Proper face grooving strategy. Need help

Hi,

previous face grooving jobs where done by milling because of the low volumes and now im having a 100+pcs production run with the face grooving operation so for that reason i have purchased Iscar's HFAIR blade with holder and 5mm width (0.2inches) inserts. But the problem is we are getting a very noisy cutting and the tool life is way too short... I have attached a grooving element drawing (in mm and inches) for detailed information.

Material is AISI 420 (32HRC), cutting speed 40m/min and 0,05mm/rev. The strategy is pecking with constant depth of 0.5mm. We do it for chipbreaking because im afraid it might break the tool if we will go full depth without intermediate retracting. The grooving element takes about 10 minutes to cut.

Maybe you can suggest me more productive cycles? Thank you

Don't plunge it, turn it out. Then you get the chip control you want and save the insert too. Rough it, then a single finish pass down each side.

Try using thinner inserts, like maybe 3mm or .125". Then stagger your plunges. Or work across the face at one plunge depth, then the next.

Doing face grooves on these small diameters kinda sucks. It's hard to get enough support under the insert in these small sizes. But I would not peck. Doing face grooves on gears I just plunge that baby on in there, no biggy. Then use a smaller tool to finish the contour.

But then, I used Manchester, not Iscar

Even did it that way on an engine lathe with a 1" wide high speed steel hand-ground tool. And a lot of horsepower ! But the trick there was to hollow grind the tool so that the chip curled inwards.

I wonder if you might want to try a hollow mill for getting most of the material out first ? Or you could even make one, say three round inserts on a tubular body. Sandvik had some smallish round inserts that were just held down with a screw, it wouldn't be that hard to make something up for experimenting.

Tonytn36 said:

Don't plunge it, turn it out. Then you get the chip control you want and save the insert too. Rough it, then a single finish pass down each side.

Click to expand...

Not sure what you have as a method here.
"turn it out" ??? What the heck does that mean to us with less experience than you?
Bob

40 m/min appears a little slow to me. That chromium steel needs to but cut faster in order to be heated up enough. Then the iron burns and the chips break more easily. I’d try out 80 to 100 m/min. Feed rate seems fine. Don’t peck when you have through coolant, remember that coolant never reaches the contact surface but cools the chips flying off and the workpiece.

A thought ;- Is there a Rotabroach type cutter that would leave you enough for finishing both diameters? .........if so I'd definitely give that a try to get rid of most of the metal.

CarbideBob said:

Not sure what you have as a method here.
"turn it out" ??? What the heck does that mean to us with less experience than you?
Bob

Click to expand...

I believe he meant feeding back and forth in X with incremental Z infeeds. At nearly .6" depth I'm not sure I wouldn't attempt the same.

Brent

yardbird said:

I believe he meant feeding back and forth in X with incremental Z infeeds. At nearly .6 depth I not sure I wouldn't attempt the same.

Click to expand...

Mmm, generally those face grooving tools are much stronger in the z axis than in x. So plunging in z then facing in x might be less than wonderful. Also, they have pretty poor geometry for facing, compared to plunging.

I could see maybe plunge, retract, move over, plunge, repeat repeat if you were worried about the depth of the plunge but ... personally, if the lathe has any poop, I'd rather run a stronger tool right up the middle, then profile the sides last, maybe with a second tool, instead of using a flimsier tool and trying to contour with it.

Sometimes pouring the coals to a strong tool works better than pussy-footing around with a flimsy one. Run a Gleason straight-bevel machine for a while and you won't be so nervous about taking metal off

but as always, ymmv ...

SeaMoss said:

Mmm, generally those face grooving tools are much stronger in the z axis than in x. So plunging in z then facing in x might be less than wonderful. Also, they have pretty poor geometry for facing, compared to plunging.

I could see maybe plunge, retract, move over, plunge, repeat repeat if you were worried about the depth of the plunge but ... personally, if the lathe has any poop, I'd rather run a stronger tool right up the middle, then profile the sides last, maybe with a second tool, instead of using a flimsier tool and trying to contour with it.

Sometimes pouring the coals to a strong tool works better than pussy-footing around with a flimsy one. Run a Gleason straight-bevel machine for a while and you won't be so nervous about taking metal off

but as always, ymmv ...

Click to expand...

For me face grooving has kinda been a PITA at this depth. I don't have any of the latest and greatest tooling. Typically I have to jack around at the post grinder modifying some old stuff we've have since before I got here. The insert takes a shit and the blade/pocket gets fucked up then I'm back to square one. So in this particular situation I'd "pussy foot" it in hopes I got thru the job. Funny I part 3 1/2" but face grooving not even close?

In the picture in the link is the outdated stuff I'd sift through to find something to attempt to do something as such and if you read the post and post #13 I haven't found a single do all system as of yet.

