Cutting a concave hole

[Mike K]

I need to cut a concave depression that'll be used to grip a 1" plastic ball.  Is there any way to do this on the mill?  The plans for the part suggest simplifying it by making it 30* instead, but it would be nice to have the curve to limit wear on the ball.  Also, the position on the part prevents me from using the lathe anyway, as my lathe doesn't have enough swing.

I recently read in Guy Lautard's "Machinist's Bedside Reader" (great book, by the way) of cutting curves on the lathe without using a radius cutter, by moving the cross slide and saddle to a set of coordinates and then filing/sanding.  I was thinking about doing this with a boring tool in the mill.

Any thoughts?

Mike

[John Hill]

In to what material? 

How about drilling a series of steps (using different sized drill bits) to rough out the hole then finishing the job with a shaped bit cut from a flat piece of steel, or maybe put a ball end on a rod then grind it to half diameter to make a combination 'D' bit and form tool?

[sbwhart]

I think I can remember Bernd making a D bit and posting it on her, if my memory serves me correct he turned a disc up on the lathe the required diameter silver soldered it to a shank, backed it off an used it in a mill to put a rad round some plate, may be worth doing a search.

Good luck

Stew

[arnoldb]

I also remember seeing it Found it

You could also make it in the mill with a rotary table and coordinates...  Cut successively deeper rings toward the middle of the workpiece...  A ball-end mill would do a good job, and if you use close coordinate spacing it should come out pretty good...

Cheers, Arnold

[Mike K]

Thanks, guys.  You've armed me well.  Now to try it!  That D bit looks interesting.  It'll be my first.  I'll let you know if I manage not to goof it up.  I'm also going to test out the rotary table idea, since I haven't used mine yet (only been using the mini-mill for a couple months).

Mike

[No1_sonuk]

mklotz (just recently joined this forum ) has something on his web site that calculates the steps for you for making balls.  You'd probably just need to modify the numbers a bit to make a socket.

http://www.myvirtualnetwork.com/mklotz/  Look for ballcut.zip

I'm only going by the description there - I have no idea if it's suitable for your application.

[Divided he ad]

As the maker of the first "very badly designed" bit shown in that there post I'll say this.... Please be very, very careful with this idea....

The spinning one would not work as I'd centred it incorrectly, also the speed would need to be down to very low.

The stepping of the work piece is required to get the approx' size and then the re-designed tool was used to finish it off..... Bogs was the man who saved me from my own lack of knowledge 




As most people say.... What it is for will help with the answer.... Maybe a C-o-C ?






Ralph.

[mklotz]

Arnold beat me to it but I'll expand a little.

Assuming that you want to create a hemispherical cavity, one way to do it would be to rough it out and then mount it on a rotary table.  Then, with a ball mill take cuts around the inside surface of the cavity, each cut adjusted in radius and depth so the ball cutter was just tangent to the desired hemisphere.

What would result would be a cusped surface with the cusp height dependent on the number of cutting steps used.  Polish out the cusps and you're done.

If this method appeals to you, I can write a program that will generate the radii/depth pairs needed for the incremental cuts.

[Mike K]

Yeah, I guess I should have mentioned what I'm making.  I don't have a scanner to post the picture, but it's the "simple grinding rest" from Harold Hall's "Tool and Cutter Sharpening".

The one part is too long for me to spin in the mini-lathe to make the suggested 30 deg. cut.  So I figured I should be able to do something on the mini-mill.  Don't have much choice, though. Heh heh.

Ralph, I'm always careful.  Okay, usually.   First, I have to attempt the roughing steps.  And to be honest, I don't think I could do that D bit right now anyway...My mini-lathe is apart and the only drill rod I have is too small.

Marv, thanks for the offer.  I managed to work up a spreadsheet of offsets.  Although I may come knocking if this doesn't pan out.

Now that it's been suggested a few times, I'm dying to try this stepped cut thing.

Mike

[Raggle]

This is bigger than a 1" pocket but a pretty good description of the procedure

http://translate.google.com/translate?hl=en&sl=fr&u=http://romubricoltout.canalblog.com/&ei=sH-USrEYmcqMB7_RkPMN&sa=X&oi=translate&resnum=1&ct=result&prev=/search%3Fq%3Dromubricoltout%26hl%3Den%26client%3Dopera%26rls%3Den-GB%26hs%3D0zl

I hope that link works. It's a google translation  -  should keep everybody busy with the rest of the site, a superb 5" gauge DeCauville loco. Scale is 2.5" to the foot.

Warning: This site contains strawberries, the occasional onion and I'm sure I saw a greenhouse. I rather hope no-one submits too many "better translations"

Ray

[Bernd]

Ray,

Thanks for the link to that web site. I ran across that quite a while ago but never saved it. I see the translator takes literal translations. I think the pics and vids explain a lot. Don't need to know French.

Bernd

[Jonny]

If you havent a rotary table, could you drill through or deeper than necessary with say a 1/4" to alleviate centre cutting aspect?
Still preferable to remove as much metal as poss before using a bull nose cutter. If you are careful, lock the beds and tension up the spindle you can get away with a router cutter but think it will cut larger or chaff which will show the flexing of the machines castings and any play.

Regularly use router cutters on aluminium, no problem. Made a fair few as well.

[Mike K]

I haven't made any progress on the concave hole.  I'm looking for a ~1" plastic ball, making sure I have one before machining the recess to the wrong size.  The $1 store is my next shot.

I did, however, try out the "stepped cut" method on a couple of parts.  Works pretty well.




I modified the cutting method just a bit.  I think the Lautard book showed using a constant increment for one axis, and calculating the other axis values.

The problem is that the slope of the curve changes drastically, from very steep to very low (unsteep?):



So I used a constant increment for one axis for half of the coordinates (up to 45 deg) and then flipped the numbers:



I figured setting up the little brass crossfeed nut on the rotary table might be a chore.  But the table part could probably be setup on the RT with stops to place the part against to enable running through the corners quickly?

Mike

[mklotz]

When doing incremental contours like this, you'll be well advised to use a constant angular step size rather than a constant step of the X or Y value.  For example...

N = number of increments
ang = total included angle of cut / N

x = R*cos(k*ang)
y = R*sin(k*ang)

where k varies from zero to N-1 in steps of one.

[Mike K]

Oh, yes, that's even better!  Thanks, Marv.

Mike