552,801 active members*
2,197 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking > General MetalWork Discussion > DRILL/MILL for center drilling
Page 1 of 2 12
Results 1 to 20 of 27
  1. #1
    Member
    Join Date
    Aug 2020
    Posts
    90

    DRILL/MILL for center drilling

    I have been using the tool at the link below for chamfering. I thought when I purchased it that it would also be good for center drilling. I only have 10 tool slots in my CNC so combining center drill, chamfering tool, and even side milling would be great. Unfortunately I have been breaking the tip off these tools when trying to use them for center drilling in 6061. In hindsight I think I was probably feeding the tool down too fast given the fine tip on it. Sorry, I don't remember the exact plunge rate, it was a while ago. But I need to buy a new one for a job so looking into this again now.

    The tool says it is center cutting, but it also says does not have drill point geometry. So, are these tools meant for plunging or not? If so, what sort of plunge rate would you use for 6061 and low carbon steels?

    https://www.garrtool.com/product-details/?EDP=58214

  2. #2
    Member
    Join Date
    Apr 2004
    Posts
    5522

    Re: DRILL/MILL for center drilling

    If that''s what you want to do, use a tool that does have drill point geometry. The tool you've got can be used for countersinking, but not for center-drilling. Here's a site that discusses drill-point endmills: https://www.harveyperformance.com/in...drill-vs-mill/
    Andrew Werby
    Website

  3. #3
    Member
    Join Date
    Nov 2013
    Posts
    1921

    Re: DRILL/MILL for center drilling

    Hi,

    So, are these tools meant for plunging or not? If so, what sort of plunge rate would you use for 6061 and low carbon steels?
    Centre cutting endmills can plunge, but slowly.....they don't like it.

    For instance if I had a nominal cutting feed rate of 400mm/min in a given material with 50% tool engagement, I would slow that to 200mm/min for a slotting toolpath,
    endmills hate slotting too, and slow to 75mm/min to 100mm/min plunging.

    You might imagine that the angled grind would improve the situation but from your description ......no, they behave very much like regular endmills.

    Craig

  4. #4

    Re: DRILL/MILL for center drilling

    the tips on those garr mill drills are far too fragile to be plunging with them , junk in my opinion
    if only needing a tool for chamfering and spot drilling - I'd ditch the mill drills and just get decent solid carbide spot drills or inset spot drills .

  5. #5
    Member
    Join Date
    Jun 2015
    Posts
    3695

    Re: DRILL/MILL for center drilling

    hy try a local tool guy, that can make such a combi tool
    Attached Thumbnails Attached Thumbnails Untitled.png  
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  6. #6
    Member
    Join Date
    Aug 2020
    Posts
    90

    Re: DRILL/MILL for center drilling

    Thanks everyone for your replies. It has confirmed what I thought that those tools are not suitable for plunging. Oh well, guess I will need to use two tool slots. Does anybody have any recommendations of good chamfering tools? Or are there some 90 degree spot drilling tools that do have drill point geometry, but are designed for chamfering too? I don't really need to use the tool for slotting or side milling.

  7. #7

    Re: DRILL/MILL for center drilling

    a standard spot drill will chamfer , unless your running massive chamfers at which there is a wide variety of insert spot drill/chamfer mills available . As much as I hate garr their spot drills are decent

  8. #8
    Member
    Join Date
    Aug 2020
    Posts
    90

    Re: DRILL/MILL for center drilling

    Another question on this. If I was to use a 90 deg spot drill / chamfer tool.... Is a 90 deg spot drill a good idea?

    I know that generally for carbide drills, you should use a spot drill of higher angle than the drill point so that the drill touches the center of the spot drill hole first. I mainly use HSS drills, and only aluminum or soft steel. Does that spot drill angle thing still apply?

