Drilling and Milling Questions...

[cterry352]

Using a Haas VF3 older machine, 15HP.. Machining A572 Grade 50 material .750 thick.. Drilling three 13mm holes, with a 1.5 Dia hole in the center.. Pretty good on the 13mm holes.. Need some info on Drilling the 1.5 hole.. has a +.005 -0.00 tolerance.. So as of now im center drilling, drilling with a 59/64 drill, roughing with a 5/8 4flute endmill, then finishing with a .500 4 flute endmill... I would like to use a bigger drill and then just use one endmill to find... maybe a 5/8 6 flute carbide..?? Looking a using a indexable drill... Will take any info i can get.. THANKS...

[mfgbydesign]

Spade drill. No center drilling required, should hold .005 on diameter. If not drop size & finish like you are.

[cterry352]

Ok, thanks im checking into that.. Looking at some Kennametal spade drills.. Is there any brand that you have used and had good luck with?

[Geof]

Here is a bit of code you can try. It is from a stock program I have for banging out big holes when I am building fixtures. It starts with a drilled hole and spirals out to 1.5 diameter and then does three spring passes.

Cycle time just for this operation is a bit less than 30 seconds. I run dry with a strong air blast.

%
O11111 (FAST INTERPOLATION)
N1 (STARTING WITH 59/64 HOLE)
N2 G90 G54 G40 G49 G20 G80
N3 G53 G00 Z0.
N4 (---------)
N5 G10 L12 G90 P1 R0.625
N6 (---)
N7 T1 M06 (5/8 FOUR FLUTE MILL)
N8 G43 H01
N9 M03 S4000
N10 G00 X0. Y0. Z1.
N11 Z0.1
N12 G41 D01 G01 X0. Y0.45 Z-0.8 F200.
N13 G03 I0. J-0.46 Y-0.47 F100.
N14 G03 I0. J0.48 Y0.49
N15 G03 I0. J-0.5 Y-0.51
N16 G03 I0. J0.52 Y0.53
N17 G03 I0. J-0.54 Y-0.55
N18 G03 I0. J0.56 Y0.57
N19 G03 I0. J-0.58 Y-0.59
N20 G03 I0. J0.6 Y0.61
N21 G03 I0. J-0.62 Y-0.63
N22 G03 I0. J0.64 Y0.65
N23 G03 I0. J-0.66 Y-0.67
N24 G03 I0. J0.68 Y0.69
N25 G03 I0. J-0.7 Y-0.71
N26 G03 I0. J0.72 Y0.73
N27 G03 I0. J-0.74 Y-0.75
N27 G03 I0. J0.75 Y-0.75 L3
N56 G40 G00 X0. Y0. Z1. M09
N57 (-----)
N58 G00 Z1. M09
N59 (--------)
N60 T1 M06
N61 G40 G53 X-13. Y0. M30
N62 (-----)
%

[mfgbydesign]

We use Allied Machine & Engineering Universal Spade Drills with 130 degree Super Cobalt blades. They also have chamfer and flat bottom blades. Coolant thru the spindle helps quite a bit.
There's no spot drilling, no pecking.
http://alliedmachine.com/default.aspx

[cterry352]

Thanks for the info... I order a Kennametal spade drill and tool holder yesterday.. But i will also check into the Allied Machine & Engineering Universal Spade Drills.. Never used them so its all new to me.. As far as center drilling and pecking, you don't need to use these steps?? That so save a lot on time..

And thanks for the program, thats running pretty quick... are you using a solid carbide endmill or just a HSS??? and that is cutting into a Low alloy steel right??

[mfgbydesign]

I wouldn't worry too much about which brand spade. You might focus on which one is stocked locally so you can get different size blades on short notice.

You're not going to break any speed records with a spade. It does eliminate the additional tools and on short runs might get you thru the job faster. We leave a couple different sizes in the magazines so the programmer knows which tool number to use. The operator merely changes the blade for different sizes.

With a spade you'll create problems if you peck or pilot drill. And unless the surface is irregular skip the spot drill. Use a conservative speed but aggresive feed. .010 to .015 feed per rev. works pretty good in steel.

