What's new
What's new

Boring bar for interrupted cut in 304 SS

kb0thn

Stainless
Joined
May 15, 2008
Location
Winona, MN, USA
Hi Guys,

I have a 304 stainless lathe part that is 1.58" ID and has a 0.266" diameter hole that is half in the 1.58" bore. Depth of bore is 2.75". Machine is Mazak QT15.

So I drilled the 0.266" diameter holes in the slugs on the VMC before putting in the lathe. On the lathe I drill a inch hole with indexable drill and then *attempt* to bore it to the 1.58" diameter. It goes fine until I start getting the interrupted cut.

Once the diameter gets to hitting the 0.266" hole diameter, the corners on the boring bar inserts start dieing quickly. Breaking off. Sometimes I get a most of a part, sometimes I'm losing a corner within 0.5" of cuttings. Cutting parameters are 550 SFPM / 0.005" DOC. Upping the DOC just makes more spectacular insert failures. Boring bars are steel Widia / Circle SSBI bars with coolant through. I am using a TD-6P-1-CG5 insert. There doesn't appear to be a lot of insert choices for these bars. These are the inserts Widia recommended.

I also tried a cheap DNMG inserted boring bar and it blew the corner off the insert instantly as well.

So ... what do I do. Scrapping 3/4 of my parts and going through multiple inserts per part isn't working well for me.

Is there a boring bar that can do this? Specific recommendations, please.

I've considered buying an expensive 1-1/2" indexable drill and doing the bulk of the material removal with it. But I would still have interrupted cutting to bring it up to 1.58". So I'm going to need a boring bar / insert that can handle it.

Help please!

Thanks

20180627_101023.jpg
 
Hi Guys,

I have a 304 stainless lathe part that is 1.58" ID and has a 0.266" diameter hole that is half in the 1.58" bore. Depth of bore is 2.75". Machine is Mazak QT15.

So I drilled the 0.266" diameter holes in the slugs on the VMC before putting in the lathe. On the lathe I drill a inch hole with indexable drill and then *attempt* to bore it to the 1.58" diameter. It goes fine until I start getting the interrupted cut.

Once the diameter gets to hitting the 0.266" hole diameter, the corners on the boring bar inserts start dieing quickly. Breaking off. Sometimes I get a most of a part, sometimes I'm losing a corner within 0.5" of cuttings. Cutting parameters are 550 SFPM / 0.005" DOC. Upping the DOC just makes more spectacular insert failures. Boring bars are steel Widia / Circle SSBI bars with coolant through. I am using a TD-6P-1-CG5 insert. There doesn't appear to be a lot of insert choices for these bars. These are the inserts Widia recommended.

I also tried a cheap DNMG inserted boring bar and it blew the corner off the insert instantly as well.

So ... what do I do. Scrapping 3/4 of my parts and going through multiple inserts per part isn't working well for me.

Is there a boring bar that can do this? Specific recommendations, please.

I've considered buying an expensive 1-1/2" indexable drill and doing the bulk of the material removal with it. But I would still have interrupted cutting to bring it up to 1.58". So I'm going to need a boring bar / insert that can handle it.

Help please!

Thanks

View attachment 231642

.
length of boring bar sticking out to dia ratio is important, probably the most important thing
.
obviously 550 sfpm is not helping with controlling vibration
 
.
length of boring bar sticking out to dia ratio is important, probably the most important thing
.
obviously 550 sfpm is not helping with controlling vibration

On the DNMG bar I cut the shank down so it was as short as possible. It didn't seem to have any positive effect.

What sort of feed rate and DOC would you recommend? 550 has worked out to be the happy spot on these bars (that I have found) for non-interrupted cutting.

Thanks
 
My 2 cents..

But first what is your feed rate???

You may get away with 550sfm while turning (I think its kind of high), but you really
aren't going to get away with it in an interrupted cut... And you aren't..

When I have an interrupted cut, my 'GoTo' method is high DOC and LOW feed.. Preferably get
past the interruption, and into a constant cut in one pass.... For example, when turning Hex
stock, I like my first pass to take all the interruption off and have the nose buried in solid
round material.. In your case you would have the nose in the interruption.

Some of Y'all will probably laugh at me on this one, and say it won't work.. But my first instinct on
this part, (getting through the interruption), probably a .150+ DOC(deep enough that some of the insert
is still cutting solid material), and .0016 (yes, 2 zeros) a rev at 175sfm... Using whatever inserts
Curtis sent me for nasty stainless.
 
