topic Re: Delete projected entity in Inventor Programming Forum

Delete projected entity

tim11_manhhieu — Fri, 23 May 2025 03:29:55 GMT

Hi experts,

I am writing a macro to use in assembly environment, to punch a threaded hole by picking edge of drill hole.

The problem is that after creating the threaded hole, there are projected entities left.

I want to delete the yellow sketch circle and yellow sketch point as shown in the image.

iLogic or VBA are both fine.

Option Explicit Sub XXX() Dim oAssemDoc As AssemblyDocument Dim oAssemDef As AssemblyComponentDefinition Dim oFace As Object Dim oOcc As ComponentOccurrence Dim oPartDoc As PartDocument Dim oPartDef As PartComponentDefinition Dim oSketch As PlanarSketch Dim oEntity As Object Dim oEntityProxy As Object Dim oSketchProxy As Object Dim oEntityOcc As ComponentOccurrence Dim x As Double Dim y As Double Dim oHoleCenters As ObjectCollection Dim oHoleTapInfo As HoleTapInfo Dim oTransGeom As TransientGeometry Dim h As HoleFeature Set oAssemDoc = ThisApplication.ActiveDocument Set oAssemDef = oAssemDoc.ComponentDefinition Set oFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Select face on part for new sketch") If oFace Is Nothing Then Exit Sub Set oOcc = oFace.ContainingOccurrence oOcc.Edit Set oPartDoc = ThisApplication.ActiveEditDocument Set oPartDef = oPartDoc.ComponentDefinition Set oSketch = oPartDef.Sketches.Add(oFace.NativeObject) oSketch.Edit Set oEntity = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAllEntitiesFilter, "Select entity to project") If oEntity Is Nothing Then Exit Sub Set oEntityOcc = oEntity.ContainingOccurrence Call oEntityOcc.CreateGeometryProxy(oEntity, oEntityProxy) Call oOcc.CreateGeometryProxy(oSketch, oSketchProxy) Call oSketchProxy.AddByProjectingEntity(oEntityProxy) oSketch.Adaptive = False Set oTransGeom = ThisApplication.TransientGeometry x = oSketch.SketchCircles.item(1).CenterSketchPoint.Geometry.x y = oSketch.SketchCircles.item(1).CenterSketchPoint.Geometry.y Set oHoleCenters = ThisApplication.TransientObjects.CreateObjectCollection Call oHoleCenters.Add(oSketch.SketchPoints.Add(oTransGeom.CreatePoint2d(x, y))) Set oHoleTapInfo = oPartDef.Features.HoleFeatures.CreateTapInfo(True, "ISO Metric profile", "M6x1", "6H", True) Set h = oPartDef.Features.HoleFeatures.AddDrilledByThroughAllExtent(oHoleCenters, oHoleTapInfo, kPositiveExtentDirection) oSketch.ExitEdit ThisApplication.CommandManager.ControlDefinitions.item("AppReturnTopCmd").Execute oOcc.Adaptive = False End Sub

Re: Delete projected entity

bradeneuropeArthur — Fri, 23 May 2025 11:22:33 GMT

How to define and keep that definition for the hole feature than?

Re: Delete projected entity

WCrihfield — Fri, 23 May 2025 11:47:57 GMT

What about turning the visibility of that sketch off instead. The sketch needs to be there, because the HoleFeature is dependent on it.

PlanarSketch.Visible = False ('oSketch.Visible = False' in your code example)

Re: Delete projected entity

WCrihfield — Fri, 23 May 2025 12:35:25 GMT

Another idea would be to use a WorkPoint as the location of the HoleFeature, instead of a projected sketch. If doing it that way, you could use the HoleFeatures.CreatePointPlacementDefinition method to create a PointHolePlacementDefinition (uses a WorkPoint to define hole location). We would usually have used the HoleFeatures.CreateSketchPlacementDefinition to create a SketchHolePlacementDefinition when defining the locations of HoleFeatures by way of SketchPoints, but they continue to support the older way of using an ObjectCollection containing SketchPoints also. I would likely be a good idea to use the newer methods in any important future automation solutions though. Just some additional thoughts.

Re: Delete projected entity

patrick.schlambHPACQ — Fri, 23 May 2025 13:19:49 GMT

Alternatively, you can remove reference of the projected item and it will no longer be a projection. The following code will break the reference to the projection and then ground the entity so you aren't left with unconstrained sketches.

For Each sketchEnt As SketchEntity In oSketch.SketchEntities
	sketchEnt.Reference = False
	Try
		oSketch.GeometricConstraints.AddGround(sketchEnt)
	Catch : End Try
Next sketchEnt

Re: Delete projected entity

marcin_otręba — Mon, 26 May 2025 07:14:56 GMT

try:

Dim oProjEnt As SketchEntity = oSketchProxy.AddByProjectingEntity(oEntityProxy)

instead of

Call oSketchProxy.AddByProjectingEntity(oEntityProxy)

and then just delete it after creating hole centers:

oProjEnt.Delete()

Re: Delete projected entity

tim11_manhhieu — Wed, 28 May 2025 02:30:39 GMT

Thank you for response.

