CUT METRIC THREAD ON CNC LATHE

[katsbobo]

HELP!!!

I feel like an beginner. I have a Haas CNC SL-20 lathe that im tring to cut an external m5 x .8 thread. It just aint happening. Im using the mlpfan post. my O.D. is .196 and im have 7 equal pass and 2 spring pass and i plugged in m5 x .8 in the correct fields. I think. If anyone could help I would be forever grateful. Ill attach the program in case someone feels my pain and knows what im doing wrong. Thx to everyone

[Guest]

So what is not coming out right?

[katsbobo]

here is the program im using to cut or not cutting the m5x.8 threads. Please Help

 

G0T0505

G97S300M13

G0G54X.3968Z.0293

X.3969

X.1926

G99G32Z-.1869E.0315

G0X.3969

Z.045

X.1926

G32Z-.1869E.0315

G0X.3969

Z.0281

X.1883

G32Z-.1869E.0315

G0X.3969

Z.0438

X.1883

G32Z-.1869E.0315

G0X.3969

Z.0269

X.184

G32Z-.1869E.0315

G0X.3969

Z.0426

X.184

G32Z-.1869E.0315

G0X.3969

Z.0257

X.1797

G32Z-.1869E.0315

G0X.3969

Z.0414

X.1797

G32Z-.1869E.0315

G0X.3969

Z.0245

X.1754

G32Z-.1869E.0315

G0X.3969

Z.0402

X.1754

G32Z-.1869E.0315

G0X.3969

Z.0233

X.1711

G32Z-.1869E.0315

G0X.3969

Z.0391

X.1711

G32Z-.1869E.0315

G0X.3969

Z.0221

X.1668

G32Z-.1869E.0315

G0X.3969

Z.0379

X.1668

G32Z-.1869E.0315

G0X.3969

Z.021

X.1628

G32Z-.1869E.0315

G0X.3969

Z.0368

X.1628

G32Z-.1869E.0315

G0X.3969

Z.021

X.1628

G32Z-.1869E.0315

G0X.3969

Z.0368

X.1628

G32Z-.1869E.0315

G0X.3969

Z.021

X.1628

G32Z-.1869E.0315

G0X.3969

Z.0368

X.1628

G32Z-.1869E.0315

G0X.3969

Z.021

X.1628

G32Z-.1869E.0315

G0X.3969

Z.0368

X.1628

G32Z-.1869E.0315

G0X.3969

Z.0293

G28U0.W0.M05

T0500

M30

%

[katsbobo]

My o.d. was too big to start out with

[gcode]

What's it not doing??

Are you getting an alarm??

[YoDoug®]

I am at home now so I can't check, but I believe that the E in the feedrate needs to be a F.

[Philcott]

Kats,

 

You have a few problems going on here.

 

First of all you are making 2 passes at each depth of cut for a total of 22 passes. You must have clicked the button for multiple starts.

 

Two perhaps.

 

With this on, Mastercam changes the starting "Z" position by the value of one pitch. It will alternate back and forth between the two start positions as the "X" works it's way down to the minor diameter. So make shre you do not have multiple starts on. Unless, of course, you want a double start thread. I would also start a little further back from Z zero to allow for the feed to get up to speed before actually making a cut. This typically should be a minimum of 1.5 times the pitch of the thread.

 

I would guess Doug is correct that the E should be F for feed rate. Check in your machine manual.

 

One other thing, I saw that your RPM is 300. This is probably too slow. I don't know what material you are cutting but you should calculate the correct cutting speed for the diameter you are turning.

 

Good luck,

 

Phil

[g-codeguy]

I have to agree with Phil, tho I have no experience with Haas lathes so I wouldn't venture a guess as to what the correct feed code should be.

 

S3000 would be about 150 sfm which is pretty darn slow! We thread 316 SS at 365 sfm with the normal threading inserts we use. Most of the lathes we have had will thread at least at 120 ipm. This equates to S3800 so your S300 is way too slow.

 

That slow is not good for the insert. Material will stick to it and either chip the insert or build up giving a nasty looking thread.

 

As an example, several years ago I tested roughing inserts on 420 SS. First test was on a small part where SFM went down to 245. Insert from one company wouldn't last more than 10 pieces. Yet when tested on a part large enough to keep RPM within the specified sfm for the insert, it was one of the best. Insert kept chipping on the smaller part.

[EZ3PUTT]

I have run a few lathes that allow an E command to control feed for threading. With an F command they were limited to 4 decimal places. Using E allowed 6 decimal place feed rates.