topic Re: Multibody parts in Inventor Forum

Multibody parts

chachaman — Sun, 05 Jan 2025 22:30:09 GMT

Hello,

Is there a way to callout the name of a body of a multibody part in the IDW drawings ?

For example, is there a way for teh ballon callouts to identify the body ? Can the text Annotations be made to point to the body ?

Thx

Re: Multibody parts

pcrawley — Sun, 05 Jan 2025 23:38:06 GMT

No... and yes.

Balloon looks for Part properties, so don't waste too much effort making them look for anything else. Leaders are generally the same - so neither option does what you need.

However, this old post shows how you can do what you ask: Solved: Re: Reference solid body name in balloon text? - Autodesk Community - Inventor

Since the post is approaching the Autodesk 10-year cull policy, here (for the next 10 years hopefully) is code.

Note - you need to place balloons on the drawing of the multibody (they'll all show the same value). Next select the balloons one at a time and run the rule. The balloon text should update to reflect the body name.

Sub Main() Dim oSS As SelectSet oSS = ThisApplication.ActiveDocument.SelectSet oSS.Item(1).BalloonValueSets.Item(1).OverrideValue = GetSolidName(oSS.Item(1)) End Sub Function GetSolidName(oBalloon As Balloon) As String Dim oLeader As Leader oLeader = oBalloon.Leader Dim oNode As LeaderNode Dim oModelGeom For Each oNode In oLeader.AllNodes If Not (oNode.AttachedEntity Is Nothing) oModelGeom = oNode.AttachedEntity.Geometry.ModelGeometry Exit For End If Next If oModelGeom.Type = ObjectTypeEnum.kEdgeObject oSurfaceBody = oModelGeom.Faces.Item(1).SurfaceBody Else oSurfaceBody = oModelGeom.SurfaceBody End If GetSolidName = oSurfaceBody.Name End Function

Re: Multibody parts

chachaman — Mon, 06 Jan 2025 16:18:01 GMT

Hello PCCrawley,

It's very kind of you to dig this up and present it so helpfully ! This really helped me !

All my gratitude and kindest regards ! HNY too !

Thanks again !

Re: Multibody parts

kacper.suchomski — Mon, 06 Jan 2025 18:08:20 GMT

I will add that in the case of a larger number of shapes, it is worth creating a form to have the command close to the cursor and not have to travel around the screen every time.

(view in My Videos)

Re: Multibody parts

chachaman — Mon, 06 Jan 2025 19:19:36 GMT

That's a fan tastic tip ! Thx !!

Re: Multibody parts

chachaman — Mon, 06 Jan 2025 19:43:09 GMT

Hello,

Can you tell me what seeting in the forms dialog allows you to switch focus between the form and the ballon ? Presently, when the form is displayed, I cannot select the balloon .....

Thx

Re: Multibody parts

kacper.suchomski — Mon, 06 Jan 2025 19:48:36 GMT

Please change modal setting.

https://help.autodesk.com/view/INVNTOR/2025/ENU/?guid=GUID-40B1D589-4D0C-4B46-AB52-896F0C7D78F4

Re: Multibody parts

chachaman — Mon, 06 Jan 2025 21:56:18 GMT

Thanks a million Kacper ! 😀

Re: Multibody parts

pcrawley — Mon, 06 Jan 2025 22:28:00 GMT

Ok, if it's a competition for making it easier... 😉

Modify the code as follows. Now you can select multiple balloons - then run the code - and they all change 🙂

Sub Main() Dim oSS As SelectSet oSS = ThisApplication.ActiveDocument.SelectSet Dim ObjB(oSS.Count) As Balloon NB = oSS.Count For i = 1 To oSS.Count ObjB(i)=oSS.Item(i) Logger.Debug(GetSolidName(oSS.Item(i))) Next For i = 1 To NB ObjB(i).BalloonValueSets.Item(1).OverrideValue = GetSolidName(ObjB(i)) Next End Sub Function GetSolidName(oBalloon As Balloon) As String Dim oLeader As Leader oLeader = oBalloon.Leader Dim oNode As LeaderNode Dim oModelGeom For Each oNode In oLeader.AllNodes If Not (oNode.AttachedEntity Is Nothing) oModelGeom = oNode.AttachedEntity.Geometry.ModelGeometry Exit For End If Next If oModelGeom.Type = ObjectTypeEnum.kEdgeObject oSurfaceBody = oModelGeom.Faces.Item(1).SurfaceBody Else oSurfaceBody = oModelGeom.SurfaceBody End If GetSolidName = oSurfaceBody.Name End Function

Re: Multibody parts

kacper.suchomski — Mon, 06 Jan 2025 22:34:50 GMT

I love this kind of competition 👏👏🙌

Re: Multibody parts

chachaman — Tue, 07 Jan 2025 00:05:38 GMT

Awesome !

How do I buy you a coffee !!!

Thanks

Re: Multibody parts

pcrawley — Tue, 07 Jan 2025 00:41:11 GMT

You just did 🙂

I had to do this myself once and thought about coding it - but I was too lazy and just over-rode the text manually. Today I was thrown a project where everything has been modelled as a single multi-body part - so this routine has been sooooooooooooooooooooo helpful - so thanks for making me less lazy!

Seriously though, it's a great question and probably should be a "standard feature" - like having iProperties on individual solid bodies and letting the drawing tools recognise those body-properties.