Adding dimension constraints to a sketch

[NickBrege]

I have a couple quick questions regarding the Inventor API.  I can create a sketch rectangle using this code:

        Dim oRectangleLines As SketchEntitiesEnumerator
        oRectangleLines = oSketch.SketchLines.AddAsTwoPointRectangle(oTransGeom.CreatePoint2d(0, 0), oTransGeom.CreatePoint2d(10 * 2.54, 6 * 2.54))

Now how do I add dimension constraints to this rectangle? (both width & height)

Also, what is the default unit when creating sketch geometry?  It appears to be centimeters.  It there a way to change this, to inches for example?  Thanks...

[DRoam · Accepted solution]

Here's a link to the API page with the available DimensionConstraint.Add... methods: DimensionConstraints Object.

It appears there's not a method for adding a dimension to a line itself, so you'll have to dimension between its endpoints instead. Here's a link to the API help page for that method: DimensionConstraints.AddTwoPointDistance Method.

You can follow the "Parent Object" links to find out how to get to this method.

Based on how that method works, you'll need to get the endpoints of each line that you want to dimension. To access the lines in your new rectangle, you can use:

Dim oSketchLine As Inventor.SketchLine
oSketchLine = oRectangleLines.Item(1) 'Enter a different item number to get a different line.

Once you have a line, here's a link to the help page for the SketchLine object: SketchLine Object. You can use the StartSketchPoint and EndSketchPoint methods to get the endpoints of your line.

You'll have to do this for 2 lines. I would guess that Item(1) and Item(2) would work, but you'll have to experiment to see.

The API reference manual is extremely handy for learning how to do new things in iLogic. Here's a link to the main page: Inventor API User's Manual. I'd recommend bookmarking it. Once you get to that page, expand the "Inventor API Reference Manual" node in the tree on the left, and then expand the "Objects" node. You can then use Ctrl+F to search for terms (like "Dimension" or "Sketch") to see what objects there are, how to get to them (by following the "Parent Object" or "Accessed From" links), and what methods/properties are available for them.

Hope that helps!

[DRoam]

Oh and regarding the units, yes, the iLogic working units (referred to as the "internal database units") are centimeters, and unfortunately there's no way to change this. Certain iLogic functions use the document units (like Parameter), but some of them use the internal database units.

Not surprisingly, there's an API help page for the "UnitsOfMeasure" object which has some handy tools for working with and converting between units: UnitsOfMeasure Object.

But in general, you'll have to do exactly what you did and multiply by 2.54 when assigning an inch value to your model, or divide by 2.54 when getting one.

[NickBrege]

Thank you...

[NickBrege · Accepted solution]

I got it to work.  Here is my code ... it might help someone in the future.

        Dim oSketchLine As Inventor.SketchLine
        oSketchLine = oRectangleLines.Item(1)
        oSketch.DimensionConstraints.AddTwoPointDistance(oSketchLine.StartSketchPoint, oSketchLine.EndSketchPoint, DimensionOrientationEnum.kHorizontalDim, oTransGeom.CreatePoint2d(0, -2))
        oSketchLine = oRectangleLines.Item(4)
        oSketch.DimensionConstraints.AddTwoPointDistance(oSketchLine.StartSketchPoint, oSketchLine.EndSketchPoint, DimensionOrientationEnum.kVerticalDim, oTransGeom.CreatePoint2d(-2, 0))

Thanks again for the help...

[jewol64392]

Hi could you post the whole code including creating the rectangle with dimensioning in the sketch? Thank you

[jewol64392]

Hi could you post the whole code including creating the rectangle with dimensioning in the sketch? Thank you

[A.Acheson]

Hi @jewol64392 

Have you looked at the VBA samples in the API Help? Here is the sample for adding rectangles in VBA

the codes below are posted in descending starting with VBA sample at the bottom, conversion to VB.Net/ilogic and finally adding dimensions. 

Here is a rectangle creation with dimension constraint. It is untested so post any issues you find.

