PDA

View Full Version : Lathe tool grind w/lowest cutting force?



DICKEYBIRD
03-08-2010, 03:23 PM
I'm making 16 widgets from 1/4" 6061 for a paying job. It's a simple turn down to .236" dia x .850" long plus a bit for parting off. The deflection due to cutting forces is giving me .003" taper even after a second pass which is too much. I don't have a follow rest (yet) and don't want to center drill and use a t/s center unless nothing else works.

I'm using my homemade tangential cutter with a HSS bit which usually does great on small stuff like this. I have already made sure the tool is dead on center and sharpened well with a diamond lap. Is there a particular grind on a conventional tool that creates lower cutting forces than my tangential?

reggie_obe
03-08-2010, 03:47 PM
Aren't you using a live center? Usual rule of thumb I believe is: stickout beyond 4 x dia., needs support. A round nose would cut aluminum like butter.

DICKEYBIRD
03-08-2010, 04:49 PM
Thanks Reggie, I was trying not to use a center in the t/s due to the extra couple of ops but I may have to.

I did this job a year ago or so and don't remember having a problem then. May be that my Q.C. checks are better now than then.;)

DaHui
03-08-2010, 05:39 PM
What is the DOC of your final pass? Seems like if you crank up the rpm and take a skim cut a sharp HSS too should cut without too much deflection. How much top rake/back rake are you using? Might have to skim forward and back...

DICKEYBIRD
03-08-2010, 06:31 PM
I'm only making the one cut of about .007" as fast as my lathe will turn (around 2000 rpm) with a sharp tangential tool. It should do fine without any problems.

One thing I'm going to try tonite is another piece of stock. I forgot that I have some 1/4" hardware store gummy aluminum cr@p lying around. I may have picked that up instead of 6061.

Evan
03-08-2010, 06:48 PM
Put a foot or so of stock in the lathe centered by the tailstock. Turn it down in one pass by using a small brass plate with a hole in it clamped to the tool holder and just barely leading the tool. You could even sharpen up a stick of HSS so that the plate with hole can be clamped directly to the tool. Butter up the stock with a bit of grease.

Evan
03-08-2010, 07:13 PM
Here is the trick using a small block of walnut to steady a piece of .25 drill rod while I easily shave off a .005 DOC. Instead of following the cut it is leading the cut.

http://ixian.ca/pics7/follower.jpg

steverice
03-08-2010, 07:25 PM
Run out of wrenches?

JCD
03-08-2010, 07:31 PM
The smaller the radius on the cutting tool, the lower the cutting force. So you may consider a smaller radius on the tip of the cutting tool. Positive top rake will produce less force than negative rake. If the leading edge of the tool is perpendicular to the work, it will help. HHS will allow a sharper cutting edge than carbide, Try using a stone to smooth and sharpen the cutting edge after grinding. Slow feed rate will produce less cutting force. If you can change the work piece material to a free machining material, that will also help.

J Tiers
03-08-2010, 09:09 PM
Don't put ANY radius on the tip...... SACRILEGE, I know....

Grind a good slope straight across the end, going down towards lathe bed from left to right, and then take the end back on an angle going down from left to right when looking straight down on the tool.

Knock back the very tip to a very slight taper/relief left to right when looking down on it, for a distance of maybe 50 thou

The left edge should be STRAIGHT and perpendicular to the spindle axis.

With that tool, you can take a 3/8" rod down to 1/16" in one pass if your machine will stand the DOC, and NOT bend the 1/16" spigot.

Tip radius ALWAYS converts some of the cutting force to radial force, which reacts on the part and the tool, leading to taper, bending, etc. etc.

The straight edge "knife" tool cuts essentially ONLY with an axial force, and so has almost no tendency to form tapers, etc, etc.

here's one, not the most aggressive, but works quite well.

http://img.photobucket.com/albums/0803/jstanley/slicer1.jpg

http://img.photobucket.com/albums/0803/jstanley/slicer2.jpg

DICKEYBIRD
03-08-2010, 09:59 PM
Some GREAT tips gentlemen; thanks!:)

DICKEYBIRD
03-10-2010, 11:01 PM
Put a foot or so of stock in the lathe centered by the tailstock. Turn it down in one pass by using a small brass plate with a hole in it clamped to the tool holder and just barely leading the tool. You could even sharpen up a stick of HSS so that the plate with hole can be clamped directly to the tool. Butter up the stock with a bit of grease.I didn't use brass and I bolted it to the carriage frame instead of the toolholder but the tip worked a treat!

I cobbled up this rig from a piece of angle iron bolted to the carriage with a 1/2" thick scrap of what I think is HDPE plastic bolted to that. I then clamped a 6.5 mm drill bit (my 1/4" 6061 stock measured .255") in the collet chuck and drilled the plastic block using the carriage feed so it would be concentric with the lathe spindle. I then lubed it well with ReLion oil and let 'er rip. One small move inward with the tool to get it spot on the .236" that I needed and voila...done! All the way to the chuck. The finish iis actually better than the pic cuz' there's some oil residue on it. It's clean as a whistle after a wipe down.

Great tip Evan, thanks. I'll be using this one again.:)

http://i57.photobucket.com/albums/g227/DBAviation/EvanSteady.jpg

reggie_obe
03-11-2010, 02:10 PM
Short parts, like the one you are running are ideal for a tailstock mounted box tool. It turns to size quickly and the rollers provide great rigidity and burnish the finish as well. http://en.wikipedia.org/wiki/File:Boxtool.jpg

DICKEYBIRD
03-11-2010, 04:39 PM
Thanks for the link Reggie. I had a vague idea what box tools looked like but that clears it up.

It's not likely that I'll ever need to make a run of parts big enough to warrant ponying up for one. It sure looks expensive! I'm usually making only 8 to 12 of the little widgets I make but I'll keep an eye out for one on the cheap though.:)

JoeCB
03-11-2010, 05:05 PM
Now if you clamped a HSS bit right to the back side of your aluminum block, all set to turn the right dia you will have a dedicated "box" tool for the next time you do that job.
I milled groove and a clamp screw would do it nicely

Joe B

Evan
03-11-2010, 06:21 PM
That is actually what I suggested but whatever works is quite good enough.

reggie_obe
03-12-2010, 04:21 PM
Actually box tools, commonly used on screw machines and turret lathes can be found cheaply sometimes. Once you have one, you be surprised how much use you find for it. Of course, only useful when running multiples of the same part.

john hawkins
03-12-2010, 06:03 PM
I am looking for some box tooling to purchase. 1 inch shank. W&S bar machine.