Drilling .394" holes in large diameter titanium tubing

I have to drill 50 .394" holes into the body of a titanium tube that is approximately 36" diameter X 44" long with 1/4" wall thickness.
The part is programmed at 900 RPM with a feedrate of 1.9 IPM. I am using a solid carbide drill. The problem I am having is the force of the drill is compressing the tubing as it drills and when the drill breaks through the tubing snaps back into place and chips the drill, causing the drill to cut over-sized on the holes that follow. I have been successful slowing the feedrate to .9 IPM, but had a drill fail on me this week and am looking for a better solution. In the past when I did my own programming I would drill a small pilot hole in situations like this to lessen the load on the larger drill. Is this something I should recommend to the programmers at my new company? Are there any other suggestions for getting around this problem? Any help would be appreciated.
Howard

There are about Eleventynine ways to approach it differently. I would start out with NOT using a Drill, and using a 3/8" Endmill. Either Plunge and cut the Diameter with the same Tool. Or just Helix into the hole. Less force, less breakthrough energy. An Indexable Drill doesn't use much Z Axis force either. But there are literally dozens and dozens of ways to make holes, it's the most practiced and defined part of our trade.

R

If we presume you're using a VMC or HMC for this job, then I agree with Litlerob1 on using an endmill and helixing in, but I'd use a smaller one, 1/4" in three of four flute, to further lessen forces and deflection. If you wanted, pre-drill with a 1/4" cobalt stub drill (not carbide), then follow with the EM. The cobalt drill will be much more tolerant of the pipe moving around, and a lot cheaper if it does break.

Let's all say it together...helical.... interpolation

I had a similar issue with a recent part. Carbide drills would chip from one hole. Switched to cobalt drills to lessen the force applied from a lower federate and RPM and that worked great. It was nice to have one drill finish everything else.

I'd poke an undersized hole with a cobalt screw machine drill then mill to size with a 1/4" endmill.

SND said:

I'd poke an undersized hole with a cobalt screw machine drill then mill to size with a 1/4" endmill.

Click to expand...

The guy in post #3 agrees with you...

I agree with pre drilling

Wait tho, 1/4 inch wall thickness, flexing the part, I think your setup sucks, or the big giant machine you are running it on has a 100 thou of backlash in the Z

Get a 2x4 and sand it to roughly the right size. tap it into place just to the side of where the hole is to be drilled. The perfect size would probably flex the tube enough to see with an indicator but obviously not damage the tube, and not be loose enough to fall out and cause the same problem you are having

Just imagining the size of the toe clamps to hold the tubing down.........

Hi hkahn117:
In my opinion, how you fixture and support this big floppy part will be everything as you're already discovering.
Since it's 50 holes per part, you will spend a lot of time positioning and re-positioning the 2 x 4 if you do as gustafson suggests, but you may find that it's profoundly worth it, even if it means a guy fucking around for a day crawling around inside the tube with a hammer and a wedge and a tape measure to position the 2 x 4 while another guy runs the machine.

Depending on how you calculate where the most effective time is spent, you could simply go with this, or you could build something more elaborate.
Do I assume correctly, that the part is mounted on a rotary and the holes are distributed around the circumference of the tube, or are they all in a straight line?
Do you only have one of these parts to do?

The answers to those questions will help you decide what kind of support to build but I fully agree with gustafson that any kind of support will help you tremendously whether you decide to drill or helical mill.
If you end up making an internal cradle out of wood, make it adjustable so you can jack the support out against the walls of the tube to be sure you have good contact with the tube walls.
If they're all at one end a plywood end cap with adjustable internal jaws like a big lathe chuck is a good design, but it would be useless if the holes run along the length of the tube, in which case a simple sled with a 4 x 4 post sticking up that can be jacked against the tube wall in one spot and moved to a new spot quickly and easily could do the job brilliantly.

If there's only one tube to make, rude and crude is your obvious way forward...if you have 10 to make, maybe you can justify making something a bit more user friendly out of scrap steel with UHMW wear pads and simple screw or bottle jacks, but I don't think you have a choice other than to make something to support the tube and prevent flexure against drill forces and mitigate resonance that will eat milling cutters.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Oh, I misread, I was thinking one hole 50 times

nevermind.........

