topic Re: Code for retrieve model Annotations in drawing in Inventor Programming Forum

Code for retrieve model Annotations in drawing

richie_rQYQ8U — Tue, 20 Feb 2024 21:32:08 GMT

Hi All,

Is there a code for retrieving model annotations in the drawing ?

Thank you

Re: Code for retrieve model Annotations in drawing

BM_Ashraf — Wed, 21 Feb 2024 08:22:18 GMT

Hi,

This is the Syntax

GeneralDimensions.Retrieve Method

Parent Object: GeneralDimensions

Description

Method that retrieves sketch and/or model dimensions into the drawing.

Syntax

GeneralDimensions.Retrieve( ViewOrSketch As Object, [DimensionsToRetrieve] As Variant ) As GeneralDimensionsEnumerator

So, You need a Drawing sheet and Drawing view

Ex.

Dim oDrawView As DrawingView = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, "Please select a View, Esc to Cancel ")
If oDrawView Is Nothing Then Exit Sub 
Dim oSheet As Sheet = oDrawView.Parent

oSheet.DrawingDimensions.GeneralDimensions.Retrieve(oDrawView)

Re: Code for retrieve model Annotations in drawing

d_bouvy — Thu, 29 Feb 2024 10:30:11 GMT

Hello,

It seems impossible to make model annotation of an assembly visible in a drawing with VBA... Is anyone know this ?

The code above put all dimensions of sketches and features, but not model annotations....

Re: Code for retrieve model Annotations in drawing

WCrihfield — Thu, 29 Feb 2024 13:16:11 GMT

Hi @d_bouvy. Have you already tried turning this setting on?

DrawingView.Include3DAnnotations

Also, if those 3D model annotations were not directly created within the main/top assembly, then you would need to dig for the 'real' ones within the components, then get a reference to their 'proxy' representations within the main/top assembly, then gather those proxy versions to be included in the drawing. The 'retrieve' process generally only works for top level stuff in the main model, not for stuff below that level.

Re: Code for retrieve model Annotations in drawing

richie_rQYQ8U — Fri, 01 Mar 2024 00:37:03 GMT

Hi Thank you for your reply,

No i didn't try that

Can you show me how to do that please?

Re: Code for retrieve model Annotations in drawing

WCrihfield — Fri, 01 Mar 2024 12:40:21 GMT

Sure. Below is a link to a similar post I responded to in a similar way about 2 years ago which contains a very basic iLogic example.

https://forums.autodesk.com/t5/inventor-programming-ilogic/retrieve-3d-dimensions-placed-on-an-assembly-in-a-drawing/m-p/10904845/highlight/true#M133892

But I can post another example here too. This example will iterate through each sheet, and each view on each sheet, setting that view property to True on each one. I believe this setting is similar to the one you see on the 'Recovery Options' tab of the Drawing View editing dialog, where there is a checkbox named 'All Model Dimensions'.

Sub Main Dim oDDoc As DrawingDocument = TryCast(ThisDoc.Document, Inventor.DrawingDocument) If oDDoc Is Nothing Then Logger.Debug(iLogicVb.RuleName & " exited (wrong DocumentType)") : Return Dim oSheets As Inventor.Sheets = oDDoc.Sheets Dim oASheet As Inventor.Sheet = oDDoc.ActiveSheet 'record originally active sheet For Each oSheet As Inventor.Sheet In oSheets oSheet.Activate Dim oViews As DrawingViews = oSheet.DrawingViews If oViews.Count = 0 Then Continue For 'skip to next sheet For Each oView As DrawingView In oViews '<<< setting that Boolean type property to True here >>> oView.Include3DAnnotations = True Next 'oView oSheet.Update Next 'oSheet 'restore originally active sheet to active again If oDDoc.ActiveSheet IsNot oASheet Then oASheet.Activate End If End Sub

At the following link, I had also responded to another similar forum post about 3 1/2 years ago where I showed a code way to simulate the manual process of retrieving model annotations in a drawing, but I generally do not recommend using a command execution and SendKeys type routine anymore, due to the inherent dangers of using the SendKeys methods (the keystrokes could potentially get sent to the wrong place, which could have an unknown effect).

https://forums.autodesk.com/t5/inventor-programming-ilogic/retrieve-model-annotations-ilogic/m-p/9753719/highlight/true#M116033

There are also other forum posts out there on this subject too, which may offer more insights, and different code examples.

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Re: Code for retrieve model Annotations in drawing

richie_rQYQ8U — Mon, 04 Mar 2024 01:06:24 GMT

thank you for your solution @WCrihfield
Good thing is the code is working
but i can use the code one time next time if i try it
it was not working

i need to double click the view to get the annotations.

Re: Code for retrieve model Annotations in drawing

d_bouvy — Mon, 11 Mar 2024 08:55:24 GMT

Hello,

Thanks, it works !

I don't know why, but with CommandManager.ControlDefinitions.Item("DrawingRetrieveDimsCmd").Execute, dimensions don't appear when I was printing in PDF.

Now it seems great with drawingview.include3Dannotations