center of mass revisited

Is there a way to use the center of mass coordinates to create a point
that will be dynanically updated (new CG) each time that the geometry
of my part or solid bodie would change?
I know this has been posted before but perhaps there have been
enhancements that may change the way this can be done. It would be
great to be able to do this without VB.
Thanks for your help.
Reply to
Loading thread data ...
Here's the text of a macro that inserts a point at the CG, and updates it every time the macro is run. To have this update on every rebuild, you would need to re-implement this as a macro feature. There is no way to do this other than manually or with programming.
Beware word wrap:
' *********************************************************************** ******* ' C:\DOCUME~1\dshoebri\LOCALS~1\Temp\swx284\Macro1.swb - macro ' recorded on 07/12/02 by Dshoebri ' *********************************************************************** *******
Dim swApp As Object Dim objDoc As Object Dim status As Long Dim CG_3DSketch As Object Dim objNewPoint As Object Dim ObjSelectionMgr As Object Dim objSketchToRename As Object Dim objCG_Point As Object Dim objSketch As Object Dim objSketchPoint As Object
Sub main() Set swApp = CreateObject("SldWorks.Application") Set objDoc = swApp.ActiveDoc MassProperties = objDoc.GetMassProperties2(status) On Error Resume Next X_pt = MassProperties(0) If Err 0 Then X_pt = 0 Y_pt = 0 Z_pt = 0 Else Y_pt = MassProperties(1) Z_pt = MassProperties(2) End If On Error GoTo 0
CG_3DSketch_Name = "Center-Of-Gravity" Set CG_3DSketch = objDoc.FeatureByName(CG_3DSketch_Name) On Error Resume Next Junk = CG_3DSketch.Name If Err 0 Then On Error GoTo 0 objDoc.Insert3DSketch objDoc.CreatePoint2 X_pt, Y_pt, Z_pt objDoc.Insert3DSketch Set objNewPoint = objDoc.FeatureByPositionReverse(0) objDoc.FeatureByPositionReverse(0).Name = CG_3DSketch_Name Set objNewPoint = objDoc.FeatureByPositionReverse(0) objDoc.EditRebuild Else On Error GoTo 0 objDoc.SelectById CG_3DSketch_Name, "SKETCH", 0, 0, 0 objDoc.EditSketch Set objSketch = objDoc.GetActiveSketch2 SketchPointArray = objSketch.GetSketchPoints PointCount = UBound(SketchPointArray) + 1 For i = 0 To (PointCount - 1) Set objSketchPoint = SketchPointArray(i) Junk = objSketchPoint.SetCoords(X_pt, Y_pt, Z_pt) Next i objDoc.EditRebuild End If End Sub
Reply to
Dale Dunn
Dale Dunn wrote:
Reply to
I have one written by someone else that does almost the same thing, only it doesn't update the existing point - it either puts a new point in the existing sketch, or if you have renamed that sketch, it adds another sketch. I can see benefits to both. Maybe merge the two together with options?
Reply to
Wayne Tiffany

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.