CNC Power vs. Cycle time

We are figuring the amount of Z-axis thrust required to push a 1.5 inch drill through 316L stainless steel at .004" per revolution. I have this figure as 3,411 lbs using Machinery's Handbook.

That is over the capability of the machine we are looking at.

Let's say you had to make a ring out of stainless on a CNC (using a CNC lathe for finish requirements). The ring is 1.625 OD 1.5 ID, .625" long.

How long would this part take you to make? Would you push a 1.5" drill through it to make that hole? I seem to think you could push a 3/8" drill to pop a hole and single point cut the entire ID. Why use a HSS twist drill when you can single point the hell out of it with a box tool?

Am I thinking about this wrong, or do we want to look into a machine with the Z-axis thrust to drill up to these sizes?

Atetsade, I think I would use a .75 indexable drill. Punch you hole to depth, and then use the drill to "bore" the hole. What I mean is, if your outside flute of the drill is colinear with the x axis on the cnc lathe you can use it as a boring bar. Simply move o a larger dia. and drill again.A straight "g01 z-whatever f.005)or a g85 command. A .75 drill should not take that much in the way of h.p. or z axis thrust. Finish the hole using a boring bar, if you need to for a tight tolerance. Best of luck.
Doug.

Doug925 is right. That would be the way I would approach a job such as this. Depending on the finish requirements of the I.D. you could probably finish with this tool also. There are alot of indexable drill manufacturers out there and some are quite pricey. For the best price/performance ratio I use the SBM brand (Komet style)from US SHOP TOOLS. www.usshoptools.com


You can see the catalog pages of these drills at the following link:

http://www.usshoptools.com/2001/2002_03_sitemap_pdfs/indexable_cutting_tools/174_181.pdf

is production machining a sell out?

What do you mean buy a "sell out"? If you mean that you must make as many parts as quickly as possible with minimal quality standards jsut to beat the other guy by a nickle, yeah it's kinda like that. But with a little innovation and a lot of motovation (and some perspiration) production work can be very rewarding.

Oh you're talking about an insert drill. That makes sense.

Shall I take it to mean, then, that understanding the options available to you in CNC lathe machining is a matter of creativity? if that's the case, you're only limited to cutting that which can be fit into geometry and that which can be cut.

of course, you guys have what you want or you know what you want, in a machine. it's probably a matter of familiarity, knowing whether or not this machine or the next does automatically vary its spindle speed to maintain a finish, or if its main bus is big enough to handle quick movements, or if its programming will be robust and adaptable.

what are some of the things you would absolutely demand in a controller that may not be in a mid-nineties machine? rigid tapping? linear/circular controllable axes? designation system incremental and absolute?

I agree with Doug(the previos post) I would look for lots of canned cycles, graphical varification, quick editing, already loaded "quick cycles"(preprogramed thread, tap cycles) LOTS OF MEMORY, and a 3.5 floppy is always nice too. As far as the machine goes, BIGGER is always better! Less h.p. worries, less setups, and less hassle. You can always machine a small part on a big lathe, but not always the otherway around. Unless you are making very small parts.
B.t.y. I was talking about an insert drill. My personal (this week only) favorite is Kyocera. Best of luck, Doug.

Thanks E-stop, Doug, doug. Sorry to be so agonizingly green. No worries.

We bought our Daewoo 10HC, will be arranging delivery on Monday. There's about a bucket of tooling coming with it, so I'm going to wait until I can see that stuff before I have tools bought.

I don't think we're going to need more than 10 tool holders to start.

I'm beginning to get excited about this project. I doubt this lathe will match our screw machines in production, but hey it might.

I would go with the insert drill, I have a Komet 1.5 Dia. indexable drill that works really good in 300 or 400 type stainless steels, I'm not sure what the thrust load is but I don't think it takes near the load as a twist drill, I can drill 300 type stainless at 1200 RPM @ .004 feed and set the drill to drill 1.490 dia. then use the drill or a boring bar to get the last .010 out of the hole if it has to be a perfect size.

Consider 316 SS. You can purchase tubing which is readily available off of the shelf. Less waste, faster cycle, much easier on the machine.

