View Full Version : Speeds and feeds deep drilling

08-02-2013, 12:56 PM
Tried asking this in another forum but got no reply.

I have just cncd my sx2 mill with 280 oz in (1.89Nm ) motors, xylotex controller and 1605 ball screw and nuts.

I'm drilling deep holes 27mm through aluminium with a new 5mm hss drill.

I'm using the following deep drill gcode G98G83X6.749Z-27.066Q0.531R3.0F10 spindle running at 2500Rpm.

It's taking over 35 minutes to drill 4 holes and I'm losing steps.

There's no counter balance or gas struts on the mill and I'm using WD40.

Question should I expect to get faster results without losing steps.

08-02-2013, 03:12 PM
Short answer is probably yes.

It's hard to say weather the motor will stall without knowing what voltage your driving it from, ideally the specific motor and the drive ratio between the motor and 5mm pitch ballscrew. Just as an example, lets suppose the motor outputs 1.2Nm at the speed you're running it at and it's a 5mm pitch screw with a 1:1 ratio. Use the following formula to find the force the Z-axis can apply:


(F=Force, T=Torque, e=screw efficiency, p=pitch)

So using the numbers above, F=1.2*2*3.142*0.9/0.005=1357N ... which is a large force. So as you can see, the mechanical advantage from using a screw drive is very high so I'm surprised that it would stall, especially at such low speed. Perhaps the gib strips are too tight on Z? What rapid feedrate do you get?

For the parameters you specified, I'd try about 9mm peck depth and if using 2500rpm at about 200mm/min.

08-02-2013, 03:37 PM
Oh Man-O-Man your massively out of wack with those settings.? . . . 3mm peck and 300mm/min would be easily achieved.
My spindle spins twice the speed and I peck at 5mm and 800mm/min with no problems. I can and do drill straight thru 20mm plate single pass @600mm/min at times if just few holes and I'm in a rush, I often drill 12mm plate in 2 pecks no matter how many holes.!!

By the sounds of it you have other issues thou and those need sorting first.? Obviously go thru all the usual checks for sticking or binding etc.
Really you shouldn't be having missed steps at these feeds even without any counter balance so I'd be suspect of the drives or BOB and connections if there's no mechanical issues.
Check the drives and motor connections etc, make sure you have the motor phases correct on the drives IE: A+ A- not switched round.

It could be you have the control settings screwed up.? What you using for control Mach3 or EMC.?
If Mach then what's the motor tuning settings.?

08-02-2013, 03:53 PM
Oh forgot to say Check your motor couplings or pulleys are not slipping.? Mark them with paint.

08-02-2013, 04:33 PM
Thanks fellas something to think about.
its only a small machine so I don't know just what it capable of.
at the moment I'm facing 13mm off some alli at 1700 rpm feed 92.79mm min 1.5 mm depth with a 1/4 end mill.
using mach3 see if anything gives or moves.

08-02-2013, 08:39 PM
Hi jazz cnc this is my Mach settings.
Mach3 settings
Steps per x 323.31 velocity x663.6 accel 77.708 step pulse x5 stepdir 5
For y 319.82, 431.34, 18.38, 5. 5
For z. 324.14, 348.72, 18.51. 5. 5

I have just checked the vref on the xylotex and there set at 2.16v =1.5Amp so have increased z to 3.42v =2.5Amp I think the voltage is 30v ?

im losing steps when drilling down not when raising the head makes no difference with or without the counter balance.
with power off I can move the head up and down with one finger turning the Handel on top of the motor.

09-02-2013, 01:11 AM
Deep drilling can be a pain.

Going by the spreadsheet I made up, a 5mm standard point dull drill in alloy should need a maximum 450N of thrust at a feed rate of 0.1mm a revolution (a 5mm drill will probably need a lower depth of cut, but it depends on the drill type you're using). A similarly dull split-point drill will only need a max of 350N.

Make sure your feed rate is high enough, otherwise the drill will rub more than cut, causing excess heat and alloy build up on the drill, greatly increasing the thrust required. You want the drill to make a continual definite cut.
Play with the peck depth, as you need to ensure the drill is cleared at deeper depths. If the drill clogs, then it's a recipe for lost steps.

