Cutting speed and feeds for indexable drills

cncdude1 · May 22, 2014

I am using a Techniks Nexus .875 dia indexable drill in the Haas ST 10 Lathe.

I don't have any data on feeds and speeds - currently using 500 rpm ( 114 SFM ) with F.0025 in 1018 CRS. and thru coolant.
I also do a peck of Q.150.

I am thinking we need to be much faster RPM but I don't want to go in small increments if I am way slow.

DMF_TomB · May 22, 2014

cncdude1 said:
I am using a Techniks Nexus .875 dia indexable drill in the Haas ST 10 Lathe.

I don't have any data on feeds and speeds - currently using 500 rpm ( 114 SFM ) with F.0025 in 1018 CRS. and thru coolant.
I also do a peck of Q.150.

I am thinking we need to be much faster RPM but I don't want to go in small increments if I am way slow.

.
check with the indexable drill manufacturer on speeds and feeds. i find hole depth matters as well as drilling horizontal or vertical. you have through spindle coolant which should help with tip cooling and getting chips out of the hole.
....... some manufacturers recommend no peck on shallow holes. some drills have 1 effective tooth and other have 2 effective teeth. it would help to know if insert is hss, cobalt, carbide, etc and how long is the drill bit as short drills can take more feed that long ones.
......... you have to balance going faster and the drill insert breaking in the hole and possibly loosing the part. for many they would rather go 1/2 speed and never loose a part from drill failure

cncdude1 · May 22, 2014

I took you advice and sent off an e-mail to Techniks - I had contacted the applications guy that had set me up with all the lathe tooling but still wating to hear.

More Info techniks index drill 1.00 shank drill x .875 cut diameter with thru coolant

One effective tip ( 2 inserts - overlap one on each flute)
Insert is carbide
Max Depth hole = 3.50" per Nexus specs

I think you are right about deep hole as it does change sounds the deeper it goes

This is a teaching machine for our CNC class - so better safe than sorry on the setup.

Index drill specs web site

Nexus Indexable Drills

Dave K · May 22, 2014

I'd say that rpm is way too slow. I would be running about 500 sfm, which equates to about 2180 rpm, and .002 per rev feed. That's just a starting point, but 114 sfm seems way too slow for any carbide insert whether it's on a drill, boring bar, turning tool...etc.

DMF_TomB · May 23, 2014

drilling

cncdude1 said:
I took you advice and sent off an e-mail to Techniks - I had contacted the applications guy that had set me up with all the lathe tooling but still wating to hear.

More Info techniks index drill 1.00 shank drill x .875 cut diameter with thru coolant

One effective tip ( 2 inserts - overlap one on each flute)
Insert is carbide
Max Depth hole = 3.50" per Nexus specs

I think you are right about deep hole as it does change sounds the deeper it goes

This is a teaching machine for our CNC class - so better safe than sorry on the setup.

Index drill specs web site

Nexus Indexable Drills

.
when drilling 1018 steel long stringy chips can be a problem. you may have to peck to breakup long chips
.......horsepower is a concern as carbide drills often need 4-10x more horsepower
.
the reason to ask manufacturer is some carbide inserts are big and tough and can take a lot more feed. trying to do the same with small inserts and they can fail suddenly. carbide insert drills are often expensive sometimes $500 - $1500 not to mention the cost of the part.
....... many places you could get fired (loose job) if you were to change programmed feeds and speeds. other places allow an operator to change rpm from 10-120% and feed from 10-200%
.
in general i would only make 10% changes. with gradual changes you can see how drill bit handles it without hopefully sudden failures and just gradual wear which you can check drill after every few holes or every so many minutes like 20 minutes........... the other reason to get manufacturers data on feeds and speeds is IF you loose the drill or part you stand a greater chance of keeping your job if you have the drill manufacturers recommended speeds and feeds to back you up explaining the loss to your boss.
.
trying to explain to your boss some guy on the internet told you to increase speeds 400% and feeds 300% and you did it and destroyed a drill and or a part is highly likely to get you immediately fired.

