What's new
What's new
By:
Advanced search…

CNC Lathe Face Grooving Help

D

dstryr

Diamond
Joined
Jan 22, 2010
Location
Nampa Idaho
This may be a dumb question but I am very new to Lathe work and have to do some face grooving in 304l. It seems everytime I get this job in I have to dial out this problem. My solution will work for a full batch and then the next time I run the job it fights me again. I have an iscar face grooving tool with a .156 wide insert.

The groove dimensions are as follows
OD: 1.230
ID: .5
Depth .05

I'm currently plunge grooving out the material and then turning the bottom depth and walls but somewhere I'm getting chatter. I think it is due to the first initial plunge cut.

On face grooving, the tools show min and max diameters? I can't quite wrap my head around this specification? Is this the first cut diameter range or max / min range for the tool?

So if my tool range is from 1.15 to .4 and I try and take a cut at 1.230 it is going to rub correct? Will I be successful if I take a cut at 1.0 and then step out to the larger diameter?
 
dstryr said:
So if my tool range is from 1.15 to .4 and I try and take a cut at 1.230 it is going to rub correct? Will I be successful if I take a cut at 1.0 and then step out to the larger diameter?
Click to expand...

Correct, it will rub that way. Your proposed method should work fine. Don't baby it with the feed rate. Run it in at .004" to .008" per rev for an insert that wide. You also shouldn't have to step it out to the larger and smaller diameters. With the right insert and a depth of only .05", you should be able to plunge in at Ø 1" and then just face cut it. No need for multiple plunging.
 
PixMan said:
Correct, it will rub that way. Your proposed method should work fine. Don't baby it with the feed rate. Run it in at .004" to .008" per rev for an insert that wide. You also shouldn't have to step it out to the larger and smaller diameters. With the right insert and a depth of only .05", you should be able to plunge in at Ø 1" and then just face cut it. No need for multiple plunging.
Click to expand...

right now I'm running at around .003 and on the first cut it really squeels which makes me think its rubbing but I put dikem on the holder and didnt see anything.

By face cut you mean plunge in and then turn the dimensions?

Another problem I'm having is the outside of the groove deflecting on initial plunge. I've tried multiple depths of cuts and even tried programming .001 deeper on the initial cut but I still get .001 difference form the outside to the center on the depth.

I'd like to get it closer if I can.
 
My current technique is rough plunging at .049 deep and then profiling the walls and the bottom at .050 deep.

The material is 304L.
 
If it's squealing like a banshee, it's in need of FEED. Double it and see what happens. Your problem of deflection needs to be properly analyzed. Just how thick is the workpiece, how much of it are you chucking and how rigid is the setup? Are you trying to do a big workpiece out of tough material on a little import home shop lathe?

It really sounds to me like the deflection problem might be one of work-hardening from too light of a feed rate. What cutting speed are you using, what is the full spec of the insert and holder?
 
PixMan said:
If it's squealing like a banshee, it's in need of FEED. Double it and see what happens. Your problem of deflection needs to be properly analyzed. Just how thick is the workpiece, how much of it are you chucking and how rigid is the setup? Are you trying to do a big workpiece out of tough material on a little import home shop lathe?

It really sounds to me like the deflection problem might be one of work-hardening from too light of a feed rate. What cutting speed are you using, what is the full spec of the insert and holder?
Click to expand...

It only seems to squeel loudly on the first plunge. It gets better as the cut goes to smaller diameters.

SFM: 400
Feed: 003 ipr
Depth of cut : .049 on rough
.001 on finish

Iscar Integral Face Grooving Holder with GRIP .156 wide insert.

Work piece is 1" 5/8 dia
Holding on .125 in pie jaws.
Material is 304L waterjet out of plate . I mill the back skin off the blanks and cut a step on them for proper grip due to waterjet taper.

Doing this on a Doosan CNC Puma Lathe

I'm going to trouble shoot more tomorrow when I go in for a bit. I'll try upping the feed. Should I change my program to leave more for depth of cut?
 
With the right insert and a depth of only .05", you should be able to plunge in at Ø 1" and then just face cut it. No need for multiple plunging.
Click to expand...

Not sure I understand this. The difference between his O.D. and I.D. of the groove is .73 in diameter. To catch all that in one plunge would require a tool width of .365 wide. Is that what you're suggesting to him?
 
All I'm saying there is once you plunge in, stay there and feed it in & out along the X axis at the .050 depth with perhaps a .005" per rev feed rate. A .050 depth of cut is cake for most .156-wide groove/turn inserts. Another reason I asked just what insert is being used. Some are much better than others for turning.
 
PixMan said:
All I'm saying there is once you plunge in, stay there and feed it in & out along the X axis at the .050 depth with perhaps a .005" per rev feed rate. A .050 depth of cut is cake for most .156-wide groove/turn inserts. Another reason I asked just what insert is being used. Some are much better than others for turning.
Click to expand...


Oh, now I get it. Brain was stuck on a one lane track.:o
 
dstryr said:
It only seems to squeel loudly on the first plunge. It gets better as the cut goes to smaller diameters.

SFM: 400
Feed: 003 ipr
Depth of cut : .049 on rough
.001 on finish

Iscar Integral Face Grooving Holder with GRIP .156 wide insert.

