Solidworks API: How to change Dimension text

[MikeEd]

Hello

I have been looking how to change the dimension text from within the solidworks api. I can change the value and position no problem but not the displayed text.

I am looking to get the text such as

"4 Holes<MOD-DIAM><DIM> THRU ALL"

The only values I can get is <MOD-DIAM><DIM> but I need to be able to change the comment section.

I've spent hours going through examples and the API help but I can not find a reference.

The code I have got that is accessing the dimension object is as follows. I can access the general dimension name, value, full name, tolerance details just not the dimension text.



//=============================================================
SldWorks swApp = new SldWorks();
ModelDoc2 l_Model;
DrawingDoc l_Draw;
Sheet l_Sheet;
RevisionTableAnnotation l_Revtable;
Dimension dim;
SolidWorks.Interop.sldworks.View l_View;
RevisionTableAnnotation tab;
l_Model = (ModelDoc2)swApp.OpenDoc("PartTwo.SLDDRW"
,(int) swDocumentTypes_e.swDocDRAWING);

l_Draw = (DrawingDoc)l_Model;
l_Sheet = (Sheet) l_Draw.GetCurrentSheet();
l_Revtable = l_Sheet.RevisionTable;
l_Revtable.GetColumnCustomProperty(10);
MessageBox.Show( l_Revtable.GetRevisionForId(10).ToString() );
dim = (Dimension)l_Model.Parameter("RD5@Drawing View6");
MessageBox.Show(dim.FullName);
MessageBox.Show(dim.Value.tostring());
//=============================================

 

[brengine]

Enjoy,
Ken

Option Explicit

Sub main()
   
    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swSelMgr As SldWorks.SelectionMgr
    Dim swDispDim As SldWorks.DisplayDimension
    Dim swDim As SldWorks.Dimension
    
    Dim sCurrPrefix As String
    Dim sCurrSuffix As String
    Dim sCurrCalloutAbove As String
    Dim sCurrCalloutBelow As String

    Dim sNewPrefix As String
    Dim sNewSuffix As String
    Dim sNewCalloutAbove As String
    Dim sNewCalloutBelow As String
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    
    If swModel Is Nothing Then
        MsgBox "Must have a SolidWorks document open." & Chr(13) & "Routine ending.", vbCritical, "Change Dimension Text"
        End
    End If

    If swModel.GetType <> swDocDRAWING Then
        MsgBox "Macro only works for Drawing files." & Chr(13) & "Routine ending.", vbCritical, "Change Dimension Text"
        End
    End If
    
    Set swSelMgr = swModel.SelectionManager
    
    If (swSelMgr.GetSelectedObjectType3(1, -1) = swSelDIMENSIONS) Then
        Set swDispDim = swSelMgr.GetSelectedObject6(1, 0)
        Set swDim = swDispDim.GetDimension
        
        'Current Dimension Text
        sCurrPrefix = swDispDim.GetText(swDimensionTextPrefix)
        sCurrSuffix = swDispDim.GetText(swDimensionTextSuffix)
        sCurrCalloutAbove = swDispDim.GetText(swDimensionTextCalloutAbove)
        sCurrCalloutBelow = swDispDim.GetText(swDimensionTextCalloutBelow)
        
        'New Dimension Text
        sNewPrefix = "My New Prefix "
        sNewSuffix = " My New Suffix"
        sNewCalloutAbove = "My New Callout Above"
        sNewCalloutBelow = "My New Callout Below"
        
        '*Change* Dimension Text
        swDispDim.SetText swDimensionTextPrefix, sNewPrefix
        swDispDim.SetText swDimensionTextSuffix, sNewSuffix
        swDispDim.SetText swDimensionTextCalloutAbove, sNewCalloutAbove
        swDispDim.SetText swDimensionTextCalloutBelow, sNewCalloutBelow
        
        '*Add to Current* Dimension Text
        swDispDim.SetText swDimensionTextPrefix, sCurrPrefix & sNewPrefix
        swDispDim.SetText swDimensionTextSuffix, sCurrSuffix & sNewSuffix
        swDispDim.SetText swDimensionTextCalloutAbove, sCurrCalloutAbove & sNewCalloutAbove
        swDispDim.SetText swDimensionTextCalloutBelow, sCurrCalloutBelow & sNewCalloutBelow
    End If
    
    swModel.GraphicsRedraw2
    
End Sub

 

[MikeEd]

Awesome thanks heaps. I was going in the wrong direction in use of componets by the looks of it.