How to Get Model's Name on Drawing
Hi @BeKirra. Not sure if this is similar to what you want either, but here is a relatively simple iLogic rule that will first allow you to 'Pick' a drawing view, then gets the document the view is referencing, then gathers info (name, material, & mass) from it, then creates a new general note on the sheet containing that information. For additional information, parts have a material, but assemblies do not. Assemblies only contain other components, and those other components that represent parts have their own material. The only exception is when it is a weldment type assembly, where we can specify the material to use for the weld beads, or when creating 'virtual' components, where we can specify what material the virtual component should be using.
Dim oView As DrawingView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Select a Drawing View.")
If oView Is Nothing Then Return
Dim oViewDoc As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim sModelName, sMaterial, sMass As String
sModelName = System.IO.Path.GetFileName(oViewDoc.FullFileName)
If TypeOf oViewDoc Is PartDocument Then
Dim oViewPDoc As PartDocument = oViewDoc
sMaterial = oViewPDoc.ActiveMaterial.DisplayName
sMass = oViewPDoc.ComponentDefinition.MassProperties.Mass.ToString
ElseIf TypeOf oViewDoc Is AssemblyDocument Then
Dim oViewADoc As AssemblyDocument = oViewDoc
sMass = oViewADoc.ComponentDefinition.MassProperties.Mass.ToString
End If
Dim oSheet As Sheet = oView.Parent
Dim oGNotes As GeneralNotes = oSheet.DrawingNotes.GeneralNotes
Dim oPos As Point2d = ThisApplication.TransientGeometry.CreatePoint2d(5, 5)
Dim sFText As String = "Model Name = " & sModelName _
& vbCrLf & "Material = " & sMaterial _
& vbCrLf & "Mass = " & sMass
Dim oGNote As GeneralNote = oGNotes.AddFitted(oPos, sFText)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)
@BeKirra wrote:
I find a function "Model Document Name" in "Advanced Drawing API" folder in the snippets browser.
IO.Path.GetFileName(ThisDrawing.ModelDocument.FullFileName)
@BeKirra , in that same snippet folder are a couple of snippets that will allow you to work with any view to get the model that view references.
Hope that helps,
Curtis
example:
Dim viewModelDoc = ActiveSheet.View("VIEW1").ModelDocument 'get the model name sName = viewModelDoc.FullFileName MsgBox(sName) 'set an iprop value in the model viewModelDoc.PropertySets.Item("User Defined Properties").item("My iProp").Value = "Hello World"
Hi @BeKirra.
- Could you provide an example of what you would like the resulting note to look like on your drawing sheet?
- Should one note include names and information about all models represented on that sheet, or should there be a different note for each one of them?
- Would it just be a regular general text note without any leader, a leader note, a table with columns for each piece of data, and rows for each directly referenced model on that sheet, or some other type of note?
- Please explain in more detail.
- Does the data shown within the note need to be 'live' or 'linked' to the model in some way, so that when the model changes, the data in the drawing will also automatically update?
- If so, that will greatly complicate any code based solution needed to make that happen properly, if it is possible at all.
- What version/year of Inventor are you currently using?
- FYI: The 'DisplayName' of the Material that a part is currently set to is not one of the properties that we can drop into a drawing note as linked information, but Mass is. So, if we included the name of the material that a referenced part was using in a drawing note, it would be static information, instead of linked information.
Hi @chris. I don't do screen recorded videos for posting online while at work. I am already pushing the limits of my employer's grace by spending as much time as I currently do on the forums, helping others, when it was originally intended as research for improving our own automation solutions, which in turn is intended to improve productivity. Plus, it includes privacy and security related issues / policies. Plus typed text can easily be selected and translated, for those who do not speak English.
