I am not saying this is better but I can do the same in 6 lines of code.
Dim doc As DrawingDocument = ThisDoc.Document
doc.Sheets.Cast(Of Sheet).Where(Function(s) s.DrawingViews.Count = 0).ToList().ForEach(Sub(s) s.Delete())
doc.SheetFormats.Cast(Of SheetFormat).ToList().ForEach(Sub(s) s.Delete())
doc.TitleBlockDefinitions.Cast(Of TitleBlockDefinition).Where(Function(t) Not t.IsReferenced).ToList().ForEach(Sub(t) t.Delete())
doc.BorderDefinitions.Cast(Of BorderDefinition).Where(Function(b) Not b.IsReferenced And Not b.IsDefault).ToList().ForEach(Sub(b) b.Delete())
doc.SketchedSymbolDefinitions.Cast(Of SketchedSymbolDefinition).Where(Function(s) Not s.IsReferenced).ToList().ForEach(Sub(s) s.Delete())
In fact, this code is terrible. it's hard to read and very hard to debug but it works! My point: I pretend to have some knowledge but coding styles are mostly based on opinions. And like each opinion, you don't have to agree with me but take from it what you like 😉 Let's have a serious look at the code.
Lines 1, 2
On line 1 the variable "oDrawDoc" is declared. Then on line 2, the variable is set. This can be done on one line and in my opinion easier to read. If something can be done in one line and you use 2 then I consider it clutter. (But it is also possible to exaggerate this. Then you get a situation like the example above.) I also understand why people do this. Most of the example codes you will find online (and the Autodesk help files) are written voor VBa (not VB.Net/iLogic.) The issue is that combining those 2 lines was not possible in VBa therefore are most examples you find outdated. (Just like VBa is obsolete and I find it terrible onoing that Autodesk still uses creates examples based on VBa. But that's a whole other discussion...) So I can understand why people learned to code like this.
' So instead of this:
' Dim oDrawDoc As DrawingDocument
' oDrawDoc = ThisDoc.Document
' I would use:
Dim doc As DrawingDocument = ThisDoc.Document
Lines 5, 6
only in this "for each" loop items are saved in memory/variable (the "oSheets" variable). So outside of the "for each" loop. In theory, this is better because of "References" calls Instead of "Inline" Calls. This means that only 1 "References" call is made to the Inventor API and the information is saved in a variable. "Inline" calls are used In the other "for each" loop. If you do this you make a call to the inventor api each time you iterate 1 item of the list. That is not as fast as reading from memories using "References" calls. "References" calls can be almost 50% faster. (have a look at this blog post "Improving Your Program’s Performance" chapter: "Use References Instead of Inline Calls".) However for this rule that is a theoretical improvement. I guess most drawings have only a couple of sheets. So the improvement is probably only a few milliseconds. So you could argue that this is clutter because it could be done in 1 line.
' So instead of this:
' Dim oSheets As Sheets = doc.Sheets
' For Each oSheet As Sheet In oSheets
' I would use:
For Each oSheet As Sheet In doc.Sheets
Lines 13, 14
The variable oSheetFormatDef was declared on line 13 and set on line 14. This was (again) the only way in the VBa era... Same problems as I have with lines 1, 2 and I would remove the clutter.
' So instead of this:
' Dim oSheetFormatDef As SheetFormat
' For Each oSheetFormatDef In oDrawDoc.SheetFormats
' use this:
For Each oSheetFormatDef As SheetFormat In doc.SheetFormats
Line 21
Some people would argue that you should not check if a value is "False". (Especially automated coding style check tools don't like this.) You could use the "Not" keyword here. This is a pure readability issue and maybe this is something for you to consider.
' So instead of this:
' If oTitleBlock.IsReferenced = False Then
' consider using this:
If Not oTitleBlock.IsReferenced Then
Lines 21 to 23
The most annoying thing I see in code is wrongly used indentation. I know it is a pure readability thing but... (If it's done wrong, I will not understand the code until I have fixed it.)
' So instead of this:
' If Not oTitleBlock.IsReferenced Then
' oTitleBlock.Delete() ' Missing indentation here
' End If
' do this:
If Not oTitleBlock.IsReferenced Then
oTitleBlock.Delete()
End If
Line 29
I'm missing parentheses in the if statements. Also in all other if statements but here is the problem more obvious. (As far as I know, only vb.net allows this.) Using parentheses helps to read what is checked (and in which order).
