Printable View
I need to do a set of 4.3 and 5.3 mm holes, at least 20mm deep.
I can drill these but will need to buy specific drill bits which may never get used again (around £15 each, carbide).
I could interpolate, problem is that a 3 or 4mm endmill typically only has a flute length of around 10mm max. There would likely be long reach endmills, will have to source.
Accuracy needs to be fairly good, how would you do this?
Those are about the size of a No4 and No18 drill if these are cheaper and accurate enough.
Thanks, ive not seen those sizes before, checking prices.Quote:
Originally Posted by EddyCurrent
Any idea who sells them in the UK?
So your going to be doing some tapping?
I would just spot drill (good them osborn/europa), then open them up as normal i.e jobber/twist drill bit, I've been using these Heller HSS German made bits pretty much exclusively recently without fail.
They do HSS-R and HSS-G versions, R is for non alloyed steels and G is aimed at alloyed, the G have a 135 degree split point for optimum centering and dimensional accuracy.
You can find them all over eBay if you search, I've even got their 15 and 20mm "black smith" type to open up clearance holes for my leadscrews...they worked sweet as a nut!
I wouldn't go anything less than the 4.3 you need, use the 4.3 for the 5.3 as well so you've got a nice pilot hole you can then open up, use plenty of cutting oil and take your time, dont forget to give the holes a small chamfer to help the tap locate :)
Thanks.Quote:
Originally Posted by Lee Roberts
Phantom Drills came back and offered this:-
Phantom drill 11.770
They are cheaper than carbide, around £5 each. This was based on my requirement to do 'high speed' drilling due to limited low speed torque with the Chinese spindle.
This wont be tapped, its a through hole for a bolt.
Ok so the .3 is putting you in the middle of standard and close fit, what I've linked to should give you what you need for a through/clearance hole of fairly good accuracy surely?Quote:
Originally Posted by Chaz
Yep, exactly. Ill order those drill bits, seems good value for money and keep for future if I ever need to do similar again.Quote:
Originally Posted by Lee Roberts
Cool, if you look I think you can just buy 1 bit at a time for 99p all in or something from another seller, saves buying a box of 10.Quote:
Originally Posted by Chaz
I'll confirm what I've got if you want and send you?
Number Drill set; http://www.ebay.co.uk/itm/RDGTOOLS-6...EAAOSwx~JWFOOB
Sure, thanks, happy to pay.Quote:
Originally Posted by Lee Roberts
Thanks.Quote:
Originally Posted by EddyCurrent
Are these clearance holes for 4 and 5mm bolts?
If so you can just drill them 4 and 5 mm because the bolts are slightly under size.
I often drill 0.5mm larger just to get me some assembly allowance but that is just a convenience
I think one of your worries is whether the Chinese spindle will drill holes in this size due to limited torque. Well because the drills are small you can spin them quickly so there are no issues there and I regularly mill 3 mm holes using a twist drill to 15mm depth.
You need to watch the flutes blocking after about 10mm so need to do small pecks and wipe the bit with an oiled brush each time it comes out of the hole between pecks. If it welds in the hole it will snap off and ruin your day.
Are these shoulder bolts? If so you can ream them after drilling to register on the shoulder.
Ye, just clearance for bolts and agreed, 4mm should work too. Ill do very slight pecks and take my time with the drilling.Quote:
Originally Posted by routercnc
Many thanks to Lee Roberts for providing some drills that will be suitable for these holes :-)
I have 4mm endmill length 22mm.
Where did you get these from?Quote:
Originally Posted by cncmachineokk
So I tried to drill this today, 0.25mm pecks, 24K RPM, 75mm/min plunge. Went OK initially however about a third of the way and the drill snapped. I didnt want to go faster however it was just rubbing most of the time, was the feedrate too low? It had a mix of air and WD40 on it all the time.
Argh.
what material are you drilling?
Alu.Quote:
Originally Posted by johngoodrich
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.Quote:
Originally Posted by m_c
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.
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?
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.Quote:
Originally Posted by m_c
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.
Hi Chaz,
If it helps - in the line boring video I posted recently you can see 3 mm holes being peck drilled (with full retract to clear the chip) at ~12,000 rpm. Can't remember the feed - maybe 300 mm/min? Drill bit is plain HSS.
You can see the chip fly out each time, and a dab of oil keeps it running smoothly. Starts at 0:32
https://www.youtube.com/watch?v=sYhDtuqzf2I&t=6s
Been using this method for some time and it works well.
Thanks.Quote:
Originally Posted by routercnc
I did some checking last night. My VFD's current looks to be set correctly.
There is an auto compensation value for increased torque demand. Set to default of 2% but can go to 10%. That's now changed.
There are also some parameter values between PD005 and PD010 which allow different torque curves. I *think* default is a constant curve, there is an option to go for what's called high torque where it provides better torque at lower speeds. This will help a bit, Ill lower the speed and see. Clearly the feedrate of what I was doing was too slow too.
Also, what oil do people use? Anything specific or just 2 in 1 oil? Ive got big container of VG220 Mobil oil that I got with one of my ballscrew / rail orders. Would that work and is it better than trying to spray WD40?
Ok, pushed up the VFD power a bit, it doesnt seem to like this but has worked.
I used a 4mm drillbit for the 4.x mm holes and the bolts fit well, no need for the slight oversize IMHO. Redid the failed 5mm holes, done.
12500 rpm, 0.25 depth, full retract, 500mm/min plunge.
I did have a problem with Thor which cost me about 2 hours, the bearing nut came loose and caused problems. I had heard something but didnt investigate it earlier, no damage done, phew.