What Is the Secret To Drilling A Straight Hole?

For reasons I can't understand, I seem to have a hard time getting deep drilled holes to go anywhere near straight. If I drill a hole, of almost any size, 1" deep, even through aluminum, the bottom will be significantly offset, in a seemingly random direction, from the top. The machine is well trammed, and I'm using quality, name-brand drills, and peck-drilling.

When I need both ends of a hole to be properly positioned, I'll drill half-way through one side, then re-drill the full depth from the other side, but this should not be necessary....

Regards,
Ray L.

Make sure your fixture isn't allowing the part to flex or move under load.
Make sure you have good spindle bearings.
Could be trying to feed to fast or spindle speed too slow.
Make sure your coolant is to proper mix.
If all else fails,drill undersize,then drill to size with a core drill.
Without seeing the machine or the setup,that's about all the advice I can give.

Quote:

---

Originally Posted by Mazaholic

Make sure your fixture isn't allowing the part to flex or move under load.
Make sure you have good spindle bearings.
Could be trying to feed to fast or spindle speed too slow.
Make sure your coolant is to proper mix.
If all else fails,drill undersize,then drill to size with a core drill.
Without seeing the machine or the setup,that's about all the advice I can give.

---

That's pretty much all the things I could think of, and have pretty much ruled out, other than possibly rpm/feedrate, though I think my numbers are reasonable. For example. yesterday I was drilling 0.196" holes 1" deep. I did it at 3900 RPM, 20 IPM, which is close to what HSMAdvisor gives me, and 0.049" per peck.

Regards,
Ray L.

Did you center drill first to ensure you didn't flex the bit on the first peck?

-Jason

Center drill or spot drill first

Peck depth less than 1X the diameter

Use a stub or "screw machine" length drill bit whenever possible

Split point drills seem to help

My chart says 200-250 SFPM, Feed 0.003 per tooth.

-Dan

The top of the holes are always exactly on-position. But the drills often don't go straight down, so for deep holes, the bottom ends up off position. So, spot-drilling won't help.

Regards,
Ray L.

You might want to try screw machine drills (stubby). Shorter drill means les flex.

Quote:

---

Originally Posted by kvom

You might want to try screw machine drills (stubby). Shorter drill means less flex.

---

Or carbide, if only as a test to eliminate stiffness as a factor. However, I thought that wandering holes can often be attributed to drill bit flutes that aren't ground evenly. Maybe you got a bad batch of bits or a bit of BUE on one cutting edge.

Quote:

---

Originally Posted by SCzEngrgGroup

For reasons I can't understand, I seem to have a hard time getting deep drilled holes to go anywhere near straight. If I drill a hole, of almost any size, 1" deep, even through aluminum, the bottom will be significantly offset, in a seemingly random direction, from the top. The machine is well trammed, and I'm using quality, name-brand drills, and peck-drilling.

When I need both ends of a hole to be properly positioned, I'll drill half-way through one side, then re-drill the full depth from the other side, but this should not be necessary....

Regards,
Ray L.

---

Have you checked that your column is square to your table? Even if the drill is always perpendicular to the table it could be moving sideways if the column is not square.

Quote:

---

Originally Posted by SCzEngrgGroup

For reasons I can't understand, I seem to have a hard time getting deep drilled holes to go anywhere near straight. If I drill a hole, of almost any size, 1" deep, even through aluminum, the bottom will be significantly offset, in a seemingly random direction, from the top. The machine is well trammed, and I'm using quality, name-brand drills, and peck-drilling.

When I need both ends of a hole to be properly positioned, I'll drill half-way through one side, then re-drill the full depth from the other side, but this should not be necessary....

Regards,
Ray L.

---

Ray

I have had excellent results with "Walter Titex" carbide bits. They are made in Germany, rigid and drill straight as an arrow.
They are primarily metric with corresponding imperial values. For the most popular imperial sizes they have exact matches.
For your application probably a 5.0mm (0.1969) diameter with a 6.0mm (0.2362) shaft diameter.
Another feature is the ability to dispense with spot or center drilling on sizes above 1/4".
You're on the line so I would try both ways.
NOT cheap but if you're drilling a lot of holes, well worth the price of admission.

I use their 5.1 mm (0.2008) exclusively instead of a # 7 for 1/4-20.
Did I mention they last forever.

John

HIYA Ray, Spot drilling DOES help. It can appear to be on position BUT the centerpoint be off a smidge. The deeper you drill the worse it will get.

Does the offsetting appear to be only in 1 direction. What you are saying indicates the spindle is not square with the part OR the drill is starting off center (hole in correct spot but center offset causing it to wonder off the deeper you get.

Try doing an undersize drill full depth, Spot drill the center point ,Check for offset of exit. DOES the offset show up?? THEN redrill the same hole oversize with a 4 flute end mill to full depth. Did the offset still exist. IF it did you may have a machine alignment problem. IF it did not then you need to revisit your tooling .