    ' Get the active part document.
    Dim partDoc As PartDocument = ThisApplication.ActiveDocument
    
	Dim partDef As PartComponentDefinition = partDoc.ComponentDefinition
    
    ' Create a new sketch.
    Dim sketch As PlanarSketch = partDef.Sketches.Add(partDef.WorkPlanes.Item(3))
    
    Dim tg As TransientGeometry = ThisApplication.TransientGeometry
   
    ' Draw rectangles by center point.
	Dim rectangleLines As SketchEntitiesEnumerator
    Dim rectangleLines = sketch.SketchLines.AddAsTwoPointCenteredRectangle(tg.CreatePoint2d(0, 0), tg.CreatePoint2d(8, 3))
   'Dim oRectangleLines = sketch.SketchLines.AddAsThreePointCenteredRectangle(tg.CreatePoint2d(20, 0), tg.CreatePoint2d(28, 3), tg.CreatePoint2d(24, 9))
	 
	 Dim recSketchLine As SketchLine 
	 recSketchLine = rectangleLines.Item(1)
     sketch.DimensionConstraints.AddTwoPointDistance(recSketchLine.StartSketchPoint, recSketchLine.EndSketchPoint, DimensionOrientationEnum.kHorizontalDim, oTransGeom.CreatePoint2d(0, -2))
     
	 recSketchLine = oRectangleLines.Item(4)
	 sketch.DimensionConstraints.AddTwoPointDistance(recSketchLine.StartSketchPoint, recSketchLine.EndSketchPoint, DimensionOrientationEnum.kVerticalDim, oTransGeom.CreatePoint2d(-2, 0))

    ThisApplication.ActiveView.Fit

Here is the VBA sample converted to VB.Net for use in ilogic editor with shortest possible method. Note you can remove all the set lines VBA required and declare and set the object variable in one line. 

    ' Get the active part document.
    Dim partDoc As PartDocument = ThisApplication.ActiveDocument
    
	Dim partDef As PartComponentDefinition = partDoc.ComponentDefinition
    
    ' Create a new sketch.
    Dim sketch As PlanarSketch = partDef.Sketches.Add(partDef.WorkPlanes.Item(3))
    
    Dim tg As TransientGeometry = ThisApplication.TransientGeometry
    
    ' Draw rectangles by center point.
    sketch.SketchLines.AddAsTwoPointCenteredRectangle(tg.CreatePoint2d(0, 0), tg.CreatePoint2d(8, 3))
    sketch.SketchLines.AddAsThreePointCenteredRectangle(tg.CreatePoint2d(20, 0), tg.CreatePoint2d(28, 3), tg.CreatePoint2d(24, 9))
    
    ThisApplication.ActiveView.Fit

Here is the VBA sample converted to VB.Net with minimum changes for use in ilogic editor

Sub Main
	SketchCreation()
End Sub

Public Sub SketchCreation()
    ' Get the active part document.
    Dim partDoc As PartDocument
	partDoc = ThisApplication.ActiveDocument
    
	Dim partDef As PartComponentDefinition
    partDef = partDoc.ComponentDefinition
    
    ' Create a new sketch.
    Dim sketch As PlanarSketch
    sketch = partDef.Sketches.Add(partDef.WorkPlanes.Item(3))
    
    Dim tg As TransientGeometry
    tg = ThisApplication.TransientGeometry
    
    ' Draw rectangles by center point.
    Call sketch.SketchLines.AddAsTwoPointCenteredRectangle(tg.CreatePoint2d(0, 0), tg.CreatePoint2d(8, 3))
    Call sketch.SketchLines.AddAsThreePointCenteredRectangle(tg.CreatePoint2d(20, 0), tg.CreatePoint2d(28, 3), tg.CreatePoint2d(24, 9))
    
    ThisApplication.ActiveView.Fit
End Sub

Here is the VBA version API Help

Public Sub SketchCreation()
    ' Get the active part document.
    Dim partDoc As PartDocument
    Set partDoc = ThisApplication.ActiveDocument
    Dim partDef As PartComponentDefinition
    Set partDef = partDoc.ComponentDefinition
    
    ' Create a new sketch.
    Dim sketch As PlanarSketch
    Set sketch = partDef.Sketches.Add(partDef.WorkPlanes.Item(3))
    
    Dim tg As TransientGeometry
    Set tg = ThisApplication.TransientGeometry
    
    ' Draw rectangles by center point.
    Call sketch.SketchLines.AddAsTwoPointCenteredRectangle(tg.CreatePoint2d(0, 0), tg.CreatePoint2d(8, 3))
    Call sketch.SketchLines.AddAsThreePointCenteredRectangle(tg.CreatePoint2d(20, 0), tg.CreatePoint2d(28, 3), tg.CreatePoint2d(24, 9))
    
    ThisApplication.ActiveView.Fit
End Sub