Page 3 of 3 FirstFirst 123
  1. #21
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 14 Hours Ago Has been a member for 5-6 years. Has a total post count of 1,192. Received thanks 85 times, giving thanks to others 58 times.
    Quote Originally Posted by m_c View Post
    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.

  2. #22
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 14 Hours Ago Has been a member for 5-6 years. Has a total post count of 1,192. Received thanks 85 times, giving thanks to others 58 times.
    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?

  3. #23
    m_c's Avatar
    Lives in East Lothian, United Kingdom. Last Activity: 9 Hours Ago Has been a member for 9-10 years. Has a total post count of 2,121. Received thanks 233 times, giving thanks to others 5 times.
    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.
    Avoiding the rubbish customer service from AluminiumWarehouse since July '13.

  4. #24
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 14 Hours Ago Has been a member for 5-6 years. Has a total post count of 1,192. Received thanks 85 times, giving thanks to others 58 times.
    Quote Originally Posted by m_c View Post
    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.

  5. #25
    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.
    Last edited by routercnc; 08-08-2017 at 05:52 AM.
    Building a CNC machine to make a better one since 2010 . . .
    MK1 (1st photo), MK2, MK3, MK4

  6. The Following User Says Thank You to routercnc For This Useful Post:


  7. #26
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 14 Hours Ago Has been a member for 5-6 years. Has a total post count of 1,192. Received thanks 85 times, giving thanks to others 58 times.
    Quote Originally Posted by routercnc View Post
    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.

    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?

  8. The Following User Says Thank You to Chaz For This Useful Post:


  9. #27
    Chaz's Avatar
    Lives in Ickenham, West London, United Kingdom. Last Activity: 14 Hours Ago Has been a member for 5-6 years. Has a total post count of 1,192. Received thanks 85 times, giving thanks to others 58 times.
    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.
    Last edited by Chaz; 08-08-2017 at 10:01 PM.

Page 3 of 3 FirstFirst 123

Similar Threads

  1. just how deep does a water trough need to be?
    By nobby in forum Plasma Table Machines
    Replies: 1
    Last Post: 09-07-2017, 03:27 PM
  2. foam cnc carver- deep z axis - 4x4 bed
    By marbles in forum Hotwire Cutting Machines
    Replies: 9
    Last Post: 17-05-2016, 08:20 AM
  3. What tooling to drill lots of 10mm holes 45mm deep?
    By AlanMJackson in forum Tool & Tooling Technology
    Replies: 24
    Last Post: 13-01-2014, 07:53 PM
  4. How deep can i cut MDF?
    By MrWiz73 in forum Machine Discussion
    Replies: 6
    Last Post: 24-08-2011, 09:38 PM

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •