I have a job boring a bunch of 316 stainless, and am having a really hard time getting the chips to break. They ratsnest in the hole, and break insert after insert. I first drill a 1" hole with an insert drill, and am following it up with a 3/4" diameter carbide boring bar. Bore needs to end up 1.32" +- .01, surface finish not important. Anyone have recommendations for inserts and/or strategy for getting these chips to break, and getting them out of the hole? I have ccmt 3252 inserts for the boring bar, and have tried every insert I have with no luck. Surface speed at 300sfm. Tried both a bit more and less. Feed I've tried everything from .005" per rev to .015" per rev. DOC everywhere from .005 to .040. Wondering if there isn't a specific chipbreaker / coating / some other magic juju that'll help me get these [email protected]#$%g chips to break. I've tried feeding +Z direction too with shallow DOC as an experiment, and that didn't seem to work either... Surely there's a way....
Largest Manufacturing Technology Community on the Web
Stay Connected:
Lathe Boring 316 Stainless - Getting Chips to Break
- Thread starter BernieB
- Start date
- Replies 21
- Views 4,199
plastikdreams
Diamond
- Joined
- May 31, 2011
- Location
- upstate nj
Send it down the hole deeper than your cut and fast, basically making relief grooves. That's about it really. 300 series is a bastard for making a mess.
plastikdreams
Diamond
- Joined
- May 31, 2011
- Location
- upstate nj
That too...
EmanuelGoldstein
Diamond
- Joined
- Apr 14, 2018
- Location
- Airstrip One, Oceania
And get rid of the positive rake .....
TeachMePlease
Diamond
- Joined
- Feb 11, 2014
- Location
- FL
Got a bar that takes VC or DC inserts? Drill closer to size, use an insert with more clearance for chips to not build up on the insert....
plastikdreams
Diamond
- Joined
- May 31, 2011
- Location
- upstate nj
It's funny, everyone I work with pretty much has only machined aluminium or carbon steel...they used to order 304 because it was stainless then be like oh stainless is so hard. Then I introduced them to 316ss lol...they haven't tried the 17-4 yet, I can't wait for that lol.
But it's like, they have no idea about different materials machinability or composition. It's to the point they send everyone to me when they have questions about materials lol.
But it's like, they have no idea about different materials machinability or composition. It's to the point they send everyone to me when they have questions about materials lol.
It's harder to make chips from 316 when boring than OD turning, don't know why.
On boring I use a Kenna DNMG insert - MS grade - (5090742). 2-3 mm DOC typically. Feed typ. 0.25 mm/rev, SFM approx 140 m/min.
Still get rats nests frequently when the insert wears a bit or if the 316 batch is a bit different than others (not unusual I find).
Best trick we do is to bore to full ID (apart from finishing pass) in steps in depth along the bore with intermittent full retract out of the hole. This allows for better chip evacuation and the HP coolant tends to flush out (most) of the rats nests. Then just a normal finishing pass to finish it off, Don't expect any chips there.
EDIT: I use DNMG, not DCMT on my Ø50mm boring bar, and it's MS inserts, not MP. Corrected above, along with actual feed & speed & DOC. I can confirm that this makes good chips on my machine when using HPC.
On boring I use a Kenna DNMG insert - MS grade - (5090742). 2-3 mm DOC typically. Feed typ. 0.25 mm/rev, SFM approx 140 m/min.
Still get rats nests frequently when the insert wears a bit or if the 316 batch is a bit different than others (not unusual I find).
Best trick we do is to bore to full ID (apart from finishing pass) in steps in depth along the bore with intermittent full retract out of the hole. This allows for better chip evacuation and the HP coolant tends to flush out (most) of the rats nests. Then just a normal finishing pass to finish it off, Don't expect any chips there.
EDIT: I use DNMG, not DCMT on my Ø50mm boring bar, and it's MS inserts, not MP. Corrected above, along with actual feed & speed & DOC. I can confirm that this makes good chips on my machine when using HPC.
