How to model a wire mesh basket?
How to model a wire mesh basket?
(OP)
I'm stumped and need some help. I'd like to create a 3D model of a simple basket made from hardware cloth (wire mesh). The basket has a 6 inch diam (or hex shaped) bottom with sides that come up about 1 inch. I'm looking for a clever way to model the wires on the side with the bend on the bottom, so I don't have to model each wire individually.
I can easily create the bottom wire mesh with a rectangular pattern. But then what?
Another approach is to create all the wire centerlines by intersecting a series of offset planes with a revolved surface, but how do I add ribs to each centerline?
A powercopy would work, but I think I'd have to run it for each wire.
Anyone have some ideas on how to do this?
I can easily create the bottom wire mesh with a rectangular pattern. But then what?
Another approach is to create all the wire centerlines by intersecting a series of offset planes with a revolved surface, but how do I add ribs to each centerline?
A powercopy would work, but I think I'd have to run it for each wire.
Anyone have some ideas on how to do this?





RE: How to model a wire mesh basket?
RE: How to model a wire mesh basket?
Interesting challenge
Regards
Fernando
https://picasaweb.google.com/102257836106335725208
https://picasaweb.google.com/103462806772634246699...
RE: How to model a wire mesh basket?
CODE -->
Sub CATMain() Dim documents1 As Documents Set documents1 = CATIA.Documents Dim partDocument1 As Document Set partDocument1 = documents1.Add("Part") Dim part1 As Part Set part1 = partDocument1.Part Dim bodies1 As Bodies Set bodies1 = part1.Bodies Dim body1 As Body Set body1 = bodies1.Item("PartBody") R = 5 h = 5 R1 = 1.5 WD = 0.125 SptRad = (WD / 2) * 25.4 Sep = 0.25 Dim oRelations As Relations Set oRelations = part1.Relations For j = 0 To WD Step WD Set HSF = part1.HybridShapeFactory Set P0 = HSF.AddNewPointCoord(0, 0, 0 - j) Set P1 = HSF.AddNewPointCoord(R + j, 0, 0 - j) Set P2 = HSF.AddNewPointCoord(R + j, 0, h) 'part1.Update Set hybridShapePolyline1 = HSF.AddNewPolyline() Set hybridBodies1 = part1.HybridBodies Set hybridBody1 = hybridBodies1.Add() 'hybridBody1.Name = "Geometrical Set." & j Set hybridShapes1 = hybridBody1.HybridShapes part1.InWorkObject = hybridShapes1 Set hybridShapePointCoord1 = P0 Set Reference1 = part1.CreateReferenceFromObject(hybridShapePointCoord1) hybridShapePolyline1.InsertElement Reference1, 1 Set hybridShapePointCoord2 = P1 Set Reference2 = part1.CreateReferenceFromObject(hybridShapePointCoord2) hybridShapePolyline1.InsertElement Reference2, 2 Set hybridShapePointCoord3 = P2 Set reference3 = part1.CreateReferenceFromObject(hybridShapePointCoord3) hybridShapePolyline1.InsertElement reference3, 3 If j = 0 Then hybridShapePolyline1.SetRadius 2, R1 Else hybridShapePolyline1.SetRadius 2, R2 End If Dim oRefPolyLineElement As Reference Dim oElementRadius As Length hybridShapePolyline1.GetElement 2, oRefPolyLineElement, oElementRadius hybridShapePolyline1.Closure = False hybridBody1.AppendHybridShape hybridShapePolyline1 part1.InWorkObject = hybridShapePolyline1 'part1.Update Dim Par3 As RealParam If j = 0 Then Dim Par0 As RealParam Set Par0 = part1.Parameters.CreateReal("WD", WD) Dim Par1 As RealParam Set Par1 = part1.Parameters.CreateReal("R", R) Dim Par2 As RealParam Set Par2 = part1.Parameters.CreateReal("H", h) Set