Drilling holes

[cqualls]

I'm about to be drilling & reaming about 500 holes in A2, the blocks have not been hardened yet and are 1.0" thick. All of the holes are thru holes the tolerances are +.001 and -0.000 . Hole sizes are .125 , .188, .199

Questions:

1) What kind of drill bit, what speeds and feeds, peck or no peck?

2) What kind of reamer (carbide or hss), speeds and feeds?

3) How many holes can I drill before needing to replace the drill and reamers?

[Threept82]

Cobalt (.125)S1375 F1.2 (.188,.199)S900 F1.75

Peck on all.

 

Carbide Reamers.

 

Depends on brand of drills, set-up and drill length. (stub is best for rigidity and because of the 135 deg. drill point of cobalt drills)

 

I would not finish holes now, during heat treat

the holes will shrink in size (Most of the time)

I had some shrink and some grow in the same part.

 

[cqualls]

We have no choice but to do everything in the soft state. The plates will go back to the customer soft.

Should we be spot drilling the holes instead of Center drilling them?

[Threept82]

Center drill.

I never use spot tools on anything. They are not

accurate enough for true locations.

 

But thats just me.

 

In this case use a center drill for location as well as your holes are started that much deeper into the material, so when

they break thru the walking effect will be that much less.

[Müřlıń®]

Watch out for hole runout towards the back when your drill gets dull.

I would center, step drill and ream it to size.

 

A2 is the most stable material there is during heat treat if they Vacume and do it right.

 

The book says that it will only move .0002 per inch.

 

If your part is very big I would worry about hole locations rather than hole size.

[MACHINEMASTERG]

i would also use screw machine drills (stub drills)for tool steel i might?? c-drill but most of the time with the stub drills i dont !!!

[HEAVY METAL]

sgs hi-percarb drills. these drills are a little salty but you will make it up in the cycle time you save. 230 sfm .003-.005 per rev. yours would be slightly lower because you are drilling 3x the dia deep.

[john_070]

i use a spot drill only centerdrills are unrealiable.

[connormac]

I agree with Murlin. Centerdrill , drill and ream. I have also had good luck with bearly starting an endmill in hole the same size as the reamer.The reamer is less likely to walk.

[35K chipper]

See if you can use a6 tool steel (carpenter vega) more stable than a2. Make sure tha part is vacuum heat treated. Spot with a carbide spot drill with the tip angle to match your first stub carbide drill. Spot dia. @ 80>90% of the first drill. Drill with the primary with a G73 cycle at 1.5 > 2.0 dia. deep. Second drl carbide .002 >.004 larger than the first drl. Drl to 4 dia deep with a G83 cycle peck at 30% of this drill dia. Never leave the hole until final retract. Last drill same dia as the second drl. Peck G83 at 20% of drl. dia. until break thru dwell at .3 seconds after brk. thru. Do not leave the hole until final retract. Now use a 90 deg carbide 4 flute chamfer mill. chemfer hole .002>.004 larger than the reamer G81 no dwell. Now ream to size with a carbide reamer bore in stop spindle rapid out.(G86 no dwell) All tools in clean collets. Do not over extend any tool. Check run out on all. lots of coolant.

 

good luck,

35k chipper

[Thad]

We rarely do holes this size, but any reamed holes get a spot drill, reamer drill .03 under finish, stab with a 2 flute endmill .01 under finish (to establish true position), and ream.

 

Thad

[ChuckM]

+.001 -.000?

 

Look at all your tolerances and let us know what they are cause the tolerancing callouts determine the processe$ necessary in producing your parts. If you're just out for hole size with positioning accuracy within a couple thousandths then you can do it the old fashioned way by spotting, drilling then reaming or you can do it the least expensive way by using a good carbide drill in as accurate (TIR) a toolholder as you can afford.

 

I have drilled holes to +.0003 of drill size using quality carbide drills... no centering and no reaming necessary. If hole size is all you're after, then you don't need all the extra machine time. Not to mention, if you start out with a crooked hole, no amount of tru positioning and reaming is going to fix it.

 

Just my opinion, but for a job like this (500 holes) you can't afford to use cobalt.

 

-Chuck

[john_070]

Iwould never double drill a hole . Who has time for that tolorance does need to be stated. for your dia tol iwould think your positioning is critical drill+stab +ream good luck

[Müřlıń®]

The A meterial's are very brittle and are prone to heat cheacking if improperly machined.

Even in their annealed state.

 

Carbide tools will glow the edge under certain conditions. Making tapping the hole a biach.

This is why we will double drill the hole with cobalt. If done this way, no stress will be added to the part. and it will stay put during HT.

 

Even on old Bridgeports, we could drill precision holes if we center, step, plunge with an undersize endmill to position the hole and then drill and ream.

 

It seams like a lot of trouble, but we use to lold very tight tolerances before the CNC was concepted.......

[cqualls]

Thanks for all of the input.