Our company has a Daewoo DHM-800 Horizontal Machining Center. We have been having tooling issues for the past few months. This machine only drills bolt holes in 1045 forgings. Hardness of parts that the tool has failed on are usually around 200 BHN, which is in the center of specs. Hole sizes range from 3/8"-3/4". We started out using Allied spade inserts with Allied tool holders.

The problem is this. After making roughly 4-5 holes, the insert completely fails and sometimes take the toolholder with it. Since this has been happening, we have had to reduce the feed down to .006 ipr so that it doesn't fail. In doing so, the nest of material wrapped around the tool holder needs to be removed after 1-2 holes, which requires the operater to babysit the machine. This is unacceptable. So, now we are trying Guhring solid carbide step-drills which also blast a chamfer on the hole. We are experiencing extremely short tool-life with these as well.

We are only getting about 180 in. of tool-life whereas we should be getting inexcess of 1000 in. of life. TIR on all tooling is less than .001" and the hone on the Allied inserts were in spec, so this shouldnt be a problem either. We are having a very difficult time trouble-shooting this, so if anyone has had similiar problems with an HMC or this particular machine, it would be of extreme help.

Thanks for your help.

bma137,
I would start out with Dykem 107 hyspot Bluing. This is the greasy kid stuff, a little dab will do you. Clean out the spindle and blue up a tool holder. Clamp the tool holder in the spindle then release the tool holder. Check the contact between the tool holder and the spindle taper. Normal wear will be a slight bell mouthing in the big end of the taper. If you see light contact in the front on one side and the same light contact on the opposite side in the slamm end of the spindle, you had a wreck.
The next thing to check would be tool retention, check with the manufacturer to determine what it should be. Poor tool life can be caused by excessive end play in the spindle bearings. Mount an indicator on the side of the spindle housing, arrange the indicator to look at the face of the spindle. Hit tool unclamp, see how far the spindle assembly moves and then release tool unclamp and see if the indicator goes back to the zero you had when you hit unclamp.
Anything that is loose could give you problems with tool life.
To check bearing runout, use a test bar or a precision ground bar, get as far from the bearings as you can and while running the spindle slow, look at the runout.
If the indicator just goes from 0 to say .0030" and back to 0 and back to .0030", the
bearings are no doubt good. If the bearings are bad, the indicator will go from 0 to say .0030" and then it will go to maybe .0005" and then to .0035" and then back to 0. What I am trying to say is the high and the low will not repeat. The amount it does not repeat is bearing runout. Could be caused by loose preload on the bearings or it could be just worn bearings.
Are you getting any chatter? loose bearing preload, bad taper, low retention.
Let us know how you make out.
Regards Walt

I am assuming that you are using through spindle coolant. I have had the same problems with Allied spades lately. It has been hit and miss with the inserts. Try increasing your coolant concentration. You may have to peck drill it. I would say just enough to break the chip. I have had better luck with the Gen II TiN coated inserts rather than the AM200 coating. I will look at a program tomorrow to see what I did to get the insert to chip. The material I was drilling was 4130. The drill size was 1 7/8, 1 3/4" and 1 3/8 on a vmc.

bma 137,
Just checked your profile, We were just in Grove City at some engine plant.
They were in your town before they went to Grove.
Regards again Walt.

Hey Walt, sounds like a lot of great advise, ill see if I can try some of that by the end of the week. No chatter as well. Also Im guessing you were at the GE plant that makes the deisel engines that come up here to go into the locomotives at GE Rail.

Wolog, yes we are using thru coolant @ 1000psi, and also GenII AM200.

Ill let you know if anything helps.

Thanks for the advise.

Since this has been happening, we have had to reduce the feed down to .006 ipr so that it doesn't fail.


You failed to mention what your sfm was? My Allied book recomends 140 sfm for TiN and 220 for AM200 both of which seem fast to me. Also .006 - .013 ipr which seems ok. As an example I used an allied spade in 4340 forging at 350 bhn and the best I could get was 40 sfm / .003 ipr I was able to make it thru 4 holes 1.375 dia. and 10." deep. Any way it's all in the speeds and feeds good luck!


A.J.L.

For the .503 spade we were running at about 211-230 SFM and .009-.011ipr

But for the Guhring Drills, we started at 2646 RPM and 31 IPM (433SFM and .012 ipr) ...the rep for guhring says that since its a step drill that you should use the speed based off of the shank which is .625 and the feed based of of the cutting diameter which is .503. with this combo we are getting 180in. of life.

The tips of the drill are crapped up a little, so im assuming this is a sign of excessive speed. Anyway, our new recommended settings are 2139 RPM and 27.8 IPM (350 SFM and .013 IPR) for the guhring drill.

Also we are currently waiting for a new "special" Allied grind on the inserts to try.

Interestingly though, with the Allied spades, the previous holes show no indication of tool wear or breakage....it seems to be only right when it enters the material.

I have in the past had to start in the mat'l slow until full dia. is reached the speed-up to normal.



A.J.L.

Buy the way have you ever tried an Iscar Chamdrill? (see them at www.iscar.com) We have good luck with these. Might have to peck for deep holes though.

Never tried the Iscar, but the Allied holders we used had inserts built into the holder to buzz the chamfer.

The Iscar Chamdrill (pronounced cam-drill) has several type of chamfering bodies as well. Along with sub-micron grade carbide.

I just noticed on your last line a comment about the spaid drill failing at the entry into the cut.
Are you spottinr the hole?
Is the spot drill exactly the same angle os the drill?
Incorrect spoting of any hole can and will cause poor tool life on
any type of drill.