I'm thinking almost 'hanging' the part on a structure rigid enough to take the tool force, or just multiple 2x4s wedged before running, say one every foot, and understand they are going to get drilled

Obviously this is not a big deal to this person. So who knows what he is doing?

R

He set that bish on fire

I work with titanium all day, everyday. I drill a lot of holes in tubing as thin as 0.0290”. Either support the ID with a wood or plastic rod, and drill with the same feed and speed, plunge with a 5 flute, or helical interpolation....or several other ways. Depending on alloy, your RPM is a little high.


Last week I had to drill a 9.75” deep 0.343” diameter hole in 8-1-1 (suckier to drill than 6Al-4v or CP) with no coolant). Feeds, speeds, and forethought are far more critical in Ti than more common materials.

On really thin wall I back it with plastic.....anything else I just use a 5 flute EM and plunge. On deeper holes I just regrind HSS drills by hand with more suitable geometry.


It’s one of the few materials that you can take a 3/8” drill that usually cuts oversized, and drill an oversized hole. 45 minutes later it’s no longer oversized.

Hi 9finger:
You wrote:
"support the ID with a wood or plastic rod"
I agree in principle, except this tubing is 3 feet in diameter and 4 feet long.
Gustafson's idea of an adjustable internal prop is the adaptation of your recommendation that makes the most sense to me.
All that's left to decide is how elaborate the prop needs to be to get 50 holes out of it without breaking the bank either building it or using it.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

implmex said:

Hi 9finger:
You wrote:
"support the ID with a wood or plastic rod"
I agree in principle, except this tubing is 3 feet in diameter and 4 feet long.
Gustafson's idea of an adjustable internal prop is the adaptation of your recommendation that makes the most sense to me.
All that's left to decide is how elaborate the prop needs to be to get 50 holes out of it without breaking the bank either building it or using it.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Click to expand...

Yeah that would certainly be the challenging part. If it was going to be a regular job, I’d weld a jig that is shaped like a plus sign, asterisk, whatever, with curved pieces of wood or plastic that are curved to the radius needed to slip fit the ID, and just slide it along as I go. Even if the contact points weren’t radiused but square, it would probably support it well enough.


If it’s one part, I might would do the same thing depending on how much that part is worth. Even two wooden crosses out of 2x4”s, with one attaching them together, that barely fits the ID, can give the rigidity needed in really large tubing.


Regardless of how I did the job, I would most certainly find a much better way to do it once I was done with the very last part.

9finger said:

Regardless of how I did the job, I would most certainly find a much better way to do it once I was done with the very last part.

Click to expand...

Man oh man, ain't that the truth!

Thank you to all that replied and made suggestions. I shared them with the tooling engineer and the mechanical engineer on the job. They will likely ignore them all. They have been making this part the same way for 20 years and seem to be willing to accept the occasional oversized set of holes (which can be weld repaired) rather than correct the process through proper tooling, technique, and fixturing. This is my first job where I am not programming and selecting my own tools and it is frustrating. No, I’m not going to tell you about the 1/2” carbide endmill with 1.25 flute length that is sticking 2” out of an 8 inch long thin holder that shatters the moment it touches the part at the programmed feeds and speeds. Thanks again for those who responded.

hkahn117 said:

No, I’m not going to tell you about the 1/2” carbide endmill with 1.25 flute length that is sticking 2” out of an 8 inch long thin holder that shatters the moment it touches the part at the programmed feeds and speeds. Thanks again for those who responded.

Click to expand...

Maybe that was the intended result.

Would you get in trouble if you stuck a couple 2x4s in the ID as others have suggested?

Sounds like you should be looking for a new job.

dandrummerman21 said:

Would you get in trouble if you stuck a couple 2x4s in the ID as others have suggested?

Sounds like you should be looking for a new job.

Click to expand...

Yes, I would get in trouble. No deviating from the op sheet. As far as a new job, they kind of priced me out of the market for now. I’m going to try and make things more productive where I am but it is going to be a challenge.