Need advice on drilling a deep hole

[protrxrptr17]

I need to drill a hole all the way through some 10" long 1045 chrome plated rod. The hole is 0.1875" diameter. I have a CNC lathe that doesn't have through coolant. It doesn't matter how long it takes to drill. I only have to make 2 parts. I don't really want to spend alot on tooling because its just a couple parts. My machine has a 6T control. Is there a cycle that fully retracts between pecks? I have been using G75 for all my other projects. I guess I could program it longhand if I had to. I have some aircraft extension drills in the proper size. Could I use those and just make short pecks? I don't care if it takes 30 minutes per part.

[neilw20]

Not sure whether your control program has this but I have seen it in other machines not using Mach3.

Here is what I use:

G83 X Y Z Q R F
X1 Y1 Z-2 (more holes Z spec can change)
X1 Y2 Z-3 (more holes Z spec or others can change)
..

G80

F feed.
Z is the final depth.
Q is the peck amount before retract. Just positive number. Zero or negative is an error.
R is the Retract height. + above for Z0 = top of job.

In Mach3 the return Z is just above where last peck finished.
It is in the config screen somewhere.
Other systems... No Idea, but default probably OK
See if it kills a short half dead drill.


Ref:
http://www.isd.mel.nist.gov/personne...a.html#1001538

3.5.16.4 G83 Cycle

The G83 cycle (often called peck drilling) is intended for deep drilling or milling with chip breaking. The retracts in this cycle clear the hole of chips and cut off any long stringers (which are common when drilling in aluminum). This cycle takes a Q number which represents a "delta" increment along the Z-axis. Program G83 X- Y- Z- A- B- C- R- L- Q-

• 0. Preliminary motion, as described above.
• 1. Move the Z-axis only at the current feed rate downward by delta or to the Z position, whichever is less deep.
• 2. Rapid back out to the clear_z.
• 3. Rapid back down to the current hole bottom, backed off a bit.
• 4. Repeat steps 1, 2, and 3 until the Z position is reached at step 1.
• 5. Retract the Z-axis at traverse rate to clear Z.

It is an error if:
· the Q number is negative or zero.G0 X Y to the first position.

Link to index:
http://www.isd.mel.nist.gov/personne...74NGC_3IX.html

[scadvice]

... is the most important, right up there with very good split point drills. Make sure you have the minimum run out you can get on the bar. Stock wobble will also cause run out problems. The best trick I know, in your case and equipment, is to start the hole about .02 per side undersize and as deep as you can bore with a little carbide boring bar. Bore to the full depth of the drill as you can and (between 5 and 10 diameter depths), on size to the drill diameter, within a .001 or better. This will start the first drill very straight. Peck and retract fully back each peck. Also peck between 40% and one diameter max, each peck. I would also feed hold at the end of the retract and clear chips using a long small plastic tube on the air gun. You have to use your best judgment as to how often.
A further process would be to using the technique I just described, go only half way through then turn the bar around and repeat the process on the other side. This further improves the concentricity of the hole to the bar OD.
I’ve used this process a number of times and it works very well.
Sorry, I do not remember the full retract G code for drilling I think it is g83.

[protrxrptr17]

The size of the hole doesn't have to be precisely 0.1875". The part is a shaft for a shock absorber and the hole is for fluid to pass thru and will have an adjustable orifice on one end.

[scadvice]

Originally Posted by protrxrptr17 The size of the hole doesn't have to be precisely 0.1875". The part is a shaft for a shock absorber and the hole is for fluid to pass thru and will have an adjustable orifice on one end.

In this case, you need to be very close to on size to assure the best alignment. It acts like a precise drill bushing and boring it assures it is concentric .

Steve

[scadvice]

I understand and good luck. Steve

[mcarvey]

Have you considered drilling a larger hole and inserting a piece of tubing? McMaster has tubing .183" ID X .3125" OD. You'd probably have less difficulty getting a 0.3125 drill to drill straight (if that's an issue).
Just a thought...

-Matt

[SQT18MS]

Could you drill it from both sides?

I would definetly go for a peck drilling cycle with a short step, like 0,05" or in that area.

Take youre time on this and cool it well.

I use G83 all the time, hope youre control has it

[protrxrptr17]

Yeah, I can drill it from each end. Any recommendations on tooling?

[ALLtra Mach]

Start with shorter drills first, then increase in length as you run out of flute. As stated above, make sure tool is perfectly centered. If you center drill, which you should, either your first drill that you use should be very short and basic purpose is to make sure the difference in tip angles from your center drill doesn't cause you to flex the drill. How you start the hole will make a huge difference in how it ends up.

Tooling suggestions, Center drill, carbide screw machine drill, carbide jobber length, parabolic extended, aircraft extension.

And read this for parameter info
http://www.precisiontwistdrill.com/t...?image=contact

my two pennys

[SQT18MS]

If you dont want to invest in tools you dont already have, I would go for a regular HSS drill and just drill it from both sides.

Of corse you have to center drill it first.

I meen, its just 5 inches deep.

Go for it...

But go slow

[g-codeguy]

G75 is O.D peck, G74 is for drill pecking. Not what you want. It won't retract to a point in front of the part. Do you have the G83 cycle mentioned? Lot of lathes don't.

If not, do you have Macro B? If yes, I can give you a drill cycle that allows you to control the depth of the first peck, the amount for minimum peck, and how long it will dwell in front of the part.

Can send me a PM if you want.