Create centerline on a plate with iLogic
Hi @sbcJLYKK. Unless the mostly rectangular cutout in the middle of the part was made with a sheet metal punch tool, you are most likely not going to get a Centermark or Centerline at its center using the automated centerline settings tool. If the part was modeled centered on the origin planes, and aligned parallel/perpendicular with the origin planes you could turn the visibility of those origin planes on within the view to form the center lines similar to what you seem to be wanting. To do something like that by code you could use the DrawingView.SetIncludeStatus(oWorkPlane1) method. That will both 'include' the work plane, but also set its visibility to True.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @sbcJLYKK. Sure. Here is an example of an iLogic rule for the task I mentioned (including the two WorkPlanes in the view). In this example, I have eliminated the loop of each sheet, and eliminated the loop of each view on each sheet, because this bit of code will only work on specific views that are oriented correctly with the right two work planes. Only the two work planes that are perpendicular to the view will show properly as lines in the view. I don't clearly recall right now, but I believe that trying to include the other work plane that is flat with the view may throw an error, because it won't produce any new geometry in the view. Anyways, this example shows the basic process of how to do this specific task for a drawing view. I included several lines of comments within the code too, in order to help a bit. You may need to change the number 1 to a different number if the first view on the sheet is not the right one. Or we may need to change how we are specifying which view to target.
Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet = oDoc.ActiveSheet
'specify which view to act upon
'you will likely only want to do this with a single view
'in this example, I'm just specifying the first view that was placed on this sheet
Dim oView As DrawingView = oSheet.DrawingViews.Item(1)
'get the model document being referenced by this view
Dim oModel As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
'a generic Document doesn't have WorkPlanes, only parts & assemblies do
'so in order to maintain 'intellisense' recognition going forward
'we must identify the document's specific type, then create that type of variable
'set its value, then work from that new document variable to get the WorkPlanes
If oModel.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim oPDoc As PartDocument = oModel
Dim oWPlanes As WorkPlanes = oPDoc.ComponentDefinition.WorkPlanes
oYZPlane = oWPlanes.Item("YZ Plane")
'oXZPlane = oWPlanes.Item("XZ Plane")
oXYPlane = oWPlanes.Item("XY Plane")
'only include the two planes that are perpendicular to this view
'which ever two they may be for your case
oView.SetIncludeStatus(oYZPlane, True)
oView.SetIncludeStatus(oXYPlane, True)
End If
Wesley Crihfield
(Not an Autodesk Employee)
OK. I could not tell what the error message said, because it was in a language I don't understand, but I was able to download the part and drawing files, and open them OK. I had to modify the code very slightly, because one of the origin work planes I was using was the wrong one. So, I simply got rid of the third work plane line of code, then un-commented the second one, then fixed the one 'SetIncludeStatus' line to the correct variable. Then it worked just as planned.
Here is the exact code I used within a local iLogic rule (saved within the drawing document) and it ran perfectly for me.
Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet = oDoc.ActiveSheet
Dim oView As DrawingView = oSheet.DrawingViews.Item(1)
Dim oModel As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
If oModel.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim oPDoc As PartDocument = oModel
Dim oWPlanes As WorkPlanes = oPDoc.ComponentDefinition.WorkPlanes
oYZPlane = oWPlanes.Item("YZ Plane")
oXZPlane = oWPlanes.Item("XZ Plane")
oView.SetIncludeStatus(oYZPlane, True)
oView.SetIncludeStatus(oXZPlane, True)
End IfBecause the first DrawingView just happened to be the main front view on the drawing, and the two WorkPlanes in the model that are perpendicular to that front view in the part are the two that we want to work with here.
Wesley Crihfield
(Not an Autodesk Employee)
There are several ways to specify exactly which view you want to target, and since we usually want to do it by view name, here is the same iLogic rule that includes a way to get the view by its name. This is the long way, using Inventor API code, instead of the iLogic shortcut snippet way. It also worked just fine.
Dim oDoc As DrawingDocument = ThisDoc.Document
Dim oSheet As Sheet = oDoc.ActiveSheet
Dim oView As DrawingView
For Each oDView As DrawingView In oSheet.DrawingViews
If oDView.Name = "Front_View" Then
oView = oDView
End If
Next
If oView Is Nothing Then
MsgBox("A DrawingView named 'Front_View' was not found. Exiting rule.", vbCritical, "")
Exit Sub
End If
Dim oModel As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
If oModel.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim oPDoc As PartDocument = oModel
Dim oWPlanes As WorkPlanes = oPDoc.ComponentDefinition.WorkPlanes
oYZPlane = oWPlanes.Item("YZ Plane")
oXZPlane = oWPlanes.Item("XZ Plane")
oView.SetIncludeStatus(oYZPlane, True)
oView.SetIncludeStatus(oXZPlane, True)
End IfWesley Crihfield
(Not an Autodesk Employee)
