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When I enter a drawing made from a sheet metal part, inventor always defaults the flat pattern to have all the bends going down. I actually need the bends coming in as 'up' instead. Is there any way to automate this ?
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You know that you can change that in the flat-pattern definition within inventor!?
Or do you need it with coding?
And do you need it in i-logic; VBA; Vb.net; or else?
Regards
Regards,
Arthur Knoors
Autodesk Affiliations:
Autodesk Software:Inventor Professional 2025 | Vault Professional 2024 | Autocad Mechanical 2024
Programming Skills:Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
Programming Examples:Drawing List!|Toggle Drawing Sheet!|Workplane Resize!|Drawing View Locker!|Multi Sheet to Mono Sheet!|Drawing Weld Symbols!|Drawing View Label Align!|Open From Balloon!|Model State Lock!
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Yes, I do it manually every time as of now. Trying to automate processes for my company. Preferably ilogic. Will try to incorporate this with a code that streamlines most of the process of making drawings.
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Dim a As Inventor.PartDocument = ThisDoc.Document 'Dim su As Inventor.DocumentTypeEnum = a.DocumentSubType If a.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then Dim s As Inventor.SheetMetalComponentDefinition = a.ComponentDefinition Dim f As Inventor.FlatPattern = s.FlatPattern 'f.FlatPatternOrientations.ActiveFlatPatternOrientation.FlipAlignmentAxis Dim fl As Inventor.FlatPatternOrientation = f.FlatPatternOrientations.Item(1) fl.FlipBaseFace= True 'MsgBox ("") End If
Regards,
Arthur Knoors
Autodesk Affiliations:
Autodesk Software:Inventor Professional 2025 | Vault Professional 2024 | Autocad Mechanical 2024
Programming Skills:Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
Programming Examples:Drawing List!|Toggle Drawing Sheet!|Workplane Resize!|Drawing View Locker!|Multi Sheet to Mono Sheet!|Drawing Weld Symbols!|Drawing View Label Align!|Open From Balloon!|Model State Lock!
Posts and Ideas:Dimension Component!|Partlist Export!|Derive I-properties!|Vault Prompts Via API!|Vault Handbook/Manual!|Drawing Toggle Sheets!|Vault Defer Update!
! For administrative reasons, please mark a "Solution as solved" when the issue is solved !
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Or use this to flip it back an forward:
Dim a As Inventor.PartDocument = ThisDoc.Document
If a.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
Dim s As Inventor.SheetMetalComponentDefinition = a.ComponentDefinition
Dim f As Inventor.FlatPattern = s.FlatPattern
Dim fl As Inventor.FlatPatternOrientation = f.FlatPatternOrientations.Item(1)
If fl.FlipBaseFace = False Then
fl.FlipBaseFace = True
ElseIf fl.FlipBaseFace = True
fl.FlipBaseFace= False
End If
End If
Regards,
Arthur Knoors
Autodesk Affiliations:
Autodesk Software:Inventor Professional 2025 | Vault Professional 2024 | Autocad Mechanical 2024
Programming Skills:Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
Programming Examples:Drawing List!|Toggle Drawing Sheet!|Workplane Resize!|Drawing View Locker!|Multi Sheet to Mono Sheet!|Drawing Weld Symbols!|Drawing View Label Align!|Open From Balloon!|Model State Lock!
Posts and Ideas:Dimension Component!|Partlist Export!|Derive I-properties!|Vault Prompts Via API!|Vault Handbook/Manual!|Drawing Toggle Sheets!|Vault Defer Update!
! For administrative reasons, please mark a "Solution as solved" when the issue is solved !
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Looks great, would you happen to know if this rule can be run from a drawing ? It is usually in the drawing where my coworkers notice that the part needs to be flipped. (The majority of the bends need to be up instead of down).
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sure it can hang on..
Regards,
Arthur Knoors
Autodesk Affiliations:
Autodesk Software:Inventor Professional 2025 | Vault Professional 2024 | Autocad Mechanical 2024
Programming Skills:Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
Programming Examples:Drawing List!|Toggle Drawing Sheet!|Workplane Resize!|Drawing View Locker!|Multi Sheet to Mono Sheet!|Drawing Weld Symbols!|Drawing View Label Align!|Open From Balloon!|Model State Lock!
Posts and Ideas:Dimension Component!|Partlist Export!|Derive I-properties!|Vault Prompts Via API!|Vault Handbook/Manual!|Drawing Toggle Sheets!|Vault Defer Update!
! For administrative reasons, please mark a "Solution as solved" when the issue is solved !
