Im looking for an inventor rule that will automate the process for adding centerline bisectors to square punches on an inventor drawing. Essential I'm looking for a rule to automate turning a drawing from this:
To this:
Is this possible? Thanks!
Automate adding centerline bisectors to drawing
Accepted solution
Hi @Anonymous. After a lot of work creating the models and punches to be able to fully test this idea, I think I finally have something that should work for you, because it worked for me in the same scenario. I created a sheet metal part that looks just like yours. Created a rectangular sheet metal punch iFeature to use for this example. Created a sketch of center points for the punch tool to use as centers. Used the Punch tool to add the single punch feature to the model tree that represented a pattern of punched holes (one for each center mark in the sketch). Then created a drawing of this part. Then created this iLogic rule to tackle this task for you. I'm using the same technique I mentioned in the other post (Centermarks.Add()), but added some additional code to help manage them, and avoid duplicates. Here's the code that I ended up with, that created the perfect looking center marks on each rectangular punch hole in the view, just as I was expecting.
Sub Main
Dim oDDoc As DrawingDocument = ThisDoc.Document
oSheet = oDDoc.ActiveSheet
oView = oSheet.DrawingViews.Item(1)
oCLs = oSheet.Centerlines
oCMs = oSheet.Centermarks
Dim oModel As PartDocument = oView.ReferencedDocumentDescriptor.ReferencedDocument
oPunch1 = oModel.ComponentDefinition.Features.Item("iFeature1:1")
oCurves = oView.DrawingCurves(oPunch1)
Dim oList As New List(Of Inventor.Centermark)
For Each oDCurve As DrawingCurve In oCurves
oIntent = oSheet.CreateGeometryIntent(oDCurve)
oCM = oCMs.Add(oIntent, True, True)
If oList.Count = 0 Then
oList.Add(oCM)
Else
Dim oFound As Boolean = False
For Each oCMk As Centermark In oList
If oCMk.Position.IsEqualTo(oCM.Position) Then
oFound = True
oCM.Delete
End If
Next
If Not oFound Then oList.Add(oCM)
End If
Next
End SubWhew... 🙂
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Wesley Crihfield
(Not an Autodesk Employee)
Well, I did run into an interesting situation when creating this. For some reason, this local rule in the drawing wasn't finding any 'iFeature' objects in the model, even though I used the 'Punch Tool' in the Sheet Metal tools of the model to create the feature, and the feature was named "iFeature1:1". I later remembered that those PunchTools are a bit harder to find, because you first have to define then dig into the 'SheetMetalComponentDefinition' object, then define and dig into the 'SheetMetalFeatures' object below that to find them. So, instead I just specified the feature by its name, which worked for my test at the time.
There are definitely some things that can be done to make this rule more robust. I updated my rule code a bit to help eliminate some potential error prone areas. Now it also loops through all views, and will also add the side profile centerlines, and add centerpoints in the ISO view (although not angled/rotated), but you can easily eliminate that loop to just process a single view if needed. I also added a Transaction in there to help control the length of the Undo list, but it doesn't appear to be working as expected yet.
Here's my updated rule code as it is now:
Sub Main
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
MsgBox("A Drawing Document must be active for this rule to work. Exiting.",vbCritical, "iLogic")
Exit Sub
End If
Dim oDDoc As DrawingDocument = ThisApplication.ActiveDocument
oSheet = oDDoc.ActiveSheet
'Dim oView As DrawingView = oDDoc.SelectSet.Item(1)
Dim oTrans As Transaction = ThisApplication.TransactionManager.StartTransaction(oDDoc, "PunchCenterPoints")
For Each oView As DrawingView In oSheet.DrawingViews
AddCentermarksToPunchToolHoles(oView)
Next
oTrans.End
End Sub
Sub AddCentermarksToPunchToolHoles(oDView As DrawingView)
If oDView.ReferencedDocumentDescriptor.ReferencedDocumentType <> DocumentTypeEnum.kPartDocumentObject Then
Exit Sub
End If
Dim oPDoc As PartDocument = oDView.ReferencedDocumentDescriptor.ReferencedDocument
If Not TypeOf oPDoc.ComponentDefinition Is SheetMetalComponentDefinition Then Exit Sub
Dim oSMDef As SheetMetalComponentDefinition = oPDoc.ComponentDefinition
Dim oSMFeats As SheetMetalFeatures = oSMDef.Features
If oSMFeats.PunchToolFeatures.Count = 0 Then Exit Sub
For Each oPunch As PunchToolFeature In oSMFeats.PunchToolFeatures
Dim oCurves As DrawingCurvesEnumerator
Try
oCurves = oDView.DrawingCurves(oPunch)
Catch
End Try
If IsNothing(oCurves) Then Continue For
If oCurves.Count = 0 Then Continue For
Dim oList As New List(Of Inventor.Centermark)
For Each oDCurve As DrawingCurve In oCurves
oIntent = oDView.Parent.CreateGeometryIntent(oDCurve)
Dim oCM As Centermark
Try
oCM = oDView.Parent.Centermarks.Add(oIntent, True, True)
Catch
Continue For
End Try
If oList.Count = 0 Then
oList.Add(oCM)
Else
Dim oFound As Boolean = False
For Each oCMk As Centermark In oList
If oCMk.Position.IsEqualTo(oCM.Position) Then
oFound = True
oCM.Delete
End If
Next
If Not oFound Then oList.Add(oCM)
End If
Next
Next
End Sub
Wesley Crihfield
(Not an Autodesk Employee)
I will attach the files I was working with, but they were created in Inventor Pro 2022.1.1, so if you're using an earlier version, they may not work for you. The attached ZIP file contains the Part (.ipt), the Drawing (.idw), and the Punch Tool (.ide). You would need to put that punch tool into your Punches folder, inside your Catalog folder, so that when you use the Punch tool, it will be able to easily find it. But there's honestly not really anything too special about it.
Wesley Crihfield
(Not an Autodesk Employee)
Maybe. It can be hard to tell, because they don't put revision notes in the online help pages that would tell you when abilities of methods or properties have changed, just the Inventor version the main method or property was first added. You would almost have to search through all the 'What's New in XXXX' version pages.
For example:
DrawingView.DrawingCurves() - version 11
Centermarks.Add() - 2009
Point2d.IsEqualTo() - 2008...etc.
Wesley Crihfield
(Not an Autodesk Employee)