Spot for Deep hole in Aluminum??

I am trying to drill a 4" deep hole .406" in diameter through 6061-T6. Supposed to be decent aluminum from Kasier.

I bought this spot drill. I was under the impression I should spot at a wider angle than the drill point.

I have tried drilling with a Titex parobolic drill and also 135 deg split point cobalt.

I am drilling a block that is machined on all sides in a vise on a VMC. No through spindle coolant. After I drill the hole I measure from the hole to the edge at the top and at the bottom. The bottom on the worst block measures .030" different. So the hole is off .015"

Here are some of the procedures I have dried.

1. Spot with 142 deg spot drill. Peck drill with Titex drill. Initial peck of 1.5" each peck after was .406" 1650rpm, 13ipm.
hole was visibly off on a 2 block.

2. Spot with a 142 deg spot drill, then drill .1" deep with a 135 deg cobalt screw length drill, drill with titex. Not much better.

3. Drill 3.4" deep with 135 deg cobalt, no spot, finish with titex to get depth.
a little better but not a lot.

I kept thinking the problem was the drills. Finally I started looking at the spotting tool as it was new and I was not that familiar with it. I spotted a new piece to .410" diameter. I put layout ink in the holes and brought down the 135 deg screw length and fed it down by hand until it rubbed and I could see it. The drill was hitting about 1/2 way up the spot. I thought it should be hitting right in the point. You can actually hear the first peck sound terrible like the drill is trying to find center. So I thought I would just spot it with a cobalt screw length drill then switch to the cobalt jobber length. Both are from Precision Twist. I did the exact same thing as above with the layout ink and same problem these 2 drill were not even the same point.

If anyone has any suggestions I would really appreciate it.

I don't mind buying some tools, hence the spot drill and titex drills were brand new specifically for the job.

The parts will work just fine if they are off .010" as it is only a bolt clearance hole, I would like them a little closer if possible.

I have never drill any deep holes so I am not really sure how much drill wandering is expected. Anyone have any typical walk amounts.

I was also told the problem was the aluminum as it may not be very uniform and harder spot could be causing the problem.

Is there a particular reason why you couldn't use a regular center drill, rather than a
spot drill ??? I would think that you might have better luck, as the drill will want to follow
the pilot on the center drill, helping to align it better.




Frank

I would try a shallower peck and see what happens.

Maybe and initial peck of .750 then peck .25 after that.

ARB,

Thanks for the response. I would try shorter pecks, but with what drill combination.

I was hoping for the money I spent on the Titex I could spot and then start and finish with that. I am trying to save some tool changes.

I'd use a spot drill with the same point angle as the drill to follow. Any drilling procedure that brings the corners of the drill into contact first is asking for chatter: this is exactly what happens when you try to enlarge a hole by 1/32" or so with a drill. Stabilize the point of the drill, and you should be good to go.

If you can get a spot drill with exactly the same diameter as the drill, then use that and spot deep enough to get the full body diameter of the drill started for the first 1/16" or so.

The other thing to check would be the actual squareness of these blocks. "Machined all over" is not equal to "square all over" and a small tilt error on 4" could produce bad location. If the direction of maximum deflection of the drill seems to be in one preferred direction, the setup is a likely suspect.

we sometimes use a small spot .050 dp then let the drill do all the work. i agree with the small peck's also. most important indicate the drill to see if its running out we indicate all drills now. better off using 3/8 pilot to 1' depth if poss. unless your running large qty.

Ok... so your drill is walking sideways...
Now I started learing how to do this sort a stuff well over 50 yrs ago and we never had that sorta trouble as long as the drill point was good, start there. Then we had another marvelous invention probably a thousand years old called a Drill JIG... It was just a bushing the same ID as the drills OD to guide the drill and it was held in the jig that also held the part being drilled...

Now I'm not telling you to toss out your fancy CNC Vertical and go back to making drill jigs, but why not start with a pilot hole the EXACT same diameter as the long drill? Poke that SHORT SPOTTING DRILL into the part aprox 1 or 1 1/2 drill diameters deep and then switch to a longer drill with a PERFICT DRILL POINT. IF it's not a purfict drill point?...IT WILL WALK....garandamteeeit.

Good luck

Ohh.... and look at how GUN Drills work to drill little holes through very long rifle barrels...
Hint... they start the hole with the gun drill in a bushing.

I have checked the blocks for square and parallel and thought maybe this was the issue. The blocks are not perfect most are parallel with in .0015" and the thickness is +/-.002.

Once the block is in the vise I run an indicator up and down the face to see if it is in the vise square. Most are with in .001"

I have checked the holes and no they are not always in one direction.

I understand about the same drill point angle but, bought a spot drill and even tried 2 different lenght drills from the same company, supposedly both 135 deg drills, but they both spot at different angles. the screw length drill has a much thinner web and the jobber length has a wider web.

What I don't understand is if the spot drill is 142 deg why doesn't the 135 deg drill hit in the center first. It does not hit at the outside of the flutes either but in the middle. Say the spot is .41" I would guess it is hitting at about .25"

I can hear when the drill first makes contact with the spot, kind of like it is walking.

I will see if I can find a stub length and pre drill .1" deep.

did you indicate the drill?

Brepins said:

did you indicate the drill?

