584,861 active members*
4,867 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Haas Machines > Haas Mills > Production drilling on a haas
Results 1 to 19 of 19
  1. #1
    Join Date
    Jan 2007
    Posts
    1389

    Production drilling on a haas

    I have a job that requires 50 holes per part. finish isnt a big deal cause we have to mill .020 out after the drilling. the depth is about .750 deep in alum 6061.
    hole ranges are 3/8 7/16 and 1/2

    we are running the 1/2" drill at 23.5 inchs per min on a peck cycle to break the chip better at 4500 rpm. which isnt bad except I have over 1000 parts to do with other features on the part. the drill time takes the longest along with spot driling.

    What drill breaks chips best with NO Peck drilling and one that will last a while. I was looking at the gurhing(sp) line as we always had good luck with them on incos and stainless, but never tried them on Alum.
    We are using precision twist drills cobalt 135º split point stubbies.
    any other suggestions for Quality drills.
    Delw

  2. #2
    Join Date
    Jul 2005
    Posts
    12177
    Just a thought. On the 7/16 and 1/2 at least use an uncoated carbide drill running very fast no spotting, no pecking and flooded with coolant.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  3. #3
    Join Date
    Apr 2005
    Posts
    713
    With the same drills as you are using except with a #31, I drilled several hundred holes in 6061 at 7960 RPM and 64 IPM, no peck, flood coolant, .250" deep. That's the same or more L/D ratio than what you're doing, and I'm positive it could have handled much more.

    It boils down to experimenting. Triple your feed and no peck and see what happens. Worst case is you break a cheap drill.

    Other than that, what Geof said about solid carbide is a good place to look too. No spot, no peck and a whole lot of feed/speed. If you have through spindle coolant, that's a whole other world.

  4. #4
    Join Date
    Jan 2007
    Posts
    1389
    Never even thought about carbide cause I had pecking on my mind. Not a bad idea.
    plus eliminating the spot drill will save a ton of time in the long run. thanks Geoff.

    Matt tried the experimenting this am, with a 3/8 stub drill(same make and style) and I was way better off peck drilling .200 instead of straight feeding.
    I was at 6500 rpms and 35.0ipm and going straight in was really pushing the drill (pressure wise as I could hear it) with pecks it wasnt too bad.
    On the bright side its a repeat job so I got some time to play with. I will give another try on monday. if I could get it down I will run it on my fadals that way I wont tie up my haas for proto type pcs for the next month.

    Thanks Guys
    Delw

  5. #5
    Join Date
    Apr 2005
    Posts
    713
    Something doesn't seem right here. As a rule for low volume stuff, I feed my HSS drills at 25 IPM at 250 SFM. So for your 3/8" drill that would be 2545 RPM. To maintain my standard every day chip load at your RPM, I would be feeding at 65 IPM. Again, I want to make it clear that that's the chip load I use every day in 6061 on parts that cycle time means next to nothing. Why you can't get close to that is bothersome. I wonder if you tried going back to around 300 SFM if you couldn't feed it harder. Something isn't adding up there.

    Or, just go with carbide and be done with it.

  6. #6
    Join Date
    Apr 2005
    Posts
    713
    One more thing Del. You may know this, but make sure your exact stop setting is turned on so you can cut your retracts hole-to-hole really close without any gouging.

  7. #7
    Join Date
    Jul 2005
    Posts
    12177
    I know this is something of a hijack so I beg forgiveness.

    Exact stop slows things down slightly simply because the machine has to stop one axis before starting the other. Is it really quicker to have really close retracts and exact stop than having a bit more space and no exact stop?
    An open mind is a virtue...so long as all the common sense has not leaked out.

