Drilling steel with a bridgeport

What would be the biggest diameter that I could drill with a drill
bit. I am deciding if I have any need in my collection of MT4 drill
bits. I am aware that I can bore holes to any diameter.
Reply to
Loading thread data ...
I drill up to 1" and use other methods beyond that.
Reply to
Grant Erwin
My vertical mill has a belt drive and 1 3/4 hp motor. I used to drill holes with a twist drill up to about 1 3/8". I had the power, but when those big flutes stick, it's hard to get the 1/2 shanks I used to hold. When I was doing that, I would work my way up to the final size in several steps, so it took a while. I could go bigger but I'd have to use a 3/4" or 1" shank, but I don't like the idea of those big flutes sticking. Now, btw, I do these holes and larger ones with hole saws. I saw up 1 1/2" diameter and 1 1/2" deep in mild steel. I could probably go bigger. The only problem with holes saws is that they tend to cut 10 or 15 thou oversize, so you have to plan around that. They go a LOT quicker. All I do is (sometimes) make a pilot bit-sized pilot hole and a 5/16" hole at the inside edge of the periphery of the saw for chip clearance and then cut the hole.
Pete Stanaitis ------------------------------
Ignoramus27175 wrote:
Reply to
Ignoramus27175 wrote in news:p_ednVYKRPqdAPnbnZ2dnUVZ snipped-for-privacy@giganews.com:
That's kind of a tricky question Ig as there are many variables. IIRC, you have a 1 HP motor? In that case you couldn't drill a 1/2" diameter hole in 1018 steel at the proper speeds and feeds. 95 sfm .010 IPR. But you could back the feed rate down to .005 IPR and easily drill through. It won't do wonders for tool life, but you're probably not running production or drilling a huge number of holes.
The other issue is the amount of thrust you'll need to apply to the quill. It goes up significantly with diameter. Bridgeport quills and feed levers are notoriously weak, so it's easy to start breaking stuff if you're not careful. The weak link is usually the pin in the handle/lever. Which is as it should be, because the pin's weakness prevents the breaking of the more expensive innards in the head. The power feed is also very weak and is usually broken on older machines. It's really meant to be used for boring but the world is full of people that don't know any better.
I would think twice about drilling much larger than 1/2" in steel without a pilot hole. And I'm not a big fan of pilot holes, but in a pinch you gotta do what you gotta do. In the bad old days before CNC we would layout the work and drill bigger holes in a drill press. Then on to the bridgeport for any operations that it was suited for.
But I've also used trepan tools to machine very large through holes on a Bridgeport. Not a bad way to go if you've got the time and don't have a geared head radial drill press handy. Just be careful with the break through.
Also drilling thin plate is a whole differnet matter as the drill point is often through the plate before the body diameter of the drill is fully engaged, so the horsepower and thrust requirements are lower.
Then there is aluminum, where almost anything is possible.
Reply to
D Murphy
Don't abuse that poor BP, drill only as big as your smallest boring head/bar.
Reply to
Tom Gardner
Before I got my radial arm drill press, I routinely abused my old BP. Holes up to 2" after a 1/2" pilot. That machine has a lot of torque in bottom gear. Lots o' coolant and you had to have the touch for break through.
Reply to
Karl Townsend
Twist drill? Mild steel? Hougen or Jancey-type hole saw? Minimum RPM of your BP? Coolant?
Regards, Joe Agro, Jr. (800) 871-5022 01.908.542.0244 Automatic / Pneumatic Drills:
formatting link
Spindle Drills:
formatting link
Reply to
Joe AutoDrill
If you have CNC, you can do away with many big drill jobs by orbiting the diameter with an end mill. That way, you cut a slug out of the part rather than turn the entire hole into chips. This is often much faster. I do this a LOT on various panels, in sheet materials up to 1/2" and more.
You can do the same with blind holes (pockets) although in that case you do have to turn the material into chips. You start at the center and spiral out, sometimes in several depth steps.
For really massive stock removal in thick material, though, a big drill bit can be much better than slowly milling out pockets with extended-length end mill. A lot of people prefer plunging into the work with a bunch of closely-spaced drill holes, then removing the remaining lacework with end mills.
I have a set of 9/16 up to 1.5" or so Morse taper drills. I use them only on rare occasions, but they are real nice to have for those deep big drilling operations. They can remove a lot of material in a short time, and the upper parts of the hole support the drill so it doesn't shake the whole machine, like trying to mill the side of a cavity with long end mills.
Reply to
Jon Elson
I could do the same thing wit a rotary table also.
That's good to know... I will definitely keep my drills...
Reply to

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.