On the DNMG bar I cut the shank down so it was as short as possible. It didn't seem to have any positive effect.

What sort of feed rate and DOC would you recommend? 550 has worked out to be the happy spot on these bars (that I have found) for non-interrupted cutting.

Thanks

every length to dia change on a boring bar effects its performance the cube law or when length reduces to 1/2 the rigidity goes 2x2x2 = 8 times more rigid is one of those laws of the universe. doesnt matter in the slightest if you never noticed any effect.
.
i got a chart of 500 different tools setup to precise standards like length and have over 2000 different feed and speeds recorded and chart i list any sudden tool failures and or other problems. i cant say i have every seen any tool with only one feed and speed setting good for everything.
.
304 is famous when work hardened or cold rolled or worked it will be over 200% harder to machine. that alone means there is no one feed and speed for 304.
.
its like saying you cut all tool steel the same from annealed for 65 rockewell C hard. obviously not.
 
But first what is your feed rate???

Whoops. Forgot that. 0.005" as well. See attached screen shot for process 7.

You may get away with 550sfm while turning (I think its kind of high)

What do you use for happy parameters for 304SS turning? Prior to getting this lathe online last year, I've never operated a CNC lathe. Trial by fire as I'm slowing bringing more of my product machining in house.


Some of Y'all will probably laugh at me on this one, and say it won't work.. But my first instinct on
this part, (getting through the interruption), probably a .150+ DOC(deep enough that some of the insert
is still cutting solid material), and .0016 (yes, 2 zeros) a rev at 175sfm... Using whatever inserts
Curtis sent me for nasty stainless.

I will give it a try! I've already ruined a inserted drill body, a boring bar, and a pile of inserts trying to figure out how to make this part. What's another boring bar? ;-)

Thanks!

20180627_122830.jpg
 
its like saying you cut all tool steel the same from annealed for 65 rockewell C hard. obviously not.

I hear you. But the problem is that I am ignorant. I'm a business owner trying to make my product. I wasn't born with any knowledge of where to start on feeds and speeds. The cutting tool manufacturers cutting conditions, backed off a little usually, is about all I've got.
 
I understand "Trial by FIRE".. I wish I knew about this place 18 years ago... Did this place
even exist 18 years ago????

If you change nothing else, Jack your DOC up.. You are taking 60 passes, almost half of them interrupted,
that is going to beat the shit out of your tool. DOC is FREE, most of the time.

In general, though not always, you want to get past your nose radius... Especially
when boring, if you are less DOC than the nose radius, you are pushing the bar sideways,
if you are past the nose radius, you start feeding forces straight back through the bar, kind
of like the forces on a drill.. It can can really help stabalize the cut, even if you have
to give up some feed..
 
Some of Y'all will probably laugh at me on this one, and say it won't work.. But my first instinct on
this part, (getting through the interruption), probably a .150+ DOC(deep enough that some of the insert
is still cutting solid material), and .0016 (yes, 2 zeros) a rev at 175sfm... Using whatever inserts
Curtis sent me for nasty stainless.

So tried that. It's a lot closer to working than my little passes were. I went with 0.140" DOC which nicely chews out the un-interrupted part in the first pass and then gets to full diameter on the second pass. It goes thunk thunk thunk, of course.

It did flake off the the top of the insert (see photo), but it still left a pretty nice surface finish and came out 0.01" under size. If I can reliably do that, I can finish the bore with a different tool and probably be fine.

Speaking of finishing. Is there some way to tell Mazatrol T2 that I don't want a finish pass?

Thanks thanks thanks!

20180627_150415.jpg
 
It did flake off the the top of the insert (see photo), but it still left a pretty nice surface finish and came out 0.01" under size. If I can reliably do that, I can finish the bore with a different tool and probably be fine.

I would use a C shape insert, right away. I wouldn't even try using that little corner radius, or that T style. If you don't have one, get one. For Roughing difficult Material and Interruptions, C and W hold up best.

As far as the Finish pass, isn't that it's own process? I forget, but Bob knows.

R
 
When I have an interrupted cut, my 'GoTo' method is high DOC and LOW feed.. Preferably get
past the interruption, and into a constant cut in one pass.... For example, when turning Hex
stock, I like my first pass to take all the interruption off and have the nose buried in solid
round material.. In your case you would have the nose in the interruption.

