[dneisler]

Ok, I am attempting to drill some 12L14 with a 27/64 drill bit 2" deep. I have tried many setups, currently 2500rpm, .001 FPR.
I keep getting either collet slip, or missed steps I think. I have the collet tighten as tight as I can get it and my bar puller still work. I have the bar puller at 90psi currently.

Someone smarter than I have a better drilling setup or idea what I am doing wrong here?

[cbyrd]

I have drilled some 12l14 and was only running 300-500rpm. I also drilled a 1/4" hole first and then drilled my 5/8". Was at a feed rate of .002 per rev and did not have any problems with slip. I tried running at 1200rpm to start and was not getting good results.

Chris

[MichaelHenry]

HSMAdvisor recommends 600 rpm and 0.7 ipm (0.0012 ipr) for that combination of tool and material. As cbryd suggested, you might want to pilot with a smaller drill first. My personal experience is that cheap import tools quickly get too expensive to use so if the bit is at all suspect, try a better one.

[dneisler]

Drill bit is a good PTD bit. That feed don't help me any really. I have thousands to make and need to go faster than that. I pretty much have determined I am missing steps somewhere.


Sent from my iPhone using Tapatalk

[dneisler]

This what I am running now. I have got to figure out why I am losing steps. .


Sent from my iPhone using Tapatalk

[dneisler]

This after one part how much I lost in Z.


Sent from my iPhone using Tapatalk

[zero_divide]

Drill bit is a good PTD bit. That feed don't help me any really. I have thousands to make and need to go faster than that. I pretty much have determined I am missing steps somewhere.


Sent from my iPhone using Tapatalk

Are you using coolant?

Any way. Assuming coolant and the mildest hardness i would run it like follows: 969 RPM and 5.16 ipm (0.0053 ipr)
It seems like you would still have HP room to spare, but be careful - start slow.
If it still slips make some adaptor to 0.5" (what?) side-lock holder and your problem will go away.

Have to also add some pecks, it us unlikely to make all the way in one go.
Attachment 329604

[dneisler]

Not sure what you mean by adapter.... Also running less rpm and faster would require more z axis power right? If it is already missing steps then? I just don't understand why I am missing steps.


Sent from my iPhone using Tapatalk

[dneisler]

I am pecking at alternating 1/8 and 1/4.


Sent from my iPhone using Tapatalk

[zero_divide]

Not sure what you mean by adapter.... Also running less rpm and faster would require more z axis power right? If it is already missing steps then? I just don't understand why I am missing steps.


Sent from my iPhone using Tapatalk

perhaps your drill became dull and it is pushing away too much?

A proper drill at proper speed and feed does not require titanic force to push in to the material.

[soymilk]

perhaps your drill became dull and it is pushing away too much?

A proper drill at proper speed and feed does not require titanic force to push in to the material.

I agree with this. Using a high speed and low feed could be prematurely wearing out the cutting edges of your drill.

I highly doubt the machine is losing steps. But here is a way for you to test it. Use a tool and touch it off with something that won't move like the face of the chuck. Measure before and after the drilling cycle. If the numbers change then theres a good chance its losing steps like you said. If not, then its the collet.

[dneisler]

I will put in a new drill and give it a try with say 1000rpm and .005fpr?

[cbyrd]

I went back to my fusion cam setup for drilling. All the parts had a pre-drilled hole of 7/16. I then opened the hole to 5/8. I was running 500rpm at .003 fpr. I was using chip breaking with .05 Pecking depth. 2.1 accumulated pecking depth and chip break distance of .0025in with .1s dwell.

This worked really well and did not push into the collet. The OD on this was 7/8"

Chris

[dneisler]

I am just drilling 27/64 (.4219) which is smaller than your pilot size. I need to get this process going fast as I have 1200 parts that need to go out quick, to the point I need to machine at least 30 per hour. (2 minutes Each) Currently I am at 2m 17s but if I could speed up the drilling process and get rid of this issue I would be real happy.

[cbyrd]

You might try .0035 or .004 feed per rev or even use a solid carbide drill. Sometimes they drill faster. I know if I go above the 500rpm the bits seem to dull very quickly, even using coolant.

[dneisler]

I'm new to the lathe world so I was using the same speed feed etc that I was on mill for same part and hope and I would get 1000 plus parts out of the drill. I'm just not getting this lathe stuff yet. I will see what I can do when I get home


Sent from my iPhone using Tapatalk

[cbyrd]

When I was drilling 1018 for threaded inserts, I could drill about 25 5/8" - 3" deep holes before I would touch up my drill bit on the drill doctor.
I mounted 2 drills in a gang setup. I had the same program twice with the different tool selected.
When one would start getting dull, I would change the program and drill with the second drill while I sharpened the first.
When I switched back I would go to Z0 and bump the drill against it so I would not have to change the tool length.


Chris

[rcs60]

most sfm for hss drills are in the range of 100sfm for low carbon steel
but i found that in 12L14 i could run about 130 sfm and about .005 per revolution first peck would be 1.00 deep 2nd 1.625 3rd 2.000
I would try a high performance drill like a parabolic as these tend to have the points reduced making the cut use less hp on the z axis which i causing the part to push back in the collet
and added bonus is you might not have to peck when using a good parabolic drill
i am not sure what kind od collet closer that you have (air,mechanical, or hydraulic ) these make a difference in the holding power
The other thing to try is a 5c serrated collet this allows the collet to bite in to the material and hold it tighter (Hardinge brothers sells these )
I used to run a hardinge chnc1, air collet closer and these were my solutions to the part pushing back in to the collet
good luck

[dneisler]

1000rpm. .005 fpr is 10 times worse. I can visually see it missing steps. It kind of jumps back and forth. It touched stock and it did not move. New TG or YG(I can never remember) drill bit. When it was missing it steps it was not drilling at all. It was like it was sitting there spinning.



Sent from my iPhone using Tapatalk

[MichaelHenry]

Well HSMAdvisor says 571 rpm and 0.67 ipm for a 0.422 HSS twist drill in 12L14 and suggests a 0.04" peck and needs 0.1 HP. For a carbide drill, it suggests 1304 rpm and 1.54 ipm. G-Wizard says 411 rpm and 2.9 ipm for a roughing cut at 0.42 peck and that this needs 0.7 HP. I'd guess that anything above 600 rpm is going to burn out the drill bit in short order at which point HP requirements probably go through the roof. If that's true you are pretty much stuck with more than 2 min/drill cycle.

BTW, it looks like your ER holder sticks out quite a ways from the turret and that the flutes on the bit extend into the collet a bit. Is that necessary?

On edit:

Just noticed that HSMAdvisor suggests 571 rpm and 2.93 ipm for a parabolic drill bit and that pecking is not necessary so that you should be able to drill the hole in one shot. If that works, it would bring you close to 1 min/drill cycle. I've used parabolic HSS bits from McMaster-Carr in 303SS and 304SS with good luck. I only mention them because they are usually very quick to deliver.