In one part I make Belt drive pulleys for racing karts I predrill the tooth areas to help with profiling with small tooling 1/8" the Pulleys are 1 inch wide so the holes are 1 inch deep and I use a spot drill to ensure a good centerpoint and a carbide drill bit just long enough to drill through to ensure as rigid a bit as possible. It always works out that it drills straight +- a couple of thousands.

Just a thought, (;-) TP

Quote:

---

Originally Posted by vmax549

HIYA Ray, Spot drilling DOES help. It can appear to be on position BUT the centerpoint be off a smidge. The deeper you drill the worse it will get.

Does the offsetting appear to be only in 1 direction. What you are saying indicates the spindle is not square with the part OR the drill is starting off center (hole in correct spot but center offset causing it to wonder off the deeper you get.

Try doing an undersize drill full depth, Spot drill the center point ,Check for offset of exit. DOES the offset show up?? THEN redrill the same hole oversize with a 4 flute end mill to full depth. Did the offset still exist. IF it did you may have a machine alignment problem. IF it did not then you need to revisit your tooling .

In one part I make Belt drive pulleys for racing karts I predrill the tooth areas to help with profiling with small tooling 1/8" the Pulleys are 1 inch wide so the holes are 1 inch deep and I use a spot drill to ensure a good centerpoint and a carbide drill bit just long enough to drill through to ensure as rigid a bit as possible. It always works out that it drills straight +- a couple of thousands.

Just a thought, (;-) TP

---

Terry,

I'll give it a try (again), but the holes don't go in any particular direction. One will wander off to the left, another to the right, or back, or front, or somewhere in-between. The spindle is well-trammed.

Regards,
Ray L.

Are you sure you are not over tightening the collet? Try spinning the tool holder real slow to see if there is any noticeable wobble.

Don H.

Quote:

---

Originally Posted by SCzEngrgGroup

The top of the holes are always exactly on-position. But the drills often don't go straight down, so for deep holes, the bottom ends up off position. So, spot-drilling won't help..

---

You do need to spot for the smaller holes, but not much, the small holes
- spot at least to be larger than the chisel point of the drill, to stop any minute wander at the start of drilling

I tend to spot (CBD NC spotting drill ) to create a chamfer, so no need to run another op after the drilling

Your RPM looks fine, feed may be a little high ( 0.0051" rev), as it would force a tool to flex & go off-line, I use approx 30% (drill dia) for peck depth
--- IMO 0.0030-0.0035" rev (12-15 IPM) would improve straightness

What tool ? silver HSS jobber type ?
new, used, sharpened......what are the corners like ?

Got a pic of your setup?
I'm curious as to why every hole you drill goes off C/L
:cheers:

You might try interpolating a smaller size first. 3/16" end mill would do. Then just bore out the rest with the bit. It would have no choice but to follow where the end mill went.

Ray,

When I have to drill a critical hole, I do as does Lee. I'll use the largest carbide EM that is smaller than the desired hole dia., then finish with the appropriate drill or reamer. Have you tried doing the holes on your Hass also? That would eliminate any question about the Tormach.

Haas? Tormach? :p

Guys,

I'll give spot-drilling another try in the next day or two, and report back.

Regards,
Ray L.

Quote:

---

Originally Posted by vmax549

HIYA Ray, Spot drilling DOES help. It can appear to be on position BUT the centerpoint be off a smidge. The deeper you drill the worse it will get.

Does the offsetting appear to be only in 1 direction. What you are saying indicates the spindle is not square with the part OR the drill is starting off center (hole in correct spot but center offset causing it to wonder off the deeper you get.

Try doing an undersize drill full depth, Spot drill the center point ,Check for offset of exit. DOES the offset show up?? THEN redrill the same hole oversize with a 4 flute end mill to full depth. Did the offset still exist. IF it did you may have a machine alignment problem. IF it did not then you need to revisit your tooling .

In one part I make Belt drive pulleys for racing karts I predrill the tooth areas to help with profiling with small tooling 1/8" the Pulleys are 1 inch wide so the holes are 1 inch deep and I use a spot drill to ensure a good centerpoint and a carbide drill bit just long enough to drill through to ensure as rigid a bit as possible. It always works out that it drills straight +- a couple of thousands.

Just a thought, (;-) TP

---

hello everyone

I cant tell you if my experience drilling deep holes is the best one. but I'm going to share my efforts.
Machine: Haas
Holder: Hydraulic

Spot: 5mm 142 deg. Walter brand Vc 144.78 m/min - . Fz 11938 mm/min. = S9216.98 F1100.32 Dwell of .5 of a second

Drill: 3.969mm thru. coolant Walter brand Vc 50m/min - Fz .0711 mm/min = 4009.950 F 285.107

Reamer: 3.98mm (.156) Monster brand Vc 19.9 m/min Fz .1875 m/min = S1600 F 300. dwell .5 of a second . im getting .006 microns of cylindricity perpendiculary of .008microns 3.982mm on the diameter buttttttttt its true positing varys from .003 microns all the way to .150 microns. like you said its the machine s trem i check and its around .020 microns withch is in Haas Specs. what i did was if drilling more then one one in a part i spot,drill and ream each hole in that order . hope it helps but our main eenemy is the back lash for true position. amen.