  8. #8
    Join Date
    Jan 2007
    Posts
    1389
    Quote Originally Posted by Matt@RFR View Post
    Something doesn't seem right here. As a rule for low volume stuff, I feed my HSS drills at 25 IPM at 250 SFM. So for your 3/8" drill that would be 2545 RPM. To maintain my standard every day chip load at your RPM, I would be feeding at 65 IPM. Again, I want to make it clear that that's the chip load I use every day in 6061 on parts that cycle time means next to nothing. Why you can't get close to that is bothersome. I wonder if you tried going back to around 300 SFM if you couldn't feed it harder. Something isn't adding up there.

    Or, just go with carbide and be done with it.
    Matt doesnt make much sence to me either, However I didnt run the speeds and feeds via any book I adjusted to max via sound.
    Its funny cause the 1/2" cut far better and smoother.
    the only thing I can think of is the drill being smaller doesnt have good web relief? for the chips to bug out. was going to try a different type of drill not a 135º split point.
    I have noticed that when I run smaller drills I can get no way near what others are getting. but I am thinking because of the .135º split point.
    Kinda like what you posted about your #31 drill I am like WTF I cant get any where close to that and would love too on drills that size. we do lots of 1/16 holes in parts. but again I am using screw machine drills( the 135º split point stubs always work best for me on the lathes and omniturns) and it might make a difference in changing to a different drill geometry for small holes in a mill.

    Quote Originally Posted by Matt@RFR View Post
    One more thing Del. You may know this, but make sure your exact stop setting is turned on so you can cut your retracts hole-to-hole really close without any gouging.
    what geoff said below. on alot of holes it makes quite a bit of difference. I Have tried it in the past.(not on this job)
    right now I am holding .050 off Z0.0 also I saved a few mins per part by adjusting the peck length to be an equal number instead of just hitting .020 on its last peck. saved one peck cycle on 50 holes adds up.
    for the heck of it when I get it running like I want(as fast as machine possible) I might try to get a time using your suggestion and see if we can prove geoff wrong for once LOL

    Quote Originally Posted by Geof View Post
    I know this is something of a hijack so I beg forgiveness.

    Exact stop slows things down slightly simply because the machine has to stop one axis before starting the other. Is it really quicker to have really close retracts and exact stop than having a bit more space and no exact stop?

    Thanks again guys

    Delw

  9. #9
    Join Date
    Jul 2005
    Posts
    12177
    One thing I know does save time when you're using the G83 peck cycle is to program I, J, and K especially on deep holes. Make I something like 1-1/2D, J 3/4D and K 1/4D
    An open mind is a virtue...so long as all the common sense has not leaked out.

  10. #10
    Join Date
    Apr 2005
    Posts
    713
    Quote Originally Posted by Geof View Post
    I know this is something of a hijack so I beg forgiveness.

    Exact stop slows things down slightly simply because the machine has to stop one axis before starting the other. Is it really quicker to have really close retracts and exact stop than having a bit more space and no exact stop?
    I never did back to back testing, but my feeling is that exact stop is faster on my machine. It's a VF-2ss so it's got the fast pitch ball screws, and I bet that has something to do with it.

  11. #11
    Join Date
    Apr 2005
    Posts
    713
    Del, I just looked at that #31 drill I used, and it's a PTD cobalt 135º NON split point screw length. I would think a split point would be better with easier penetration, but I'm no expert there.

    Is the material you're working with domestic? I got my hands on some Chinese material one time and I couldn't use ANY of my standard feeds on that crap.

  12. #12
    Join Date
    Jan 2007
    Posts
    1389
    Matt My machine is a vf2ss as well a 2009
    I got sme drills coming in in the next few days some different ones. also a carbide tipped one I am going to try.
    I like the 135º splitpoints the best however I have noticed that on some material a standard junk drill works better in a mill. usually plastic.
    Material is domestic.
    Thanks again I'll let ya know how it pans out next week or sooner.

    Delw

  13. #13
    Join Date
    Jan 2007
    Posts
    1389
    The drills I got coming in are garr alum star 3 fluters solid carbide.
    1180 series

    Delw

  14. #14
    Join Date
    Apr 2005
    Posts
    713
    Quote Originally Posted by Delw View Post
    The drills I got coming in are garr alum star 3 fluters solid carbide.
    1180 series
    My tooling supplier has been wanting me to try some 3 flute drills. I'm curious to know how they did for you when you get them running.