If you're doing lots of these, then you may want to consider doing some manual coding.
Start of with a simple single drill to a depth just before clogging becomes an issue (2 x diameter is a good start), then start a peck cycle at that depth. You may want to use more than one peck cycle, with a full retract between them.

A couple drops of some proper cutting/tapping fluid will help avoid alloy build up on the drill, and improve chip clearance.

09-02-2013, 11:11 AM
Thanks fellas turning the amps may have helped? Or it may be changing the drilling cycle to deep drill 3 pecks feed 300 mm min but it seems to go through like hot knife in butter. No stalling and lost steps.
Problem I find is when having problems your instinct is to go easier and slower but most of the time it's better to go harder and faster.

09-02-2013, 11:47 AM
Thanks fellas turning the amps may have helped?

Until the iron saturates, torque is proportional to current, so yes it's likely to help. Keep an eye on the motor temperature though - no more than 80C on the case is allowed. Do you have the model number of the motors so we can check what current they should be run on? Iff the motors, drivers and power supply are safe operating from 3.5A you might as well put them all on that current and get better feedrates or reliability.

09-02-2013, 12:06 PM
Taking a decent cut of metal will of made a big difference.
If you don't take a deep enough cut, the heat builds up at the tip, leading to work hardening, and chip build up on the drill, which then reduces cutting effiency further.

It's best to look at the speeds/feeds for what you're using, and work out what the limiting factor of your machine is. Mostly in aluminium, spindle speed is the limiting factor.

09-02-2013, 01:20 PM
These are the motors Xylotex Stepper Motors (http://www.xylotex.com/StepperMotor.htm) I think as I bought it of a guy that split his cnc machine, motors and controller, ball screws and nuts, x2 mill, no idea whey said he got more for the parts than compleat. There's no label on the motors.
Speed of the spindle does that affect quality of cut or speed of cut.

09-02-2013, 01:55 PM
Just speed of cut.

I just ran through some figures, and for a standard polished HSS drill suitable for soft alu, gives aprox. 2500-3100rpm.
The recommended feed rate is 0.19mm per rev, which equates to 475 to 590mm/min feed rate.

To acheive those feed rates, requires 450N of thrust and a 0.25kw spindle, and that's with a sharp split point drill. With a dull standard point drill, those figures rise to nearly 700N and 0.33kw.

However all those are theoretical, and just provide a best case to start from. Experience and experimentation on your particular machine will find the best for you.

10-02-2013, 03:27 PM
Mach3 settings
Steps per x 323.31 velocity x663.6 accel 77.708 step pulse x5 stepdir 5

Your missing steps are not likely to be from cutting or drilling with wrong settings given the slow feeds you were using and the fact the head is so easy to move.
Much more likely to be dropped pulses from either incorrect setup or poor parallel port.

I see one potential cause so first Change the Step pulse=0 Dir= 5 and your missing steps may come back.

Check the Kernal speed. If it's above 25K then drop to 25K and retune motors, you must retune motors.!!.
Mach works best at 25K and the only reason to go higher is if you can't achieve the speeds you require and even then above 45K isn't advised unless very fast and stable PC.
For your machine it doesn't need high Kernal speed and using at higher speeds will potentially make the system unstable.

The steps per are bit Odd number at 323.31 and the number indicates micro stepping around 1600 with 5mm pitch screw which if your parallel port is struggling would put it under stress enough to drop steps.
Consider dropping to 800 micro steps so the PP and PC are not working so hard.!. . Again you must retune the motors.

First check Kernel speed and change if above 25K then change Step/Dir pulse then retune motors. IF kernel Ok then change Step/Dir and try again before changing any thing else.

10-02-2013, 09:00 PM
[QUOTE=JAZZCNC;42305]Your missing steps are not likely to be from cutting or drilling with wrong settings given the slow feeds you were using and the fact the head is so easy to move.

I think the step,losses was because the motor was stalling, the figures in motor settings were from using a digital callipers to measure the distance traveled in settings.
easy way of calculating them, backlash was with a dial indicator.
It's working ok as,I'm able to drill 20 odd holes 30mm deep and go back and drop the drill back down any of the holes. Lot of reading and experimenting at the moment. As they say turning big bits of scrap into smaller bits.