iLogic Coding to Create Automated Drawing
You can't just shove an extra enum in there. He was probably trying to do the same thing as you and then found out he couldn't. He should have deleted that dingle berry out before publishing it.
Remember that everyone on the internet knows everything and if someone can post on a forum everything he does is perfect.
Mike (not Matt) Rattray
Unfortunate that it's not that easy 
Now I'm trying to save the drawing as I'm trying to run the rules inside of my template automatically
I need to find out how to save the document and the closing it will be pretty much the same I assume
ThisDoc.Document.Close
This will save and close the document.
ThisDoc.Document.Close(False)
This will close without saving.
ThisDoc.Document.Save
This will save without closing.
ThisDoc.Document.SaveAs(filePath & "\" & fileName & ".idw" , False)
This does a save-as without closing. This is copy/pasted out of a sub that I'm using it in where filePath and fileName are strings that hold the obvious information. In other words there are earlier in the code several lines like the following:
Dim filePath As String Dim fileName As String filePatch = "C:\temp" fileName = "temp"
You could also just replace that garble with a regular line of text like: "C:\temp\temp.idw"
I don;t remember what he False is for and it's time for me to go home.
Mike (not Matt) Rattray
Mitch,
About the options to create the view initially:
The Level of Detail will be taken directly from your model document. If you activate the LOD that you want before running the rule, that's the LOD that will be shown in the drawing views.
You can add the View Representation name to the function to create the base view:
oBaseView = oSheet.DrawingViews.AddBaseView(oPartDoc,oPoint1, 3/16,kFrontViewOrientation, kHiddenLineDrawingViewStyle, "Default")
It looks like the API doesn't provide a way to specify the options for reference components when you create a view:
Line Style = "As Parts"
Hidden Line Calculation = "All Bodies"
About the dimension error: are you looking for a DrawingDimensions object directly on the Document? It's on the Sheet instead:
oSheet.DrawingDimensions
Again, I would recommend using VBA or VB.NET to develop this code. It might take you a while to get started, but it will save you time in the long run.
Mike Deck
Software Developer
Autodesk, Inc.
Hello and welcome to Monday 
In doing some more reseach and making the changes that Mike suggested with a few extras of my own, the code and drawing have improved.
With the research I have found a way to place dimensions but the suggested way is only possible by manually pre-selecting the line then running the vba code. This worked and placed the dimension, and I understand how to manipulate this code to change the type of dimension as well as where it is placed.
But as you know, I do not wish to manually pre-select the line. Through more looking around a found a user who was looking to apply centerlines in views (which I will also need to do later on).
One of the suggested methods is to use the "ModelEdge" object. I looked in the object browser and did not find anything their myself but I could be missing something.
To me, this sounds to be exactly what I'm looking for. If I can pre-select the line by programmically calling the model edge I wish to dimension, I can run this code that dimensions the selected line.
You can find the code so far attached
The commented line "oCurve = oDrawDoc.SelectSet(1).Parent" is what was used to get the manually selected line
Here is the Centerline forum, Message 13 is the reference:
Thanks
Mitch
Mitch,
It should work if you add these lines at the top of the iLogic rule:
Imports Inventor.PointIntentEnum
Imports Inventor.DimensionTypeEnum
Lines like this are required whenever you create rules from VBA code that contains Inventor constants that start with a "k", such as kStartPointIntent. Search the Inventor API help for the constant name, and it should show you an Enum type.
Mike Deck
Software Developer
Autodesk, Inc.
Mitch,
I'm glad to hear that you found answers to most of your questions.
To return a value, you have to create a Function instead of a Sub. Here's a very simple example:
Function Average(a As Double, b As Double) As Double
Return (a + b) / 2
End Function
Sample code to call it:
av = Average(4.5, 6.2)
If that doesn't fit what you're doing, please attach your rule (or at least the part of it that gets the compile error).
Mike Deck
Software Developer
Autodesk, Inc.
Mitch,
iLogic uses VB.NET. VB.NET supports passing arguments by reference with the ByRef keyword. (& is used in C++). An example with ByRef:
Function RemoveTrailingBackslashes(ByRef strX As String) As Boolean
Dim hadBackslash As Boolean = False
While (strX.EndsWith("\"))
hadBackslash = True
strX = strX.Substring(0, strX.Length-1)
End While
Return hadBackslash
End Function
Here's some documentation: http://msdn.microsoft.com/en-us/library/c84t73c2.aspx
Mike Deck
Software Developer
Autodesk, Inc.
On this line:
oPartDoc = oPartPath + "\" + PartNumber + ".iam"
You're putting together an assembly file name, but assigning it to a part document. Do you want to open an assembly? Or is it already open and you just want to get the document?
Mike Deck
Software Developer
Autodesk, Inc.
Conversion from string "C:\Vault_Work\PROJECTS\iLogic Pa" to type 'Integer' is not valid.
This is because you're using a + instead of an &. Use &'s to combine strings. Also, what the other Mike said.
It's giving you a conversion error because it sees the +'s and thinks you're trying to do math. If you had numbers stored as strings then this would work. iLogic would convert the strings to numbers and add them up, but it fails because they're not numbers.
Mike (not Matt) Rattray