Let's not forget that 316 SS will need to be chamfered or radiused on all edges. This is pretty hard to do by hand.
If you don't do it you'll have burrs that are imposible to deal with, especialy if you want to push you tools a little, when the edges get a little dull watch out.
Here is my summary:

If you buy tubeing, get seemless.
1-rough turn
2-1-3/8 insert drill (if bar stock)
3-rough bore
4-finish turn
5-finish bore
6-chamfer back ID edge
7-chamfer back OD edge and cutoff

Job is no brainer, but it can be turned into a nightmare if not aproached right.
If you have small quantity, you may want to use just one tool for turning and one for boring.
Use short and stuby insert drill, you may have to peck it to break chips into short chunks, do not use full retract, retract only enough to break chips then go gack in.

Why seemless tubeing ? Because the seem is on the ID of the tube and it will mess up your boring bar insert. Area around seem is harder and fat, it will cause part to spring out of round after cutoff.
If you do tube, all of your boring chips will get packed in the tube, constant fight to get them out, solid bar will run much cleaner and more consistant, it may be trivial but drilling the stock is not all that significant or dificult.

Oh, and cycle time wars are for the birds.
No matter what is involved you have to find compromise among all variables. Pushing fast only means you will spend more time recovering your setup, clearing the debree, missmanaged chips and so on ............ or you can set the pace and have predictable, managable and steady production that will add up to expected.

What's that ? ........ you quoted the job to beat your competitor so now you have to run it 15 seconds a peace, sory to hear that because one condition stayed the same as you were playing a hero without knowing if that cycle time was posible to acomplish, you see 316SS is still 316SS and you have to cut it at speeds that will not fry your tools on contact.
Better pay attention when that greesball tels you it can't be done, he may know more then he is getting credit for.

Please note, caracters in this scenario are fictional and I assume no responcibility for missinterpreted statements or things being taken out of context.

[This message has been edited by Vic (edited 06-27-2003).]

I was thinking about grooving the face of the bar to the depth of the length of the ring and making a recess tool with drill rod to come in and break the corners.

I would shoot rings all over the inside of the machine I think, but cycles might be a little faster and there would be less chips.

and if that's the case, couldn't I groove with a good size insert that will leave the interior 'slug' tapered enough so the ring will spin off and fall somewhat reliably? A parts catcher made of tin could be affixed to the arm that would catch something like that. then the slug would be cut off to fall onto the chip conveyer.

well, assuming all of that and assuming provided tool geometry to do the job, how would you finish the critical ID? is HSS tooling good for finishing stainless, and if so would it last very long? the shank would have to be pretty thick to dissipate heat but not too thick to fit into the big tapered groove.

anyway I'm totally rambling at this point. would anyone care to comment on if they think it would work?

I suppose you could do face groove past the cut off depth, chamfer outside edges and cut off the part.
This would leave you with cutting off the slug in the middle before you can do another ring.
Now, managing front and rear ID edge is in question, it requires elaborate workaround or extra operation on bench lathe.
I still don't know what the specs are on sizes and finishes, but rest assured plowing through one feature will impair you and penalize you somwhere else, cutting off the middle slug looks atractive but it complicates finishing ID. Use of wide face groowing tool will prove to be a pain, slowing down the process and eating tools.
You must go with indexable carbide tooling to manage the flow of work. 316 SS is not a cheese but it is very managable with right tooling and order of operation.
In my opinion, drilling is the only way to remove ID stock and provide faverable conditions for all other work.

If you don't have a parts catcher you can still automate the process to some degree.
Have a bucket under the spindle, yes it will collect chips as well, manage your chips to prevent long strings, swap buckets at apropreate intervals and collect your parts while machine runs.
To prevent slaming parts all over the inside of the machine, use normal feeds and speeds during cutoff, .01 before breaking through, slow down RPM by about 50%, use feedrate of .0005/rev, part will drop in the bucket and fall on mix of chips and other parts.
Your only burr should be at the intersection of ID grooving tool and cutoff tool. Use of 5 degree slanted cutoff insert should leave ring on the barstock and not part, extend the cutoff tool path down untill you remove the leftover ring, this preps the bar face for locating against the bump stop as you go on to the next ring.
Your key to productivity is in controlled layout of tooling and sequences where each tool carries it's own load and works to it's best potential. Timely tool changes keep dimensions on target and running without stops.
Having more detailed info on all aspects of job would help me narrow it down to minimum required but sufficiant process for you.