Some of Y'all will probably laugh at me on this one, and say it won't work.. But my first instinct on
this part, (getting through the interruption), probably a .150+ DOC(deep enough that some of the insert
is still cutting solid material), and .0016 (yes, 2 zeros) a rev at 175sfm... Using whatever inserts
Curtis sent me for nasty stainless.

Yupp, all that right there.

As far as the tool, my go-to boring bar for blind, interrupted, deep, nasty or all of the above: 2FL endmill set up as a bar.
 
I would go the expensive rout, and get a 1.5" flat bottom indexable drill. It won't care about the interupted cut. You could also bore with it, depending on your finish requirement,you might not need a boring bar. I would recommend a Sumitomo WDX for this, but many manufacturers make good drills that will work. If you do need a finish, at least that way you could fit a larger Ø bar in it.

If you need a finish... Ultradex S20S MCLNR/L4 will fit. US made, high quality tool, decent price. I buy all of my bars from them now.
 
By the looks of things - your bar and insert could be beefed up tremendously!

What is that - a 5/8 bar?
Going 4.5D deep?
A 1" bar would be good for the troublesome pass at least. It may be a bit tight for your first pass, but you could switch to it.

And a bigger guage insert will help too, even if it is the same style.


-----------------------

Think Snow Eh!
Ox
 
^^^^YuP….What he said.

Use up a tool location (for a second boring bar) or start with a bigger drill.

Always stuff the biggest bar you can get in there, make it
a negative rake (old school I know) and as big of a nose
radius as you can get away with.
 
First off I'm going to recommend running a larger drill, around 1.250+ if possible to give you more room to work with a 1" boring bar. Technically you could put one in now making sure that the first pass is deep enough to clear the min bore spec of the bar, but then you are making pretty wide chips with little room to remove them. I'm sure you are well acquainted at this point with the joys of chip evacuation when boring 304. Also 550SFM is too much for rough boring 304 with carbide, knock it down to 350SFM for now then try gradually increasing later if necessary after you have a reliable process nailed down.



Next, here are the guides to the nomenclature for ANSI/ISO standard inserts and boring bars.

Insert Designation Chart - provides ANSI and ISO designation code definitions for carbide insert shapes, relief angles, tolerances, chipbreaker codes, hole types, size values, thickness values, radius values, wiper lead angle, wiper clearance angle,

Boring Bar ANSI Designation Chart - provides ANSI and ISO designation code definitions for the boring bar material, diameter, length, insert holding type, insert shape, boring bar style, insert relief angle, direction, insert inscribed circle (IC)

There's a lot there to take in, just keep them handy and reference specific things as you come across them. In time you will start to remember the codes by heart and not have to look up everything. Know that some manufacturers use variations of the codes that are basically the same thing but just different enough that google won't find it right away. A few (Hertel comes to mind) sometimes use a totally proprietary naming system for products that are actually standard and interchangeable with other makes.

----------------------------------------------------------------

What I'm going to recommend first is a 7 degree positive insert ("C" relief angle), either "C" shape (80 degree diamond) or "S" shape (square).

If you need this tool to machine the bottom face of the hole you need a negative end cutting angle, like the following: 3.48mm Min Bore Diam, 1" Shank Diam, 12" 62181631 - MSC

If you need to get close to the bottom face but can finish with another tool you can use a neutral end cutting angle, like the following: 3.48mm Min Bore Diam, 1" Shank Diam, 12" 86461894 - MSC

If it is acceptable to use something that can't get near the corner (it looks like your problem interruption hole doesn't go all the way down the bore so this may be a good option in tandem with another bar) you can use a positive end cutting angle with a square insert. These are kinda rare in positive insert geometries but they are around: S16R SSKCR4 – Ultra-Dex USA

Those 3 are in order from weakest to strongest out at the corner doing the cutting. It's also possible to use the 100 degree corner of the C shape inserts for positive end angle cutting which is even stronger than the square inserts, but I can't find off the shelf boring bars for positive inserts that accommodate it.

