SetAutomatedCenterlineSettings not working
Hi @CAD_CAM_MAN. I don't really see anything wrong with the code contents, but there may be other factors influencing this behavior that the rest of us can not see. I am not that familiar with doing things through an add-in, but one thing that comes to mind is that the Sheet being worked on by that code most likely needs to be the 'active' sheet (actually visible on the screen at that time) of the 'active' document. I don't think you can apply those settings to the views on in-active sheets. But that is just one possible complication involved in the process, while there may be more. Another possible small detail that may prevent this from working correctly is if the view is not looking 100% perfectly squarely at the model, or the model is not 100% perfectly square with the view. When that is the case, the round holes may be ellipses, and the arcs may be elliptical arcs. I have seen that scenario before on multiple occasions, but don't recall the series of events that lead to that happening.
As for doing selections and command executions, in an attempt to simulate user interactions, those can be tricky to get working correctly also. Once again, the drawing would need to be the 'active' one, and that sheet that the view was on would need to be the 'active' one. But also, depending on what else may have been going on just before that section of code is acted out, you may need to ensure that the 'system focus' is on the Inventor application, instead of elsewhere. To ensure that, I used to use the simplistic AppActivate(ThisApplication.Caption) type line of code. Just throwing some thoughts around, but not sure if any of them are the real issue, if if any of them will help any.
Wesley Crihfield
(Not an Autodesk Employee)
I changed your code a bit to run as an iLogic rule.
Dim PrintDoc As DrawingDocument = ThisDoc.Document
Dim POSheet = PrintDoc.ActiveSheet
Dim BaseView As DrawingView = POSheet.DrawingViews.Item(1)
Dim ACLSettings As AutomatedCenterlineSettings = PrintDoc.DrawingSettings.AutomatedCenterlineSettings
ACLSettings.ApplyToCylinders = True
ACLSettings.ApplyToHoles = True
ACLSettings.ApplyToRevolutions = True
ACLSettings.ApplyToRectangularPatterns = True
ACLSettings.ProjectionNormalAxis = True
ACLSettings.ProjectionParallelAxis = True
BaseView.SetAutomatedCenterlineSettings(ACLSettings)This works for me. That makes me think that your code is working from line 5. Maybe you can run your code (and see if the views are created) and then run this rule.
It should add centre lines to the first view of the active sheet.
Jelte de Jong
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Blog: hjalte.nl - github.com
I did some more tests and could reproduce the problem. I could solve the problem by activating the document before adding the centerlines. So the solution in my situation is on line 12
Dim PrintDoc As DrawingDocument = ThisDoc.Document
Dim partDoc As PartDocument = ThisApplication.Documents.Open("D:\forum\bakje.ipt")
Dim BaseViewPoint As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(25, 20)
Dim BaseViewScale As Double = 0.4
Dim BaseViewOrientation As ViewOrientationTypeEnum = ViewOrientationTypeEnum.kFrontViewOrientation
Dim BaseViewStyle As DrawingViewStyleEnum = DrawingViewStyleEnum.kShadedHiddenLineDrawingViewStyle
Dim POSheet = PrintDoc.Sheets.Add()
Dim BaseView As DrawingView = POSheet.DrawingViews.AddBaseView(partDoc, BaseViewPoint, BaseViewScale, BaseViewOrientation, BaseViewStyle)
PrintDoc.Activate()
Dim ACLSettings As AutomatedCenterlineSettings = PrintDoc.DrawingSettings.AutomatedCenterlineSettings
ACLSettings.ApplyToCylinders = True
ACLSettings.ApplyToHoles = True
ACLSettings.ApplyToRevolutions = True
ACLSettings.ApplyToRectangularPatterns = True
ACLSettings.ProjectionNormalAxis = True
ACLSettings.ProjectionParallelAxis = True
BaseView.SetAutomatedCenterlineSettings(ACLSettings)
Jelte de Jong
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Blog: hjalte.nl - github.com
Just dropping a link here to another forum discussion about automated centerlines/marks back in 2021, where we encountered another problem preventing them from being added to the views as we wanted them to be. The part was cylindrical, but real hole features were used to place holes through the sides of the cylinder that were perfectly passing through the center axis of the part. There were two sets of holes which were perpendicular to each other, so that they would be 'flat' with the standard views of the part in the drawing. We even created section views of it, so that we would get the two parallel lines of the holes through the part. But that auto tool would not recognize them. Likely due to there not being true, flat, circular edges.
https://forums.autodesk.com/t5/inventor-programming-ilogic/automated-centerlines/m-p/10764592
Wesley Crihfield
(Not an Autodesk Employee)