Last edited:
How deep are you going? If its only around 2xD You should be able to open that to size in 2 cuts around .010" feed, lots of coolant and make sure the chips come out of the hole, they should be breaking at that DOC, if not try .016" nose rad and drop the feed to around .008". 350-400SFM if the bar stickout isn't too long and just chatters. I use carbide shank bars for pretty much everything.
I mainly use Sandvik's 1115 but 2220 is good also.
Definitely way better if you can poke a bigger hole close to finish start to start with and just do 1 finish cut.
When it comes to gummy stringy chips duplex and Grade2 Titanium are hard to beat...
I mainly use Sandvik's 1115 but 2220 is good also.
Definitely way better if you can poke a bigger hole close to finish start to start with and just do 1 finish cut.
When it comes to gummy stringy chips duplex and Grade2 Titanium are hard to beat...
MaxPrairie
Hot Rolled
- Joined
- Jul 9, 2015
I will see what ccmt insert I use. I would be taking at least 50 per side on the rough pass. Never had that issue. Probably feeding 6-8 per rev on it. If you were to go to cnmg or dnmg should be taking 100-150 per side and 8 per rev. At least that is what works for me.
https://www.travers.com/product/walter-5615012-turning-boring-insert-25-001-405
This looks like what I use on my 1/2” bar. Never bought from travers, but msc or your rep probably has them in the correct size for you.
https://www.travers.com/product/walter-5615012-turning-boring-insert-25-001-405
This looks like what I use on my 1/2” bar. Never bought from travers, but msc or your rep probably has them in the correct size for you.
Rapid_Tech
Aluminum
- Joined
- Oct 27, 2014
- Location
- Toronto
How deep is the hole? Can you rough the bore with the indexable drill?
Neat idea! I'll try it. Thinking I may try going in with an ID groover and making relief grooves every .5", and see how that goes.
Orange Vise
Stainless
- Joined
- Feb 10, 2012
- Location
- California
They make insert drills in increments of 0.5mm.
Your tolerances are wide open.
Hit it with a 33.5mm indexable in one shot and call it a day.
Your tolerances are wide open.
Hit it with a 33.5mm indexable in one shot and call it a day.
Think I'll get a bigger insert drill to simplify it all. Any recommendations on drill and insert for this material in 1.25" size? The 1" insert drill I have has similar issue to the boring bar. Chips don't want to break, unless I really get after it with the feed, and at the point the inserts don't last more than a hole or 2 without chipping.
Orange Vise
Stainless
- Joined
- Feb 10, 2012
- Location
- California
Peck drill.
Compared to birds nesting, it's the lesser of two evils.
Feeding beyond the recommended parameter range isn't a real option.
Compared to birds nesting, it's the lesser of two evils.
Feeding beyond the recommended parameter range isn't a real option.
plastikdreams
Diamond
- Joined
- May 31, 2011
- Location
- upstate nj
316 is better to cut than 304 but really some ops make them seem closer though. Sometimes ya gotta push through it...tomorrow at work I have to machine 6 pieces of 44 inch x 1.000 pure copper bars, full radius on one end and 1/2-13 x 1.000 id threads on the other side...wanna trade lol
For the low price, Korloys king drills are pretty great. Travers has 1.25" 3xD for $365, comes with a nice case and 2 boxes of inserts. 5xD is $507.
I use a smaller one in duplex often.
Sandvik had a nice sale on their newer DS drills in september but that's over now. Their old 880's are good too.
Don't worry about breaking a chip so long as the chips make it out of the hole its fine, around .0032" feed and good through coolant to get the chips out. I use a 880 .937" up to 4.5" deep in 316, Duplex, 625 Inconel, no problem at all. Insert life isn't too good in inconel but in stainless it'll drill all day long without changing edge.
I have been smitten with Walter D4120 insert drills for stainless and even nasty exotic materials. I have a 25mm that has drilled over 100,000 holes in 17-4 and still looks great, and a 24mm that has drilled over half a million dollars worth the most heinous flavor of nickel (270) that I have ever come across and is still running as I type this. Both are just beasts. By far my favorite after experimenting with Sandvik, Iscar, and KM. Get that in a 33mm and offset drill to get your hole to size and you'll be rocking.