Brent


http://www.practicalmachinist.com/v...-tool-holders-324137-post2818000/#post2818000

yardbird said:

I believe he meant feeding back and forth in X with incremental Z infeeds. At nearly .6" depth I'm not sure I wouldn't attempt the same.

Brent

Click to expand...

Yes, that is what I was suggesting. Probably best to use a dogbone to rough it with first, then finish with the square insert.

I keep posting about these tools but they have been a game changer in my lathe department. Check out the Sandvik CXS line of small tools for Face grooving, I.D grooving, boring, threading and internal contouring.

The tools change over like and insert with one screw in the holder. You need to buy a holder but they are short money. I have gone over an inch deep with this .118 wide face grooving tool(Picture #1)on a 100 piece run in 6061 aluminum with little trouble.

yardbird said:

For me face grooving has kinda been a PITA at this depth. I don't have any of the latest and greatest tooling. So in this particular situation I'd "pussy foot" it in hopes I got thru the job. Funny I part 3 1/2" but face grooving not even close?

Click to expand...

Your tools look okay but kind of a motley collection If you are happy with partoff, just treat it the same way. It's real similar except maybe a little easier - the groove catches some coolant so you don't have to worry as much about getting coolant to blast in there. I'm guessing many people have the same problem as they do with partoff ? not enough feed ? Same deal, you want to cut, not rub.

Those Sandvik thingies look cool for little stuff. Because there are so many different diameters I made myself a holder for high speed steel tools - worked fine for short runs and was easier than buying all new support blades for every diameter. If the O.P. here is gonna do a gazliion parts, I'd do something similar except use standard bought-out support blades and clamps, then make up a bar with two inserts 180* apart. Then you could double the feed. Rough it out that way then come in with a smaller insert for a quick finish pass.

SeaMoss said:

Your tools look okay but kind of a motley collection If you are happy with partoff, just treat it the same way. It's real similar except maybe a little easier - the groove catches some coolant so you don't have to worry as much about getting coolant to blast in there. I'm guessing many people have the same problem as they do with partoff ? not enough feed ? Same deal, you want to cut, not rub.

Those Sandvik thingies look cool for little stuff. Because there are so many different diameters I made myself a holder for high speed steel tools - worked fine for short runs and was easier than buying all new support blades for every diameter. If the O.P. here is gonna do a gazliion parts, I'd do something similar except use standard bought-out support blades and clamps, then make up a bar with two inserts 180* apart. Then you could double the feed. Rough it out that way then come in with a smaller insert for a quick finish pass.

Click to expand...

Yeah its a hodge podge collection that's for sure. Face grooving isn't something I'm asked to do all to often, mostly I try to mount a top notch holder in a face adapter if possible? If the depth is too deep then I have to cobble something together out of shit from 40yrs ago, inserts are a incomplete motley set that are obsolete. Short of buying something for each individual job that comes up without lead time I have no choice to use this stuff.

I'm in a tool room setting, making stock repair parts for the tool crib for use in-house in aluminum die cast, mostly already hardened tool steel. A lot of times slower end up being much faster if it runs reliably.

Speaking of OP. In stead of pecking I would try turning like Tony mentioned, if the chip isn't breaking at least there will be more room for it with it wider then a plunge cut? Different insert geometry of insert could help with chip control. Not pecking IMO should help with tool wear?

Brent

evidence_UA said:

Hi,

previous face grooving jobs where done by milling because of the low volumes and now im having a 100+pcs production run with the face grooving operation so for that reason i have purchased Iscar's HFAIR blade with holder and 5mm width (0.2inches) inserts. But the problem is we are getting a very noisy cutting and the tool life is way too short... I have attached a grooving element drawing (in mm and inches) for detailed information.

Material is AISI 420 (32HRC), cutting speed 40m/min and 0,05mm/rev. The strategy is pecking with constant depth of 0.5mm. We do it for chipbreaking because im afraid it might break the tool if we will go full depth without intermediate retracting. The grooving element takes about 10 minutes to cut.

Maybe you can suggest me more productive cycles? Thank you

View attachment 213635

Click to expand...

Can use G74 for axial pecking.

sinha said:

Can use G74 for axial pecking.

Click to expand...

Hello Sinha,
To expand on your suggestion, something like the following could be used to execute multiple iterations of the G74 Cycle, thus turning a relatively deep groove into a number of shallow grooves.