[cterry352]

Well i ordered the Kennametal Tools from MSC, and we usually get the stuff next day... And the company I work for is pretty small ( maybe 20 workers ) But its a fab shop, we run lasers, punch press, press breaks, paint booth, and mostly welders... But they had a Haas machine that nobody could run and i had went to a local college and worked in a plastic plant as a Tool and Die machinist, so i come here and picked the machine shop up,, now we are getting a lot more work in, and im getting in the need for some better tooling..

But back to the spade drill, yes its just a small 3/4 in thick plate.. maybe 5"X5" with the 1.5in +.005 -.000 hole in the center and then three 13mm hole drilled around it.. and the part is flat.. Really small production, but big for us. Prob, around 500-700 parts per month..

But thanks for all your help,

[Geof]

.....thats running pretty quick... are you using a solid carbide endmill or just a HSS??? and that is cutting into a Low alloy steel right??

Carbide, TiAlN coated running just over 600 fpm. This is on the fast side but that coating needs a hot chip to be most effective. Which is why its needs airblast not coolant.

The speed is on the high side and could be taken down a bit but sometimes with these coated tools you can remove more material per tool life by running fast. The tool doesn't last as long measured in time but it has done more work.

If do do get a spade drill keep your eye on the spindle load, 1.5" dia at 0.015 per rev is aggressive for an older VF3.

[cterry352]

Ok i will have to give it a try then, i will just have to get an air blast set up.. But im using a cheaper tool, i don't really but high price stuff because its usually quick little jobs i do... but these will be high production for us.. But buy the Accupro endmills.. ( Just bought some Accupro CAT40 tool holders to, they are really nice or so i think) And with drilling the 1.5 hole i was wondering about how the machine would handle it, as of now when drilling with the 59/64 drill the load gets up to about 35% pecking only .150... But if the drill get dull and will give the Z-Axis over current.. So i have to keep the drill in pretty good shape.. THANKS

[Geof]

If this is a high production it will be worthwhile spending some time optimizing things.

On your 59/64 drill I think your peck is too small, unless you are doing this to control chip size. I would consider using the I, J and K options in the G83 canned cycle and also make the value in Setting 52 G83 RETRACT ABOVE R, 1" to 1-1/2".

I is the depth of the first peck which could easily be 0.6" on that size of drill.

J is the amount the peck reduces on each pass which could be about 0.2".

K is the minimum cutting depth which I would make large enough that the tip of the drill was about 1/32" away from breaking through.

I have found with drilling through holes that the drill suffers badly during the break through. You have probably seen the drill caps that get pushed off the bottom of the hole are often blue. This is because when the drill is getting close to the bottom of the plate there is very little material ahead of it to act as a heat sink so it gets very hot. Almost the worst thing is to have your pecks set up so the drill partially breaks through and then retracts for a peck.

Having Setting 52 at 1-1/2" means that the chips clear effectively and the hole fills with coolant so on the breakthrough peck things have been cooled down as much as possible.

You don't mention your drilling feed but do mention the spindle load goes to 35%. It is possible you could boost the feed a bit which can reduce the heating at break through.


And a final suggestion if you are the shop owner. If you do optimize things so your time is below what you estimated and you are making more money than you expected make sure your customer doesn't find out. You want to keep the time/money you save for yourself not pass it on.

[cterry352]

Yes, it will be high production for our company.. And sad to say im not the owner lol so i just get my reg 40 hr pay... :-( But as for the small peck, there is not really a reason for it.. Just have not done a lot of drilling in production before.. But im running the 59/64 drill at 456rpm with a feed of 4.6ipm which seems a little slow.. which is 110sfm X 3.82 / .921 = 456rmp and then 456 x 2 x .005 chip load for the 4.6ipm.. And all this is coming from FEATURE CAM, which does not have a good material selection so im just using something close... Trying to get a material set up for some Grade 50 A572 but have not got it done yet.. But im just not used to doing a lot of drilling operations.. Coming from tool and die where i was milling, and using wire and sinker edms...