First of many questions in learning curve

[STS_John]

Our Daewoo 2500 LSY is our first production CNC lathe, So we are really green. Some of my questions are based on learning curve for the lathe, some will be lack of knowlwdge on tooling for cutting down cycle times. We have alot of work for the lathe, and would really like to get the most out of its' potential

We are currently making 4340 Q&A parts that have 8 6-32 holes tapped in them. Tapping cycle is running pretty fast. Tapping at 640 RPM. What is really killing the cycle time is the drilling. Using a #36 cobalt stub 135 degree split point drill. 2500 RPM, peck at .050 total depth .300, feed at 6 IPM. Haven't tried anything faster, mostly becuase we don't know any better.. Any suggestions on decreasing cycle time. All other operations are running pretty fast.

Thanks in advance

[mrainey]

Look at how much air you're cutting after each peck - in other words, how close you're rapiding to the previous drill depth. This can usually be controlled by a parameter in the control (assuming you're using a canned drill cycle).

You might even try not pecking so much. Just make sure that coolant gets to the drill tip.

[solgood]

hello sts john

it sounds like you need a coated solid carbide tap drill (#36). no need to spot and no need to peck. sumitomo makes some great drills but thy will cost more than your cobalt drills. but in the end look at a 3 to 4 times faster run time in your tap drill with a sumitomo.

if you have more Q let me know

[STS_John]

Originally Posted by mrainey Look at how much air you're cutting after each peck - in other words, how close you're rapiding to the previous drill depth. This can usually be controlled by a parameter in the control (assuming you're using a canned drill cycle). You might even try not pecking so much. Just make sure that coolant gets to the drill tip.

Originally Posted by solgood hello sts john it sounds like you need a coated solid carbide tap drill (#36). no need to spot and no need to peck. sumitomo makes some great drills but thy will cost more than your cobalt drills. but in the end look at a 3 to 4 times faster run time in your tap drill with a sumitomo. if you have more Q let me know

Thanks for the input, we need the help.

We did get the feed on the #36 drill up to 15 IPM. And with some other tweaks got cycle time from 11m 15s to 7m 5s.

I will check the parameters of the peck cycle, and yes it is a canned drill cycle. I am a little worried about increasing peck distance. .106" drill diameter at 2500 RPM, worried about chip evacuation, especially with uncoated HSS drill. What are your thoughts

On the Sumitomo drill. Sounds like a good idea. No peck, how about coolant, do you run dry. We have had problems with carbide drills in our mills with chipping. We beleive it is from pecking with coolant. I hear all kinds of suggestions on carbide and coolant. Any input. I have some Valainite mills that work much better dry on 4340. The Valinite rep turned me on to that one.

Anyway, thanks again

[Bluesman]

Emuge corp I beleive is the comp that suplys our rep. We have used them sucsefully for a while now. Drill and thread mill in one pass. A bit pricy but well worth it for the cycle time reduction.





http://news.thomasnet.com/fullstory/17849


Bluesman

[STS_John]

[QUOTE=Bluesman;198251]Emuge corp I beleive is the comp that suplys our rep. We have used them sucsefully for a while now. Drill and thread mill in one pass. A bit pricy but well worth it for the cycle time reduction.


Unf'ing believeable. Looks like a killer tool. We are big on thread milling in our VMC. Have not seen this tool. Unfortunately, according to the Emuge web site, the smallest size they make for blind holes is 1/4" or #10 for thru holes, our holes are 6 and 8-32. But, I will be looking at these for our next jobs with larger threaded holes.

Thanks to all, this site is proving to be an excellent resource. All the guys in the shop are registering and will have their own bonehead questions. They are all registering with the STS_, so you will be able to recognize them.

[diarmaid]

Sorry to intrude on the thread, but can someone tell me what "pecking with coolant" means?
Thanks and sorry again.

[STS_John]

Originally Posted by diarmaid Sorry to intrude on the thread, but can someone tell me what "pecking with coolant" means? Thanks and sorry again.

We have had problems with carbide drills chipping in mill applications (drills under 1/4 diameter). We tried pecking cycles dry (no coolant) and pecking cycles with flood coolant (pecking with coolant). We got our best results cutting dry with no peck. We would appreciate hearing any better ways.

[diarmaid]

Thankyou.

[Bluesman]

[QUOTE=STS_John;198300]

Originally Posted by Bluesman Emuge corp I beleive is the comp that suplys our rep. We have used them sucsefully for a while now. Drill and thread mill in one pass. A bit pricy but well worth it for the cycle time reduction. Unf'ing believeable. Looks like a killer tool. We are big on thread milling in our VMC. Have not seen this tool. Unfortunately, according to the Emuge web site, the smallest size they make for blind holes is 1/4" or #10 for thru holes, our holes are 6 and 8-32. But, I will be looking at these for our next jobs with larger threaded holes. Thanks to all, this site is proving to be an excellent resource. All the guys in the shop are registering and will have their own bonehead questions. They are all registering with the STS_, so you will be able to recognize them.

I will get you our reps number Bud Hurbert is his name, They will acually make you any size you want. I think our 4mm are specials and not off the shelf. As long as you got a check book anything is posible. You would not believe some of the goofy stuff I get made. I got pop bottle "G" syle drill that will drill chamfer and back inerpolate an inside cmfr all in one cut, It saves me tons of cycle time. When I first started using them we had to draw them up and show them what we wanted, Now i think they may be stock items i some suplyers catalogs. As long as you can aford it the mind is the limmit when it comes to tooling. That is where all this goofy looking stuff comes from. "Nesity is the mother of invention" That is so true

Bluesman

[Geof]

Originally Posted by STS_John We have had problems with carbide drills chipping in mill applications (drills under 1/4 diameter). We tried pecking cycles dry (no coolant) and pecking cycles with flood coolant (pecking with coolant). We got our best results cutting dry with no peck. We would appreciate hearing any better ways.

I think you have found the better way. The chipping you encountered with coolant was almost certainly due to thermal shock. The best result obtained by not pecking is probably because 4340 can work harden; when you peck everytime the drill re-enters the cut it has to break through the work hardened surface from the previous peck. Driving full depth in one pass means the drill never encounters a work hardened surface.

[STS_John]

Originally Posted by Geof I think you have found the better way. The chipping you encountered with coolant was almost certainly due to thermal shock. The best result obtained by not pecking is probably because 4340 can work harden; when you peck everytime the drill re-enters the cut it has to break through the work hardened surface from the previous peck. Driving full depth in one pass means the drill never encounters a work hardened surface.

Thanks for the confirmation Geof. We learned this after a suggestion and a bunch of trial and error. With the help of masters like yourself, and others in this thread (thanks Bluesman) we hope to correct problems with less trial and error and more advice from experts like yourself.