#1=-14.95 (ABSOLUTE COORDINATE OF BOTTOM OF GROOVE INCLUDING FINISH ALLOWANCE)
#2=-5.0 (DEPTH FOR EACH CYCLE)
#3=0.0 (FACE OF MATERIAL)
#4=#3 (MAKE WORKING COPY OF #3)
WHILE [#4 GT #1] DO1
G00 X42.90 Z[#4+1.0] (START LOCATION OF CYCLE)
#4=#4 + #2
IF[#4 LT #1]TH #4=#1 (PREVENT OVER-CUTTING IN Z)
G74 R0.1
G74 X32.1 Z#4 P4.5 Q3.0 R0.0 F_ _
END1
G00 Z[#3 + 1.0] (RETRACT TO Z CLEARANCE LEVEL)
FINISH PROFILE STARTS HERE

Variables could also be used for other components of the Cycle, such as the Step Over in X, the Peck amount used in the Cycle and the width of the Grooving Tool.

Regards,

Bill

angelw said:

Hello Sinha,
To expand on your suggestion, something like the following could be used to execute multiple iterations of the G74 Cycle, thus turning a relatively deep groove into a number of shallow grooves.

#1=-14.95 (ABSOLUTE COORDINATE OF BOTTOM OF GROOVE INCLUDING FINISH ALLOWANCE)
#2=-5.0 (DEPTH FOR EACH CYCLE)
#3=0.0 (Z START COORDINATE)
WHILE [#3 GT #1] DO1
#3=#3 + #2
IF[#3 LT #1]TH #3=#1 (PREVENT OVER-CUTTING IN Z)
G00 X42.90 Z1.0 (START LOCATION OF CYCLE)
G74 R0.1
G74 X32.1 Z#3 P4.5 Q3.0 R0.0 F_ _
END1
FINISH PROFILE STARTS HERE

Variables could also be used for other components of the Cycle, such as the Step Over in X, the Peck amount used in the Cycle and the width of the Grooving Tool.

Regards,

Bill

Click to expand...

Hello Bill,

I always considered G74 G75 pretty much useless for anything more than material removal. Sure wish there was more functionality to the cycles. I've pretty much eliminated their use for anything other than chip breaking. It's somewhat cumbersome but I try to incorporate type 2 G71 G72 in situations where multiple passes or any contouring is needed, such is not the case here though. Plus I don't understand macros all that much is the only reason I mention this. If macro isn't in your bag of tricks a pair of G71 or G72 type 2 cycles meeting in the middle could be another option. Just a thought?

Brent

Tonytn36 said:

Yes, that is what I was suggesting. Probably best to use a dogbone to rough it with first, then finish with the square insert.

Click to expand...

Won't a standard dog bone or top-notch have a side clearance problem on the outside of the cut at this size face groove?
Seems pretty hard to stuff a standard inserted cut off blade in that arc also.

Is the Iscar insert showing signs of hitting or rubbing at the base of the insert on the outboard side?
Even the drawings on the Iscar catalog page show this possible problem.
Are your starting cuts at the max OD or the min ID of the groove?
Outside gives you more room to play as following inward cuts are done on the side of the tool with lots of heel clearance.
Bob

Long hand code it with pecks... Also as suggested above 40M/min seems a bit slow, maybe bump it up to between 70-85M/min.
I used to do a lot of flange face grooving and it is what worked best for me. So approach part say
G00 X22.5 Z2.0 (leaving a bit on X for final clean up)
G01 Z-2.0 F0.07 (Play with your feed a bit but 0.05 should be good, your first peck can probably go deeper but play with it a bit)
Z2.0 F3.0 (Full retract to get that chip out)
Z-1.5
Z-4.0 F0.07
And so on till you reach nearly your depth or maybe leave 0.1/0.2 on the depth for finishing. Then step over in X to do the rest of your roughing. When finished with that finish the profile inwards on both diameters.
So something like
G00 X21.0 Z2.0 (Starting smaller to put a 0.5mm chamfer on the face)
G01 Z0.0 F0.08 (Can probably up your feed on the finishing depending on the finish you want can also probably up your speed)
X22.0 Z-0.5
Z-15.0
X35.0 (move over a bit at the bottom to clean up any variations from the tool)
Z2.0 F3.0
X44.0
Z0.0 F0.08
X43.0 Z-0.5
Z-15.0
X34.0
Z2.0 F3.0

Also maybe stagger your pecks a bit to help with the chips coming out. So maybe on your first 22.5mm size go in say 5mm, then shift over to the next diameter, finish all your roughing pecks on the other sizes and go back to the 22.5mm in the end to finish it to depth. I have tried to "turn" as Tony suggested but with not much luck. The tools I use (Grip style solid holders from Iscar) cannot take bit side loads so it would take forever to "turn" it out. I would also suggest to go for a thinner insert, I haven't had much luck using wider than 4mm. Also with a 4mm wide insert I step over between 3-3.5mm per side on the roughing in the X.

OP?..WooooHoooo......Anybody home?



Brent