No, but you can get the result you want by doing the following:
Draw a line. Use the split entities command to split the line into the desired number of segments. Select all line segments. Add an equal relation.
Why do you need a line down the center of the tube end to end? Turn on Temporary Axes. Start a 3D sketch and sketch a line. Select the line and the temporary axis in the center of the tube. Add a collinear relation.
Another way: Start a 3D sketch and sketch a line. Select one endpoint of your line. Select a circular edge at the end of your tube. Add a concentric relation. Do the same for the other endpoint and other end of the tube.
In either case if you want to constrain the endpoints of the line to the ends of the tube you can select the endpoint, then select the face or outer circular edge of the end of the tube and add a coincident relation.
'----------------------------------------- ' How to split a sketch segment into a number of equal portions ' ' Preconditions: ' 1) a part, assy or drawing is open ' ' 2) a sketch is being edited ' ' 3) a sketch segment is selected ' ' Postconditions: ' 1) sketch segment is divided into equal sections ' ' Notes: ' 1) current code calculates division points based on ' curve parameterisation NOT length. This will ' give unequal lengths for: ' splines ' parabolas ' ellipses ' ' Further Work: ' 1) support equal length division of: ' splines ' parabolas ' ellipses ' ' 2) could probably use initial display tessellation of ' pre-selected sketch segment to calculate points for ' sketch segment division
Sub main() Dim swApp As SldWorks.SldWorks Dim swModel As SldWorks.ModelDoc2 Dim swSelMgr As SldWorks.SelectionMgr Dim swSkSeg As SldWorks.SketchSegment Dim swSkLine As SldWorks.SketchLine Dim swSkArc As SldWorks.SketchArc Dim swSkEllipse As SldWorks.SketchEllipse Dim swSkSpline As SldWorks.SketchSpline Dim swSkParabola As SldWorks.SketchParabola Dim swCurve As SldWorks.Curve Dim swStartPt As SldWorks.SketchPoint Dim swEndPt As SldWorks.SketchPoint Dim vSplinePt As Variant Dim vStartPt As Variant Dim vEndPt As Variant Dim vSplitPt() As Variant Dim nStart As Double Dim nEnd As Double Dim nStartDummy As Double Dim nEndDummy As Double Dim bIsClosed As Boolean Dim bIsPeriodic As Boolean
Dim sNumSeg As String Dim nNumSeg As Long
Dim i As Long Dim bRet As Boolean
Set swApp = CreateObject("SldWorks.Application") Set swModel = swApp.ActiveDoc Set swSelMgr = swModel.SelectionManager Set swSkSeg = swSelMgr.GetSelectedObject3(1) Set swCurve = swSkSeg.GetCurve
sNumSeg = InputBox("Enter number of divisions") nNumSeg = Val(sNumSeg)
Select Case swSkSeg.GetType Case swSketchLINE Debug.Print "swSketchLINE" Set swSkLine = swSkSeg Set swStartPt = swSkLine.GetStartPoint2 Set swEndPt = swSkLine.GetEndPoint2
Case swSketchARC Debug.Print "swSketchARC" Set swSkArc = swSkSeg Set swStartPt = swSkArc.GetStartPoint2 Set swEndPt = swSkArc.GetEndPoint2
Case swSketchELLIPSE Debug.Print "swSketchELLIPSE" Set swSkEllipse = swSkSeg Set swStartPt = swSkEllipse.GetStartPoint2 Set swEndPt = swSkEllipse.GetEndPoint2
Case swSketchSPLINE Debug.Print "swSketchSPLINE" Set swSkSpline = swSkSeg
vSplinePt = swSkSpline.GetPoints2
Set swStartPt = vSplinePt(0) Set swEndPt = vSplinePt(UBound(vSplinePt))
Case swSketchPARABOLA Debug.Print "swSketchPARABOLA" Set swSkParabola = swSkSeg Set swStartPt = swSkParabola.GetStartPoint2 Set swEndPt = swSkParabola.GetEndPoint2 End Select
I gave it a try using the weldment functionality and it was extremely easy to model. All it took was two 3D sketches, insert the structural members, trim the ends as you want, create a circular pattern of the braces and you are done.
You're not supposed to post images in this group. If you do, many of the news servers will strip them out, so most of us don't see them. You did it the right way, posting it some place that we can go to see it.
Jerry Steiger Tripod Data Systems "take the garbage out, dear"
email@example.com (Hendrik) wrote in messag news:..
I gave it a try using the weldment functionality and it was extremel easy to model. All it took was two 3D sketches, insert th structura members, trim the ends as you want, create a circular pattern of th braces and you are done.[/quote:bb936a6a64
that's good to hear mike
but i have never heard of the weldment functionality, could u describ how u made the truss (in a detailed way), or sent the file to m email-adres many thank