# Drilling 4 holes, orthogonal and equidistant from the center



## dansawyer (Apr 25, 2020)

I am making several parts that are all components of a project. (I will post pictures when it is complete). 
The current problem is I need to drill 4 holes in an aluminum disc which is about 4 inches in diameter. The holes need to be at 90 degrees from each other, in a circle 2 1/2 inches in diameter, and equidistant from the center. The disc has a 1 inch bored hole in the center. 
What is the best way to do this? 
I have a SB 9 lathe and an RF 30 mill. 
Thank you in advance and for your previous help, the project is progressing nicely. 
Dan


----------



## Asm109 (Apr 25, 2020)

Mount disc,  put test indicator in spindle and center the central bore under the spindle. Zero DRO and dial +X Drill, -X Drill, 0, +Y drill, -Y Drill.
No DRO? Note which direction you have taken out the backlash on the leadscrews, 0 dials.  repeat motions above, allways coming to your dimension from the direction with the backlash taken out. 
QED
Drill hole under size and finish to size with a boring bar will make your hole round, square and on size better than just drilling the hole.


----------



## Mitch Alsup (Apr 26, 2020)

Do you have a rotary table?


----------



## Winegrower (Apr 26, 2020)

dansawyer, without your specific knowledge of what you are trying to achieve, this question cannot be answered  meaningfully without understanding the tolerances involved.   At one level, get a tape measure, a pencil, some lined paper, lay it out and punch the marks through.   At another level, you need a laser interferometer.   Possibly there are a few levels in between.
I imagine providing more information will get you some good ideas.


----------



## Tozguy (Apr 26, 2020)

What I would do with what I have:

Measure out from the bore to mark the bolt circle. 
Mount the disc in a four jaw on a lathe and zero the bore and using shims to set the disc out from the chuck face
Turn power off to the lathe.
Install a drill in the tool post with a stylus in the chuck.
Set the stylus tip on center and then align the stylus tip to the bolt circle mark.
Replace the stylus with a drill. 
Use a torpedo level (or other small level) on the front jaw to create an index.
Put the lathe in lowest gear.
Drill the first hole then repeat for each of the other three jaws.


----------



## tjb (Apr 26, 2020)

Mr. Pete's approach:


----------



## MontanaLon (Apr 26, 2020)

Put disk in vise on mill. Edge find the jaws to find the center on x axis. Edge find the edges of the disk to find center on y axis.  No need to find the center that isn't there, if you know the disk is on size then you can just move in from found edges on axis and drill your holes. It should be accurate and repeatable.


----------



## BGHansen (Apr 26, 2020)

I'd knock in the 1" bored hole on your South Bend.  Then move to the mill.  Sweep in the hole so you are one center and zero out your hand wheels.  Then move just in the X or Y 1.25" to get to your 2.5"; you'll be moving to 12, 3, 6 and 9 o'clock.  I'm assuming you don't have a DRO, so you'll need to take note of the direction you were turning each hand wheel when you dialed in to center on the mill.

If you are making a lot of them, I'd make a fixture for the mill to set the disks in place.  Could be a simple 1/4" or 1/2" thick plate of aluminum or steel.

First, locate your mill into the LH side of the fixed jaw for X and the face of the jaw for Y.  Then move to the right by 1.5" and down in the Y 1.5" (not critical, needs to be bigger than your 1.25" radius plus the radius of the 4 holes).  Set the plate on your mill vise on parallels or a block of wood to space it up (wouldn't want to drill into your vise).  Use a 1-2-3 block or suitable edge to flush the LH edge of the plate with the LH vise jaw and tighten it in place.  Then spot drill a hole, and drill a tap hole for a 1" shoulder bolt (pic of one below) and tap the hole.  You can stack your disks up on the shoulder bolt and tighten it down to your fixture place.  

For the four holes, move in just the X or Y by 1.25" (you'll be moving to 12, 3, 6 and 9 o'clock), then spot and drill the holes.  Depending on the hole sizes, you could probably skip the spotting step if you have stubby (machine screw) drill bits.




You could also make a custom "shoulder bolt" on your lathe if the 3/4"-10 thread is a challenge.  A 1/2"-13 or 3/8"-16 might work fine too.  If you go this route, I'd chuck up a round bigger than 1" diameter and turn a shoulder to 1".  Also turn the end to either the 1/2" or 3/8" diameter and thread.  Naturally, you'll need to do the fixture plate described above with the same thread.  I'd cut a couple of flats on the large diameter of the custom shoulder bolt so you can put a wrench on it to tighten the aluminum disks down.

Advantage of the fixture plate is if you ever run the job again, you'll know where the center of the hole in the plate is.  Zero your mill on the LH fixed jaw and face of the jaw, set the plate in the vise and flush the edge with the edge of the jaw.  Your center will be whatever offset you used to make the plate in step 1.

Bruce


----------



## extropic (Apr 26, 2020)

Do it on the mill.

How many of the same bolt circles do you intend to drill? My question is intended to help decide whether any jig/fixtures are appropriate.
If multiple, do all the parts have the 1" center hole?
Does your mill have a DRO?
If NO, do you understand how to minimize the effects of backlash in your table positioning lead screws?
Is there a specific tolerance set required or "good enough"?


----------



## dansawyer (Apr 26, 2020)

Thank you all. This has been great reading. I found the center on the mill by turning a 1 inch diameter by 1/2 inch insert on the lathe. The insert had a center hole machined in. I used an center edge finder to find the center. I used that as the zero reference point. 
I then locked the mill x and y and removed the backlash by turning the controls clockwise until I felt resistance. I then zeroed the indicators and proceeded to move the ways 1.200 first x and then back (zero out backlash) then y. I then compensated for backlash in the counter clock wise direction and then drilled the second 2, same as the first. 
This all worked, thank you. 
As a note the general issue I am having seem to step from removing the part from the mill / lathe and then resetting it, usually in an other configuration for the next step. I need to figure out how to do that less and secondly how to better compensate.


----------

