Hi, I would like to add a code that automatically puts a Annotation in my model but i cant seem to find how.
What I'm doing is measuring the flat pattern and if it goes above my recommended size, i want it to show up as a annotation. Pop-ups wont work well and are way to intrusive for this. I also want the note to get deleted when it goes under my specified value.
All the measuring and stuff I can do myself but I dont know how to call the API to make/delete Annotations.
Under the PartComponentDefinition, you should find ModelAnnotations, then depending on what type of model annotation you want, you can either go the ModelDimensions, ModelGeneralNotes, or ModelLeaderNotes (or others), then you should find options for adding one.
Wesley Crihfield
(Not an Autodesk Employee)
This code will add the note:
Dim partcompdef As PartComponentDefinition partcompdef = ThisApplication.ActiveDocument.ComponentDefinition Dim noteDef As ModelGeneralNoteDefinition = partcompdef.ModelAnnotations.ModelGeneralNotes.CreateDefinition("kaka", True) Dim onote As ModelGeneralNote = partcompdef.ModelAnnotations.ModelGeneralNotes.Add(noteDef) oNote.Name = "KAKA NOTE"
And this code will delete it:
Dim partcompdef As PartComponentDefinition partcompdef = ThisApplication.ActiveDocument.ComponentDefinition On Error Resume Next Dim oNote As ModelGeneralNote = partcompdef.ModelAnnotations.ModelGeneralNotes.Item("KAKA NOTE") 'Name of note oNote.Delete
Hope it helps! 🙂
Hi @Luisfmts
I see that... I guess it's just a bug that you cannot delete ModelGeneralNotes in Assembly Environment.
Something like this as a workaround will have to do 🙂
Dim oAsm As AssemblyDocument = ThisDoc.Document Dim odef As AssemblyComponentDefinition = oAsm.ComponentDefinition Dim selSet As SelectSet = oAsm.SelectSet selSet.Clear On Error Resume Next selSet.Select(odef.ModelAnnotations.ModelGeneralNotes.Item("KAKA NOTE")) 'Name of note ThisApplication.CommandManager.ControlDefinitions("AppDeleteCmd").Execute
Hi @ngdnam88. Here is an iLogic rule you can try for deleting all ModelGeneralNote objects from a Part or Assembly document. It can be used on either a Part or an Assembly, and can also be used as an external rule if needed.
Download my free Inventor Add-in – Hole Projector (compatible with Inventor 2021-2026) 
Sub Main
Dim oDoc As Document = ThisApplication.ActiveDocument
Dim oMA As ModelAnnotations
If oDoc.DocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
Dim oADoc As AssemblyDocument = oDoc
oMA = oADoc.ComponentDefinition.ModelAnnotations
ElseIf oDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then
Dim oPDoc As PartDocument = oDoc
oMA = oPDoc.ComponentDefinition.ModelAnnotations
Else
MsgBox("A Part or Assembly must be 'Active' for this rule to work. Exiting.", vbExclamation, "iLogic")
Exit Sub
End If
If oMA.ModelGeneralNotes.Count = 0 Then Exit Sub
For Each oMGN As ModelGeneralNote In oMA.ModelGeneralNotes
oMGN.Delete
Next
End Sub
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Wesley Crihfield
(Not an Autodesk Employee)
Hi @WCrihfield
I just tested one more times and got a problem with assembly. Please help me. Thanks,
Hi @ngdnam88
The code @WCrihfield posted works for inventor 2022. For older versions though (don't know about 2021, but at least 2020 and earlier), there's a bug when it comes to deleting annotations in assemblies. That's why I wrote a workaround for that earlier in this thread. I have modified @WCrihfield's code to use this workaround for assemblies. Hope it helps!
Sub Main Dim oDoc As Document = ThisApplication.ActiveDocument Dim oMA As ModelAnnotations If oDoc.DocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then Dim oADoc As AssemblyDocument = oDoc oMA = oADoc.ComponentDefinition.ModelAnnotations ElseIf oDoc.DocumentType = DocumentTypeEnum.kPartDocumentObject Then Dim oPDoc As PartDocument = oDoc oMA = oPDoc.ComponentDefinition.ModelAnnotations Else MsgBox("A Part or Assembly must be 'Active' for this rule to work. Exiting.", vbExclamation, "iLogic") Exit Sub End If If oMA.ModelGeneralNotes.Count = 0 Then Exit Sub If oDoc.DocumentType = DocumentTypeEnum.kAssemblyDocumentObject Dim oSelSet As SelectSet = oDoc.SelectSet Dim oCol As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection For Each oMGN As ModelGeneralNote In oMA.ModelGeneralNotes oCol.Add(oMGN) Next oSelSet.SelectMultiple(oCol) ThisApplication.CommandManager.ControlDefinitions("AppDeleteCmd").Execute Else For Each oMGN As ModelGeneralNote In oMA.ModelGeneralNotes oMGN.Delete Next End If End Sub
Hi @ngdnam88. Yes. Much like before, you just have to dig down to that ModelGeneralNote object, then change the value of its Name property to something else. The following code is just a very basic example for doing that in an assembly, which has just one ModelGeneralNote. It just had its default name before running the code, then when I ran this code, it change its name to "INFO", just like in your image.
Dim oADoc As AssemblyDocument = ThisDoc.Document
Dim oMAs As ModelAnnotations = oADoc.ComponentDefinition.ModelAnnotations
Dim oMGN As ModelGeneralNote = oMAs.ModelGeneralNotes.Item(1)
oMGN.Name = "INFO"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)
