Sketch Driven Pattern if you have the points in a separate sketch
I'd create the split line first, then make sure that all the other points are in a single other sketch, converting where necessary if they aren't already. You can then use the split line you've created as the seed and the sketch with the 1000 points in it to drive the pattern. You'll then be able to recognise all the separate faces for applying load in the sim; and you should even be able to select them all just by clicking the feature.
Sketch Driven Pattern is good solution for that! Thanks.
In the meantime I made macro which imports circles into the sketch and than you just have to use this sketch in split line operation. See below:
Requiements: you have txt file with XY coordinates of points/circles. It doesnt matter if you have unit with cords or not. It works also without unit.
1. Disable "enable snapping" option (because during import points will generate in wrong positions)
2.Go into sketch mode selecting proper plane
3.run the macro
4. choose your txt file
info: in the macro below I make bold one parameter: 5 / 10000 - it's radius of your circle in metres. 5 / 10000 m = 0,5mm
Dim swApp As Object
Dim File As String
Dim DialogTitle As String
Dim InitialFileName As String
Dim FileFilter As String
Dim OpenOptions As Long
Dim ConfigName As String
Dim DisplayName As String
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
swApp.ActiveDoc.ActiveView.FrameState = 1
Dim skPoint As Object
File = swApp.GetOpenFileName("Select txt file", InitialFileName, "Text files (*.txt)|*.txt|", OpenOptions, ConfigName, DisplayName)
If File <> "" Then
Open File For Input As #1
Do While Not EOF(1)
Input #1, X, Y
Set skPoint = Part.SketchManager.CreateCircleByRadius(X / 1000, Y / 1000, "0", 5 / 10000)
'Part.ShowNamedView2 "*Isometric", 7
Are all these points that you are talking about on the same surface? Or so they span multiple surfaces and planes?
The reason that I ask is that I tried it on a part that has 2 angled surfaces with a fillet in between, and I couldn't get it to work with Iain's method.
Here is what I did:
Create a 2nd sketch and draw a circle.
Use that circle to extrude a surface body cylinder
Sketch driven pattern the cylinder using the 3dsketch of points
Run the Split line command and select intersection
Selection filter surface bodies and the box select all the surfaces you just created
Turn off selection filter and then select all the faces that the surfaces intersect
Only problem is that your cylinders won't be perpendicular to any surface that is not parallel to the original sketch face.
See the attached video:
SplitLine.mp4 6.0 MB
It's the same surface