iLogic Part contains Solidbody
you can try this rule.
Dim doc As Document = ThisApplication.ActiveDocument
'Loop through all referenced docs in assembly
For Each oDoc As Document In doc.AllReferencedDocuments
' Check if its a part document
If oDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim pDoc As PartDocument = oDoc
' Check if there are multiple solid bodies
If (pDoc.ComponentDefinition.HasMultipleSolidBodies = False) Then
' Check if its a sheetmetal part
If (pDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then
Dim oCompDefSM As SheetMetalComponentDefinition = oDoc.ComponentDefinition
'Check if unfold exists. If not try to unfold
If oCompDefSM.HasFlatPattern = False Then
oCompDefSM.Unfold()
oCompDefSM.FlatPattern.ExitEdit()
oCompDefSM.Document.Close(True)
End If
End If
End If
End If
Next
Jelte de Jong
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Blog: hjalte.nl - github.com
Hi @ToniCoelhoE8VJF. The good news is yes, I think that is possible. You would have to switch from using the regular SheetMetalComponentDefinition.Unfold method, to using the SheetMetalComponentDefinition.Unfold2 method, which asks for the Face object to use as the FlatPattern.BaseFace. You would most likely have to also include the 'Pick' function, to pause the code for manual, mouse selection of a Face for it to use there. But before calling that function, you would have to 'visibly' open each sheet metal part type document, because they are just being referenced in the background while another document is active in the example above. This would be needed so that you can see it on your screen before picking one of its faces, because that earlier code example was just doing all that processing in the background.
Wesley Crihfield
(Not an Autodesk Employee)
Yes. The code can visibly open each sheet metal part as it comes to them, then prompt the user to manually click the mouse on a face of that part to use as the 'base face', then proceed to do the unfolding, and move on to the next part. Or, if you had those specific faces 'named', then no manual user interactions would be needed at run time, and the code could just find the face by its name, and use that, without needing to visibly open each one, and without needing to prompt the user to pick a face for each one. That named face route would require preparation ahead of time though. When in a part, we can select a face, right-click on it, and choose 'Assign Name...' from the context menu, then assign a name to it. That creates an attribute on that face that we can find by code later. That works for faces, edges, and vertex objects.
Below is an edited copy of Jelte's code example. I added a line of code for visibly opening the sheet metal part only if it does not already have a flat pattern, and needs to be unfolded. Then, I added a line of code to prompt the user to select a 'base face' for the unfold. If something was picked, it will then try to unfold the part using that picked face. Then it will try to visibly close that document. Since this document is being referenced by the originally active document, it will not be fully closed, just visibly closed. I have not tested this edited code, so proceed with caution.
Dim doc As Document = ThisApplication.ActiveDocument
'Loop through all referenced docs in assembly
For Each oDoc As Document In doc.AllReferencedDocuments
' Check if its a part document
If oDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim pDoc As PartDocument = oDoc
' Check if there are multiple solid bodies
If (pDoc.ComponentDefinition.HasMultipleSolidBodies = False) Then
' Check if its a sheetmetal part
If (pDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then
Dim oCompDefSM As SheetMetalComponentDefinition = oDoc.ComponentDefinition
'Check if unfold exists. If not try to unfold
If oCompDefSM.HasFlatPattern = False Then
'<<< VISIBLY OPENING THIS REFERENCED PART NOW >>>
oDoc = ThisApplication.Documents.Open(oDoc.FullDocumentName, True)
Dim oBaseFace As Face = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Pick 'Base Face' for Unfold")
If oBaseFace IsNot Nothing Then
Try
oCompDefSM.Unfold2(oBaseFace)
oCompDefSM.FlatPattern.ExitEdit()
Catch
'what to do if that caused an error that got suppressed
End Try
End If
Try
oDoc.Close(True) 'True = skip save when closing (just closing visibly, not fully)
Catch
End Try
End If
End If
End If
End If
Next 'oDoc
Wesley Crihfield
(Not an Autodesk Employee)
I did not know that you wanted to consider that, since there was nothing about it in the original code, and no mention of it. The A-Side Face seems to be a different property (FlatPattern.ASideFace) of the FlatPattern than the BaseFace, because it can have a BaseFace without having an A-Side Face. We can access those before the FlatPattern exists through the SheetMetalComponentDefinition.ASideDefinitions property. I assume then that after code checks if the part does not have a flat pattern, it should then check for the existence of that A-Side face, before prompting the user to select a face, and use that A-Side Face if it exists instead? If that is your intention, then we can set things up that way.