Work piece is 1" 5/8 dia
Holding on .125 in pie jaws.
Material is 304L waterjet out of plate . I mill the back skin off the blanks and cut a step on them for proper grip due to waterjet taper.

Doing this on a Doosan CNC Puma Lathe

I'm going to trouble shoot more tomorrow when I go in for a bit. I'll try upping the feed. Should I change my program to leave more for depth of cut?
Click to expand...



As suggested before, either increase feed or decrease rpms if it squeals. At the outer diameters the piece is turning faster than at the center, like a an old vinyl record.
G96 (constant surface feed should help, but it isn't perfect, so help it along by adjusting feed or speed when you need to.
I wouldn't leave less than .003-.005" for finishing to make sure that the insert gets underneath the cut instead of rubbing.
 
Fwiw and to support what Dave said, I try not to take a finish cut in stainless. Rough to size, or take a fairly heavy last pass in lieu of a Finnish pass. Stainless doesn't like a light cut.
 
Okay so I made a few modifications and the part is a little better but not where I'm happy yet.

SFM now is 500
feed is now .005 ipr
Rough DOC is .035
Finish DOC is .015

I'm getting tearing the insert width away from the outside wall and chatter in the bottom corner of the outside wall. Also th e groove has about .0015 of variation on the depth from the outside wall to the inside wall. I'd like to beable to get it down to .005-.001
 
Bumping this thread. I am face grooving some transmission gears and am trying to produce something the image below but instead of chamfer edges, I will have rounded edges from my rounded bit. The gears are not crazy hard but pretty hard. A nice file is still able to marr these gears.
I am doing this on a manual Leblond 15" with a Iscar HFPR 6030 IC428 cutter with tip width of 0.235."

It cuts fine but when I get to about 90% tip contact, it chatters like a mofo! It also grabs and removes chunks sometimes. Any help here guys? Is the setup not rigid enough?

259006d1348540475-lightened-gears-lightened-105-115-gears-sept-12-001.jpg
 
I have had to do this very same process for years with the same Iscar groove tools on an array of materials from 17-4 stainless to super alloys. I had the same experience with chatter, tool deflection, chiped inserts and so on.

Ultamatley, what I found to work best is use two tools. Let's say we are machining a gear face that's 4.0" dia with a 1.0" dia hub, going .250" deep. I'd use a .156-.187 wide tool to plunge/peck out my rough diameter and depth using about 75% stepover, leaving around .010 per surface. Use an aggressive chip breaker.

To finish, I'd use another tool, around .124 - .156 wide, again with an aggressive chip breaker. This will allow your finish tool to stay sharp due to not having to rough. "Profiling" or "contouring" your entry and exit for the internal fillets will greatly reduce chatter from occurring.

I know this requires more programming and cost of another tool but it's well worth the money and time spent if you are running any level of production.

If you have a very large quantity and a lot of material removal then the next best step to take is use ceramics. I started using Greenleaf ceramics for face grooving some super alloy bevel gears. They are the cats ass for this process. I can discuss more in depth if anyone interested.
 
To elaborate more on the subject and why it works:

Plunge / peck your rough cycle, contour / profile your finish.

The " peaks " and " valleys " left from the rough process inherently help prevent the finish tool from chattering.
 
Those tools need to deflect from cutting force to give clearance on side cuts. No clearance and your full .156 is in contact and you get chatter.
Plunging you need to feed aggressive or you will get chatter.

Read thru the section on how to use and they will give recommended starting points...Iscar also has a great tech support line...use their resources, it is free and it is what they do.

I do not use their facing tools much, but for similar turned diameters with a more slender .125 insert they want a minimum of .012 DOC fed at .006 to give proper deflection. They also recommend certain approaches to attain flat square shoulders...may take up to three cuts to get your face groove correct...the good news is once you bump the feeds the extra cuts do not add time to cycle.

Your feed is on the light side for the tool and your dealing with 304SS, I'm figuring your fighting work hardening that isl compounding your problem.
 
SIM said:
Those tools need to deflect from cutting force to give clearance on side cuts. No clearance and your full .156 is in contact and you get chatter.

I've ground a small "V" in the face of these inserts to relieve the center so your don't get full contact, seems to help with the chatter.
Click to expand...
 
also dont forget that 304 in plate can be realy easy to machine one time and the next one its a pain in the ass and always get hard like hell, i personally try to avoid plate most has possible.
 
Replying to the "thread topper guy" with the gears:

Looking at your part - I would rather try a 35* diamond shaped insert instead of a face groove tool.


Note fellas - the 304 guy was from 2010, the gears guy is 2012


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

Think Snow Eh!
Ox
 
You must log in or register to reply here.

Similar threads

M
ISCAR Tang grip face grooving
Replies
11
Views
636
musall37
M
D
Turn groove surface finish
Replies
11
Views
816
bradleyk
B
B
EN24T
Replies
2
Views
135
???
???
S
CNC mirco grooves
Replies
10
Views
609
???
???
M
Inquiry About Deep Grooving or Cut-off Large diameter
Replies
7
Views
389
sinha
S








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top