  15. #15
    Join Date
    Jan 2007
    Posts
    243
    Quote Originally Posted by Geof View Post
    One thing I know does save time when you're using the G83 peck cycle is to program I, J, and K especially on deep holes. Make I something like 1-1/2D, J 3/4D and K 1/4D
    or you can try this drilling calculator: http://www.webmachinist.net/drillpeckcalculator.html
    www.WebMachinist.Net
    The Ultimate Online Source for Machinist Related Stuff!

  16. #16
    Join Date
    Jan 2007
    Posts
    1389
    Quote Originally Posted by Matt@RFR View Post
    My tooling supplier has been wanting me to try some 3 flute drills. I'm curious to know how they did for you when you get them running.
    Matt we used them back in the mid 90's when they just started getting popular. used them for 303 stainless in the omniturns and 9310 gear steel in the big lathes. they worked pretty good. We used them mainly because no need for spot drilling, they were expensive back then. However they were fantastic for finish and long deep holes on gear steel.
    I have never tried them in a mill. will let you know when I get them. the feeds and speeds dont look all that great however its double of what I am doing now. so it will definately help even if it saves me 2-5 mins per part. I am guessing its going to save me about 30% plus getting rid of the spot drilling on the smaller drills.
    I dumped the spot drilling off on the 1/2" hole heck I was running a stubby anyhow, that saved some time and I didnt notice any walk.

    Delw

  17. #17
    Join Date
    Jan 2007
    Posts
    1389
    Matt
    the alumastar 3 fluters are one of the best drills I have ever used.
    were drilling the 3/8 holes now. went with the low limit for starters and going to let that run that way for a while till I get some back up drills.
    right now we are getting 4583 rpm and 61.87 IPM part drilling part went from 8 mins too 1:53 second for 100 holes, plus no c-drilling
    price wasnt that bad something around 112 for the 3/8 drill Garr reccomends starting at 450SFM and .0045 per tooth(for the 3/8) and .0055 (for the 1/2) he said we should be able to bump it up quite a bit.

    You cannot hear the drill drilling, the only thing you hear is chips popping off., have absoluetly no chip build ups. we are using flood coolant.

    Thought I would let ya know.
    Delw

  18. #18
    Join Date
    Apr 2005
    Posts
    713
    That's moving right along Del, thanks for the feedback. Now the question is how fast can it really go, and how long will it last. I'll have to give those a try next time I have a need for it.

  19. #19
    Join Date
    Jan 2007
    Posts
    1389
    Matt if they last half as long as my alumastar endmills I would be happy.
    I am getting 6-8 months on the 3/8 endmill and 1/2" endmills using them every day for alum and lots of cutting and hogging . 12000rpms and anywhere from 50IPM to 150IPM the one in my fadal is going on almost a year its a 3/8 endmill and squares up sawed ends about .250-300 wide 1/2 deep 8500rpms and 90ipm

    Size still hold .001 plus or minus finish is 63 or better
    Delw

Similar Threads

  1. Haas VF2, good for production?
    By ashishw in forum Haas Mills
    Replies: 12
    Last Post: 05-20-2020, 10:07 PM
  2. Replies: 1
    Last Post: 03-25-2013, 09:07 PM
  3. production drilling without thru spindle coolant
    By poster in forum MetalWork Discussion
    Replies: 9
    Last Post: 04-27-2012, 04:09 AM
  4. Troublrs drilling on center in Haas SL20
    By rickkiefe in forum Haas Mills
    Replies: 3
    Last Post: 10-27-2009, 08:15 PM
  5. HAAS for production?
    By jeff.kindred in forum Haas Mills
    Replies: 12
    Last Post: 06-20-2008, 03:54 PM

Posting Permissions

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