Jashley73 · May 23, 2014

DMF_TomB said:
.
when drilling 1018 steel long stringy chips can be a problem. you may have to peck to breakup long chips
.......horsepower is a concern as carbide drills often need 4-10x more horsepower

Sorry Tom, but no pecking needed... Run that drill somewhere between 2000 and 2500 RPM, and about .003" per rev to start. With through-coolant and those starting parameters, you should be fine, provided you have about a 5hp spindle or greater...

ewlsey · May 23, 2014

300-400 SFM is about right for a drill in steel. Some can take more.

The feed rate should be about half what you would use for a twist drill. An insert drill basically functions like a single flute drill, so you have to cut the feed rate in half.

You don't need to peck, but it won't really hurt anything, especially in a lathe.

MotoX · May 23, 2014

Sounds like ewlsey is spot on.

I would run that if you cant find the manufacturer's specs.

toolsteel · May 23, 2014

I run our Sandvik Insert drills at 400-600SFM.....004-.006/rev......in 4140 and A-8, and D2. And I never peck. I would expect similar with your drill.

cncdude1 · May 23, 2014

Some good stuff - SFM will go up and I will use that 200 and 400 sfm as a goal. My feed is ok for now. I like the peck if I am going deep. It cuts like butter now and very short chips. I have 15 hp and ...... I am the boss.

Thanks everyone and have a good weekend

rustamd · May 23, 2014

Cant offer much more help, other then agree with toolsteel's numbers, but just curious where you are teaching in Sarasota?

Orange Vise · May 23, 2014

You're definitely way-slow. How slow depends on the length of the drill.

DMF_TomB · May 24, 2014

Jashley73 said:
Sorry Tom, but no pecking needed... Run that drill somewhere between 2000 and 2500 RPM, and about .003" per rev to start. With through-coolant and those starting parameters, you should be fine, provided you have about a 5hp spindle or greater...

.
depends on how deep the hole. i have seen holes 8" or deeper where drill bit is destroyed because of no peck. i have seen the same holes drilled with no problems using peck. i am aware of the no peck needed theory with through spindle coolant drills
.
i work on a big 50 hp machine. it can destroy a insert drill, push a part in a fixture and bend the machine out of alignment well before a overload would stop machine. i already done that before many times, i tend to be cautious. i like my job and want to keep it

DMF_TomB · May 24, 2014

cncdude1 said:
Some good stuff - SFM will go up and I will use that 200 and 400 sfm as a goal. My feed is ok for now. I like the peck if I am going deep. It cuts like butter now and very short chips. I have 15 hp and ...... I am the boss.

Thanks everyone and have a good weekend

.
good luck...... i am just saying it usually pays to be cautious. i have seen plenty of new guys destroy tooling and parts. old timers tend to make little changes like 10% and watch the tooling and note results. i keep a excel file of all our tooling and speeds and feeds used both the highs and lows. i especially note tool failures and failure type. this way on a new program i can check it against the excel tool list and see if it is in the normal parameters. i have caught much bad programming this way.
........ normally i will override feed and speed running the program and do not change program. some programmers are upset if you mess with their programs. i have learned over the years it is best to not piss off anybody if you do not have too. i will only change programs and save them if i have data from previous failures backing my decision up. and i make it a point to not embarrass the programmer by announcing to everybody that they made a programming mistake.

zero_divide · May 24, 2014

I totally adgee with DMF_Tomb on tthe peck thing.

I am recently doing a lot of drilling with Sandvicks indexable drils and notice when depth reaches about*4 diameters chips start to pack up and spindle almost stalls. Had 2 close calls where I had to abort and restart with peck.

I think for large drill diameters coolant volume on machine I am working on is not enough to flush the chips. I guess this is another thing to consider as only coolant pressure is most often mentioned.

DMF_TomB · May 24, 2014

zero_divide said:
I totally adgee with DMF_Tomb on tthe peck thing.

I am recently doing a lot of drilling with Sandvicks indexable drils and notice when depth reaches about*4 diameters chips start to pack up and spindle almost stalls. Had 2 close calls where I had to abort and restart with peck.

I think for large drill diameters coolant volume on machine I am working on is not enough to flush the chips. I guess this is another thing to consider as only coolant pressure is most often mentioned.