' So instead of this:
' If oBorder.IsReferenced = False And oBorder.IsDefault = False Then
' use this:
If ((oBorder.IsReferenced = False) And (oBorder.IsDefault = False)) Then
Variable Naming
The last point is also an inheritance from the VBa era. In that era, the "Hungarian Notation" was popular for naming variables. (Hungarian Notation: This notation describes the variable type or purpose at the start of the variable name, followed by a descriptor that indicates the variable’s function.) That is why variables in old VBa code usually start with the "o" to indicate that it is an object. That is not the standard any more and because new coders don't know why this is done it's used wrong. For example have a look at this variable name: "oParameterValue". The type of parameter values in inventor is always double. Therefore in correct "Hungarian Notation" would be: "dParameterValue". Doing this worng could confuse readers of your code. Therefore I would suggest complying with industry standards and using camelCasing for variable. (camelCasing: Words are delimited by capital letters, except the initial word.)
Probably over kill but if you would like to look at a good industry standard for coding styles you might want to have a look at the styles from Microsoft.
Jelte de Jong
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Blog: hjalte.nl - github.com
Hi @sbalasubramanianJJDFU. There are likely several ways that could be done by code, but you can try this. It should work on either a part or assembly, but will only work on 2D sketches right now. If you need it to also delete any unused 3D sketches, some additional code would be needed.
Dim oDoc As Inventor.Document = ThisDoc.Document
If (Not TypeOf oDoc Is PartDocument) AndAlso (Not TypeOf oDoc Is AssemblyDocument) Then Return
Dim oCDef As Inventor.ComponentDefinition = oDoc.ComponentDefinition
Dim oSketches As Inventor.PlanarSketches = oCDef.Sketches
For Each oSketch As Inventor.PlanarSketch In oSketches
If (Not oSketch.Consumed) AndAlso (Not oSketch.IsOwnedByFeature) Then
Try
oSketch.Delete()
Catch
MsgBox("Error deleting Sketch named '" & oSketch.Name & "'!", vbExclamation, "iLogic")
End Try
End If
Next
oDoc.Update2(True)If this solved your problem, or answered your question, please click ACCEPT SOLUTION .
Or, if this helped you, please click (LIKE or KUDOS) 👍.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @sbalasubramanianJJDFU. I'm glad it worked OK for you. You can try this code which includes the previous code example, and also has a section of code in it for potentially deleting 'unused' WorkPlanes. We can not delete the first 3, which belong to the model's origin, so it skips those. It then checks 3 things about each other WorkPlane. Consumed, Dependents, and IsOwnedByFeature property values. Hopefully that combination of property value checks will work OK for you. Also, when we delete a WorkPlane, it asks us if we want to retain any of its 'dependents', which I am specifying False to, since we have already checked for that. I have not tested this in all conditions and situations though, so you may want to keep an eye on it, to make sure it is behaving the way you want.
Dim oDoc As Inventor.Document = ThisDoc.Document
If (Not TypeOf oDoc Is PartDocument) AndAlso (Not TypeOf oDoc Is AssemblyDocument) Then Return
Dim oCDef As Inventor.ComponentDefinition = oDoc.ComponentDefinition
Dim oSketches As Inventor.PlanarSketches = oCDef.Sketches
For Each oSketch As Inventor.PlanarSketch In oSketches
If (Not oSketch.Consumed) AndAlso (Not oSketch.IsOwnedByFeature) Then
Try
oSketch.Delete()
Catch
MsgBox("Error deleting Sketch named '" & oSketch.Name & "'!", vbExclamation, "iLogic")
End Try
End If
Next
Dim oWPlanes As WorkPlanes = oCDef.WorkPlanes
For Each oWPlane As WorkPlane In oWPlanes
If oWPlane.IsCoordinateSystemElement Then Continue For
If oWPlane.HasReferenceComponent Then Continue For 'Derived in geometry
If (Not oWPlane.Consumed) AndAlso
(oWPlane.Dependents.Count = 0) AndAlso
(Not oWPlane.IsOwnedByFeature) Then
Try
oWPlane.Delete(False) 'RetainDependents? (True/False)
Catch
MsgBox("Error deleting WorkPlane named '" & oWPlane.Name & "'!", vbExclamation, "iLogic")
End Try
End If
Next
oDoc.Update2(True)If this solved your problem, or answered your question, please click ACCEPT SOLUTION .
Or, if this helped you, please click (LIKE or KUDOS) 👍.
Wesley Crihfield
(Not an Autodesk Employee)
Type a product name
May we collect and use your data?
Learn more about the Third Party Services we use and our Privacy Statement. May we collect and use your data to tailor your experience?
Explore the benefits of a customized experience by managing your privacy settings for this site or visit our Privacy Statement to learn more about your options.