In production on 316 st st we would use the nearest drill to 1.5 = 1.437 or nearer (36mm)to enable us to finish bore with 1 cut.The drill can be put in at 150 revs on 316 with a feed of 0.008 per rev if you have the power.To use a u-drill or a tipped insert drill 0.750 dia will take the same amount of power anyway.
If you calculate the both cycle times , boring out the after the 0.750 tipped drill it will be close but you will use a lot of tips.We run 80% in stainless and find the production is up over the day using a HSS drill over the tipped method.
We use the Cincinnati Hawks A2100 control with a 28 horse motor.

P.S. We always do any heavy drilling first
and face after (0.20 - 0.040)

Okay, when we started this topic the main concern was z-axis thrust.

NOT cycle time!

If, as stated before, you only have 15 sec.'s to make the part then you will need to be creative. I would start by facing and turning the outside to dia. I would still use a indexable drill (1.437 dia.), and then bore using a bar if finsh, and tolerance make it neccessary. Also a 82 deg. bar will enable you to chamfer the ID where the part off blade will cut. Switch to a sturdy, THIN (.093) groove/turn bit, and plunge to 1.48 @ .0035 per/rev. retract with a g0x1.55, z+.01 from part location, feed back to 1.5, chafer from z+.01 to z part location while feeding in x from 1.5 down to 1.48 @ .005, then part @ .003. The part SHOULD fall into a bucket, or a big piece of egg crate in the chip pan. The overal part can be made in 15-25 seconds to the best of my knowledge. This is all without any handwork. If you have a bar feed then you are ahead of the game. This will enable you to shave 5 seconds off the total time.
Now having said all that... I hope next time you will have a greater margin for making the parts. I can, and do all that I have just said previously, but I do not like pushing my machines that hard just to make a few pennies. If I were qouting the labor only, I would be looking for $1.25 ea.
My .o2
Doug

15-25 seconds / pc ..............!?
I thought guy is making 1.625 OD x 1.5 ID x .625 long ring out of 316 SS, not .25 x .25 pin out of brass.
Seriously people, cycle times are messured from button to button, and there is no way in hell you can cut this ring in 15-20 sec unless you are doing everithing with one tool at 15000 SFM.
No matter how you cut it, process requires at least 3 tools:
1-bump stop
2-drill
3-dog bone
Just indexing turret 3 times and moving stock to a start position will consume 20 seconds if not more.
Drill and bore to size and chamfer front ID edge, then use dog bone to face, turn and cutoff.
You should deburr back ID edge by hand tools, if any of this crap can actualy work you are still loking at few minutes a pc and a lot of hand work.

In all reality, unless ring is part of the fence that we'll be installing along Mexican border, it needs to confirm to some standards, good luck pal.

15 - 25 sec / pc , yeah dreem on, another ring that will go to China or India because there they can cut it in 5 minutes a pc for 25 cents/hr labor cost.

[This message has been edited by Vic (edited 06-30-2003).]

I forgot the Z axes trust topic, never had to deal with such a thing in past 13 years, I drilled "few" holes in 300 series SS, 1.5 dia. insert drill 6" deep in 304SS, 200-300 SFM, .002-.003/flute chipload, machine never blinked.

Generaly, if you can fit that kind of stock through machine's spindle, you have adequat power to cut it, if you get to entusiastic, watch your load meters and stay below 50% of the scale initialy, load rizes as inserts get dull, index inserts on drill BEFORE meter hits red zone or you will stall the machine and perhaps smoke something.

If we`re talking cycle time here and 15 secs seems to be it,you can forget cnc.Get the job on to a multi.The multi will make three while the cnc is indexing.This should liven it up a bit.
Regards,Mark