What's new
What's new

Set-up help in drilling shafts with a mill.

jacksonburg

Plastic
Joined
Jun 24, 2021
Greetings all,

Could use a little help. I'm tasked with drilling 3/8-16 holes every 8" in a 10' x 1-1/2" diameter shaft. I will be holding the shaft on a mill table 40" long. The shaft will have to be moved about every 4 holes. How can I keep it on center and maintain a +/- .030 tolerance on the holes. I can use mill vises or v-blocks with clamps. My mill does have a DRO. I do have a lift cart to support the shaft when not clamped to the mill. Material is TGP shaft.

Looking for some ideas on how other folks would do this. I don't mind purchasing more vises or v-blocks if necessary. Hate to have to indicate each hole. Would like to be able to set up and use my DRO to stay on the 8" BTW centers.

Thanks in advance for help.
 
Use another vise that isn't bolted to the table?

Drill your four holes, clamp the part in the movable vise close to the fixed vise, move the part along, lather rinse and repeat...
 
I usually stick a drill in the last hole, crank the part over some known distance, reclamp and continue drilling.
 
Use another vise that isn't bolted to the table?

Drill your four holes, clamp the part in the movable vise close to the fixed vise, move the part along, lather rinse and repeat...

Like that and bolt a pin in the last hole and set up a stop for that pin on your table 8" from the first hole position
Make sure the stop is not in the way of the vice Or place the sliding vice on the opposite side of the stationary vice

Peter

On edit
Just noticed the sliding vice does not work as the stroke of 4x8" is too long
So eigter clamp some longer flat stock on the table that sticks out so the vice can sit on that Or clamp a piece of flat on the end of the bar and set it level
And then each time you reset the bar you can place a level on the flat Accuracy depends on how good your level is
 
Beware hole to hole, cumulative error ( I found out the hard way many years ago), reference off hole 1, cut story rods if required
Mark
 
If only doing one bar, I would do as Booze mentioned.

If you're doing more than one bar. Have two or three vices clamped to the table. Bolt a block to the table and drill a hole in it at a known distance. Use this to locate and align your shaft. Unclamp and pin the last hole you drilled and locate it to the hole in the block.
 
Program the shaft with the first hole being X0Y0. Drill the 4 holes and then reposition the shaft placing your drill over the last hole and use it to line up your shaft. Drill the next 3 holes and repeat.
 
Clamp the shaft in a vise ,clamp a Vee Block to the shaft and indicate it square to the table (just have it hanging above the table).
Drill your holes, slide the part, indicate the Vee Block in square again (or use a machinist square), pick up the last hole,move the Vee Block back to original position....repeat.

We do this often when we have parts longer than our X travel.



OR
if the hole to hole isn't too crucial, you can skip the Vee Block altogether and put a dowel pin in a toolholder, move to position of the last hole after sliding and manually bring it down into the hole on location.
 
I'd use the table T slots.

You can drill the reference hole (every 4th one) undersize and then skim it with a 5/16 or 8mm endmill to get it straight and in position. Then you can reposition fairly confidently with a corresponding precision pin held in the spindle. You can tap the reference hole after you've used it to reposition.
 
Ten feet long and +/- 0.030" on hole location! Holes are every 8" so probably 14 of them. You can drill four holes and then you need to move the shaft. So, four then three more and then three more, etc. I count four moves so each move must be +/- 0.030" / 4 = +/- 0.0075". It would be best to cut that down a bit to allow for other inaccuracies so perhaps +/- 0.005" per move. That sounds completely doable.

A fixture with three pins, 8" apart on the bottom and a rectangular block on the top, with it's edge 8" from the third hole. Drill three or four holes and drop that fixture in the last three of them. Use an edge finder to position the shaft for the next three holes. That and proper drilling technique should take care of the spacing along the length of the shaft.

But that leaves the angular alignment and there is little or no guidance for that. No angular tolerance seems to be given so what is it? All I can see is that same +/- 0.030" being applied to the shaft's radius (0.75"). Sine x = 0.030" / 0.75" = 0.04. I get x = 2.29 degrees. This is an approximation, probably on the low side.

To be sure I was holding that angular tolerance from move to move I would clamp a Vee block to the shaft after drilling the first four holes. I would use a machinist's level (0.001" in 10" or 12") to clamp it level. Then use that Vee block and level to keep the same angular rotation after each move. That way, all the angular positions would be referenced to that first position and there would be no cumulative error. This should be far better than the 2.29 degrees I calculated above.

As for using the third vise for maintaining the angular position, it would probably be OK. But all milling vises, even the most expensive ones, can be subject to the jaw lift problem which both lifts the part off the vise's bed, but also ROTATES it. Tapping a part down can eliminate the lift, but it does nothing to eliminate any rotation of a cylindrical part and that rotation would be a cumulative effect on successive moves. So I would avoid it if possible. The Vee block and level does this.
 
I'd use the Booze method but I'd use a dowel or otherwise round piece of stock to locate the hole. Not a drill bit.

As EPA noted, the issue will be in keeping the holes in line. But if the job would allow some tolerance, I'd lay a piece of aluminum angle along the shaft as a guide line and scribe a line down the whole shaft. That'd be where I aligned the drill bit for all the holes, etc.
 








 
Back
Top