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Add parentheses to dimensions via design table

Question asked by Roy Dean on Jul 30, 2020
Latest reply on Oct 21, 2020 by Alex Burnett

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I have a part file with many configurations of parts that are all "made from" another part (ie, we take a part and machine it to one match one drawing, then it goes to another process that forms the already machined part). So the drawing for the second process should have reference dimensions for the features that were added in the previous operation.

I can step through all the configs and click the "(XX)" button for all those dimensions (2019 SOLIDWORKS Help - Using Parentheses on Particular Dimensions ), but that takes a long time. Since these dimensions are already controlled by the design table, is there a way to add the parentheses via the design table?

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Kevin Chandler Jul 30, 2020 2:00 PM
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Hello,

As long as it's DT driven, you can try concatenating "(" and ")" with your dim result and then used this compiled cell as the drawing dim text
With D38 as the computed dim text, in cell E38 put the formula ="("&round(D38, 3)&")" and have the DT references cell E38 as the dim text value.

Kevin
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- Roy Dean @ Kevin Chandler on Jul 30, 2020 2:18 PM
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  Kevin, that's an interesting solution. I'll give it a try.
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  - Roy Dean @ Roy Dean on Oct 21, 2020 11:33 AM
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    Better late than never..... but this solution doesn't seem to work. Displayed text is always without the parentheses.
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    - Kevin Chandler @ Roy Dean on Oct 21, 2020 3:40 PM
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      Can you post your formulas? Or upload the DT itself?
      
      Kevin
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      - Alex Burnett @ Kevin Chandler on Oct 21, 2020 4:55 PM
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        Here is the list of valid design table parameters 2018 SOLIDWORKS Help - Summary of Design Table Parameters
        
        It doesn't look like there's a way to control the parenthesis or circle parameters for the dimensions in question. My best guess to speed things up would be an API macro.
        
        I put this together quickly just to see if it would work on my small part. It's minimally tested but it changed all of the dims in my part to reference dimensions with parenthesis. Keep in mind, it does this to every possible display dimension.
        
        Option Explicit
        Dim swApp As SldWorks.SldWorks
        Dim swModel As SldWorks.ModelDoc2
        Dim curFeature As feature
        Dim featureTypeName As String
        Dim Msg As String
        Dim Style As Variant
        Dim Title As String
        Dim indent As String
        Dim i As Integer
        Dim dispDim As DisplayDimension
        Sub main()
        
        Set swApp = Application.SldWorks
        Set swModel = swApp.ActiveDoc
        
        If swModel.GetType <> swDocPART Then
        Msg = "Only Allowed on Part" ' Define message
        Style = vbOKOnly ' OK Button only
        Title = "Error" ' Define title
        Call MsgBox(Msg, Style, Title) ' Display error message
        Exit Sub ' Exit this program
        End If
        
        AddParens swModel
        
        End Sub
        Function AddParens(m As ModelDoc2)
        
        Set curFeature = m.FirstFeature()
        Do While Not curFeature Is Nothing
        featureTypeName = curFeature.GetTypeName2()
        
        Set dispDim = curFeature.GetFirstDisplayDimension()
        Do While Not dispDim Is Nothing
        Debug.Print "F:" & curFeature.Name & " Dim: " & dispDim.GetNameForSelection()
        dispDim.ShowParenthesis = True
        Set dispDim = curFeature.GetNextDisplayDimension(dispDim)
        Loop
        
        Set curFeature = curFeature.GetNextFeature()
        Loop
        End Function
        
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Add parentheses to dimensions via design table

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