I think you should have the reference already in your project, but maybe you need to add the namespace System.Collections.Generic for your List and KeyValuePair. So either add Imports System.Collections.Generic at the top of your class or just add the namespace to your declarations:

Ex: Dim planeInput As New System.Collections.Generic.List(Of System.Collections.Generic.KeyValuePair(Of WorkPoint, WorkAxis))

See if this code works for you:

Dim oAsm As AssemblyDocument = g_inventorApplication.ActiveDocument Dim oTransaction As Transaction = g_inventorApplication.TransactionManager.StartTransaction(oAsm, "Create slots") Dim oFace As FaceProxy = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick Face with original holes") Dim oFaceOcc As ComponentOccurrence = oFace.ContainingOccurrence Dim aFace As FaceProxy = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "Pick Face to create holes on") Dim aFaceRefKey(-1) As Byte Dim aFaceKeyContext As Integer = oAsm.ReferenceKeyManager.CreateKeyContext aFace.GetReferenceKey(aFaceRefKey, aFaceKeyContext) Dim aOcc As ComponentOccurrence = aFace.ContainingOccurrence Dim aDef As PartComponentDefinition = aOcc.Definition Dim NPBFdef As NonParametricBaseFeatureDefinition = aDef.Features.NonParametricBaseFeatures.CreateDefinition Dim oCol As ObjectCollection = g_inventorApplication.TransientObjects.CreateObjectCollection oCol.Add(oFace) NPBFdef.BRepEntities = oCol NPBFdef.OutputType = BaseFeatureOutputTypeEnum.kSurfaceOutputType NPBFdef.TargetOccurrence = aOcc NPBFdef.IsAssociative = True Dim planeInput As New System.Collections.Generic.List(Of System.Collections.Generic.KeyValuePair(Of WorkPoint, WorkAxis)) Dim cpySurf As NonParametricBaseFeature cpySurf = aDef.Features.NonParametricBaseFeatures.AddByDefinition(NPBFdef) For Each oLoop As EdgeLoop In cpySurf.Faces(1).EdgeLoops If oLoop.IsOuterEdgeLoop = False Then Dim oPoint As WorkPoint = aDef.WorkPoints.AddAtCentroid(oLoop) Dim oAxis As WorkAxis = aDef.WorkAxes.AddByNormalToSurface(oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject, oPoint) planeInput.Add(New System.Collections.Generic.KeyValuePair(Of WorkPoint, WorkAxis)(oPoint, oAxis)) End If Next cpySurf.SurfaceBodies(1).Visible = False For Each oPair As System.Collections.Generic.KeyValuePair(Of WorkPoint, WorkAxis) In planeInput Dim oPlane As WorkPlane = aDef.WorkPlanes.AddByNormalToCurve(oPair.Value, oPair.Key) Dim oSketch As PlanarSketch = aDef.Sketches.Add(oPlane) Dim oCP As SketchPoint = oSketch.AddByProjectingEntity(oPair.Key) Dim oEP As Point2d = g_inventorApplication.TransientGeometry.CreatePoint2d(oCP.Geometry.X + 1.5 / 2, oCP.Geometry.Y) Dim oSlot As SketchEntitiesEnumerator = oSketch.AddStraightSlotBySlotCenter(oCP, oEP, 0.8) Dim oLine As SketchLine = oSlot.OfType(Of SketchLine).FirstOrDefault(Function(x As SketchLine) x.Construction = True) oSketch.GeometricConstraints.AddHorizontal(oLine) oSketch.DimensionConstraints.AddTwoPointDistance(oLine.StartSketchPoint, oLine.EndSketchPoint, DimensionOrientationEnum.kHorizontalDim, oCP.Geometry) Dim oLines = oSlot.OfType(Of SketchLine).Where(Function(x As SketchLine) x.Construction = False) Dim oLine1 As SketchLine = oLines(0) Dim oLine2 As SketchLine = oLines(1) oSketch.DimensionConstraints.AddOffset(oLine1, oLine2, oCP.Geometry, False) Dim oProfile As Profile = oSketch.Profiles.AddForSolid aDef.Features.EmbossFeatures.AddEngraveFromFace(oProfile, 2, PartFeatureExtentDirectionEnum.kNegativeExtentDirection, , oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject) oSketch.Visible = False oPlane.Visible = False oPair.Key.Visible = False oPair.Value.Visible = False Next oAsm.Update() oTransaction.End()

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

florian_wenzel — Mon, 20 Jun 2022 14:06:13 GMT

Hi @JhoelForshav

Still Error:

System.MissingMemberException: "Der öffentliche Member OfType für den Typ SketchEntitiesEnumerator wurde nicht gefunden."

