iLogic Add text under dimension
Hi @jishee,
Here is some code that will add the text "DLO" to each dimension in a drawing. You said you only want it to run for a certain "style" of dimension. What do you mean by "style" (Oridinate, baseline, or the style in the image below?
' Get the currently active file.
Dim document As Document = ThisApplication.ActiveDocument
' Get text that is added to the dimensions.
Dim EXTRA_DIMENSION_TEXT As String = "DLO"
' Check if open file is a drawing.
If document.SubType = "{BBF9FDF1-52DC-11D0-8C04-0800090BE8EC}" Then
' Get currently active file as a drawing.
Dim drawing As DrawingDocument = document
' Loop through every dimension in the active sheet in the drawing.
For Each dimension As GeneralDimension In drawing.ActiveSheet.DrawingDimensions
' Update the dimension text.
dimension.Text.FormattedText = "<DimensionValue/><br/>" & EXTRA_DIMENSION_TEXT
Next dimension
End If
Give this a try:
Dim oDoc As DrawingDocument = ThisDrawing.Document
Dim oSheet As Sheet = ActiveSheet.Sheet
For Each oDim As GeneralDimension In oSheet.DrawingDimensions.GeneralDimensions
oDim.Text.FormattedText = "<DimensionValue/><br/>DLO"
NextWesley Crihfield
(Not an Autodesk Employee)
Sorry, I hadn't updated the page in a while, or I would have seen all the previous replies.
Try this instead.
Dim oDoc As DrawingDocument = ThisDrawing.Document
Dim oSheet As Sheet = ActiveSheet.Sheet
For Each oDim As GeneralDimension In oSheet.DrawingDimensions.GeneralDimensions
If oDim.Style Is oDoc.StylesManager.DimensionStyles.Item("WW Dimension DLO") Then
oDim.Text.FormattedText = "<DimensionValue/><br/>DLO"
End If
Next
End If
Next
Wesley Crihfield
(Not an Autodesk Employee)
Hi @Anonymous. Here is some iLogic rule code that should get you pretty close to your goal. The biggest hurtle within this code left for you to deal with is the raw numbers. In iLogic, any raw numbers that are representing measurements are understood by Inventor as 'database' units. This means length interpreted in centimeters, angles in radians, mass in grams, etc. So if your raw numbers need to represent other units than those you will likely have to change your raw numbers, one way or another, to get Inventor to understand it the way you want.
I use Inches, so in my test runs of this rule, I had to specify the lower tolerance as 2.54 to get it to come out as 1 in the drawing, and 5.08 for the higher tolerance, to get it to come out as 2 in the drawing. So you may need to change those numbers to suit your preferred units. I also threw in some code for a 'Transaction', to help bundle all those actions done by the rule into one item in the 'UNDO' list, to help in cleanup if the rule doesn't do exactly what you want.
Here is the rule:
Dim oDDoc As DrawingDocument = ThisApplication.ActiveDocument
'This combines all following actions into a single entry in the 'Undo' list.
Dim oTrans As Transaction = ThisApplication.TransactionManager.StartTransaction(oDDoc, "iLogic - Edit All Dims")
Dim oGDims As GeneralDimensions = oDDoc.ActiveSheet.DrawingDimensions.GeneralDimensions
Dim oInt As Integer = 1
For Each oGDim As GeneralDimension In oGDims
Try
If oGDim.ModelValue <= 400 Then
oGDim.Tolerance.SetToSymmetric(2.54)
ElseIf oGDim.ModelValue > 400 Then
oGDim.Tolerance.SetToSymmetric(5.08)
End If
'eliminate any decimal points in the tolerance numbers
oGDim.TolerancePrecision = 0
oGDim.Text.FormattedText = "Pos " & oInt & " - <DimensionValue/>"
oInt = oInt + 1
Catch oEx As Exception
MsgBox(oEx.Message & vbCrLf & oEx.StackTrace,,"")
End Try
Next
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Wesley Crihfield
(Not an Autodesk Employee)
Hi @gatuma. When you create the dimensions using those iLogic snippet codes such as IManagedGeneralDimensions.AddLinear, they allow you to specify a name for the dimension as you create it. So, if you want to get that same dimension again later by its name, you can use the IManagedGeneralDimensions.ItemByName property, then specify its name within the () area. If the dimension you specify can be found, it will return that dimension, otherwise if it can not be found, it will throw an error. As for how to change the text within the dimension...that is often more complicated. You will need to get the 'native' object (a real GeneralDimension Inventor API object, or one of its more specific derived types), instead of the IManagedGeneralDimension type object. The real GeneralDimension type object will have many methods & properties you can access. The property you will want to focus on is its Text property, which will return a DimensionText type object. Then that DimensionText object has two different similar properties (Text & FormattedText). If the text in your dimension is just simple, static text, with no special formatting, and not 'linked' to anything, then you can likely just use the Text property to do what you want. However, if the text you have in the dimension needs to maintain any special formatting, or needs to remain 'linked' to something, then you will most likely need to deal with the FormattedText property. When dealing with the FormattedText property, its value will most likely contain some XML tags, which can make the task pretty confusing, if you are not familiar with them and how they work.
Wesley Crihfield
(Not an Autodesk Employee)