Need Help!- Parting Off Clean Lathe

[nhatnam4]

Hi, I'm machining a custom washer on an HAAS SL20 lathe and would like to know how to part off clean (without sharp edges or burrs). It's fairly small, therefore a second op is not possible. I've tried everything -- offset part-off inserts, slower speed and feed. Please help. Is there a special part-off tool that I need or a special operation I have to do. Thanks in advance. BTW, I have very limited experience with machining.

[Geof]

You do not give any sizes, but if the bore is large enough to get in with a small threading tool try doing an internal groove at the parting position and then part down into this.

We use Iscar HeliGrip inserts for parting and by cutting the groove first we can get a small chamfer on the parted hole with a very tiny ridge around it. A quick swipe across some emery cloth and the ridge is gone.

If the hole is too tiny for doing the internal groove we use two parting tools; a carbide one to go nearly all the way down, nearly being within 5 thou or so of the piece actually parting off, then we finish with a high speed tool that has an extreme angle on it so it just slices the piece of with a burr so small it can be taken off with a quick swipe using a deburring tool.

[nhatnam4]

ID is .47 in and OD is .74 in

Material is 303 SS

What speed and feed should I use? I tried 150-600 RPM, but still get sharp burr.

[nhatnam4]

Forgot to mention, I'm using a 6 deg offset insert.

Thanks in advance for your replies.

[little bubba]

Geof has it right, drive an ID thread tool at a 45 degree angle so the point lines up with your partoff/back face. It may take a little tweaking, but the worse you will come up with is a small burr on the back face. A quick swipe on a deburring wheel or a rub on a piece of sandpaper will do ya. Best case it comes out burr free.

You didn't say a thickness, but sometimes it is actually quicker to second op. If you have a single toolchanger mill, or even a manual mill, a counterbore in softjaws and come in and touch with a countersink. Or mill some softjaws in a drill press vice, move the vise to a drill press, or hit it with a handheld drill, there are a million solutions. Depends on your situation (man hours and equipment available, quantity etc...)

[g-codeguy]

We make washers of various widths by the 10s of thousands per year. Follow Geof's advice. .47 is much bigger than some we make. For a hole that size we use the BB375SS groove bar from Tool Flo with a BNVR60 threading insert. You can use solid carbide threading bars if you're not going to be running thousands of them. Or even if you are...depending on how many bars you want to buy.

To further expand upon Geof's advice, here is how I do them. I program a .005 x 45 degree break on the backside (provided there is no break specification). Program the tool radius (keep it small...I use .003R if stoning one on) to be tangent at .003 past the O.A.L. A neutral cut-off insert will work fine. Better actually if the washer is thin. I finish turn and machine the back O.D. chamfer with a 35 deg. profile tool going to a .005 point-of-tangency past the finish O.A.L.

As stated this will leave a slight sharp edge on the O.D. Same for I.D., but if adjusted right will be burr free.

How thin is the washer? I often have to program a taper with the cut-off tool to keep it reasonably straight on thin washers. Neutral insert works better for this also. Part will mike parallel within .0005/.0007, sometimes less, but will be "bowed" from the pressure of the cut-off tool.

If anyone knows how to part off a thin washer without this "bow", I'd love to hear how it's done. Would be greatly appreciated.

EDIT: Should add that as little as .001 can make a difference on how well the I.D. looks. I've even moved my offset less than that to fine tune the threading insert. If the cut-off burr is straight down (blocking thru hole), move Z-offset minus. If the washer has a little bulge on the cut-off face, move the Z-offset plus.

[Delw]

g-codeguy
a micro 100 carbide parting tool works best, you know those ones everyone uses on screw machines, you may have to make a fixture to hold it, but the the bow in most case's is non existant with these.

[g-codeguy]

Originally Posted by Delw g-codeguy a micro 100 carbide parting tool works best, you know those ones everyone uses on screw machines, you may have to make a fixture to hold it, but the the bow in most case's is non existant with these.

Thanks for the idea. Will look into it Monday when I get back to work.

[nhatnam4]

Thickness is .063.