Click to expand...

not yet, I am not at work.

But I definitely will. I can't guarantee the drill points are perfect as they are all brand new factory points. I only assume they are, but I am sure it is possible to get bad drills from factory.

I've never had a bad drill grind out of Titex (though I can't say the same for some small Guhriing.) When you spot, do you have a G82 or similar where you have a brief dwell at the bottom of the stroke?

Assuming the spot is OK, try starting the hole @ lower speed and 1/2 feed until you're in by 1.5x D, then run it normal.

BTW, my TEC software (from Titex) shows the recommended drill for this to be an A1522-13/32 parabolic flute long-series drill. Is this the one you're using? The software says to run @ 1542rpm & 14ipm. BTW, that drill is a 130º point, and no pecking required.

PixMan said:

I've never had a bad drill grind out of Titex (though I can't say the same for some small Guhriing.) When you spot, do you have a G82 or similar where you have a brief dwell at the bottom of the stroke?

Assuming the spot is OK, try starting the hole @ lower speed and 1/2 feed until you're in by 1.5x D, then run it normal.

Click to expand...

Yes I am using a G82 with a .5 dwell. I was using .2 dwell but moved it up.

I guess I am thinking the problem is the spot. It looks perfect but it definitely does not allow the drill point to start first even though it is 142 deg. The best hole so face is with no spot.

Any specific suggestions for a spot drill?

Try a few holes without the spot drill and take a endmill and circle cut a starting hole for the drill,,If your hole is good after that you know the drill is good,,If not put a couple of indicators on the machine while its drilling,,possible something else besides your drill or spotter is the issue,,

You have to feed the drill properly too. I suggest about 1.6% of the drill diameter per flute.
On a .406 diameter drill it equals .006" per flute or .012" per revolution. That will be a little on the easy side and should work fine. If you hear chatter feeding into the spot drill, all bets are off for accuracy. If you feed the drill correctly you should not hear the chatter.

After the first peck of 3-3.5 diameters deep, I would suggest .5 diameters for each peck.

You're only going ten diameters deep. It should be a piece of cake. I've drilled 12 diameters deep in aluminum with a .015" diameter drill using this same formula. I did it @ 3000 rpm. and 1.5 inches per minute. I've also done it in 316 SST and copper too.

Best regards,

Stanley Dornfeld

I hesitate to say this since there are some very knowledgeable people here but I always use 90 degree spot and haven't had problems. Drilled lots of 6061 in that range. Just spot about .01 larger diameter (breaks your edge) than your drill. Peck 4x diameter first than what ever you feel comfortable with. The drill manufacturer probably has recommendations.
Anyway, that's what I've done and it works.
Interesting to read about other methods.

Metalcutter said:

You have to feed the drill properly too. I suggest about 1.6% of the drill diameter per flute.
On a .406 diameter drill it equals .006" per flute or .012" per revolution. That will be a little on the easy side and should work fine. If you hear chatter feeding into the spot drill, all bets are off for accuracy. If you feed the drill correctly you should not hear the chatter.

After the first peck of 3-3.5 diameters deep, I would suggest .5 diameters for each peck.

You're only going ten diameters deep. It should be a piece of cake. I've drilled 12 diameters deep in aluminum with a .015" diameter drill using this same formula. I did it @ 3000 rpm. and 1.5 inches per minute. I've also done it in 316 SST and copper too.

Best regards,

Stanley Dornfeld

Click to expand...

I started off with the parameters specified by Titex

165 SFPM
.0087" feed. I assume they meant per rev. but may be it was per flute.

I indicated the drill a point and it is almost perfect. I can only pick up about .0002" runout.

I have decided to start over this am and document things a little better and see what I come up with.

Thanks to all who have helped.

I started with a new part, indicated up and down to verify it was in the vise straight. I spotted on hole with a 142 deg spot drill at a slightly lower feed and speed, had a .5 sec dwell at bottom, spot looked great. Drill with titex drill at 1300rpm, 8 ipm. I used a high speed peck cycle (G73). I did 2 pecks a .100" the a full retract. Check hole at top and bottom, top off about .004", bottom off about .028". I was bad enough that at the end drilling you could fee the drill binding.

Next I circular mill a .406" hole with a .25" endmill. Drilled exactly as above.

Top off about pretty much right on, bottom less than .002". Pretty much a perfect hole. Obviously the issue is in starting the drill. I am going to try to increase peck depths now.

Thanks again to all.

Not meaning to hijack the thread, but I gotta question for Metalcutter

Where do you get your % for drill diameter number at? Do you have a chart? Do you have sort of baseline to go by?

Not questioning your methods, I like the idea! Can you point me in the direction?

Have you checked the Spindle TRAM ??

Put a rigid tram bar in the spindle and and tram the spindle.
Set the indicator at aprox a 12 inch radius if the table is 24 plus inches, if the table is less use 1/2 the tables width. With the indicator at the rear of the table set the ZERO... then report to us the Readings LEFT, FRONT and RIGHT...

It's often helpfull to not set the indicator down right on the table, but set it on a 1/2 inch gage block, this way your not bumping the indicator on the table as you rotate the spindle.

Regardless of tram, if you take a face cut so the cutter is normal to the work piece, you should have a straight hole. Are you real sure you do not have a bunch of runout?