How to Convert Normal dimension into Driven Dimension using iLogic?

[jeeva.scientist]

I want to convert "normal dimension" into the "driven dimension" & vice versa using iLogic Code.

if I have so many dimension how to I pick a specific dimension to convert.

I want to convert the,

• d0 into Driven Dimension
• d1 into Normal Dimension

[JelteDeJong]

Hi,

try running this iLogic rule and select a dimension.

Dim dimension As DimensionConstraint = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kSketchDimConstraintFilter, "Select dimension")
If dimension.Driven Then
	dimension.Driven = False
Else
	dimension.Driven = True
End If

[jeeva.scientist]

The code you gave works perfectly ( Working Proof  ), Thanks. It is not what I expected.

I sorry I did not explain my problem clearly let me explain clearly.

I don't want to pick the dimension with the mouse.

for example,

I have four dimensions,

1. d0 (normal dimension)
2. d1 (driven dimension)
3. d2 (normal dimension)
4. d3 (normal dimension)

I just want to change,

• d0 > driven dimension
• d1 > normal dimension
• d1 = d1 + (d0/2)
• d0 > normal dimension
• d1 > driven dimension

[HideoYamada]

Hello,

When the sketch is activated, You can access to the dimensions from :

ThisApplication.ActiveEditDocument.ActivatedObject.DimensionConstraints

Here ThisApplication.ActiveEditDocument.ActivatedObject is activated PlanarSketch object.

If the sketch is not activated, you must specify the sketch to edit.

For example,

Set dcs = ThisApplication.ActiveEditDocument.ComponentDefinition.Sketches(sketchNumber).DimensionConstraint

=====

Freeradical

 Hideo Yamada

[Sergio.D.Suárez]

Hello, here I show you an example of how to achieve what you want in a sketch identified as the first through the item.

Sub Convert_DimA()

    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument
    Dim oCD As ComponentDefinition
    Set oCD = oDoc.ComponentDefinition
    
    Dim oSketch As PlanarSketch
    Set oSketch = oCD.Sketches.Item(1)
    
    Dim oDim As DimensionConstraint

    For Each oDim In oSketch.DimensionConstraints
        If oDim.Parameter.Name = "d0" Then   ' Indicate the name of the parameter you want to do in the driven dimension
            oDim.Driven = True
        End If
    Next
    
End Sub

Sub Convert_DimB()

    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument
    Dim oCD As ComponentDefinition
    Set oCD = oDoc.ComponentDefinition
    
    Dim oSketch As PlanarSketch
    Set oSketch = oCD.Sketches.Item(1)
    
    Dim oDim As DimensionConstraint

    For Each oDim In oSketch.DimensionConstraints
        If oDim.Parameter.Name = "d0" Then  ' Indicate the name of the parameter you want to do not in the driven dimension
            oDim.Driven = False
        End If
    Next
    
End Sub

I hope this helps you to develop your code completely. regards

[jeeva.scientist]

Hello, thanks for your code. I made some change to suit my application. hear I attached a video, in that video, I have shown my requirement. But I did that in a long way.

I have used three separate rules to get what I need. is there a way to use just one rule to combine all three operations.

steps are,

• Enter a new value for "d1" ( when -> "d0" is driven dim & "d1" is normal dim ),now the "d0" value is driven by the "d1" value.
• In Rule0 > it converts "d1" to driven dim & "d0" to normal dim
• In Rule2 > it execute a expression (d0 = d1 * 2) 'for the new value of "d1"
• In Rule1 > it converts "d0" to driven dim & "d1" to normal dim  (reverse of Rule0, to bring it to original state)

Rule0:

	Dim oDoc As PartDocument
   	oDoc = ThisApplication.ActiveDocument
    Dim oCD As ComponentDefinition
   	oCD = oDoc.ComponentDefinition
    
    Dim oSketch As PlanarSketch
   	oSketch = oCD.Sketches.Item(1)
    
    Dim oDim As DimensionConstraint

    For Each oDim In oSketch.DimensionConstraints
        If oDim.Parameter.Name = "d1" Then   ' Indicate the name of the parameter you want to do in the driven dimension
            oDim.Driven = True
        End If
    Next
	
    For Each oDim In oSketch.DimensionConstraints
        If oDim.Parameter.Name = "d0" Then  ' Indicate the name of the parameter you want to do not in the driven dimension
            oDim.Driven = False
        End If
    Next

Rule2:

	d0 = d1 * 2
	InventorVb.DocumentUpdate()
	iLogicVb.UpdateWhenDone = True

Rule1:

	Dim oDoc As PartDocument
   	oDoc = ThisApplication.ActiveDocument
    Dim oCD As ComponentDefinition
   	oCD = oDoc.ComponentDefinition
    
    Dim oSketch As PlanarSketch
   	oSketch = oCD.Sketches.Item(1)
    
    Dim oDim As DimensionConstraint
	
	 For Each oDim In oSketch.DimensionConstraints
        If oDim.Parameter.Name = "d0" Then   ' Indicate the name of the parameter you want to do in the driven dimension
            oDim.Driven = True
        End If
    Next
	
    For Each oDim In oSketch.DimensionConstraints
        If oDim.Parameter.Name = "d1" Then  ' Indicate the name of the parameter you want to do not in the driven dimension
            oDim.Driven = False
        End If
    Next

Edit form:

Thanks for your support.

[jeeva.scientist]

Please a look at Message 6

I have used 3 different rules to make it work. 

I want to do it with just one rule.

thanks.

[jeeva.scientist · Accepted solution]

Hello,

This question has been solved by @Sergio.D.Suárez  in the other post please follow the link below.

https://forums.autodesk.com/t5/inventor-forum/how-to-convert-normal-dimension-into-driven-dimension-...

Dim oDoc As PartDocument = ThisApplication.ActiveDocument
Dim oCD As ComponentDefinition = oDoc.ComponentDefinition
Dim oSketch As PlanarSketch = oCD.Sketches.Item(1)
Dim oDim As DimensionConstraint

For Each oDim In oSketch.DimensionConstraints
    If oDim.Parameter.Name = "d1" Then oDim.Driven = True
	If oDim.Parameter.Name = "d0" Then oDim.Driven = False
Next

'd0 = d1 * 2
oCD.parameters("d0").value = oCD.parameters("d1").value *2

InventorVb.DocumentUpdate()
iLogicVb.UpdateWhenDone = True

For Each oDim In oSketch.DimensionConstraints
    If oDim.Parameter.Name = "d0" Then oDim.Driven = True
	If oDim.Parameter.Name = "d1" Then oDim.Driven = False
Next

Working proof

 

[marianYKR2R]

jeeva.scientist. Thank you very much. This is what I was looking for. Regards