The ultimate tooling

[Frank]

Hi all, I've just been informed that the next job I program, is going to be a test of my abilities. We have just purchased a Horizontal Hitachi-Seki, and out of our 36 cnc machines this is the only machine capable of 10,000 rpm's, and of course all the other bells and whisle's. We have an aluminium engine block currently running on a K & T horizontal machine....which is a very slow running machine. I know just moving it to the Hitachi, the tool change time alone would change the total run time. I have been told to reserch tools, and holders, because the big guy needs to justify the price of the machine, by the way I write this program. So what I need from all the experts on this board, is how fast can I run this part, and what tools would give me the best bang for his buck ? I've read here postings about the Iscar feed mill w/22mm inserts, do I need to use heat shrinking holders for end milling ? And what is a good starting spindle and feedrate for say a 3/8 - 16 tap ? His words were "I don't want to walk over and see this machine running drills and end mills at the feeds and speed you currently are using" So I would really like to impress the sh-- out of him.

 

any advise would be greatly appreciated !

 

 

Thanks,

Frank

[Rekd™]

It's not just tooling, tool change time and RPM.

 

It's feeds rates, acceleration, and most importantly with a horizontal, RIGIDITY and CHIP REMOVAL. Those are your friends. If you don't see 50% cycle reduction or better after all is said and done, I'll come by and hook you up..

 

'Rekd

[chris m]

All of the major manufacturers have Aluminum-specific facemilling and endmilling cutters that offer high material removal rates, 2500SFM is typically all I have the horsepower for but the tools will take more. As far as drilling goes, the drill itself has a lot more to do with holemaking speed than the machine does. If you have high-pressure coolant through I'd take advantage of it and push the tools up to the high end of the manufacturer's recommendation.

 

C

[SLJ]

Get ahold of your local Iscar rep. and have him take a look at the application. Our guy has helped tremendously on a few special jobs. We use them more for the harder to cut materials, but he has great tools and ideas for alumn. too! If you have any qty. to this part, look at thread mills instead of taps.

[mike_f]

hi Frank,

if your mainly cutting alum. I would suggest looking at SGS Ski-carbs, they rock! they have a honed cutting edge that keeps them from pulling aggresively into corners thereby eliminating most chatter. I work in a small shop with a limited budget so heat shrink tooling is something I just dream about, but I have used Iscars SHORTiN collet chucks that have a very short gage length, great rigidity and tir but can be a problem sometimes with clearance for coolant nozzles and things. I also use solid end mill holders made by a company called "Briney",they grind the i.d. slightly off-center toward the clamping screw which helps with runout inherent with those types of holders.

for pure speed and reliability i use form taps anywhere i can (mallable or ductile materials) especially in mach's with rigid tapping, one thing i try to keep in mind though on my other mach's is if you break one in a part you're s.o.l. because you can't burn them out.

good luck, happy and safe holidays to all.

Mike

[mayday]

your boss got bucks?

takes a lot of R&D to dial in what your gonna do here. some things to consider

 

custom made drill chamfer combo ( thru coolant a must)

Allied Spade,Sumitomo,OSG

 

definetly roll form taps (watch your drill size)

OSG

 

Exocarb-Disk cutters - OSG

 

skee carb end mill - SGS

 

that gets you started. you will have to rethink how you proccess your work switching to this type of tooling, but your boss will see a big change in produtivity out of the machine.

[Scott Bond]

Good Morning Frank

This is great,, I will learn something.

 

Three things

[1]Be bold- think it thru, don't let anyone screw up your personal style on this part.

[2]Don't let anyone watch the first parts run, the gossip will chew up your reputation and deminish the impact you final work.

3]Speed will not be enough deoderant if the part is ugly.

