topic create a section view from my base view using i logic in Inventor Programming Forum

create a section view from my base view using i logic

suresh.r.ext — Tue, 17 Oct 2023 09:08:13 GMT

i just tring to create a section view from my base view . im looking for te code. can any one help me with code.

view1 --> section line direction ---> distance ----> generare view

thanks in advance

Re: create a section view from my base view using i logic

FINET_Laurent — Tue, 17 Oct 2023 11:33:40 GMT

Here is some informations related to creating section views using the API : Inventor 2024 Help | DrawingViews.AddSectionView Method | Autodesk

You need to create a drawing sketch first on the main drawing view, draw the section line & then only create the section view. About this sketch, will it be already drawn? Or do we need to code it ? Where will it be ? Can you provide pictures of the derired result ?

Kind regards,

FINET L.

Re: create a section view from my base view using i logic

Curtis_W — Tue, 17 Oct 2023 15:49:48 GMT

Hi @suresh.r.ext

I had this example on hand. Note that this does some conversion from cm to inch that might not be needed for your work. It also breaks the view alignment, but you can remove that if not needed.

See attached Inventor 2023 files.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Sub Main Dim oDrawDoc As DrawingDocument = ThisApplication.ActiveDocument Dim oTG As TransientGeometry = ThisApplication.TransientGeometry Dim oUOM As UnitsOfMeasure = oDrawDoc.UnitsOfMeasure oInvUnits = UnitsTypeEnum.kCentimeterLengthUnits oCnvt_cm_to_in = oUOM.ConvertUnits(1, oUOM.LengthUnits, oInvUnits) 'cm to inch (2.54) oCnvt_in_to_cm = oUOM.ConvertUnits(1, oInvUnits, oUOM.LengthUnits) 'inch to cm (.3937...) 'get the sheet Dim oSheet As Sheet oSheet = oDrawDoc.ActiveSheet 'get base view Dim oBaseView As DrawingView oBaseView = oSheet.DrawingViews.Item(1) Dim SketchName As String = "Section Sketch" Dim SectionViewName As String = "Z" '[ delete section view if it already exits For Each View As DrawingView In oSheet.DrawingViews 'delete view from previous try if it exists If View.name = SectionViewName Then Try : View.Delete : Catch : End Try End If 'delete sketch if it already exits Try : oBaseView.Sketches.Item(SketchName).Delete : Catch : End Try Next '] Dim SectionSketch As DrawingSketch = oBaseView.Sketches.Add SectionSketch.Edit viewExtendPercent = 0.05 Left_X = oBaseView.Center.X - (oBaseView.Width / 2) -(oBaseView.Width * viewExtendPercent) Right_X = oBaseView.Center.X + (oBaseView.Width / 2) + (oBaseView.Width * viewExtendPercent) Dim SectionPoint_L As Point2d = oTG.CreatePoint2d(Left_X, oBaseView.Center.Y) Dim SectionPoint_R As Point2d = oTG.CreatePoint2d(Right_X, oBaseView.Center.Y) Dim SheetPoint_L As Point2d = SectionSketch.SheetToSketchSpace(SectionPoint_L) Dim SheetPoint_R As Point2d = SectionSketch.SheetToSketchSpace(SectionPoint_R) Dim SketchLine As Inventor.SketchLine = SectionSketch.SketchLines.AddByTwoPoints(SheetPoint_L, SheetPoint_R) SectionSketch.ExitEdit SectionSketch.Name = SketchName 'section view placement point 'the X is intially ignored because of the view alignment, but we reuse this point after alignment is broken Dim ViewCenterPoint As Point2d = oTG.CreatePoint2d(oBaseView.Center.X + 10, oBaseView.Center.Y + oBaseView.Height) Dim SectionView As Inventor.SectionDrawingView SectionView = oSheet.DrawingViews.AddSectionView(oBaseView, SectionSketch, ViewCenterPoint, DrawingViewStyleEnum.kFromBaseDrawingViewStyle, , , SectionViewName) SectionView.Aligned = False 'break alignement SectionView.Center = ViewCenterPoint 'move view SectionView.ReverseDirection End Sub

Re: create a section view from my base view using i logic

suresh.r.ext — Wed, 18 Oct 2023 06:33:43 GMT

@Curtis_WThanks it helps 😍

Re: create a section view from my base view using i logic

est_david_bermudez — Tue, 25 Feb 2025 19:39:30 GMT

Hi @Curtis_W and everyone.

I'm working on creating a section view using the code below. However, I need to crop it in a specific way, as shown in the attached images.

Does anyone know how I can make this crop in the section view?

I was considering using a work point that I already have in one of the parts (Point2), which is located exactly in the center of the connection I want to section.

I appreciate any suggestions or ideas. Thanks!

Class Detalles Public oDrawDoc As DrawingDocument Public oTG As TransientGeometry 'get the sheet Public oSheet As Sheet 'get base view Public oBaseView As DrawingView Public SketchName As String Public SectionViewName As String Public oPartDoc As AssemblyDocument Sub Main() oDrawDoc = ThisApplication.ActiveDocument oTG = ThisApplication.TransientGeometry oSheet = oDrawDoc.ActiveSheet oBaseView = oSheet.DrawingViews.Item(3) SketchName = "Section Sketch" SectionViewName = "Z" 'VistaDetalle() VistaSeccion() End Sub ' Sub VistaDetalle() ' End Sub Sub VistaSeccion() '[ delete section view if it already exits For Each View As DrawingView In oSheet.DrawingViews 'delete view from previous try if it exists If View.name = SectionViewName Then Try : View.Delete : Catch : End Try End If 'delete sketch if it already exits Try : oBaseView.Sketches.Item(SketchName).Delete : Catch : End Try Next '] Dim SectionSketch As DrawingSketch = oBaseView.Sketches.Add SectionSketch.Edit viewExtendPercent = 0.05 Dim angulo As Double = 170 X = oBaseView.Center.X + (6 * Cos((3.1416/180)*angulo)) Y = oBaseView.Center.Y + (6 * Sin((3.1416/180)*angulo)) Dim SectionPoint_L As Point2d = oTG.CreatePoint2d(oBaseView.Center.X, oBaseView.Center.Y) Dim SectionPoint_R As Point2d = oTG.CreatePoint2d(X, Y) Dim SheetPoint_L As Point2d = SectionSketch.SheetToSketchSpace(SectionPoint_L) Dim SheetPoint_R As Point2d = SectionSketch.SheetToSketchSpace(SectionPoint_R) Dim SketchLine As Inventor.SketchLine = SectionSketch.SketchLines.AddByTwoPoints(SheetPoint_L, SheetPoint_R) SectionSketch.ExitEdit SectionSketch.Name = SketchName 'section view placement point 'the X is intially ignored because of the view alignment, but we reuse this point after alignment is broken Dim ViewCenterPoint As Point2d = oTG.CreatePoint2d(oBaseView.Center.X + 10, oBaseView.Center.Y + oBaseView.Height) Dim SectionView As Inventor.SectionDrawingView SectionView = oSheet.DrawingViews.AddSectionView(oBaseView, SectionSketch, ViewCenterPoint, DrawingViewStyleEnum.kFromBaseDrawingViewStyle, , , SectionViewName) SectionView.Aligned = False 'break alignement SectionView.Center = ViewCenterPoint 'move view SectionView.ReverseDirection Dim rotacion As Double If angulo > 37 And angulo < 270 Then rotacion = (3.1416 / 180) * (angulo - 180) Else rotacion = (3.1416 / 180) * (angulo) End If SectionView.RotateByAngle(rotacion, True) End Sub End Class