I am attempting to create a "ring" of spheres. I created a single sphere and attempted the feature circular pattern, but get the error "rebuild error: select an angular dimension or a linear edge//axis/sketch entity or a cylindrical face or a conical face or a circular edge to define the pattern." I am attempting to model what is called a "micelle," layer by layer. Thanks for any assistance.
Thanks for the advice Scott. Are you saying use the circle as a "guide" for the placement of the spheres? Would that be my "circular edge" that is mentioned in the error? Thanks again.
In addition to the advice you got from Scott, make sure you select "Bodies to Pattern" (see #21 at Frequently Asked Forum Questions).
Bodies: The only way to get this to work that I know of...
That is perfect. I imagine I could do an extrude cut to halve it so it is more similar to the picture. Was this done using your suggestion for a reference circular sketch?
Well, the selecting the linear edge is solveable. Just make an referance Axis and use that. Though that will get you a cylinder pattern at best.
Can you make an excel table of the XYZ location of each of those spheres? If you can do that, you can then use the Table Driven Pattern tool to make them all.
Thanks for the incredibly quick answers. I will try to implement these when I get a chance and let you know how it turns out.
Steven Mills, I have never used the table driven patter, but am always looking to learn more. That would be great if you have some time to do that. I appreciate it.
I have and use the axis' defined in my templates.
Here's my file so you can view how I create it - very roughly thrown together.
The performance is dropped super low so it may look jagged.
Hi Joseph
I use Mesh Lab (free) to create point clouds and import into SW and sketch pattern
make sure to deselect the normal
found this macro online here
Solidworks-Using Macros to Import Points | CATI Tech Notes
Dim swApp As Object
Sub main()
Set swApp = Application.SldWorks
Set Part = swApp.ActiveDoc
swApp.ActiveDoc.ActiveView.FrameState = 1
Dim skPoints As Object
Open "C:\Users\369\Desktop\points.xyz" For Input As #1
Part.SketchManager.Insert3DSketch True
Do While Not EOF(1)
Input #1, X, Y, Z
Set skPoints = Part.SketchManager.CreatePoint(X, Y, Z)
Loop
Close #1
End Sub
Run the macro in a new part in a new assembly
Add a new sphere part and pattern
Just make sure you get the scale right, I think this is 2m across
Hi Rob
This is really cool.
You know that you can make the pattern in a part using the sketch driven pattern on the 3d sketch.
Also made point cloud with point on sphere
You gotta love sketch patterns
Amazing stuff guys!
Dave.
I smell a power user challenge coming on...
Or could that just be the double bean burrito with chili chaser you had for lunch?
Nope It's just my brain churning way too hard.
Look away or you'll go blind.
Create a reference circular sketch above all features on the tree (rollback bar to insert before). This should give you the reference to the direction desired.