Ilogic - create drawnings of all parts from an assembly
Just dropping another link here to a case I helped out with a few years ago. Just as another example of the 4 views and an example of the view scaling and orientation. In case it might help out some.
Wesley Crihfield
(Not an Autodesk Employee)
I have an idea. If you want to be able to use this rule either from an active part document, or from an assembly, then I would make some changes at the beginning of this rule, as to how it identifies what document to target with the remainder of its code. You will want to use just one main document variable, and stick with that variable, and don't use any other references like the term 'ThisDoc' or 'ThisApplication.ActiveDocument' anywhere else within the code after that point, to make sure it is working with the exact same document identified that the beginning of the rule. Once we make these changes to that code, we will leave this rule alone. Then if we need to use it in the context of an assembly, we can call it to run from another rule that is designed for iterating though an assembly, and provide a NameValueMap to the RunExternalRuleWithArguments method with the 'target document' for it to process. Preparing this rule for receiving that 'target document' is part of this idea and can be done by accessing the RuleArguments resource.
I have attached the revised code with the proposed changes to this post as a Text file due to how long it is, and for convenience.
Wesley Crihfield
(Not an Autodesk Employee)
And here is an example of the other rule that you would use from an assembly, that will run that earlier rule on its referenced documents.
Sub Main
If ThisDoc.Document.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
MsgBox("An Assembly Document must be active for this rule to work. Exiting.", vbCritical, "")
Exit Sub
End If
Dim oADoc As AssemblyDocument = ThisDoc.Document
For Each oRefDoc As Document In oADoc.AllReferencedDocuments
Dim oArgs As NameValueMap = ThisApplication.TransientObjects.CreateNameValueMap
oArgs.Add("TargetDocument", oRefDoc)
iLogicVb.Automation.RunExternalRuleWithArguments(oRefDoc, "Create 4 View Drawing Of Model", oArgs)
Next
End SubWesley Crihfield
(Not an Autodesk Employee)
Hi,
Thank you for your help and amount of work you put in into this.
I tried running your rule with proposed changes but i get an error:
in english it says : undefined error.
I also tried running it in an assembly with the second rule you provied and i got the same error.
It starts the rule and creates an empty .idw file and then gives an error before any view is generated.
I have tried to find where and why the error occurs, and by just copying lines from code from up one by one i have found that the error shows on this line:
Dim oBaseView As DrawingView = oViews.AddBaseView(oPDoc, oOriginPoint, oFullScale, _
oViewOrientation, DrawingViewStyleEnum.kHiddenLineDrawingViewStyle)
I think I see the problem. My editing mistake. The variable 'oPDoc' being used as the first input variable in the AddBaseView method will most likely need to be changed to 'oTargetDoc'. I see that I forgot to replace "oPDoc" with "oTargetDoc" in 2 locations within the code I posted in the text file. The other location was also in a AddBaseView method, but that other line of code was left commented out. See if that fixes the code for you.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @alessandro.brandestini. In the code I posted within the text file, after the two references to the variable 'oPDoc' have been switched to 'oTargetDoc', as mentioned in my last response, you should be able to add another line of code to the end if it, as follows...just before the End Sub line.
oDDoc.SaveAs(oDrawingFullFileName, False)That 'oDrawingFullFileName' variable was established fairly early within that code, so it already contains the full file name the code was planning on using when it saved this drawing document. And we have already checked to see if that file already exists, with a question type prompt to the user if it did.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @alessandro.brandestini. The code was referring to was within a text file attached to 'Message 8' of this main forum post. But I will post just that part here in a code block for you. Before that point, I had already established the variable 'oTargetDoc' as a Document Type variable, and made sure it was either a Part or an Assembly model document. Then here I am using a Try...Catch block just to avoid any potential error in case the model document has not been saved to dist yet, because if it has not been saved yet, then accessing its FullFileName will result in an error, which will stop the code. Then I made sure it had been given a value. Then I used the ChangeExtension method to generate the expected full file name of the drawing document we want to create. Then I used the File.Exists method to check if that file already exists.
'if oTargetDoc has not been saved yet, then accessing its FullFileName will throw Error Dim oTargetDocFFN As String = "" Try oTargetDocFFN = oTargetDoc.FullFileName Catch Exit Sub End Try If oTargetDocFFN = "" Then Exit Sub 'making sure it was filled in Dim oDrawingFullFileName As String = System.IO.Path.ChangeExtension(oTargetDocFFN, ".idw") If System.IO.File.Exists(oDrawingFullFileName) Then oOverWrite = MsgBox("A Drawing for this model already exists." & vbCrLf & "Do you want to over-write it?", vbYesNo + vbQuestion, "DRAWING EXISTS!") If oOverWrite = vbNo Then Exit Sub End If.
Then after that, we have variables to hold the full file name of the drawing template we want to use, and create the variable for the drawing document itself, then use the Documents.Add method to create the new drawing, which sets the value of that drawing document variable ("oDDoc"). Then the code for measuring the model, and figuring out view orientations & scale. Then after the views have been generated, I just added the line I posted earlier:
oDDoc.SaveAs(oDrawingFullFileName, False)Then @m.rymut added a final line right after that line, but before the 'End Sub' line:
oDDoc.Close(True)to go ahead and close the drawing, so he didn't end up with a whole bunch of open drawings when processing a whole assembly.
Wesley Crihfield
(Not an Autodesk Employee)