System.MissingMemberException: "The public member OfType for the SketchEntitiesEnumerator type was not found."

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

JhoelForshav — Mon, 20 Jun 2022 15:08:09 GMT

Hi @florian_wenzel

Okay, so we'll probably need to import the System.Linq namespace aswell.

Add the line Imports System.Linq to the top of your class and see if that works 🙂

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

florian_wenzel — Mon, 20 Jun 2022 15:17:19 GMT

Hi @JhoelForshav

It Works !

Thanks For help

Thanks for Solution!

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

ROBOMACH_PL_1 — Fri, 23 Sep 2022 12:42:02 GMT

Hi,

@JhoelForshav ,

I would like to modify your rule but I have a problem with that.

My point is exactly that:

1. I would like to be able to copy (pick) any number of surfaces with holes on one base surface.

2. I would like the result of this operation to be one sketch (now each projected hole is a new sketch and a new cut) with all the slots as it is now.

It seems to me that for a skilled programmer it is a small matter, but unfortunately I am a complete amateur. If point 1 would be a problem, I would be completely satisfied with solving the problem from point 2.

Would you be able to help me ??

Regards,

ralfmja

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

ROBOMACH_PL_1 — Wed, 28 Sep 2022 14:19:22 GMT

Hello All, hello @JhoelForshav

I did a few tries and dealt with point 2 from my previous post. Now the code is as follows (probably not perfect, but it works):

sprawdzanie czy jesteśmy w złożeniu If ThisDoc.Document.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then MsgBox("REGULA DZIAŁA TYLKO W ZESPOLE", vbCritical, "OSTRZEŻENIE") Exit Sub End If Dim oAsm As AssemblyDocument = ThisDoc.Document Dim oTransaction As Transaction = ThisApplication.TransactionManager.StartTransaction(oAsm, "RZUTOWANIE OTWORÓW") Dim oFace As FaceProxy 'obsluga bledu jezeli ktoś sie rozmysli przy wybieraniu plaszczyzny z otworami While True oFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "WSKAŻ PŁASZCZYZNE Z OTWORAMI") ' jesli nic nie wybrane to If IsNothing(oFace) Then Exit Sub Else Exit While End While Dim oFaceOcc As ComponentOccurrence = oFace.ContainingOccurrence Dim aFace As FaceProxy 'obsluga bledu jezeli ktoś sie rozmysli przy wybieraniu plaszczyzny rzutowania While True aFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "WSKAŻ PŁASZCZYZNE RZUTOWANIA") ' jesli nic nie wybrane to If IsNothing(aFace) Then Exit Sub Else Exit While End While Dim aFaceRefKey(-1) As Byte Dim aFaceKeyContext As Integer = oAsm.ReferenceKeyManager.CreateKeyContext aFace.GetReferenceKey(aFaceRefKey, aFaceKeyContext) Dim aOcc As ComponentOccurrence = aFace.ContainingOccurrence Dim aDef As PartComponentDefinition = aOcc.Definition Dim NPBFdef As NonParametricBaseFeatureDefinition = aDef.Features.NonParametricBaseFeatures.CreateDefinition Dim oCol As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection oCol.Add(oFace) NPBFdef.BRepEntities = oCol NPBFdef.OutputType = kSurfaceOutputType NPBFdef.TargetOccurrence = aOcc NPBFdef.IsAssociative = True Dim planeInput As New List(Of KeyValuePair(Of WorkPoint, WorkAxis)) Dim cpySurf As NonParametricBaseFeature cpySurf = aDef.Features.NonParametricBaseFeatures.AddByDefinition(NPBFdef) For Each oLoop As EdgeLoop In cpySurf.Faces(1).EdgeLoops If oLoop.IsOuterEdgeLoop = False Dim oPoint As WorkPoint = aDef.WorkPoints.AddAtCentroid(oLoop) Dim oAxis As WorkAxis = aDef.WorkAxes.AddByNormalToSurface(oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject, oPoint) planeInput.Add(New KeyValuePair(Of WorkPoint, WorkAxis)(oPoint, oAxis)) End If Next cpySurf.SurfaceBodies(1).Visible = False Dim oPlaszczyzna As WorkPlane = aDef.WorkPlanes.AddByPlaneAndOffset(oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject, 0) oPlaszczyzna.Visible = False Dim oSketch As PlanarSketch = aDef.Sketches.Add(oPlaszczyzna) oSketch.Visible = True For Each oPair As KeyValuePair(Of WorkPoint, WorkAxis) In planeInput Dim oCP As SketchPoint = oSketch.AddByProjectingEntity(oPair.Key) Dim oEP As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(oCP.Geometry.X + 1 / 2, oCP.Geometry.Y) Dim oSlot As SketchEntitiesEnumerator = oSketch.AddStraightSlotBySlotCenter(oCP, oEP, 0.9) Dim oLine As SketchLine = oSlot.OfType(Of SketchLine).FirstOrDefault(Function(x As SketchLine) x.Construction = True) ' oSketch.GeometricConstraints.AddHorizontal(oLine) oSketch.DimensionConstraints.AddTwoPointDistance(oLine.StartSketchPoint, oLine.EndSketchPoint, DimensionOrientationEnum.kHorizontalDim, oCP.Geometry) Dim oLines = oSlot.OfType(Of SketchLine).Where(Function(x As SketchLine) x.Construction = False) Dim oLine1 As SketchLine = oLines(0) Dim oLine2 As SketchLine = oLines(1) oSketch.DimensionConstraints.AddOffset(oLine1, oLine2, oCP.Geometry, False) ' Dim oProfile As Profile = oSketch.Profiles.AddForSolid ' aDef.Features.EmbossFeatures.AddEngraveFromFace(oProfile, 2, PartFeatureExtentDirectionEnum.kNegativeExtentDirection, , oAsm.ReferenceKeyManager.BindKeyToObject(aFaceRefKey, aFaceKeyContext).NativeObject) oSketch.DimensionsVisible=False oPair.Key.Visible = False oPair.Value.Visible = False Next oAsm.Update oTransaction.End InventorVb.DocumentUpdate() 'Wyłaczenie adaptacyjnosci iLogicVb.Automation.RunExternalRule(oAsm, "ADAPTACJA_OFF")

