Change the Style of an existing dimension

[robmatthews]

Hey there. I'm chasing the syntax on what i hope is a very simple procedure.

We have a project for re-design and manufacture here (Australia) of a machine that has been designed and detailed in one of our US offices. For this reason, we will be wanting all dimensions in mm etc, rather than inch.

My intention is to open the idw(s), update the styles library (done, i think...), change the active standard to "AS Metric" (got the code sorted for that too), and then change all dimensions to AS Metric.

So far i have each of these 3 processes in a different sub, called from a master. But my problem is in changing the style. I see in the help file that i could change a dimension's style to match that of another existing style:

Set oGeneralDimensions = oSheet.DrawingDimensions.GeneralDimensions.Item(1)

but I am having trouble setting is to the active style. What am i missing?

My module:

Sub ChangeStyle()
Dim oIDWDoc As DrawingDocument
Set oIDWDoc = ThisApplication.ActiveDocument
Dim oSheet As Sheet
Dim oDim As DrawingDimension
Dim oDimStyle As DrawingStandardStyle
Dim oGeneralDimensions As GeneralDimension

Set oDimStyle = oIDWDoc.StylesManager.ActiveStandardStyle
For Each oSheet In oIDWDoc.Sheets
For Each oDim In oSheet.DrawingDimensions
Debug.Print "Style Name and Val: " & oDim.Style.Name & " " & oDim.ModelValue
If oDim.Style.Name <> "HC - AS Metric" Then
oDim.Style = oDimStyle.Style 'This is where i am falling over... Help???
End If
Next
Next
End Sub


[Anonymous]

The problem is that you're not setting the Style
property of the dimension to a DimensionStyle object.  Here's a corrected
version of your program.

Sub ChangeStyle()
    Dim oIDWDoc
As DrawingDocument
    Set oIDWDoc =
ThisApplication.ActiveDocument
   
    Dim
oSheet As Sheet
    Dim oDim As
DrawingDimension
    Dim oDimStyle As
DrawingStandardStyle
    Dim oGeneralDimensions As
GeneralDimension
    Set oDimStyle =
oIDWDoc.StylesManager.ActiveStandardStyle
   

    For Each oSheet In
oIDWDoc.Sheets
        For Each oDim In
oSheet.DrawingDimensions
           
Debug.Print "Style Name and Val: " & oDim.style.name & " " &
oDim.ModelValue
           

            If
oDim.style.name <> "Brian" Then   '"HC - AS Metric"
Then
               
oDim.style =
oDimStyle.ActiveObjectDefaults.LinearDimensionStyle
           
End If
        Next
   
Next
End Sub
--
Brian Ekins
Autodesk Inventor API Product
Designer

href="http://blogs.autodesk.com/modthemachine">http://blogs.autodesk.com/modthemachine

[robmatthews]

Fantastic, Thanks heaps. I never would have found that!!

Now I just have to capture, retain and re-place the tolerancing...

[robmatthews]

And apparently the below is also incorrect syntax:

'snip
If oDim.Tolerance.ToleranceType <> kDefaultTolerance Then
eToleranceType = oDim.Tolerance.ToleranceType
uTol = oDim.Tolerance.Upper
lTol = oDim.Tolerance.Lower
end if
'snip: condition: change the style
oDim.Tolerance.SetToLimits(eToleranceType, uTol, lTol) 'wrong again, Rob!!

Is this the same type of mistake as before? I'm well out of my depth, aren't I?

[Anonymous]

Hi Rob,

I would need to see a specific case where this problem shows up to be sure
but I suspect it's a problem with the tolerance type. You're getting the
tolerance type from the current dimension and using that directly to create
a Limits tolerance. The type of tolerance of the dimension may not be
compatible with a limits tolerance. I think you'll need to have some more
logic to decide with Set method of the Tolerance object to use to create the
correct tolerance.

-Brian

[Anonymous]

Try adding the Call keyword to this line of code:

Call oDim.Tolerance.SetToLimits(eToleranceType, uTol, lTol)

Sanjay-

[robmatthews]

Thanks for the suggestions Brian and Sanjay. When i get back to work after my annual leave, i will investigate further.

[robmatthews]

Brian & Sanjay, great help thanks. Sanjay, the Call keyword sorted out my immediate problem, and Brian, your commented prompted me to use a select...case statement to establish implement the correct type.

So now i grabbed all the enums possible that describe the tolerence type from the Help file. (I should mention that i am stuck in dinosaur land with IV9, yes verion 9).

But i have not found that there are methods to set each type to active. Below is what i have:

31245 Basic Tolerance
31233 Standard tolerance.
31236 DeviationTolerance. Call oDim.Tolerance.SetToDeviation(uTol, lTol)
31238 LimitLinearTolerance.
31242 LimitsFitsLinearTolerance.
31243 LimitsFitsShowSizeTolerance.
31244 LimitsFitsShowTolerance.
31241 LimitsFitsStackedTolerance. Call oDim.Tolerance.SetToFits(eToleranceType, uTol, lTol) 'Something Like this? Where uTol is HoleTolerance, and lTol is ShaftTolerance
31237 LimitsStackedTolerance Call oDim.Tolerance.SetToLimits(eToleranceType, uTol, lTol)
31239 MaxTolerance. How do you set to this type?
31240 MinTolerance. How do you set to this type?
31234 Tolerance override
31246 ReferenceTolerance
31235 Symmetric tolerance. Call oDim.Tolerance.SetToSymmetric(uTol)

Cheers muchly.

[Anonymous]

Look for the various "Set" methods on the Tolerance object (use the VBA
object browser).

MaxTolerance -> SetToMax
MinTolerance -> SetToMin

Sanjay-

[robmatthews]

Thanks Sanjay, but I might be out of luck here? See my attached screenshot of the Object Browser. Would any methods in this area have been added after release9? (I'm assuming that I'm looking in the "member" column for methods that apply to the Tolerance class?)

[Anonymous]

Added in Inventor 10.

Sanjay-

[robmatthews]

Ah, I'm fresh out of luck then. But thank you for your time.

[ChristinaForest]

Hi Brian!

i try your rule but i have this error message?

and this the rule i use

Dim oIDWDoc As DrawingDocument
oIDWDoc = ThisApplication.ActiveDocument
Dim oSheet As Sheet
Dim oDim As DrawingDimension
Dim oDimStyle As DrawingStandardStyle
Dim oGeneralDimensions As GeneralDimension
oDimStyle = oIDWDoc.StylesManager.ActiveStandardStyle
For Each oSheet In oIDWDoc.Sheets
For Each oDim In oSheet.DrawingDimensions

Debug.Print ("Style Name and Val: " & oDim.style.Name & " " & oDim.ModelValue)

If oDim.style.Name <> "STD IMPERIAL (GD PRO)" Then
iProperties.Value("Custom", "test") = oDim.style.Name
oDim.Style = oDimStyle.ActiveObjectDefaults.LinearDimensionStyle
End If
Next
Next

Do you can help me?