I'm trying to figure out a simple task.. I want to do a ball mill path on
the surface of a part..
For example, I want to mill in a + sign on a solid, using a .25"r ball mill,
with the tip only going .100" below the surface of the material. What easy
way is there to do this?
"Tom L" wrote in
I don't know if this is the easiest way or not, but this is the first thing
that comes to mind.
Make an offset plane .15" above your surface (R.25-.10 depth = .15). Make
a sketch here with a centerline, two 90° tangent arcs, and a line to close
Use Cut-Revolve 360° to make your first cut.
Start a new sketch on the same plane and due the same thing, perpindicular
to the first. Use midpoint contraints to the first sketch if that is
Depends on what you mean by "do". If it's a flat surface, G-codes are almost
as easy as modeling the cut. Insert, Cut, Sweep a flat bottomed, U-shaped
path piercing the center of a 1/4" dia profile. If the surface isn't flat,
you'll just have to draw the path to match an offset of the surface. G-codes
for that will be a bit more involved.
Create a sketch of the cross. (.500 wide 'arms')
extrude .100" into the body, 1" out of the body
uncheck 'merge result' --> ok
add .25" radius to edges/faces of cross
combine --> subract
This will leave you with a .100" deep pocket that will be created by a
.500" diameter ball end mill.
Thanks for the help, I have learned a couple things.. However, I'm still
having the problem..
For clearity, saay I want to machine a simple K in some plastic, and do it
with 3 machined lines, using a .25r ball mill, going .100" into the service.
For CNC stuff, that's basically 3 G01 statements to cut the lines, and
So, the question is, how do I do this operation in solidworks? If I have a
simple circle or something, I can cut-sweep all day, but when I get a sharp
bend or intersecting curve, it bombs out.
cschultz way was pretty cool, but if I wanted to ball mill "SOLIDWORKS
RULES" I would be there for a long long time.
I imagine having a sphere, a solid object, and then sweeping that along
the path, and subtract what it hits?
now why would you want to engrave that in anything?! Just kidding, I
really like SW. It's usually the drivers of the system that have
I taught myself that method after banging my head against my desk
trying to get a pocket created with a BEM to look right. The sweep
thing wigs out if it doubles back on itself. You will probably have to
do each leg of the 'k' as separate bodies, fillet, subtract....if you
want it to look right.
just model it as a slot, set the CNC code up like you were cutting a
slot, and then swap the tool for a BEM and call it a day, Don't spend
all day getting the model to look like what you want, spend part of the
day making the model that will yeild you the part you want. Or just
place a sketch on the top, and on the machine minus the depth value to
the z tooloffset(if in a normal 3 axis mill).
If you're engraving with a ball end mill and it's just cosmetic I
wouldn't bother to create 3D geometry for it. I used Pro/E before
solidworks and when we had to engrave we'd generate cosmetic sketches
using single line text (essentially the path of the ball end mill). A
note on the drawing would call out the desired depth and width of the
Then in Pro/NC the programmer would choose to run an engraving sequence
using the sketched text and choose a ball end mill as his tool.
This has the benefit of keeping the part simple, being fast, and
providing lines and arcs for the tool path.
So I'd suggest just sketching your text on your surface and programming
I was actually trying to create a macro for this basically the output
would be a sweep that can have intersecting geometry or a "solid sweep"
anyway I got it to work with a tool path that was in the ZX plane but
abandoned it because my wife was complaining that I didn't have a
promise to pay. I would finish it if I had a PO. If you use it much
e-mail me @
corey scheich at
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