However, I am intrigued by point 1, i.e. how to add the possibility to choose several planes ??

I think I know what to do but I don't know how 😄

I would select several planes using the code:

Dim oSurfaces As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection While True oFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceFilter, "WSKAŻ PŁASZCZYZNE Z OTWORAMI") ' jesli nic nie wybrane to If IsNothing(oFace) Then GoTo wybor2 Else oSurfaces.Add(oFace) End While

but I have no idea how to "stitch" these planes together so that the rest of the rule would be based on this stitching ??

Would anyone be able to help on this topic ??

Thanks in advance,

Best regard,

ralfmja

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

florian_wenzel — Wed, 28 Sep 2022 18:13:26 GMT

Hi,

dont know exactly what you need.

Dont understand me wrong, it is very good to try other code or example, but it will not always working how you want 🙂

The Origin Code, was made for Curved Surface, that why i needed the all Axis etc...

The Picture on the Begining was only a Simple Example.

On your Picture i see, you have a Planar Plane, so should be relative more simply, i think so.

Are all Parts with Planar Planes, Faces?

Try to describe more what you want, or show the Assembly tree, which Part in which assembly etc..

Suggestion:

When all Parts has Planar Faces, then my spotanic Suggestion is:

You need to have a Occurence from Part A and Part B

In Part A

Select a Face, or Select a Entity, than simply Create in Part A a PlanarSketch and SketchProxy

AddEntity to The Sketch in Part A.

In Part B

Create Sketch and SketchProxy

and simply Copy Content From Part A to PartB, for this you need Proxy.

I think this should work, when your Parts has PlanarFaces.

In my Case it was Curved Surfaces, that why was a little bit Tricky.

Betreff: FaceProxy - Select Face from Assembly and Take the EdgeLoop

ROBOMACH_PL_1 — Mon, 03 Oct 2022 09:05:07 GMT

Hi @florian_wenzel ,

thanks for you answer.

Yes - all planes with holes are flat and parallel to the plane on which it is projecting.

It is intended to be a "streamlined" tool for the adaptive projection of holes from different parts onto the one in which these holes are to be formed.

Inventor's standard approach to adaptability in large assemblies causes numerous problems with adaptability. For do this I use the "copy object" tool and then project that object onto the sketches and make the appropriate holes. The rule described in this topic allows you to significantly reduce the time required for these operations. However, it would be ideal for me if I could select and project all surfaces "at once".

But I never know how many planes I want to project (sometimes one, sometimes two, sometimes maybe 10 etc.).

Selecting planes seems to be done, but needs help in "joining" them and using them to project onto a selected plane.

I agree with you that it should be easier than with "rounded" surfaces, but I don't know how to do it anyway. 🙂

Thanks in advance,

Regards,

ralfmja