Small holes 10x dia with very low runout

We're running 12L14 on a Daewoo chucker lathe.
Need to drill 0.063" hole, 0.550" deep (ok, 9x deep)
Diameter +0.002/-0
TIR over the length of the hole is 0.002" max. OD is turned in the same setup, before hole is drilled. Need 3,000 holes/month.
Currently using Metal Removal carbide drills with a low helix and split point. We do not have high pressure through coolant.
Currently running 5krpm, 0.001"/rev, 0.030" pecks with full retract (G83 Fanuc) on a spotted hole. Using a Cheap 'n Cheeful ER20 holder/ collets in a boring bar VDI tool block, we're getting very poor results. Even when drill is centered to 0.0003". Worse results as machine warms up and drill drifts 0.0015 off center. Drill life is about 150 holes and concentricity is not stable within our tolerances, even when the machine is warm and the drill is new.
Possible options: -Invest in $800 holder which can be adjusted in x and y (we don't have y-axis) and its angle can be adjusted. Made by Gyro -Go with HSS vanadium OSG 1100-series drills. Tool rep says no pecks, good runout, good size. About $20 each (which is fine, if they work) -We were thinking of building a floating holder which will ride on three ball bearings so it can "actively" float in x and y (only about 0.003 in any direction). Also adjustable in angular alignment along z.
Any thoughts? It looks like carbide is not recommended for this type of application. We've had good success with parabolic flutes in other applications. Would it help here?
We are currently outsourcing these parts to a lathe job shop who knows what he's doing, but we're eager to bring them in house.
Thanks for any thoughts.
Regards,
Robin
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

In my experience, parabolic drills wander around even worse than jobber drills.
Suggest drill a few thou undersize ( say .004 ~.006 ) and bore to finish with a single point tool--your tir will drop to an amount that's so small you won't even be able to measure and your diameter will be very easy to control by simply adjusting your X offset as needed for tool wear.
Keep the machine warmed up and a stable coolant sump temp so that it doesn't drift. ( wait till the tank is almost empty then decide to dump 25 gallons of cold tap water into it and all bets are off )
The boring bar below would need to be slightly modified for lenght and minimum entry dia but any competant grind shop should be able to handle this for you.
http://tinyurl.com/y6q455w
If it were me I would just go ahead and make up a batch of them myself from .0625 carbide blanks on a vmc in a 4th axis 5c attachment with a 4in diamond cup wheel mounted in the spindle and be done with it--as a point of reference, a carbide blank in that appx size costs about $2.50 USD but then again I have no idea where your shop rate stands.
--


Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Robin S. wrote:

Robin, I'd give the parabolic drills a try. Titex or Guhring would be my first choices. I'd probably start at 4000 RPM and .002 feed. I would write my own drill cycle instead of using G83. First peck something like .200", then maybe a couple of pecks at .125".
On your carbide drill my thought is your taking too many pecks and not enough feed.
If you go the floating holder route I wonder if one of those Hardinge floating holders could be adapted to your job.
http://tinyurl.com/y556u2u
http://tinyurl.com/y59hk5m
Best, Steve
--


Regards,
Steve Saling
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Boring: I don't have experience using carbide boring bars for 10X dia. We have one running 7X and it works well enough (until it randomly comes out of the hole in two pieces). I'd have to bore in the pull direction so chips don't get under the bar. Could be dicy, but we'd be willing to try.
Warmup: We do run a warmup cycle. Machine still wanders in the first 60min of run. Perhaps I'm doing something wrong.
Carbide drill: I suppose I didn't try any higher feed than 0.001". I suppose I should have. Did not break any drills. They only wore out.
Floating holder: We want to make not an adjustable holder (screw machine style) but one that actually moves all the time. The idea being to let a non-skilled worker run the machine. Offsets with single pointed tools are ok as you can measure the part and make an adjustment. If the operator has to indicate the drill, we're quite weary of the level of skill required. We want to run unattended eventually so this would be impossible.
Drill locaiton never varies by more than 0.002", even from cold.
Peck: I will eventually get to that point. I'll have to determine if chip evacuation is adequate to remove the necessity for pecks. Tool rep specified no pecks for these OSG drills.
Thanks for the ideas, guys.
Regards,
Robin
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Robin S. wrote:

Your rubbing and not cutting.

I've had good luck with parabolics drilling deep holes. I drill a .156 dia hole in alum. 5" deep from both ends of a part with some mismatch, maybe .010. This in in a VMC. Which reminds me, if you have a way to rotate the drill the drill better for size and location.
Best, Steve
--


Regards,
Steve Saling
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

If you're running into issues with boring bars that deep, another way to help holes stay where they should be is to drill a few thou smaller in diameter to a depth roughly 2x the finish drill diameter, then use an end mill the size of your finished hole (or a boring bar) to cut a pilot for the finish drill. It takes more tool changes, but it's pretty effective.
Later,
Charlie
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

skip the drills use a centre cutting endmill; drills wander; if your stock is aluminum use regular dishwashing liquid and water as coolant/ lubrcant and just squirt a bit on the tool; you'll have to practice the feed and speed to get it right.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Just in case you're not already....do make sure and spot to a diameter that's a tad bit larger than the drill size--also, your center drill should dwell for at least a few revolutions while at depth.
--



Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
On 4/17/2010 9:07 PM, Uhh Clem wrote:

I've always let a center drill or spot drill dwell at least 2 revolutions while at depth. P(120/RPM)
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Robin S. wrote:

Free cutting material, use a half round drill. Check with your tool supplier, excellent finish and size control.
--
Steve Walker
snipped-for-privacy@verizonwallet.com (remove wallet to reply)
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.