First of all I apologize if the question does not go in this section.
I'm looking to finish an object similar to a bird's nest, like this:
Doing research I found the tool "wrap", but the "branches" of the nest are not uniforms, and look like this:
How can I get the width of the branches to remain uniform? Thank you!
Hello,
Winging it w/o much info, but try:
Cheers,
Kevin
Hi Albert
Could you use a circular profile on a sweep and then get the intersection with your surface? Whilst not perfect I imagine it would be reasonably close
Just for fun I used a Design Table to produce a random data set of 3 points, which defined a plane.
Using Sketch Tools > Intersect Curve to get sweep path, I then cut the sweep with the original surface.
I then inserted all the configurations into a nest part, with this simple macro
Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Dim myFeature As SldWorks.Feature
Dim longstatus As Long, longwarnings As Long
Sub main()
Set swApp = _
Application.SldWorks
Set Part = swApp.ActiveDoc
Dim i As Integer
For i = 1 To 44
Set myFeature = Part.InsertPart2("C:\Users\369\Desktop\New folder\surface.SLDPRT", 1)
myFeature.UpdateExternalFileReferences swExternalFileReferencesNamedConfig, i, swExternalFileReferencesUpdateNone
Next
End Sub
Of course these are all separate bodies so the next stage is to combine them all
As they are mostly disjoint to each other it's best to subtract them from a solid block first
before subtracting the result from the original block
It takes a while but now we have access to just a couple of faces to offset and thicken
happy days
2016 files attached
Cheers Dave, this configuration pattern technique is pretty cool. I developed it for making curved staircases, where the normal pattern options were a bit tricky to deal with. It works in both an assembly or part, in the past I used Design Tables but I'm getting to grips with the api so hopefully I'll have something soon(ish) that will make it a lot easier
Thank you very much! I'll try to see how it goes out!
Hi Albert
Could you use a circular profile on a sweep and then get the intersection with your surface? Whilst not perfect I imagine it would be reasonably close
Just for fun I used a Design Table to produce a random data set of 3 points, which defined a plane.
Using Sketch Tools > Intersect Curve to get sweep path, I then cut the sweep with the original surface.
I then inserted all the configurations into a nest part, with this simple macro
Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Dim myFeature As SldWorks.Feature
Dim longstatus As Long, longwarnings As Long
Sub main()
Set swApp = _
Application.SldWorks
Set Part = swApp.ActiveDoc
Dim i As Integer
For i = 1 To 44
Set myFeature = Part.InsertPart2("C:\Users\369\Desktop\New folder\surface.SLDPRT", 1)
myFeature.UpdateExternalFileReferences swExternalFileReferencesNamedConfig, i, swExternalFileReferencesUpdateNone
Next
End Sub
Of course these are all separate bodies so the next stage is to combine them all
As they are mostly disjoint to each other it's best to subtract them from a solid block first
before subtracting the result from the original block
It takes a while but now we have access to just a couple of faces to offset and thicken
happy days
2016 files attached