4.3 mm holes, 20 mm deep

[johngoodrich]

what material are you drilling?

[Chaz]

what material are you drilling?

Alu.

[m_c]

For deep hole drilling, you really need good lubrication, and good chip clearance.

I've got an aluminium part that I drill on the lathe using a 6.8mm drill and 30mm deep (about 4.5 dia x depth). If the flood coolant fails (even just getting knocked away from hitting the drill), the drill will be welded to the part and snapped within a couple parts.
Polished drills greatly reduce chip welding (I use Phantom 11.160's, which are a polished cobalt stub drill).

For good chip clearance, you really need to ensure you're getting a good chip by using a reasonable DOC, which you may struggle to do with your spindle.

Having just ran the figures based on the drills I use, the optimum speed in soft aluminium is around 4400RPM, with a DOC of 0.135 per revolution, which should result in a required spindle torque of 0.7NM for a sharp drill.
Even with a solid carbide drill, the max speed is 12500rpm, but with a slightly higher DOC (and subsequently higher torque requirement - I've only got my spreadsheet setup for 11.160 drills)

The key thing is DOC and torque. Your spindle should be pretty much constant torque regardless of speed, so if it can't manage the require torque at a few thousand RPM, then it's not likely to manage at a higher speed. You could set the VFD to give a torque boost at lower RPM (increase the max current), but you do risk overheating the windings, however for peck drilling the load will be intermittent.

[Chaz]

For deep hole drilling, you really need good lubrication, and good chip clearance.

I've got an aluminium part that I drill on the lathe using a 6.8mm drill and 30mm deep (about 4.5 dia x depth). If the flood coolant fails (even just getting knocked away from hitting the drill), the drill will be welded to the part and snapped within a couple parts.
Polished drills greatly reduce chip welding (I use Phantom 11.160's, which are a polished cobalt stub drill).

For good chip clearance, you really need to ensure you're getting a good chip by using a reasonable DOC, which you may struggle to do with your spindle.

Having just ran the figures based on the drills I use, the optimum speed in soft aluminium is around 4400RPM, with a DOC of 0.135 per revolution, which should result in a required spindle torque of 0.7NM for a sharp drill.
Even with a solid carbide drill, the max speed is 12500rpm, but with a slightly higher DOC (and subsequently higher torque requirement - I've only got my spreadsheet setup for 11.160 drills)

The key thing is DOC and torque. Your spindle should be pretty much constant torque regardless of speed, so if it can't manage the require torque at a few thousand RPM, then it's not likely to manage at a higher speed. You could set the VFD to give a torque boost at lower RPM (increase the max current), but you do risk overheating the windings, however for peck drilling the load will be intermittent.

Thanks.

Thing is, these high speed spindles dont even turn below 150 rpm and at low speed are very easy to stall. Possibly the same at higher RPM however the momentum probably keeps it going.

Ive heard of bumping up the current, do you know where on the Chinese Hyaungyang VFD this is done?

What feedrate would you use at 12500 rpm with those drills? I did speak to them however being charged an admin fee and postage, higher than the cost of the bits put me off. Perhaps I need to look at this again.

[Chaz]

So I went back to what Phantom Drills had suggested. They indicated the 11.770 drill would be most suitable. Not sure what the differences are?

[m_c]

Having a quick look at the catalogue, 11.170 are a high helix version of what I use, which will help with chip clearance.

I'm not sure about what settings are in Huanyang VFDs, but the one you want to alter is for current. IIRC there is some setting whereby you can limit the current once a certain frequency is reached, but it's been along time since I read a manual. There will reach a frequency, where current will be limited by the maximum power available, which a good VFD will handle without any problem, but I'm not sure how a Huanyang will.

11.170 has a cutting speed of 40-65m/s (2961 to 4811rpm for 4.3mm diameter), with a suggested DOC of about 0.13 to 0.2mm per revolution. At 12500rpm, even at 0.1mm DOC, you're looking at 1250mm/m feed rate.
Running the figures through my spreadsheet, that equates to a cutting torque of 0.5 to 0.8Nm.

The postage cost from phantom is high if you're only ordering a couple drills, but I normally order over £50 at a time, so it's not so big an issue.

[Chaz]

Having a quick look at the catalogue, 11.170 are a high helix version of what I use, which will help with chip clearance.

I'm not sure about what settings are in Huanyang VFDs, but the one you want to alter is for current. IIRC there is some setting whereby you can limit the current once a certain frequency is reached, but it's been along time since I read a manual. There will reach a frequency, where current will be limited by the maximum power available, which a good VFD will handle without any problem, but I'm not sure how a Huanyang will.

11.170 has a cutting speed of 40-65m/s (2961 to 4811rpm for 4.3mm diameter), with a suggested DOC of about 0.13 to 0.2mm per revolution. At 12500rpm, even at 0.1mm DOC, you're looking at 1250mm/m feed rate.
Running the figures through my spreadsheet, that equates to a cutting torque of 0.5 to 0.8Nm.

The postage cost from phantom is high if you're only ordering a couple drills, but I normally order over £50 at a time, so it's not so big an issue.

Thanks. Ive checked some of the settings of the VFD online, Ill need to check tonight to see if its set right.

So clearly 75mm/min is nowhere near the right amount. Ive noted other machines that have high speed spindles just simply plunge and drill in what looks to be a millisecond. These are not always with spindle/tool through coolant. Clearly at 75mm/min I was just rubbing and dulling the tip.

I may order some of the German endmills and donate them for breaking / testing. Must be a way to get this right. In hindsight, I should have tested this on some scrap metal before doing it on the actual part. That said, small piece of alu, not the end of the world, the part will still work, just looks a bit crappy where the broken drill moved around in the hole.