drilling round stock

[monarch1973]

Hey all. quick question. I have to cross drill 5/8" 1018. They need to be pretty accurate location wise, and diameter wise. A coupler goes over them, and a 3/16" roll pin goes through both. I have to drill both ends, and usually do 28 at a time. I get pretty sick of using a center, and then chucking up a 3/16" bit. Is there anything out there I can accurately drill without having to start with a center drill? I tried a 3/16 end mill and ended up with an oversized hole probably from deflection.

 

[Illinoyance]

Heinrich Company - Cross-Hole Drill Jigs - Racine, Wisconsin

 

[guythatbrews]

You might try a Kennametal Go carbide drill. They are pretty robust for manual machines, cut good size, and will start themselves. Use a collet I think the shank will be 5mm. I'd use oil. Part number 4150206 about $39

 

[monarch1973]

You might try a Kennametal Go carbide drill. They are pretty robust for manual machines, cut good size, and will start themselves. Use a collet I think the shank will be 5mm. I'd use oil. Part number 4150206 about $39

would this be rigid enough to not wander at the start?

 

[Limy Sami]

I'd make up a simple box jig (aka a bit of squ or rect' bar with a hole for the work, a guide hole for the drill, an adjustable length stop for hole postion and a pinch bolt - 1 off job on a manual mill - say 1 hr - 1.5 tops (inc coffee drinking) .and you will get through 28 off in no time, on a run whatcha brung drill press.

In un-hardened steel or CI I'd make the drill guide hole a min of 3 x drill dia depth

PS if you wanna get fancy, install a hardened replaceable drill guide bush

 

[Kevin T]

PS if you wanna get fancy, install a hardened replaceable drill guide bush

Not sure if it would work for the OP but I've had good luck using a self centering dowell jig on round metal stock. I have an old one that I got from Rockler that has smooth bores for the drill bits to pass through. The 1/2 inch one is my go to with a precision drill bushing in it. I've often thought about making one that was a little beefier and more purposeful. It seems like there are a lot of cheap ones avaiable with a threaded bushing now I am not sure that is better.

 

[HappyWyo]

I don't know how your shop is set up, but I would set up my mill table with my dividing head Chuck to hold the rods in the correct position, set my DRO to zero, mill a tiny flat spot with an endmill 3/16" on each one. Then switch to a short drill bit that just reaches through the stock, drill them all, then switch to a small chamfer tool and chamfer each one slightly to give it that professional appearance. Chucking and unchucking stock is faster than changing bits. Chinese dividing heads are cheap and get used continually on a small mill. I often use a "stop" in my dividing head whether horizontal or vertical to keep the stock the same length, or in your case the hole at the correct position. I sometimes set it up and let my granddaughter run the pieces so she can make some spending money.

 

[guythatbrews]

would this be rigid enough to not wander at the start?

I believe it would. If I don't have 3/16 I have one close. I'll try it in Bridgeport tomorrow will just take a few minutes.

 

[guythatbrews]

I believe it would. If I don't have 3/16 I have one close. I'll try it in Bridgeport tomorrow will just take a few minutes.

Well I didn't have a 6mm r8 collet (i was wrong about 5mm shank) and drill chuck not true enough so I couldn't try. I've drilled literally 10's of thousands of 5/32 cross holes 2x to 3x thru in 304ss with these drills no start drill in 9/16 round tubing. In both conventional CNC equipment with water based coolant and cnc swiss with mineral oil coolant. Excellent location and you can't get a +.001 pin in the hole so works great.

In a manual machine I think it will work but tool life will suffer with no or intermittent coolant, less rigidity, and no controlled feed. I wouldn't use the quill feed in a bridgeport.

The drill jig is a great idea just be aware you've got to cut clearance for burrs or you'll have a hell of a time getting the part out. Also drill bushings drill the easiest if you can leave a space between the work and the part for chip evacuation. One to two diameters clearance will do it. If location is tight best results come with the bushing as close to the part as you can get it.

Another idea we've used is a block to hold the drill bushing that is clamped to the table while holding the part in the vise. True you have to sweep the bushing in every time you set up it so that takes a bit of time. But very quick to load/unload. Waaay back before we had CNC rotary capability we'd use this setup along with a hardinge 5c quick spacer to drill 6x 1/8 diameter cross holes in stainless steel parts and it's very quick.

If you use a kurt-style vise you can bolt a bar to the back of the fixed jaw. Bolt or weld on an arm on the bar pointing back over the part. Locate the bushing over the center of the part. If you register the bar on the little bit of vise rails showing at the rear of the vise or the top of the fixed soft jaw and an include and integral stop for end of bar all you have to do is bolt it on each time, sweep the bushing and you are set to go. If you want to get fancier make the bushing arm adjustable and use slip renewable bushing setup and now you can use for diffferent size bars and cross holes as well.

Hope you find a solution that elimnates that tool changing.