Par3 = part1.Parameters.CreateReal("R1", R1) Else 'Set Par3 = part1.Parameters.CreateReal("R2", R1 + WD) End If Dim oX Set oX = P1.X Dim oX1 Set oX1 = P2.X Dim oZ Set oZ = P2.Z Dim oZ1 Set oZ1 = P1.Z Dim oZ2 Set oZ2 = P0.Z If j = 0 Then Dim oFormula1 As Formula Set oFormula1 = oRelations.CreateFormula("Diametro" & j, "Diametro Total", oX, "R*1in") Dim oFormula2 As Formula Set oFormula2 = oRelations.CreateFormula("Diam" & j, "Altura", oX1, "R*1in") Dim oFormula3 As Formula Set oFormula3 = oRelations.CreateFormula("Altura" & j, "Altura", oZ, "H*1in") Dim oFormula4 As Formula Set oFormula4 = oRelations.CreateFormula("Radio", "Radio", oElementRadius, "R1*1in") Else Set oFormula1 = oRelations.CreateFormula("Diametro" & j, "Diametro Total", oX, "(R+WD)*1in") Set oFormula2 = oRelations.CreateFormula("Diam" & j, "Altura", oX1, "(R+WD)*1in") Set oFormula3 = oRelations.CreateFormula("Altura" & j, "Altura", oZ, "H*1in") Set oFormula4 = oRelations.CreateFormula("Radio", "Radio", oElementRadius, "(R1+WD)*1in") Set oFormula5 = oRelations.CreateFormula("Altura" & j, "Altura", oZ1, "WD*-1in") Set oFormula6 = oRelations.CreateFormula("Altura" & j, "Altura", oZ2, "WD*-1in") End If 'part1.Update If j = 0 Then Set P3 = HSF.AddNewPointCoord(0, 0, 1) Dim Reference4 As Reference Set Reference4 = part1.CreateReferenceFromGeometry(P3) Dim Linea Set Linea = HSF.AddNewLinePtPt(Reference1, Reference4) Dim Reference6 As Reference Set Reference6 = part1.CreateReferenceFromGeometry(Linea) Else End If Dim Reference5 As Reference Set Reference5 = part1.CreateReferenceFromGeometry(hybridShapePolyline1) Dim Surf 'As HybridShapeRevol Set Surf = HSF.AddNewRevol(Reference5, 360, 0, Reference6) hybridBody1.AppendHybridShape Surf 'part1.Update Dim Reference7 As Reference If j = 0 Then Set ZXPlane = part1.OriginElements.PlaneZX Set Reference7 = part1.CreateReferenceFromGeometry(ZXPlane) Else Set YZPlane = part1.OriginElements.PlaneYZ Set Reference7 = part1.CreateReferenceFromGeometry(YZPlane) End If Dim Reference8 As Reference Set Reference8 = part1.CreateReferenceFromGeometry(Surf) joe = Sep For i = joe / 2 To R Step joe Set Pln = HSF.AddNewPlaneOffset(Reference7, i * 25.4, 1) Dim Reference9 As Reference Set Reference9 = part1.CreateReferenceFromGeometry(Pln) Set Inter = HSF.AddNewIntersection(Reference9, Reference8) Inter.ExtendMode = 3 hybridBody1.AppendHybridShape Inter 'Document.Part.UpdateObject Inter 'HSF.GSMVisibility Inter, 0 Dim Reference10 As Reference Set Reference10 = part1.CreateReferenceFromGeometry(Inter) Dim Swpt Set Swpt = HSF.AddNewSweepCircle(Reference10) Swpt.Mode = 6 Swpt.SetRadius 0, SptRad hybridBody1.AppendHybridShape Swpt Dim Reference11 As Reference Set Reference11 = part1.CreateReferenceFromGeometry(Swpt) If j = 0 Then part1.InWorkObject = body1 Else part1.InWorkObject = body2 End If Set SF = part1.ShapeFactory Set Clo = SF.AddNewCloseSurface(Reference11) Next i Set Mi = SF.AddNewMirror(Reference7) If j = 0 Then Set bodies2 = part1.Bodies Set body2 = part1.Bodies.Add() 'Set body1 = bodies2.Item("PartBody") part1.InWorkObject = body2 Else End If Next j part1.Update End SubThis is my intent....
and my Result....
RE: How to model a wire mesh basket?
Regards
Fernando
https://picasaweb.google.com/102257836106335725208
https://picasaweb.google.com/103462806772634246699...
RE: How to model a wire mesh basket?