flood or through coolant for drill

[mielke]

When drilling would it be best to turn off flood coolant and only run through coolant with a drill? Would this create a higher pressure of coolant flow through the drill, as opposed to running both flood and through coolant? any suggestions?

 

[MikeHalloran]

What problem are you trying to solve?



Mike Halloran
Pembroke Pines, FL, USA

 

[mielke]

Trying to find a TEMPORARY solution. We got some drills that are designed for a higher coolant pressure than we have and they have been wearing down and becoming dull too fast. We have been running with flood and through spindle coolant.

 

[saberblue]

As a rule of thumb you need 1.5 GPM/HP used at the point of cut for big chip machining + 1 GPM per 10 feet that you need to move the chips to have enough fluid that it's application is/can't be and issue -- to answer your question check how may GPM your pump is supposed to deliver and then check the volume you are actually getting (a5 gallon bucket and a stop watch)--often times the pumps are throttled back to reduce the splash -- then run the same experiment with and with out your flood coolant --

Also be aware that if you don't keep your coolant very clean or with enough use the impeller and seals in the pump will wear and it will loose a lot of efficiency

good luck



A.R. "Andy" Nelson
Engineering Consultant
anelson@arnengineering.com

 

[MikeHalloran]

Since you haven't revealed
- material
- diameter
- depth
- rpm
- ipr

... all I can suggest is to double the feedrate, and keep doubling it until you split a drill, then back up one step.


Mike Halloran
Pembroke Pines, FL, USA

 

[mielke]

5/8" thick 304 SS material
0.384" diameter holes
running at 180 speed ft2/min (~1800 rpm)
and 0.008 feed in/rev

its a carbide drill i get about 500 holes down and then the chips dont break up and start bunching up around the drill.

 

[MikeHalloran]

Your feed seems about right, the speed might be a little high.
Try reducing the rpm by 100 rpm at a time and see how your tool life changes.




Mike Halloran
Pembroke Pines, FL, USA

 

[saberblue]

To make full use of the thru the drill coolant you need to push sufficient volume thru the drill that the velocity of the coolant will lift the chip out of the hole before the drill comes around again -- that will make sure that the chips do not birds next or get recut

A.R. "Andy" Nelson
Engineering Consultant
anelson@arnengineering.com

 

[mielke]

Thanks everyone. Would u advise only thru coolant or do both?

 

[mielke]

Also any idea of how many holes I should be getting? I'm seeing about 500 till the bit dulls and about 1000 till it breaks

 

[saberblue]

I would drill 350 to 400 holes and then re-sharping the drill -- you will get better holes with less down force and less total drill cost

A.R. "Andy" Nelson
Engineering Consultant
anelson@arnengineering.com

 

[Jaydenn]

On most machines, the flood and thru coolants are handled by seperate pumps, so running one pump should not affect the output of the other.

I'm guessing that you are not pecking, so flood is pretty useless. Virtually no coolant will get to the tip.

I would only run the thru; but that's just my opinion.

J

 

[Viktor]

Before you try to figure out about the coolant application, you should first to know if the drill geometry and carbide grade are suitable for the work material. Coolant-through drills performs ALWAYS better that those with flood coolant provided that drill geometry, machining regime, tool material (including the proper coating) and coolant flow rate are suitable for the application.

IMHO, the best way to start is to look at the wear pattern on you drills - to understand "where it hurts" - it is drill corner's excessive wear or the chisel edge presets the problem, or the major cutting edges (lips) are simply chipped. Depending upon the results obtained, the proper solution to your problem can be found: carbide grade, tool geometry, coolant, etc.

Viktor

http://viktorastakhov.tripod.com

 

[ProgressiveRacing]

Perform a little cost analysis and see if you're wasting your time or not. 500 holes doesn't really say much... are they .25" or 2.5" deep? Perhaps the tool life is fine and you just need to change tools more often. When everything breaks down; cost per part, tooling usually comes out at 1-3% of total costs. You can increase the tool life or push them harder to lower the cycle times. Do the math... but I've found, more often than not, that trying to increase tool life by 10-20% is more expensive than pushing them 10-20% harder.

YMMV.

Regards,
Chuck

The Manufacturing Reliquary

http://cmailco.wordpress.com/