PDA

View Full Version : Need Help! Single pointing 304 SS.... destroying tools!!



PoiToi
05-13-2008, 01:31 PM
hey all, i was wondering if anyone could help me out.
i have to single point a #6-32 thread on the OD of a 304 ss part, and its giving me TONS of grief. the insert nose is chipping out on the first part, and it seems to be forming the material, making the thread major diameter way oversize(.010)
I've tried a lot of different speeds and numbers of passes, from 15 passes at 1600 RPM to 6 or 8 passes at 2400 RPM, and there is no discernable difference... i;ve also tried changing the relief angle on my thread tool.

any help would be appreciated!!

thanks!

ProProcess
05-14-2008, 06:02 AM
Try using "Compound Infeed" G76

jalessi
05-14-2008, 06:41 AM
G76


G76- Canned threading cycle

G76 P010010 Q0020 R0005 (first G76 sets parameters for threading)
G76 X Z P Q F R (cuts the thread)

The first G76 isn't needed but is recommended.
- G76 P Q R

P010010 sets 3 things
- first 2 digits is the amount of finish passes - 01

- second 2 digits is % of the lead or pullout exiting the thread- 00
00 = almost no angle at pullout and 99 = 9.9 leads away start out

- third 2 digits are the angle of infeed - 10
0-99 are usable

Q0020 sets the minimum cut amount during threading .002 but no decimal
(Q00200 for sub inch)

R0005 sets the cut amount of the last pass .0005 but no decimal
(R00050 for sub inch)

The second G76 cuts the thread.
-G76 X.1876 Z.3 P0302 Q0010 F.05 (R-.002) FOR 1/4-20

X.1876 =Minor Dia. of thread

Z.3 or (W) =The ending Z of the thread

P0302 =Height of thread in radius (Maj-Min)/2 (.0302)
(P03020 for sub inch)

Q0100 =Amount of the first cut. All the rest of the cuts are calculated.
(.01)
(Q01000 for sub inch)

F.05 =Feed-rate 20 TPI 1/20=.05

R = R is optional for tapered threading. R is the amount of
difference in X from start to finish in Z. When cutting threads
moving Z and X in a positive direction R is a negative value.

PixMan
05-14-2008, 08:47 PM
First, what machine and control are you using? Only a very late-model control with fast processing time would be able to thread at those spindle speeds reliably. On most Fanuc 18i-TB, 16i-TB and 21T controls, speeds of about 2000 are where you should max out, though some Star and Maier machines with 1320ipm (33m/min) rapid rates can go as high as 2500 in G76 cycles without too much trouble as long as your approach and retract amounts aren't excessive.

DO use a full-form 32p threading insert WITH the proper angled anvil under it for that small diameter. I recommend Valenite threading tools for this application. Depending upon what shank size your lathe takes, I can recommend the right holder, but for the threading insert and anvil you will want:

Insert 16ER32UN, Grade VC929 EDP No. 01942
Anvil CAE 16 3.5P EDP No. 08264

In that G76 cycle, use a different value for the first "P" parameter, to match the thread included angle and give the tool a compound angle infeed. It should read "P010060", or better yet (to give it a clean-up chip on the backside flank and plently of "free spring passes") use: "P040059"

hth

bbox
05-19-2008, 06:14 PM
304 forms a work hardened skin as you cut your threads. You must get under that skin for a clean cut on the next pass. Try to make your cuts .005" deep at least, deeper if possible.

Bill Box

JMS4287
05-28-2008, 07:31 AM
This might sound a little too obvious...but you might want to re-check the center height of the tool....with chipping inserts and the major dia being oversized, like the material is pushing away, that would be where I would start looking....especially with a small thread...

SWISS20
06-13-2008, 10:56 PM
can you display the program from before you start turning the OD to the end of the threading cycle.