I'm creating a variable table and want to label the dimensions by letter such as 'A', 'B', etc. I create the dimension and set the type to 'Blank', add the letter to the prefix box and then want to show the tolerance in the suffix box. I haven't found a way to stack the tolerance values inside the suffix box.
This works in a note:
When I try it in the dimension suffix box it does not work:
Solved! Go to Solution.
the only way I have found immediately is, to create a real family of part, bring the master into a draft file, build the variable family table and use the replace of variables in dimensions.
I first have defined the dim style using tolerance and after changing value to variable letter the tolerance still is kept.
Thanks for the idea Wolfgang. That works but I'm not actually using family parts built into SE. We have an external server that stores the data and the model acts as a template driven when needed to create models only when requested. I'll have to test out what happens to our process when changing it to a family of parts as I have little experience with this.
I also only defined the FOP in the master part but did not create them individually.
For creating the draft this still is enough.
But it also is no big task and work to make them real parts.
So I don't see any re
Hawcad's family of parts suggestion would have worked if my work flow didn't prohibit it as a solution. I was able to inspect what happens to the dimension when linking a family of parts variable to a draft dimension and discovered there is a text override taking place. I utilized this by writing a macro to override pre-selected dimension with text the user inputs. Here is the VB code if anyone is interested in duplicating.
Module Module1 Sub Main() Dim objApp As SolidEdgeFramework.Application = Nothing Dim objDoc As SolidEdgeDraft.DraftDocument = Nothing Dim objSet As SolidEdgeFramework.SelectSet = Nothing Dim objDim As SolidEdgeFrameworkSupport.Dimension = Nothing 'Connect to a running instance of Solid Edge. objApp = GetObject(, "SolidEdge.Application") 'Access the active document. objDoc = objApp.ActiveDocument 'Get current selected object objSet = objDoc.SelectSet If objSet.Count = 0 Then MsgBox("Nothing Selected") Exit Sub ElseIf objSet.Count > 1 Then MsgBox("More than one object selected") Exit Sub End If 'Verify user selected a dimension 'SolidEdgeFramework.ObjectType.igDimension On Error GoTo getOut objDim = objSet(0) 'Ask user for override value Dim inputString As String inputString = InputBox(Prompt:="Enter override value: ", Title:="Override Dimension", DefaultResponse:="Example: 'A'") 'Verify value was entered If inputString = "Example: 'A'" Or inputString = vbNullString Then Exit Sub End If 'Get to work 'Override value and turn off not-to-scale underline style objDim.OverrideString = inputString objDim.Style.NTSSymbol = SolidEdgeFrameworkSupport.DimNTSTypeConstants.igDimStyleNTSNone getOut: objDim = Nothing objSet = Nothing objApp = Nothing objDoc = Nothing End Sub End Module