Dim doc As Document = ThisApplication.ActiveDocument
'Loop through all referenced docs in assembly
For Each oDoc As Document In doc.AllReferencedDocuments
' Check if its a part document
If oDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim pDoc As PartDocument = oDoc
' Check if there are multiple solid bodies
If (pDoc.ComponentDefinition.HasMultipleSolidBodies = False) Then
' Check if its a sheetmetal part
If (pDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then
Dim oCompDefSM As SheetMetalComponentDefinition = oDoc.ComponentDefinition
'Check if unfold exists. If not try to unfold
If oCompDefSM.HasFlatPattern = False Then
Dim oBaseFace As Face = Nothing
If oCompDefSM.ASideDefinitions.Count > 0 Then
oBaseFace = oCompDefSM.ASideDefinitions.Item(1).ASideFace
Else 'no A-Side Definitions, so have user pick a face
'<<< VISIBLY OPENING THIS REFERENCED PART NOW >>>
oDoc = ThisApplication.Documents.Open(oDoc.FullDocumentName, True)
oBaseFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Pick 'Base Face' for Unfold")
End If
If oBaseFace IsNot Nothing Then
Try
oCompDefSM.Unfold2(oBaseFace)
oCompDefSM.FlatPattern.ExitEdit()
Catch
'what to do if that caused an error that got suppressed
End Try
End If
Try
oDoc.Close(True) 'True = skip save when closing (just closing visibly, not fully)
Catch
End Try
End If
End If
End If
End If
Next 'oDoc
Wesley Crihfield
(Not an Autodesk Employee)
Hi @GosponZ. Looks like a pretty long code process with a lot of separate code routines that took a lot of time to put together. I will take your word for it that it works well, but I did not test it myself, because I'm a little short on time, and have no need for it.
Hi @ToniCoelhoE8VJF. Sure. We can break away from the original code layout, and set this up in two code routines, giving the second one a few options for how it works, to make it a bit more dynamic. A 'Main' code routine that simply deal with getting & supplying the current document and its referenced documents. And a second routine for doing the unfold task, which lets us specify if we want to use the 'A-Side' definition, if one already exists, whether we want to 'prompt user to pick face, and whether we want to create a new A-SideDefinition using the manually picked face. Once again, I have not tested this, so let me know if it works OK for you. If you do not have your iLogic Log tab open, then it would probably be a good idea to show that before running this, then set your iLogic Log level to Trace (not necessarily detailed trace), that way, if it writes anything to the iLogic Log as feedback, it will be captured, and you can look in that tab after the code is done, to see if anything was written into it. If a sheet metal part did not have a flat pattern, but was not modifiable for some reason, it writes a warning about that, to let you know. Also, if an error happens while trying to unfold one of them, the error is written to that Log, instead of a MessageBox or Msg, to speed things up.
