We have a Daewoo DHM-800 HMC and we have trying out some Guhring Drills Series Solid Carbide 5510 1/2 Dia. Firex Coating. We have changed the Speed and feeds from 24-31 IPM and 2646-2139 RPM our tool life is roughly 200-250 inches of tool life. Our material is 1045 forgings depth of cut is usually 1/2-3/4 in. Recommended Speeds and feeds are 3114 RPM and 50 IPM. These seem extreme. I know we should be getting roughly 1500+ inches.

I would like to hear what everyone else gets on these drills as far as life and speeds and feeds.

Thanks

We have a Daewoo DHM-800 HMC and we have trying out some Guhring Drills Series Solid Carbide 5510 1/2 Dia. Firex Coating. We have changed the Speed and feeds from 24-31 IPM and 2646-2139 RPM our tool life is roughly 200-250 inches of tool life. Our material is 1045 forgings depth of cut is usually 1/2-3/4 in. Recommended Speeds and feeds are 3114 RPM and 50 IPM. These seem extreme. I know we should be getting roughly 1500+ inches.

I would like to hear what everyone else gets on these drills as far as life and speeds and feeds.

Thanks

Personally I haven't tried those drills, but regular Guhring. Guhring Drills are great. I suggest using moderate Feeds and Speeds to start and if you feel it neccessary bring them up a little at a time. BTW: Use a Spot Drill before drilling. Depending on how flat the Forging is you may end up snapping drills due to deflection even if they are 1/2 inch stubs.

Spot drilling isn't an option, it takes too much time. Also we shouldn't need to spot drill with Carbide.

Depending on the roughness of the forging, like tobyaxis said, could cause enough deflection to break that drill, but I haven't used that particular brand just other carbide and usually it dont like that deflection. I would also start with the lower speeds and feeds to start and work up from there.

To me that seems about right on the speed, but even for the best super duper carbide drills, that seems like a lot of feed. The suggested feed is .016 per rev, thats seems like a heck of a lot for a 1/2" drill.

What kind of failure are you getting? Are you pecking? I wouldn't. If I had to guess, I would say that whatever damage you're getting is at the start of the hole. I don't spot either when drilling with carbide, unless I need a chamfer, but if I'm going to be pushing some high feed in the hole, I will start the hole at a low feed to avoid any deflection, this is probably more important on a forging that is probably not dead flat.

These are not rough forgings, the have already been turned in a previous operation.

Also, these are thru holes, im thinking the speed and feed arnet matched correctly and that when the drill exits the material its pushing the material instead of cutting.

If you look at the photos, they are chipping at the corners and there is a slight buildup in the very tip.

These are not rough forgings, the have already been turned in a previous operation.

Also, these are thru holes, im thinking the speed and feed arnet matched correctly and that when the drill exits the material its pushing the material instead of cutting.

If you look at the photos, they are chipping at the corners and there is a slight buildup in the very tip.


Your speed is too high. ;) That is why the outer edges are wearing like that.

Are you using coolant? If you have thru spindle, you can run it thru the collet, if the drill isn't thru cooled.

I agree with using a feed about 1/3 that of your drilling feed until the full diameter of the drill is engaged, then let'er RIP!!!!!!!

Yes we are running thru coolant.

Higher speed is what we initially thought as well.

I just discovered yesterday that when the drill is exiting the hole, the relief in the aluminum jaws holding the parts is only the diameter of the actual drill, so i think that the cap/burr that the drill is pushing out gets caught and its like a intermintant cut for the drill. This would happen on the top and the bottom hole only.

So we are going to try to mill out the relief to give that cap/burr some room to move.

Thanks for all the advice everyone.

Make sure the relief is larger in diameter, and slightly deeper than the drill will go, so the slug has room, otherwise it'll be spinning on the end of the drill, and preesing against your jaws.

Ciao

i highly doubt the speed is too high ,ive been using a similar drill in 4140 forgings 4700rpm @ 42"/min 1.75 dp

did you dial up the drill to make sure there is 0. runout

Forget the Carbide use OSG SUS Gold Drills you'll see better results, no center drilling , longer tool life and less cost?

Let me know what you think.

joe_souza@sbcglobal.net

i highly doubt the speed is too high ,ive been using a similar drill in 4140 forgings 4700rpm @ 42"/min 1.75 dp

did you dial up the drill to make sure there is 0. runout

Dertsap, this sounds crazy, what diameter is it? and what collets are you using?
also is it a VMC or HMC?

13/16 kenametal ( same stuff), on a vmc , er collets , we don t plan to drill a million holes at that but it works for what we need
spot drilling and center drilling has been pointed out a couple of times ,
the ONLY time to spot is on a really bad surface , not recommended or required for carbides otherwise

not telling you to neccessarily go by my example , only what the tools are capable of