----------------------------------------------------------------

For inserts what you need is a very tough grade with a large radius to survive the interruption. I'll make some specific recommendations for the 80 degree diamond insert bars I listed earlier:

Sumitomo CCMT32.52 ESU Grade AC6040M
https://www.mscdirect.com/product/details/59143065

Sumitomo CCMT32.52 ESU Grade AC530U
https://www.mscdirect.com/product/details/53983318

Start around 0.050" depth of cut and work up, that ESU breaker geometry is suitable for up to around 3 times that if the rest of your setup can handle it. My lathe isn't terribly rigid and I use mostly small bars so my experience is mostly on the lower end of that. I find these work well around 0.009" feed in a continuous cut for 304, but with your severe interruption you may need to run less to keep breakage under control.

If you can't get Sumitomo for some reason the following from Kennametal should be suitable. I haven't used this exact grade but I have used some of the harder inserts from this same range with good results.

Kennametal CCMT32.52 LF Grade KCM35
https://www.mscdirect.com/product/details/08342727

Kennametal CCMT32.52 MF Grade KCM35
https://www.mscdirect.com/product/details/08342743

Difference between them is the breaker, LF is for smaller cuts than MF.

------------------------------------------------------------------

You can also use 11 degree positive inserts ("P" relief angle) with mostly similar results for boring. Reason being the angle that the bar holds the insert. In the case we are looking at, a 1" bar for a CPMT32.52 will typically hold the insert perfectly level, for 11 degrees relief total. A 1" bar for a CCMT32.52 will hold the insert tilted down 4 degrees, which also comes out to 11 degrees total when added to the 7 degrees built into the insert.

Based on this, I generally use "C" inserts because of much wider insert availability (seems a lot of manufacturers have come to the same conclusion) and because they are more suitable to use for OD turning when needed.

------------------------------------------------------------------

You are going to get a lot of recommendations for using CNMG inserts, which is certainly an option but not one I like in this size range. If you look at the following: https://www.kennametal.com/en/produ...071/63840673/64022655/64022665/100001227.html

Look for A16TMCLNR4 under the catalog number heading then over to the γF° field. You'll see that they had to make the insert seat 14 degrees negative to fit it in that hole. This means that unless you get a high positive special finishing insert (that probably won't survive the interruption) with tons of top rake, you will actually end up with a negative, or at best neutral cutting action which doesn't work well at all in 304.

Furthermore, the insert and seat rising at that high angle behind the cutting edge as well as the top clamp both get in the way of chip flow.

In short I think that negative inserts in boring applications are best reserved for larger holes than we are dealing with here.

------------------------------------------------------------------

Note that I linked a bunch of stuff from MSC for convenience, but my actual recommendation at least longer term is to get in touch with some local distributors and have them send you the full catalogs from a few brands that they represent. Get used to finding things that way, cutting tool makers are generally old school and still haven't really figured out how to get their stuff into robust, intuitive electronic interfaces. This is getting better lately but there's still a long ways to go.


If you find any specific items you are considering ordering feel free to send me the relevant part numbers and I'll do a sanity check to confirm compatibility and such.
 
...Always stuff the biggest bar you can get in there, make it
a negative rake (old school I know) and as big of a nose
radius as you can get away with...

My thoughts exactly. I don't do any CNC, only manual machining but I learned a long time ago that
the biggest honkin' bar you've got choked up as short as possible is almost always the best way to bore
a hole...
 
IMHO theres anouther totaly diffrent approach you can try with 304 as well, as bob says DOC is generally free. 304 is not hard, but its odd to cut. I like to cut it with korroly HA chip breakers, the sharper cutting edge works well for me, i also don't go hard on feed, 5 thou is a lot in 304 in my experiance, bring that back to 2 thou and your interruption will be a lot less of a insert killer. Its all do to how 304 forms a chip as the cut starts, in mild steel 5 thou feed no issue even with a interruption, but 304 a finer feed really lowers the cutting force a lot more. Then regain the lost productivity with bumping up the DOC a lot 30+ thou DOC is easily doable with a 5/8" bar that far out, can go a lot more if you can get a bigger bar to fit too.

Sounds like your programming with mazatrol. Not sure how you do it there, but in std g code i would very much treat a interrupted bore like that as a very 2 step process, dialing things and especially the feed back as i encounter the interruption.

Other thing with 304 is surface speed, if in steel tool life V surface speed is a gradual thing were you trade one for the other in 304 is more a cliff edge, pays to start slow and work up and find that edge then it oftern pays to back off a fair bit as 304 also tends to vary even as you go down the same bar of stock.
 








 
Back
Top