[Harryman]

Given that you are setting this machine up for a known product, you should be able to establish a very reliable tool list. With that kind of confidence I'd say go for the good stuff (heat shrink) up front. It's easier to capitalize expensive tooling in the initial purchase than expense the tooling later. By knowing what cutters you need to hold for your product, as opposed to a job shop set up, you should reduce the boss's fear that you're buying uneeded tools. A super accurate balanced holder will spread chip load more evenly across all flutes which is also important when running the high end coated cutters to max perforance.

[mmonica]

We have 3 15,000 rpm CAT 50 spindles we use for machining aluminum. We looked at heat shrink tooling and it was expensive. We use tool life management and backup tools and we like to have them the same length (within .0005 on a optical presetter). The heat shrink rep would not commit on hold this tol on his equipment.

We use Command toolholders, they have a nice selection of coolant thru balanced toolholders. We have them install the pullstud and balance the assembly to G1.0(the balance could be out by G2.5 if we installed the pullstud). One note to add, we redline our spindles at 10,000 rpm, we doubled the spindle life this way.

Good luck on your new equipment!

[Frank]

Wow you guys are unbelievable ! thanks for all the responses, I've allready called an Iscar rep to come by, and I'm checking into using roll taps instead of cut taps. Another concern is the way we are going to fixture it. What we have done in the past is machine the blocks ends, rough the cam and crank, and finish the bulkheads on the horizontal machines. Then run it between centers on a vertical machine. Since our new machine has a pallet changer, he wants to machine both operations on the horizontal. the second operattion the block will be standing up, so rigidity will be a problem. My thought is to semi-finish the cam bore and hold the dia. so when I stand the part up I can make some kind of bar that would slide through the cam bore top to bottom, and act like a precision bolt.

 

Thanks again,

Frank

 

PS Rekd.....the boss may take you up on that

[mayday]

fixturing:

make a base plate to fit your pallets. fab on bosses to mate up to the cam/crank bores. machine them,add hold holes for clamps set the parts on and away you go. everything is blocked in and it cant move around on your fixture. makes for quick setup and tear down also. key in your base plate or block it in off the pallet sides. depends on your pallet configuration

[robk]

My advice... Look into probe systems for the machine.

[Guest CNC Apps Guy 1]

... don't forget the High Pressure Coolant and some coolant-thru drills. This will greatly increase your MRR in hole making.

 

10k really is not that much but I would not run side-lock holders that fast. Shrink fit is definitely much better. TIR is nearly 0 and as a consequence you'll get better tool life even at elevated feeds and speeds.

 

Look at getting AICC (G5.1Q1) for the control. It's a step above Look Ahead (G8P1) and gives you more control over Acc./Dec.

 

JM2C

 

 

JM2C

[Chris Rizzo]

quote:

---

Get ahold of your local Iscar rep. and have him take a look at the application

---

+1000

 

Let the reps earn their money. Put them to work for you. Bring him in and show him your job, machine, existing opperations, expectations, etc. They should come back with recommendations on tooling, inserts, speeds & feeds, material removal rate, holders. You can spend alot of trial and error time on your own, but bringing in a DECENT rep. will save you tons. I've found the ISCAR reps to be very knowledgeable and honest. Sure the reps rely on making sales, but a truly good rep. knows the value of service and assistance. Some of the other reps should be selling used cars, not tooling!

[Frank]

I know I read recently in this forum about a Iscar feed mill w/22mm inserts can anybody be more specific please

 

Thanks,

Frank

[robk]

Frank,

 

I went to the Iscar seminar a few months ago and from what I remember, I don't believe that the Feed Mill is recommended for aluminum. We use it in here with good results, but it is in 420ss. It's still scary to see a cutter that big go that fast.

 

[ 12-18-2003, 01:58 PM: Message edited by: robk ]

[Hardmill]

Check out Sandviks aluminum insert tools.

These babies scream, and will remove more

cubic inches of material than anything i've

seen out there.