They are not dependent on each other, after creating the hole, the hole will depend on the sketch point.

The projected entity can be deleted if we delete all their constraints.

Re: Delete projected entity

tim11_manhhieu — Wed, 28 May 2025 00:30:07 GMT

I'll look into HoleFeatures.CreatePointPlacementDefinition more.

Since I'm almost there, there's only one small issue left.

Re: Delete projected entity

tim11_manhhieu — Wed, 28 May 2025 02:30:56 GMT

I tried it and it worked, thank you.

sketchEnt.Reference = False

Re: Delete projected entity

tim11_manhhieu — Wed, 28 May 2025 02:31:05 GMT

Thank you for response. It still error.

Re: Delete projected entity

tim11_manhhieu — Wed, 28 May 2025 00:41:31 GMT

VBA for who need.

Option Explicit Sub zzz() Dim oAssemDoc As AssemblyDocument Dim oAssemDef As AssemblyComponentDefinition Dim oFace As Object Dim oOcc As ComponentOccurrence Dim oPartDoc As PartDocument Dim oPartDef As PartComponentDefinition Dim oSketch As PlanarSketch Dim oEntity As Object Dim oEntityProxy As Object Dim oSketchProxy As Object Dim oEntityOcc As ComponentOccurrence Dim x As Double Dim y As Double Dim oHoleCenters As ObjectCollection Dim oHoleTapInfo As HoleTapInfo Dim oTransGeom As TransientGeometry Dim h As HoleFeature Dim oSketchEntity As SketchEntity Set oAssemDoc = ThisApplication.ActiveDocument Set oAssemDef = oAssemDoc.ComponentDefinition Set oFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Select plane for tap hole: ") If oFace Is Nothing Then Exit Sub Set oOcc = oFace.ContainingOccurrence oOcc.Edit Set oPartDoc = ThisApplication.ActiveEditDocument Set oPartDef = oPartDoc.ComponentDefinition Set oSketch = oPartDef.Sketches.Add(oFace.NativeObject) oSketch.Edit Set oEntity = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFaceCylindricalFilter, "Select drill hole face: ") If oEntity Is Nothing Then Exit Sub Set oEntityOcc = oEntity.ContainingOccurrence Call oEntityOcc.CreateGeometryProxy(oEntity, oEntityProxy) Call oOcc.CreateGeometryProxy(oSketch, oSketchProxy) Call oSketchProxy.AddByProjectingEntity(oEntity.Edges.item(1)) oSketch.Adaptive = False Set oTransGeom = ThisApplication.TransientGeometry x = oSketch.SketchCircles.item(1).CenterSketchPoint.Geometry.x y = oSketch.SketchCircles.item(1).CenterSketchPoint.Geometry.y Set oHoleCenters = ThisApplication.TransientObjects.CreateObjectCollection Call oHoleCenters.Add(oSketch.SketchPoints.Add(oTransGeom.CreatePoint2d(x, y))) Set oHoleTapInfo = oPartDef.Features.HoleFeatures.CreateTapInfo(True, "ISO Metric profile", "M6x1", "6H", True) Set h = oPartDef.Features.HoleFeatures.AddDrilledByThroughAllExtent(oHoleCenters, oHoleTapInfo, kPositiveExtentDirection) For Each oSketchEntity In oSketch.SketchEntities oSketchEntity.Reference = False Next oSketch.SketchCircles.item(1).Delete oOcc.ExitEdit (kExitToTop) oOcc.Adaptive = False End Sub

Re: Delete projected entity

WCrihfield — Wed, 28 May 2025 11:45:47 GMT

I didn't actually say that the hole feature would be dependent on the projected geometry, but rather to the sketch, and did not think it would be wise to delete the sketch. But now I understand you were just talking about breaking the 'projected Link', then deleting just that projected circle, instead of the sketch. I also apparently did not pay close enough attention to one line in your code. Since you are creating a 'new' SketchPoint within the sketch at the same 'location' of the projected circle's center, instead of finding then using the projected center point of the circle itself, that eliminated any dependency on the projected geometry. If you had used the existing projected SketchPoint object to specify the hole feature's location, then deleting the projected sketch geometry would have likely broken the hole feature. Also note that the new SketchPoint that you created is not 'grounded' or constrained in any way yet, so you may want to add that, if it is important.

Glad to see that you got it working OK.

Re: Delete projected entity

tim11_manhhieu — Thu, 29 May 2025 00:11:37 GMT

I have noted that SketchPoint is not dimensionally constrained.

I will manually constrain and that is also my intention.

During the design process, the hole position often has to be changed, so constraining the hole position is something that cannot be ignored.

The operation of punching the threaded hole below often takes a lot of time, so I found a solution for it.