Page 1 of 2 12 LastLast
Results 1 to 12 of 15

Thread: Guhring Solid Carbide Drills

  1. #1
    Registered
    Join Date
    Jul 2006
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0

    Guhring Solid Carbide Drills

    We have a Daewoo DHM-800 HMC and we have trying out some Guhring Drills Series Solid Carbide 5510 1/2 Dia. Firex Coating. We have changed the Speed and feeds from 24-31 IPM and 2646-2139 RPM our tool life is roughly 200-250 inches of tool life. Our material is 1045 forgings depth of cut is usually 1/2-3/4 in. Recommended Speeds and feeds are 3114 RPM and 50 IPM. These seem extreme. I know we should be getting roughly 1500+ inches.

    I would like to hear what everyone else gets on these drills as far as life and speeds and feeds.

    Thanks


  2. #2
    Moderator tobyaxis's Avatar
    Join Date
    Jan 2006
    Location
    USA
    Posts
    4,394
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by bma137
    We have a Daewoo DHM-800 HMC and we have trying out some Guhring Drills Series Solid Carbide 5510 1/2 Dia. Firex Coating. We have changed the Speed and feeds from 24-31 IPM and 2646-2139 RPM our tool life is roughly 200-250 inches of tool life. Our material is 1045 forgings depth of cut is usually 1/2-3/4 in. Recommended Speeds and feeds are 3114 RPM and 50 IPM. These seem extreme. I know we should be getting roughly 1500+ inches.

    I would like to hear what everyone else gets on these drills as far as life and speeds and feeds.

    Thanks
    Personally I haven't tried those drills, but regular Guhring. Guhring Drills are great. I suggest using moderate Feeds and Speeds to start and if you feel it neccessary bring them up a little at a time. BTW: Use a Spot Drill before drilling. Depending on how flat the Forging is you may end up snapping drills due to deflection even if they are 1/2 inch stubs.
    Last edited by tobyaxis; 08-11-2006 at 06:25 PM.
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    www.refractotech.com


  3. #3
    Registered
    Join Date
    Jul 2006
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0
    Spot drilling isn't an option, it takes too much time. Also we shouldn't need to spot drill with Carbide.


  4. #4
    Registered
    Join Date
    May 2006
    Location
    united states
    Posts
    196
    Downloads
    0
    Uploads
    0
    Depending on the roughness of the forging, like tobyaxis said, could cause enough deflection to break that drill, but I haven't used that particular brand just other carbide and usually it dont like that deflection. I would also start with the lower speeds and feeds to start and work up from there.


  • #5
    Registered
    Join Date
    Feb 2005
    Location
    usa
    Posts
    376
    Downloads
    0
    Uploads
    0
    To me that seems about right on the speed, but even for the best super duper carbide drills, that seems like a lot of feed. The suggested feed is .016 per rev, thats seems like a heck of a lot for a 1/2" drill.

    What kind of failure are you getting? Are you pecking? I wouldn't. If I had to guess, I would say that whatever damage you're getting is at the start of the hole. I don't spot either when drilling with carbide, unless I need a chamfer, but if I'm going to be pushing some high feed in the hole, I will start the hole at a low feed to avoid any deflection, this is probably more important on a forging that is probably not dead flat.


  • #6
    Registered
    Join Date
    Jul 2006
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0
    These are not rough forgings, the have already been turned in a previous operation.

    Also, these are thru holes, im thinking the speed and feed arnet matched correctly and that when the drill exits the material its pushing the material instead of cutting.

    If you look at the photos, they are chipping at the corners and there is a slight buildup in the very tip.
    Attached Thumbnails Attached Thumbnails Guhring Solid Carbide Drills-dscn3210-c.jpg   Guhring Solid Carbide Drills-dscn3201-c.jpg   Guhring Solid Carbide Drills-dscn3204-c.jpg  


  • #7
    Moderator tobyaxis's Avatar
    Join Date
    Jan 2006
    Location
    USA
    Posts
    4,394
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by bma137
    These are not rough forgings, the have already been turned in a previous operation.

    Also, these are thru holes, im thinking the speed and feed arnet matched correctly and that when the drill exits the material its pushing the material instead of cutting.

    If you look at the photos, they are chipping at the corners and there is a slight buildup in the very tip.

    Your speed is too high. That is why the outer edges are wearing like that.
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

    www.refractotech.com


  • #8
    Registered
    Join Date
    Jun 2006
    Location
    Canada
    Posts
    615
    Downloads
    0
    Uploads
    0
    Are you using coolant? If you have thru spindle, you can run it thru the collet, if the drill isn't thru cooled.
    "It's only funny until some one get's hurt, and then it's just hilarious!!" Mike Patton - Faith No More Ricochet


  • #9
    Registered
    Join Date
    Jun 2006
    Location
    Canada
    Posts
    615
    Downloads
    0
    Uploads
    0
    I agree with using a feed about 1/3 that of your drilling feed until the full diameter of the drill is engaged, then let'er RIP!!!!!!!
    "It's only funny until some one get's hurt, and then it's just hilarious!!" Mike Patton - Faith No More Ricochet


  • #10
    Registered
    Join Date
    Jul 2006
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0
    Yes we are running thru coolant.

    Higher speed is what we initially thought as well.

    I just discovered yesterday that when the drill is exiting the hole, the relief in the aluminum jaws holding the parts is only the diameter of the actual drill, so i think that the cap/burr that the drill is pushing out gets caught and its like a intermintant cut for the drill. This would happen on the top and the bottom hole only.

    So we are going to try to mill out the relief to give that cap/burr some room to move.

    Thanks for all the advice everyone.


  • #11
    Registered
    Join Date
    Jun 2006
    Location
    Canada
    Posts
    615
    Downloads
    0
    Uploads
    0
    Make sure the relief is larger in diameter, and slightly deeper than the drill will go, so the slug has room, otherwise it'll be spinning on the end of the drill, and preesing against your jaws.

    Ciao
    "It's only funny until some one get's hurt, and then it's just hilarious!!" Mike Patton - Faith No More Ricochet


  • #12
    Gold Member dertsap's Avatar
    Join Date
    Oct 2005
    Location
    canada
    Posts
    3,874
    Downloads
    0
    Uploads
    0
    i highly doubt the speed is too high ,ive been using a similar drill in 4140 forgings 4700rpm @ 42"/min 1.75 dp

    did you dial up the drill to make sure there is 0. runout


  • Page 1 of 2 12 LastLast

    Posting Permissions


     


    About CNCzone.com

      We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

    Follow us on

    Facebook Dribbble RSS Feed


    Search Engine Friendly URLs by vBSEO ©2011, Crawlability, Inc.