I can certainly 'get' those additional pieces of information by code, but no, it will not stay 'live' or 'linked' the way I was doing it in that example above. As I'm sure you are aware, we can manually provide a link to the Part Number and Description iProperties within drawing notes, so we can also do that by code, but it is a lot more complicated to do it by code, because it must be done through the note's FormattedText property value, which is a String that includes lots of special XML tags, and special pointers to that very specific information, in that document. However, body name and body mass are not available as pieces of information we can include a 'link' to manually within the Format Text dialog, so it can also not be included in a drawing note as 'linked' by code either, but it can be included as 'static' (will not update when the model changes) information. I have created notes in drawings by code before that included information that was 'linked' to 'the model', but since drawing automation is not really my area of focus, I do not have a lot of experience creating notes like that by code, especially when they need to include multiple linked and non-linked pieces of information, formatted in specific ways, that would only be useful to someone else. Besides the complexity the XML tags mentioned above, there can also be multiple other variables involved, that are either too complicated for me to type explanations for, or that I simply do not understand, that can make creating 'linked' notes by code even more complicated or unpredictable. Some pieces of data that can be 'linked' are considered 'derived', because there is no normal parameter or property for them, so the information they are supposed to represent is extracted on-the-fly, so it can be shown in the note, in its place. Those are specified by DerivedID numbers, instead of my their names, when creating them by code, with no Intellisense help to guide us about what is available, or possible. And some can not be included in the same drawing note as any other linked data.
Usually, when someone wants to know how to create drawing notes that include 'linked' information in them, I point them to that online help documentation page linked to above, and I also tell them to 'reverse engineer' the note. What I mean by reverse engineering the note is...create the note manually, using the very powerful, and helpful Format text dialog. Then inspect the contents of that note's FormattedText property, to see how what they did manually changed its value. Some of the stuff I see in some of those values seems a bit unpredictable, or simply undocumented, so there is not a good source of information or instructions on creating every possible variation of them by code. There could likely be an entire university course on creating drawing notes with linked information in them, and it likely could not cover all possible pieces of information, in all possible scenarios.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @BeKirra. Here is an updated version of the code I posted earlier, with most of those changes. However, this code will only gather current information and put it in a new note. It does not create a new note that contains 'links' to that information from within the view's model that would automatically update itself as the model changes. It might be possible to create a note like that, but you would have to get the model name from a different source, such as maybe Part Number or something like that, and including the links would require a longer and much more complex code.
Dim eFilter As SelectionFilterEnum = SelectionFilterEnum.kDrawingViewFilter
Dim sPrompt As String = "Select a Drawing View - or press ESC key to exit."
Dim oTG As TransientGeometry = ThisApplication.TransientGeometry
PickAgain:
Dim oView As DrawingView = Nothing
oView = ThisApplication.CommandManager.Pick(eFilter, sPrompt)
If oView Is Nothing Then Return
Dim oViewDoc As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim sModelName, sMaterial, sMass As String
sModelName = System.IO.Path.GetFileNameWithoutExtension(oViewDoc.FullFileName)
If TypeOf oViewDoc Is PartDocument Then
Dim oViewPDoc As PartDocument = oViewDoc
sMaterial = oViewPDoc.ActiveMaterial.DisplayName
sMass = Round(oViewPDoc.ComponentDefinition.MassProperties.Mass, 0).ToString & " kg"
ElseIf TypeOf oViewDoc Is AssemblyDocument Then
Dim oViewADoc As AssemblyDocument = oViewDoc
sMass = Round(oViewADoc.ComponentDefinition.MassProperties.Mass, 0).ToString & " kg"
End If
Dim oSheet As Sheet = oView.Parent
Dim oGNotes As GeneralNotes = oSheet.DrawingNotes.GeneralNotes
'point below center of view
Dim oPos As Point2d = oTG.CreatePoint2d(oView.Left + (oView.Width / 2), (oView.Top - oView.Height) -.5)
Dim sFText As String = "Model Name = " & sModelName
If sMaterial IsNot Nothing AndAlso sMaterial <> "" Then
sFText &= vbCrLf & "Material = " & sMaterial
End If
sFText &= vbCrLf & "Mass = " & sMass
Dim oGNote As GeneralNote = oGNotes.AddFitted(oPos, sFText)
GoTo PickAgain
Wesley Crihfield
(Not an Autodesk Employee)
