Insert Sketch Symbol to Snapped Dimension Point

[ngdnam88]

Dears,

I'm working in drawing that have insert some sketch symbol to dimension annotation. Is possible insert sketch symbol to green points?

Please help me how to do it with iLogic/VB.NET,

Thank very much!

[FINET_Laurent · Accepted solution]

Hi @ngdnam88,

Yes indeed, you can. Here is a small code as an exemple (make sure to change the sketched symbol name according to your sketched symbol name) :

Dim d As Inventor.DrawingDimension = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingDimensionFilter, "")
Dim p As Inventor.Point2d = d.DimensionLine.MidPoint

Dim doc As Inventor.DrawingDocument = ThisApplication.ActiveDocument
Dim s As Inventor.Sheet = doc.ActiveSheet

Dim def As Inventor.SketchedSymbolDefinition = doc.SketchedSymbolDefinitions.Item("YourSketchedSymbolName")
Dim sk As Inventor.SketchedSymbol = s.SketchedSymbols.Add(def, p)

Does this suits your need?

Kind regards,

FINET L.

[FINET_Laurent]

@ngdnam88,

You can of course get the other points like so :

Dim p As Inventor.Point2d = d.DimensionLine.MidPoint
Dim p As Inventor.Point2d = d.DimensionLine.EndPoint
Dim p As Inventor.Point2d = d.DimensionLine.StartPoint

 And so on : 

Dim p As Inventor.Point2d = d.ExtensionLineOne.MidPoint
Dim p As Inventor.Point2d = d.ExtensionLineOne.EndPoint
Dim p As Inventor.Point2d = d.ExtensionLineOne.StartPoint

Dim p As Inventor.Point2d = d.ExtensionLineTwo.MidPoint
Dim p As Inventor.Point2d = d.ExtensionLineTwo.EndPoint
Dim p As Inventor.Point2d = d.ExtensionLineTwo.StartPoint

Just pick the one you need. 😃

Kind regards,

FINET L.

[ngdnam88]

Thank you very much @FINET_Laurent 
I got it!

[ngdnam88]

Dear @FINET_Laurent 
I got problem that when move view/dimension the symbol didn't move!

How to keep symbol constrain with dimension line?
Thanks for your help!

[FINET_Laurent · Accepted solution]

Hi @ngdnam88,

Here is an article about this specific subject : How to attach sketch symbol to dimension in Inventor drawing (autodesk.com)

From this, I made this small code (from the previous code) to add a leader and make it invisible :

Dim d As Inventor.DrawingDimension = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingDimensionFilter, "")
Dim p As Inventor.Point2d = d.DimensionLine.MidPoint

Dim doc As Inventor.DrawingDocument = ThisApplication.ActiveDocument
Dim s As Inventor.Sheet = doc.ActiveSheet

Dim def As Inventor.SketchedSymbolDefinition = doc.SketchedSymbolDefinitions.Item("Boiler axis (note)")
Dim sk As Inventor.SketchedSymbol = s.SketchedSymbols.Add(def, p)

Dim g As GeometryIntent = s.CreateGeometryIntent(d, p)

Dim pc As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection
pc.Add(p)
pc.Add(g)

sk.Leader.AddLeader(pc)
sk.LeaderVisible = False

Does this suits your needs ? You can mark multiple replies as solution to a topic.

Kind regards,

FINET L.

[ngdnam88]

Supper @FINET_Laurent 
Is there any difference between normal dim and chain set dim?
I tried your code with chain set dimension, the symbol snap to the end of dim and can moveable with dim value

 How to snap to green point in chain set dimension?
Thanks,

[FINET_Laurent · Accepted solution]

Hi @ngdnam88,

Are we talking about this ?

If yes, selecting a chain dimension like this gives you a collection of dimensions. You can loop trough each of these dimensions and do the same as before. Here is an exemple :

Dim d As LinearGeneralDimension  = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingDimensionFilter, "") 'gives you a collection of dims

For Each dd As Inventor.DrawingDimension In d.ChainDimensionSet.Members 'loop trough this collection
	Dim p As Inventor.Point2d = dd.DimensionLine.MidPoint

	Dim doc As Inventor.DrawingDocument = ThisApplication.ActiveDocument
	Dim s As Inventor.Sheet = doc.ActiveSheet

	Dim def As Inventor.SketchedSymbolDefinition = doc.SketchedSymbolDefinitions.Item("Boiler axis (note)")
	Dim sk As Inventor.SketchedSymbol = s.SketchedSymbols.Add(def, p)

	Dim g As GeometryIntent = s.CreateGeometryIntent(dd, p)

	Dim pc As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection
	pc.Add(p)
	pc.Add(g)

	sk.Leader.AddLeader(pc)
	sk.LeaderVisible = False
	
Next

Does this suits your needs ? 

Kind regards,

FINET L.

[ngdnam88]

Thanks for your fast support @FINET_Laurent 
Another case, I only wanna put sketch symbol to one of chain set dimensions not at all. Is it possible?

[FINET_Laurent]

Hi @ngdnam88,

I'm not aware of a way to do this. The only thing I can see is to have the folowing workflow coded :

1. Select a chainset dimension, by clicking near the desired dimension.

2. Get the point2d of where you clicked with the mouse one 1.

3. Loop through the chainset dimensions one by one and compare with the point2d created on 2.

4. Get the closes dimension

5. Add the sketch symbol to this dimension.

To me this looks complicated, but it can be done. 

An easy fix to this issue is to use the other chainset dimensions tool that produces separate dimensions :

Thus, avoiding the issue of getting a collection of dimensions. 

Kind regards,

FINET L.