Sub Main
Dim oDoc As Inventor.Document = ThisDoc.Document
UnFoldSheetMetalPart(oDoc, True, True, True)
For Each oRefDoc In oDoc.AllReferencedDocuments
UnFoldSheetMetalPart(oRefDoc, True, True, True)
Next
oDoc.Update2(True)
End Sub
Sub UnFoldSheetMetalPart(doc As Inventor.Document, _
Optional UseASideFaceIfAvailable As Boolean = False, _
Optional PromptForFace As Boolean = False, _
Optional CreateASideDefinition As Boolean = False)
If (doc Is Nothing) OrElse (Not TypeOf doc Is PartDocument) Then Return
Dim oPDoc As PartDocument = doc
If Not TypeOf oPDoc.ComponentDefinition Is SheetMetalComponentDefinition Then Return
Dim oSMDef As SheetMetalComponentDefinition = oPDoc.ComponentDefinition
If oSMDef.HasFlatPattern Then Return
If Not oPDoc.IsModifiable Then
Logger.Warn("Following sheet metal part with no FlatPattern was 'Not Modifiable':" _
& vbCrLf & oPDoc.DisplayName)
Return
End If
Dim oBaseFace As Face = Nothing
Dim oASideFace As Face = Nothing
Dim oNewView As Inventor.View = Nothing
Dim oASideDefs As ASideDefinitions = oSMDef.ASideDefinitions
If UseASideFaceIfAvailable = True Then
If oASideDefs.Count > 0 Then
oASideFace = oASideDefs.Item(1).ASideFace
oBaseFace = oASideFace
End If
End If
If PromptForFace = True Then
If oBaseFace Is Nothing Then
'make the part visible, and the active document
If oPDoc.Views.Count = 0 Then
oNewView = oPDoc.Views.Add()
oNewView.Activate()
Else
oPDoc.Views.Item(1).Activate()
End If
'prompt user to pick face
oBaseFace = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kPartFacePlanarFilter, "Pick 'A-Side Face'")
If oBaseFace Is Nothing Then Return
End If
If CreateASideDefinition = True Then
oASideFace = oBaseFace
'add an ASideDefinition for that face
oASideDefs.Add(oASideFace)
End If
End If
If oBaseFace Is Nothing Then
Try
oSMDef.Unfold()
Catch ex As Exception
Logger.Error("SheetMetalComponentDefinition.Unfold method error for:" & _
vbCrLf & oPDoc.DisplayName & vbCrLf & ex.ToString())
End Try
Else
Try
oSMDef.Unfold2(oBaseFace)
Catch ex As Exception
Logger.Error("SheetMetalComponentDefinition.Unfold2 method error for:" & _
vbCrLf & oPDoc.DisplayName & vbCrLf & ex.ToString())
End Try
End If
If oNewView IsNot Nothing Then oNewView.Close()
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Wesley Crihfield
(Not an Autodesk Employee)
I do design a lot of sheet metal parts using the sheet metal tools in Inventor, but I honestly rarely ever 'need' to unfold it or create a FlatPattern of it. We outsource most sheet metal part fabrication that requires complex machining &/or bending to other local companies. Since different fabrication companies can be using different tooling & production processes, the materials can get stretched or deformed in different ways, or result in slightly different internal/external radiuses in non-important places, so we leave our sheet metal settings (bend radius, kFactor, unfold rules) at (mostly) default settings, rarely include detailed flat pattern views in their drawings, and if we do, we point out that it is just for reference, and that the folded part specs are of primary concern. In other words, we don't care how they get there, as long as the result meets the finished/folded part specs, and 'our" flat pattern may not be exactly what they would need to 'cut' before bending to get there.
Because of this, I generally don't need any code based solutions for creating sheet metal flat patterns, or views of them, or DXF's of them...I just help others with their code for achieving those things because I understand most of what is involved, and like to help others when I have the time and resources to do so, while getting my other work done. I usually learn quite a bit along the way too, which is a reward of its own, as well as getting faster at throwing similar codes together later, if needed. Utilizing the custom iLogic Snippets for saving useful chunks of custom code also helps when assembling new custom codes faster, when needed. Unfortunately, I haven't done the best job of also keeping URL Links to where I first posted or copied the original code chunk to/from, so that I can refer others back to it later, instead of just posting the code again somewhere else. 🤔
Wesley Crihfield
(Not an Autodesk Employee)