 

PEACE

[chris m]

Sandvik's CoroMill 790 cutter looks like it would be pretty sick in a high-horse, high-rigidity machine. These sport a 22MM insert option; I'd call the Sandvik guy and say 'come down and look at my new machine; treat us right on the $$ and every tool in it can say Sandvik on it'

 

Whomever you use for cutting tools you should definitely get them involved and let them spec tools, speeds/feeds, give you demo tools, etc.

 

C

[mike_f]

I haven't beeen around long and don't know how to insert a quote, but chris_m is right, get demo tools ! these reps will be tripping over each other to sell you their stuff, it seems like a waste some times but for me it usually pays off in the long run to let these guys come in and "go to town" with their tooling, on my machines in my parts, real world. They will all claim to be the best, let them prove it. I'd like to see iscar's new helitang ( i think thats what they call it) in a high h.p. rigid set-up. it looks sweet

[McRae]

This Installation will be very interesting indeed. I once out preformed a K&T using a file fashioned with an elastic band to maintain the reciprocating motion...

 

Anyhow, This advice here is excellent, but I would like to suggest that a 3 pronged attack take place here.

 

The first part of the question has to be, how many parts do I need to manufacture and what part of the total cycle takes the longest anount of time to do. If for example a $5000 PCD Milling cutter that will run at 3 Million SFM will only save .02 seconds per part on a 30 minute cycle, then really there is no savings by using top technology. Layout your current process steps sequentially and assign the current time to the operation. With this information in hand, sort the data by time and then chart the results for a paretto analysis - look for the 20% of operations that take 80% of the cycle time, you will be surprised I'm sure. (Any Boring of the part?? - Think Helical for Roughing)

 

Step 2 - Now armed with Data - (without data, you are just someone else with an opinion) discuss with 3 suppliers their suggestion for tooling alternatives for improving the machining cycle - and as Scott Bond indicates - the part quality and appearance need to be a given. Don't focus on "Cost" at this point, look at productivity first and formost. Also make the suppliers complete a time study on the part features and then you can consolodate the information and look for the biggest opportunities for improvement and also select the strongest pieces from each supplier. Make the orders contingent on a given quality expectation - CPK of 1.5 or better - this will make the weak companies cower and shy away and this is an indicator of actual long term reliance and capability of the tooling. Focusing on the result, rather than the buzz and trends in current tooling will als help (ie - Shrink or not to Shrink - Let the process capability answer that for you)

 

Don't get snookered by their fancy presentations - your customer doesn't care who had the nicest power point presentations - they will only see the parts that you ship to them and get angry if they are late because you had to wait for a $5.00 Insert to arrive from Isreal/India/Sweeden/Japan and then get even more discusted when the parts don't fit!

 

Step 3 - Dial in the setup information and get the best fixture that you can with an eye on Quick Change Over time and something that will allow the most features to be machined in one setup.

 

Best of all, watch the profit margins - sometimes expensive equipment will distort our thinking that we need to keep it busy all the time rather than using the right tool for the job. Don't let too much stuff creep into the mix.

 

[ 12-19-2003, 12:42 PM: Message edited by: McRae ]

[Frank]

thanks again for all the great information. I am going to be doing the cyl. bores while the part is standing on end, and I suggested Helix boring, we have a felix cutter that works great going through solid stock, but can only travel .08 per rev. I was wondering has anybody used a say face mill, or something with an insert that can helix bore but travel deeper and faster than the felix cutter ? I think blasting through them with a twin blade Kaiser bar is pretty fast but I'm worried about the part being pushed on the upper bores.

 

Thanks,

Frank

[F. JAVIER]

One thing to keep in mind is that this will be the first of many jobs that might be put in this machine so I would not tool the machine "just" for this job, also think of methods that will allow you greater productivity without sacrificing the future production.

I agree that shrink fit holders does not fit the needs for your speeds.

focus mainly on good roughers and ask for the thru spindle coolant, it can be a great timesaver for your application.

Good luck