Drilling & Reaming SS 316L

[Jay17]

I am brand new to the CNC world. My company just bought our first machine (Doosan DNM 400) and are in need of guidance in selecting drilling and reaming tooling.

We are trying to end up with reamed holes that are 0.378" OD through 2" of stainless steel 316L. The advice we got was to start with CJT Coolant through carbide drill 0.368" OD (metric U), then ream with a straight 4-flute carbide reamer that is 0.378" OD.

The drilling was successful, but the reaming is a nightmare. 12 holes into a 230 hole part the tool snapped in half and had severe damage to the tip. Presumably, a stringy piece of 316L that was creating a birds nest got into the hole. We then tried to monitor the strings, but had a the next tool literally twist itself on the way out of the hole.

Now the tooling folks are suggesting a spiral coolant through carbide reamer.

My thought is to just drill to 0.375" OD and then ream the last 0.003" off slowly with a cobalt reamer.

Cycle time is not critical. Accurate holes and tool life is the focus.

Any advise would be GREATLY appreciated.

Thank you

[Chrliev]

The tooling people are wrong, sounds like the guy doesn't have much experience with cutting tools and metals.

300 series stainless is not a hard metal, it is a tough metal. The difference is that a hard metal can not easily be deformed by with a hammer, a tough metal can. Tough materials molecules don't separate easily they tend to cling and gall which makes them "tough" to cut, these different qualities makes tooling knowledge and selection critical.

You have to cut hard materials with hard cutting tools but when making holes in tough materials you must use a tough cutter not a hard cutter or you will get what you got broken tools. Instead of carbide drills and reamers get some M42 cobalt drills and reamers, they are tough much tougher and will resist shock and breakage and they are not as hard and brittle as carbide. Slow down to approximately 60 sfpm, .004 IPT chip load.

For a 3/8" drill, run a peck drilling cycle (G83/G73) at about 750 RPM and 3" per minute feed, run the reamer using a reaming cycle (G85) at about 8" per minute. The other benefit of tough tooling is that cobalt tools are a lot cheaper than carbide.

Maybe thats why the guy recommends carbide tools...

[Jay17]

I suspected something like this may be the case. Thank you very much for your very quick response.

Another question, though, about Cobalt Reamers. We run them on a radial drill with 0.375" holes that we ream to 0.378". Would those numbers still make sense on a CNC machine?

We were told carbide reamers need approximately 0.010" OD in order to work... anything less would just burn the material we were told. Is that the same for Cobalt? Or can cobalt ream just 0.003" with no problem?

[Chrliev]

The reason for using a reamer is that twist drills will either drill over size and/or make holes that are not very round, reamers tend to cut round because the amount of material removed is less and they have more cutting flutes. The less material being reamed for finishing the better, as long as there is some amount of material to ream, it should make a nice hole, you should feed the reamer much faster than the drill, like 3x or 4x faster, rubbing or very slow feedrates in tough metals can cause a condition known as workhardening so keep the tool moving and cutting at all times. The type of machine doesn't really matter, drill press, manual mill, jig borer or CNC machine, the numbers should be the same for all machines.

As long as the hole is smaller than the reamer it will take it to the correct size. Reamers do tend to follow the hole that is already there because they don't cut on their sides, for close tolerance true positioning work, I usually run an end mill to make a pilot, in your case a 3/8, for a very small distance (.05-.10) first, to make sure the hole is in the precise position.

BTW, a reamer's od is ground round with no clearance they also taper smaller (back taper) as you go up the flutes, so that they don't bind as they go deeper.

Glad to help...

[JCMills]

Peck the carbide reamer about .300 pecks. use heavy coolant to hold the size and blast away strings at the top of the hole if they come out

[JCMills]

I suspected something like this may be the case. Thank you very much for your very quick response.

Another question, though, about Cobalt Reamers. We run them on a radial drill with 0.375" holes that we ream to 0.378". Would those numbers still make sense on a CNC machine?

We were told carbide reamers need approximately 0.010" OD in order to work... anything less would just burn the material we were told. Is that the same for Cobalt? Or can cobalt ream just 0.003" with no problem?

reaming large numbers of holes with cobalt reamers especially reaming .003 is a losing proposition im sure you will find. that .003 is operating right in the work hardened zone. Carbide reamers are the way to go. drill--interpolate the top part of the hole about .300 deep--then carbide ream with coolant pecking the reamer for deep depths--not a typo--peck the reamer. interpolating assure true tracking of the reamer--and should almost always be done regardless of position requirements..doing those few things you will soon look back at hss reamers as a costly nightmare of the past. Not true at all that less than .010 make carbide reamers "only burn"-if that condition exists its because of not doing the first suggestions. also the tool salesmen do not understand fully what takes place during reaming. what he said shows it--also if you ask him about pecking a reamer--he will quickly say that person who said that should be fired--further showing their lack of knowledge