.
often the new guys have no fear and try radically different feeds and speeds. they have not done enough different types of machining to see the failures and the tooling, part, and machine damage.
.
if i have learned one thing, if your get fired for taking excessive risks don't count on the old employer who fired you to give you a good recommendation when you end up looking for your next job....... many places could not care less what is on a resume or the diplomas you might have or anything else BUT talking to your last employer and asking them what they think of you as a machinist. it is not good if the old employer recites how much tooling you damaged or all the parts you scrapped.

zero_divide · May 24, 2014

DMF_TomB said:
.
often the new guys have no fear and try radically different feeds and speeds. they have not done enough different types of machining to see the failures and the tooling, part, and machine damage.
.
if i have learned one thing, if your get fired for taking excessive risks don't count on the old employer who fired you to give you a good recommendation when you end up looking for your next job....... many places could not care less what is on a resume or the diplomas you might have or anything else BUT talking to your last employer and asking them what they think of you as a machinist. it is not good if the old employer recites how much tooling you damaged or all the parts you scrapped.

Have not broken anything yet. But the funny thing is my leadhand insists on me NOT pecking on ANYTHING when using coolant through drills.
Either he is trying to screw me, or i dont know. I just agree with him now and do it my way, cause i know what works and what doesn't.

He says that when you peck with indexed drills, you run the risk of landing cutting edge on a chip inside the hole. Which would lead either to insert failure or decreased insert life.
At the same time, i believe when you retract the drill, you pull most of the chips out. And then when you plunge back in, drill always starts 0.01" above, so there is very little chance of recutting anything.

I now peck on depths after 3x dia. Just to be safe.

DMF_TomB · May 24, 2014

zero_divide said:
Have not broken anything yet. But the funny thing is my leadhand insists on me NOT pecking on ANYTHING when using coolant through drills.
Either he is trying to screw me, or i dont know. I just agree with him now and do it my way, cause i know what works and what doesn't.

He says that when you peck with indexed drills, you run the risk of landing cutting edge on a chip inside the hole. Which would lead either to insert failure or decreased insert life.
At the same time, i believe when you retract the drill, you pull most of the chips out. And then when you plunge back in, drill always starts 0.01" above, so there is very little chance of recutting anything.

I now peck on depths after 3x dia. Just to be safe.

.
as a CNC operator i also use manual pecking. that is when the drill starts to make noise i do a feed hold, wait, then start, and feed hold again when noisy, then start, keep doing as needed. this is not as good as pulling the drill completely out of the holes and washing it with coolant but it is better than nothing.
.
on my fanuc 15 control there is a setting for G83 full peck and G73 high speed short peck........ basically the amount where rapid ends and feed begins again above the last drill depth specifically so you do not hit a chip sticking up hard when drilling begins.
.
when G83 or full peck i reduce rapids as drill bit out of the hole it may be whipping eccentric wise and smacking the drill tip going back in the hole at full rapid is hard on the drill. with Rapids at 25% i have never had trouble peck drilling easily more than 10,000 of holes over 34 years, not even once had i ever had the slightest problem pecking. i definitely have had many hundreds of drilling problems over the years by NOT pecking

Dave K · May 24, 2014

I have been told time and time again, not to peck with those drills, and also solid carbide twist drills. Funny, I still do it all the time, and have never had a problem.
I understand their theory on it, and many times it ends up being exactly what works well, but there just are certain times where you have to go against the general rule. Some people just don't seem to get that. I had one tooling applications guy tell me I should never peck my solid carbide drills on this one job I have. When I told him I've been doing it for 3 years now, and haven't broken 1 drill, he looked at me like I was from Mars. :crazy:

DaVicki · May 26, 2014

DMF_TomB said:
.
i keep a excel file of all our tooling and speeds and feeds used both the highs and lows. i especially note tool failures and failure type.

Tom

Any chance of getting a copy of that spreadsheet. Sounds like a lot of helpful information.

Cutting speed and feeds for indexable drills

Plastic

Diamond

Plastic

Diamond

Diamond

Titanium

Diamond

Cast Iron

Titanium

Plastic

Cast Iron

Titanium

Diamond

Diamond

Stainless

Diamond

Stainless

Diamond

Diamond

Plastic

Similar threads