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Dim dwg As Inventor.DrawingDocument = ThisDrawing.Document
Dim v As Inventor.DrawingView = dwg.ActiveSheet.DrawingViews.Item(1)
'v.ReferencedDocumentDescriptor.ReferencedDocument
Dim a As Inventor.PartDocument = v.ReferencedDocumentDescriptor.ReferencedDocument 'ThisDoc.Document
If a.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
Dim s As Inventor.SheetMetalComponentDefinition = a.ComponentDefinition
Dim f As Inventor.FlatPattern = s.FlatPattern
Dim fl As Inventor.FlatPatternOrientation = f.FlatPatternOrientations.Item(1)
If fl.FlipBaseFace = False Then
fl.FlipBaseFace = True
ElseIf fl.FlipBaseFace = True
fl.FlipBaseFace= False
End If
dwg.Update
End If
Regards,
Arthur Knoors
Autodesk Affiliations:
Autodesk Software:Inventor Professional 2025 | Vault Professional 2024 | Autocad Mechanical 2024
Programming Skills:Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
Programming Examples:Drawing List!|Toggle Drawing Sheet!|Workplane Resize!|Drawing View Locker!|Multi Sheet to Mono Sheet!|Drawing Weld Symbols!|Drawing View Label Align!|Open From Balloon!|Model State Lock!
Posts and Ideas:Dimension Component!|Partlist Export!|Derive I-properties!|Vault Prompts Via API!|Vault Handbook/Manual!|Drawing Toggle Sheets!|Vault Defer Update!
! For administrative reasons, please mark a "Solution as solved" when the issue is solved !
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More user friendly with a Picker selection from the user:
Dim dwg As Inventor.DrawingDocument = ThisDrawing.Document
Dim v As Inventor.DrawingView '= dwg.ActiveSheet.DrawingViews.Item(1)
v = ThisApplication.CommandManager.Pick(Inventor.selectionfilterenum.kDrawingViewFilter,"Select a Flat Pattern View")
Dim a As Inventor.PartDocument = v.ReferencedDocumentDescriptor.ReferencedDocument 'ThisDoc.Document
If a.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
Dim s As Inventor.SheetMetalComponentDefinition = a.ComponentDefinition
Dim f As Inventor.FlatPattern = s.FlatPattern
Dim fl As Inventor.FlatPatternOrientation = f.FlatPatternOrientations.Item(1)
If fl.FlipBaseFace = False Then
fl.FlipBaseFace = True
ElseIf fl.FlipBaseFace = True
fl.FlipBaseFace= False
End If
dwg.Update
End If
Regards,
Arthur Knoors
Autodesk Affiliations:
Autodesk Software:Inventor Professional 2025 | Vault Professional 2024 | Autocad Mechanical 2024
Programming Skills:Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
Programming Examples:Drawing List!|Toggle Drawing Sheet!|Workplane Resize!|Drawing View Locker!|Multi Sheet to Mono Sheet!|Drawing Weld Symbols!|Drawing View Label Align!|Open From Balloon!|Model State Lock!
Posts and Ideas:Dimension Component!|Partlist Export!|Derive I-properties!|Vault Prompts Via API!|Vault Handbook/Manual!|Drawing Toggle Sheets!|Vault Defer Update!
! For administrative reasons, please mark a "Solution as solved" when the issue is solved !
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Next the error will occur when the View is no Flat Pattern view:
Now you receive a message if it is not:
Dim dwg As Inventor.DrawingDocument = ThisDrawing.Document
Dim v As Inventor.DrawingView '= dwg.ActiveSheet.DrawingViews.Item(1)
v = ThisApplication.CommandManager.Pick(Inventor.selectionfilterenum.kDrawingViewFilter, "Select a Flat Pattern View")
If v.IsFlatPatternView = True Then
Dim a As Inventor.PartDocument = v.ReferencedDocumentDescriptor.ReferencedDocument 'ThisDoc.Document
If a.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
Dim s As Inventor.SheetMetalComponentDefinition = a.ComponentDefinition
Dim f As Inventor.FlatPattern = s.FlatPattern
Dim fl As Inventor.FlatPatternOrientation = f.FlatPatternOrientations.Item(1)
If fl.FlipBaseFace = False Then
fl.FlipBaseFace = True
ElseIf fl.FlipBaseFace = True
fl.FlipBaseFace= False
End If
dwg.Update
End If
Else
MsgBox("This View Contains no Flat Pattern")
End If
Regards,
Arthur Knoors
Autodesk Affiliations:
Autodesk Software:Inventor Professional 2025 | Vault Professional 2024 | Autocad Mechanical 2024
Programming Skills:Vba | Vb.net (Add ins Vault / Inventor, Applications) | I-logic
Programming Examples:Drawing List!|Toggle Drawing Sheet!|Workplane Resize!|Drawing View Locker!|Multi Sheet to Mono Sheet!|Drawing Weld Symbols!|Drawing View Label Align!|Open From Balloon!|Model State Lock!
Posts and Ideas:Dimension Component!|Partlist Export!|Derive I-properties!|Vault Prompts Via API!|Vault Handbook/Manual!|Drawing Toggle Sheets!|Vault Defer Update!
! For administrative reasons, please mark a "Solution as solved" when the issue is solved !
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