Using a CNC mill as a CNC lathe.


About a year ago I had a job making three each of a number of parts. It
went smoothly except for a valve assembly component that didn't lend
itself to milling, so was turned on my only lathe, a manual without
even DRO.
Think way back to the last time you had to accurately turn a
complicated part on a manual lathe.
It ended up taking hours to make the three parts.
About a week ago I got the same job again. This time the plastic parts
were missing (already tooled for injection molding) but the quantity
was up to 12 each of the remaining 11 parts. Not looking forward to the
tedium of turning 12 of those valve parts, I decided to try turning
them in a CNC mill. It worked out very well.
I'm not a lathe guy, and I did not program this in a lathe CAM program.
I didn't program it manually either. I tricked my mill software into
doing it. Very simple really.
I changed the CAD data to make a square protrusion out of the round
section. I brought it into CAM and laid it on its side where X and Z
were reversed so operations could come from Z, even thought they'll
really be comming in from X. To keep things simple (no tool changes) I
ran the entire part with a .075" grooving tool (shut up, it worked
fine). I told the program I was milling with a .075" diameter EM.
I made flat square surfaces behind the part profile for each zone I
wanted to rough. I roughed with a simple profile program on those flat
surfaces, with a .005" step depth using the part profile as a check
surface. After roughing an area, I'd finish with a surface milling
routine. All chamfers and fillets were interpolated with the square end
grove tool. I squared up the end, made an o-ring grove and parted off
the final part with hole drilling routines.
After posting the g-code I used Notepad's "replace all" function to
swap all the Z to X, and X to Z. I put the lathe tool in a vice and the
round stock in a tool holder, zeroed out and started making parts. Part
accuracy (after one adjustment to the program) and surface finish are
good, the program took about 12 minuets to run each, unattended. I'm
sure a lathe guy could have done it in a couple minuets.
If I get adventuresome in the future, I might add multiple vices with
multiple tools.
Reply to
Polymer Man
Loading thread data ...
================= Good example of innovation and initiative in this age of cnc "canned" solutions.
Hope you got more than an "attaboy" for this.
Reply to
F. George McDuffee
Bah, 10 years ahead of you, made some spool looking parts this way for years
Reply to
yourname
You said the accuracy was good - have still got the numbers? I'd like to know, for future reference.
Hul
Polymer Man wrote:
Reply to
Hul Tytus
Get a couple of toolholders that are the same and you can make real time. Something like a pallet changer in reverse.
John
Reply to
john
===================== Another good profit making suggestion that doesn't cost anything.
Anyone writing these down????
Reply to
F. George McDuffee
Hul,
The different diameters were .375, .260, .125, .306 and .1875. There were two chamfers and two fillets and a number of shoulders. The first part was .001" oversized on all the diameters except the oring groove at.1875" which was .003" over. The tolerance was .005", so the first part met print. I adjusted my X zero .0005" and the "drill depth" for the oring and every diameter was nominal according to a pair of digital calipers (I didn't use micrometers). I had to tweak a Z dimension too. I measured the second part, a few dimensions of most parts, and I measured the last part and the repeatability was good. It was only 12 parts though.
The reason the o-ring groove was oversize relative to the rest of the part was probably deflection due to the severity of the plunge. I could have programmed a dwell perhaps, but I just plunged deeper to compensate. I suspect that dimension would have started to go out due to a dull tool sooner than others.
So the short answer is, the repeatability (and accuracy) of these 12 parts was probably around + - .001". My tolerance was + - .005 so I didn't give it any extra attention beyond that.
Reply to
Polymer Man
We have done something similar to this using a right angle head on our Proto Trak B'port. Hold the work piece in the right angle head and the tool in a vise and, Bob's your uncle, the job was done.
Errol Groff
Instructor, Manufacturing Technology H.H. Ellis Technical High School 613 Upper Maple Street Danielson, CT 06239
New England Model Engineering Society
formatting link
Reply to
Errol Groff
Thanks for the info; it does sound good. Hul
Polymer Man wrote:
Reply to
Hul Tytus
I love the creativity.
If only I can figure out how to revolve the patient while drilling the implant hole!
Charles Friedman DDS Ventura, by the Sea
Reply to
Charles Friedman

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.