Tormach 440 Drilling

[sirgreggins]

I tried a .203" drill, 120-150 sfm .002" feed per rev, pecking depth=25% of drill diameter in 1018 and the spindle stalls, or it drills but the bit gets pushed into the drill chuck. I was wondering if it's the machine or me? I tried a variety of speeds and feed and even have the belt in low speed mode but the tormach doesn't seem to want to drill it.

Similar Threads:

• Need Help!- F360 - Tormach PCNC 1100 Post Issue on Drilling
• Drilling a surface plate for measuring Tormach TTS tool length
• solidcam naming drilling geometry to drilling radius automatically
• Need Help!- Spot Drilling/Center Drilling Steel 55 HRC

[GLCarlson]

I tried a .203" drill, 120-150 sfm .002" feed per rev, pecking depth=25% of drill diameter in 1018 and the spindle stalls, or it drills but the bit gets pushed into the drill chuck. I was wondering if it's the machine or me? I tried a variety of speeds and feed and even have the belt in low speed mode but the tormach doesn't seem to want to drill it.

My go-to idjit start point on drilling a quarter inch hole in mild steel is 1000 rpm and 3 ipm, with a 0.1-.3 or so peck and a G83 cycle (full retract) if I'm running a program, with cutting oil. For a few holes, coordinate drill with the shuttle. Double rpm if the diameter halves, etc. This totally ignores sfm, feed, and all the other stuff, and all the tables. Drill in a chuck or ER20. I used to get all knotted up in calculating the theoretically correct numbers, which sometimes worked and sometimes needed tuning, and decided that I needed a standard answer that didn't strain the machine, burn bits, or require an hour of messing around for a 2 minute hole. Mostly, this keeps me around 60 sfm with a thou chip, and my bits last 25-50 holes or so between grinds.

Yes, I know this is offensive to the gods of CNC. And usually wrong, formally, and would get a really, really dirty look from anyone doing anything like production. I'm not.

All that said, the next (actually, first) thing to check is whether you have a good quality drill (PTD, Cleveland, etc- not box store) and that it's properly sharpened. I generally use a 4 facet style grind now; the drill really looks like a 2 flute mill. Drill-doctor also works. Do not assume that a new drill is sharp, accurately ground, point centered, or has a relief. Check. Or just regrind the minute you pick it up.

[Steve Seebold]

Sounds to me like you’re trying to run way too fast.

Your 1000 RPM is ok, but if you have flood coolant, use it and kick your feed up to about 12 IPM.

At 1000 RPM and 3 IPM, you’re probably just burning up the sip of the drill and glazing your work piece.

If you’re using jobber length drills, get rid of them and switch to a screw machine length cobalt drill and eliminate your spotting or center drill if you’re using one.

Again, using G83 and a Q value of .1 drill your holes all the way through your part.

[sirgreggins]

i did try running at 1000 rpm 3 ipm and still had the same problem. Since most of these holes are just clearance holes for SHCS's I'm just spotting the holes on the Tormach and drilling them out on the drill press until i figure out how to drill steel on this machine. Or interpolate the holes

[C*H*U*D]

Also, what drill angle are you using?

[popspipes]

try .25 IPM and use the slider to increase feedrate slowly, 3 ipm is pretty aggresive for steel in my opinion.
take a video and post it here, pictures are worth a lot trying to solve a problem........

I have seen guys try to drill a hole in reverse spindle rotation,something to check.

You say the drill is pushed up into the chuck, that indicates feed is too fast or a dull drill, or spindle rotation.

a video woud sure help....

[sirgreggins]

This is a brand new Hertel drill bit. 118 deg tip. Even at 1,000 rpm and 1ipm, it doesn't have the torque to make the cut. It's not a huge deal for the moment as these are only tests. I machine mostly aluminum parts and the machine does fine with that. I think i'm going to start interpolating holes in steel on this machine. I'm so used to Haas machines that the tormach is a little bit of a challenge to determine speeds and feeds. Mfg recommendations are way too much for the 440. FWIW, The higher sfm seems to cut a little better. Thanks for all the input guys!

[sirgreggins]

Well, after some more experimentation 200 sfm .0007 ipr seems to be the butter zone