machining a "hex" socket

hi, can someone please help me. i was wondering if there was a formula for machining a hex shape somewhere. i have manual machines with readouts and am wanting to make something to take out a 9/16" bolt. i was thinking about using like an 1/8" endmill, is there a formula for getting X and Y? i appreciate any help i can get, thanks in advance.
Darren
[email protected]

hemi altered 378 said:

hi, can someone please help me. i was wondering if there was a formula for machining a hex shape somewhere. i have manual machines with readouts and am wanting to make something to take out a 9/16" bolt. i was thinking about using like an 1/8" endmill, is there a formula for getting X and Y? i appreciate any help i can get, thanks in advance.
Darren
[email protected]

Click to expand...

Not really sure what you mean, but it is simple maths to work out the coordinates for the hex, but you would have to move the x and y axis together to be able to generate the hex. A rotary table would be far easier.

Tony..
thanks for the response. i have an index head, and a rotary table as well. basically i want to machine a socket....like you use to take out a bolt/nut....that will fit a 9/16" hex. thanks for any help

A hex 5C collet block sometimes works well for this type of work.

You might find that info in Machinerys Handbook. Look up 6 hole bolt circle and scale it to your size

thanks for the response. i have an index head, and a rotary table as well. basically i want to machine a socket....like you use to take out a bolt/nut....that will fit a 9/16" he

Click to expand...

just lay it out, drill the hole and carefully file to the hex lines - i've all the weapons you mentioned but would not bother for this sort of job because it surprising quick bench work and can be done to a fair degree of accuracy

to layout, look up the formula for across the points distance, (here, did it for you http://www.functionx.com/geometry/polygons.htm) scribe circle for the points. set dividers to the radius and space off around the circle - here this shows it http://en.wikipedia.org/wiki/Hexagon - radius of the points circle = the spacing of the six points on the circle

What I tend to do is set the part up and find center. Put in a (small) center drill and move either X or Y (lock the one you don't move) 1/2 the width of the socket across the diagonals.

For a hex, the diagonal is 1/cos x w/2 = 1/2 the diagonal. (w is the width across the flats, or 9/16. w/2 = 9/32). In this case 9/32" x 1/cos30° = .3248"

I then use the center drill to pop a divot deep enough to start a 1/16" drill. Rotate the index 60° and make the next center pop, etc around to the 6th hole. Then change to a 1/16" drill and drill all the spots down to the expected depth.

Then I rotate the index 30° and keeping the 60° spacing on the sector arms, reset them to this new starting point. Now you are centered 1/2 way between 2 points & parallel to one flat. The table has to be moved back toward center until the endmill is _inside_ a line that would connect the 2 dots on the axis you locked. Don't cut too close to the line to start, there is a lot of deflection on small endmills.

Lock the axis that located the end mill inside and perpendicular to the line. Now use the axis that was first locked and start milling the flats, visually staying inside the line Once you've gone around the whole way, measure the width across flats and step out accordingly to finish size. The 1/16" holes will be about 1/32 deep in the corners, but they make it easy to file the corners straight after milling close with a 1/8" or 3/32 endmill. You can even put a square bit in drill chuck in the mill spindle and slot out the corners by manually operating the quill (spindle off, obvioulsy ) to shave out the excess in the corners.

If you need corners that don't have the slight round "over-run", just subtract the necessary amount from the size bit you use to define the corners, from the amount you step out at the beginning.

Here's an example of what the process looks like. I needed a 3/4" square collet, but offset to the center. IOW, not a stock square collet. So made it the way described above, this shows how the corners look. In case it is objectionable for your purpose, just subtract the bit width. For me, it makes it really easy to square the corners

slotting out the corners

smt

i just wanted to say thank you for all those that responded. i very rarely post on here, but i have learned a ton! thanks again to everyone
Darren

hemi altered 378 said:

hi, can someone please help me. i was wondering if there was a formula for machining a hex shape somewhere. i have manual machines with readouts and am wanting to make something to take out a 9/16" bolt. i was thinking about using like an 1/8" endmill, is there a formula for getting X and Y? i appreciate any help i can get, thanks in advance.

Click to expand...

In addition to general guidance already provided, this tutorial presents equations for locating the corner holes:
Drilling a Hexagonal Hole by R. G. Sparber (2013)

9/16" hex and 1/8" end mill model. Dimensions are in mm :

There's probably a good answer to this but why not just buy a socket that size?

Hex or Rotary broach. I would drill out the corners then drill out the main body before broaching.
I think I did 7/16 using a section of a allen wrench in a hydralic press. really should have made a guide as it got cocked off normal several times.
Bill D