Sorry haven't got back to you guys -- been busy trying out your advices and other methods. I wasn't able to make it burr free even with the .005 x 45 deg break suggested by little_budda. However, I found that by adding the break and parting ~.001 after it ends a thin flimsy burr is formed, which can be easily removed when checking I.D. with a no-go gage. Burr is gone and the break serves as a nice chamfer.

BTW, speed is 500 RPM and feed is .0007.

Thanks for all your help everyone.

[g-codeguy]

Originally Posted by nhatnam4 Thickness is .063. Sorry haven't got back to you guys -- been busy trying out your advices and other methods. I wasn't able to make it burr free even with the .005 x 45 deg break suggested by little_budda. However, I found that by adding the break and parting ~.001 after it ends a thin flimsy burr is formed, which can be easily removed when checking I.D. with a no-go gage. Burr is gone and the break serves as a nice chamfer. BTW, speed is 500 RPM and feed is .0007. Thanks for all your help everyone.

Hmmm. Don't know what material you are running. I've got a 420 SS washer .115/.113 thick running at 200 SFM and F.002, and one in 52100 steel .050/.053 thick running at 300 SFM and F.002 with no burrs. I normally specify S3000 as max. RPM. Have had jobs that I ran as slow as F.001. Did run a few pieces at F.003 on the 420 SS job today, but switched back to F.002 since it was dropping off with a beautiful finish & I wasn't sure how the faster feedrate would affect tool life. Did have to program a .002 taper with the cut-off tool to maintain parallelism, tho.

Cycle time on cut-off tool must be rather long. Glad to hear that you did get it to drop off relatively burr free. As I stated in my earlier post, Z-axis stopping point for the I.D. back chamfer is critical for best results.

The 52100 washer has .005 flat on the thru hole before I chamfer it. Course QC complains that they don't see the .005 flat! Hey, can't have your cake and eat it too!

[nhatnam4]

Originally Posted by g-codeguy Hmmm. Don't know what material you are running. I've got a 420 SS washer .115/.113 thick running at 200 SFM and F.002, and one in 52100 steel .050/.053 thick running at 300 SFM and F.002 with no burrs. I normally specify S3000 as max. RPM. Have had jobs that I ran as slow as F.001. Did run a few pieces at F.003 on the 420 SS job today, but switched back to F.002 since it was dropping off with a beautiful finish & I wasn't sure how the faster feedrate would affect tool life. Did have to program a .002 taper with the cut-off tool to maintain parallelism, tho. Cycle time on cut-off tool must be rather long. Glad to hear that you did get it to drop off relatively burr free. As I stated in my earlier post, Z-axis stopping point for the I.D. back chamfer is critical for best results. The 52100 washer has .005 flat on the thru hole before I chamfer it. Course QC complains that they don't see the .005 flat! Hey, can't have your cake and eat it too!

303 SS

So you have CSS on when you're parting off? If I understand you correctly, your program reads G97 S3000 M03; G96 S200. At what diameter are you turning on CSS?

I've been using just G97 S500

[g-codeguy]

Originally Posted by nhatnam4 303 SS So you have CSS on when you're parting off? If I understand you correctly, your program reads G97 S3000 M03; G96 S200. At what diameter are you turning on CSS? I've been using just G97 S500

I have CSS on when cutting. My program reads G50S3000; G96S200. The G97 block has the correct starting RPM for the X-approach position of the c-o tool.

My program would look something like this:

G97S971M3
X1.18Z-.145M8
G50S3000
G96S300
G1X.64W#500F.002

If S3000 was throwing the parts, you could cancel the G96 about .1 (diameter) before it cuts off, and program a slower G97 spindle speed.

Thusly

G97S2046M3
X.56Z-.182M8
G50S3000
G96S300
G1X.35W#500F.002
G97X.25S1500

Generally we let them drop into the chip conveyor as long as the part isn't getting dinged rather than lengthen the cycle time. You can also slow the feedrate down on the last block if necessary.

G97X.2F.001S1500

BTW, I use 300 SFM on 303 SS with the inserts we use.

You can experiment with feedrates. I don't run a lathe much anymore. Might be able to increase the feedrate, maintain parallelism, and tool life while cutting cycle time. Problem is our guys are running 2 or 3 machines. They don't need to be worrying about an insert failing.