  9. #9
    Member
    Join Date
    Jun 2015
    Posts
    3695

    Re: DRILL/MILL for center drilling

    hy dont worry: for common parts, is enough to point the entrance

    for deep holes/longer drills, you need better aproacch, so to avoid tool buckling

    for same l/d, carbide drils are more rigid than hss, and may even go without a spot drill where a hss requires one / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  10. #10

    Re: DRILL/MILL for center drilling

    90 degree spot drills are the most common used angle in the industry . There are other angles available but 90's work perfectly fine for aligning a drill . 90 degree spot drills have more or less taken over the need for center drills . There are circumstances when a center drill would be the better choice but their use for aluminum and mild steel is almost obsolete

    Keo makes nice hss spot drills which may be worth looking at . They are much cheaper than carbide and they can spot and chamfer a lot of mild steel before they wear out . They along with the garr have finer tips than some other companies , which makes them good for engraving serial numbers etc , usually .005" depth is good for reasonably sized number or letters . It basically gives you three tools in 1 , and more with a bit of imagination

  11. #11
    Registered
    Join Date
    May 2017
    Posts
    26

    Re: DRILL/MILL for center drilling

    Hi Ashes-man!

    Here is what I have found on Drill Points: A High Performance Solid Carbide Drill generally has a 140 Degree Point so it is ideal to match the 140 Degree Point for your spot drill (or a 120 Degree Point will work). When you Spot with a 90 degree point and then Drill with a a 140 degree point what happens is the Drill hits the material in the middle of the drill point instead of at the tip of the drill point and all Drills are designed to start forming the chip off the tip of the drill point. This will cause it to chatter, drill in-accurately or break especially in difficult to machine materials (you can get away with it in softer materials).

    I know you said you only have 10 tool stations so you may not be able to but it is best to match up the spot drill point to the drill point if possible to get a better quality hole and longer drill life. Also, if your 140 degree point drill is 3XD or 5XD then there is no need to spot, they will locate extremely well and hold up better at 5XD and under without a need to spot (vs using a 90 degree spot). If it is 8XD or longer then you definitely need a spot.

    I hope this helps! There are really good indexable spot drills out there that can Drill/Chamfer/Side Mill and that would be a good way to go for a universal tool. If you would like some recommended let me know.

    -Mike
    www.toolhit.com

  12. #12
    Member
    Join Date
    Aug 2020
    Posts
    90

    Re: DRILL/MILL for center drilling

    Quote Originally Posted by ToolHIT View Post
    Hi Ashes-man!

    Here is what I have found on Drill Points: A High Performance Solid Carbide Drill generally has a 140 Degree Point so it is ideal to match the 140 Degree Point for your spot drill (or a 120 Degree Point will work). When you Spot with a 90 degree point and then Drill with a a 140 degree point what happens is the Drill hits the material in the middle of the drill point instead of at the tip of the drill point and all Drills are designed to start forming the chip off the tip of the drill point. This will cause it to chatter, drill in-accurately or break especially in difficult to machine materials (you can get away with it in softer materials).

    I know you said you only have 10 tool stations so you may not be able to but it is best to match up the spot drill point to the drill point if possible to get a better quality hole and longer drill life. Also, if your 140 degree point drill is 3XD or 5XD then there is no need to spot, they will locate extremely well and hold up better at 5XD and under without a need to spot (vs using a 90 degree spot). If it is 8XD or longer then you definitely need a spot.

    I hope this helps! There are really good indexable spot drills out there that can Drill/Chamfer/Side Mill and that would be a good way to go for a universal tool. If you would like some recommended let me know.

    -Mike
    Yup, definitely keen to know. My machine is very small. It is a Mazak, but has similar cutting capacity to a Tormach 1100. I had assumed indexable tools for things like spotting would be large. I make mostly smaller parts, drilling below 10mm etc.

  13. #13
    Registered
    Join Date
    May 2017
    Posts
    26

    Re: DRILL/MILL for center drilling

    I see, at the smaller diameter a Drill Mill or Chamfer Mill is a great way to go. Their drill points are not the strongest but if you keep your feed rate low when plunging you should be able to make them work. I would be at around .0008" IPR (.02 mm/rev) when plunging.

    The best indexable Spot/Chamfer Drills that I have seen is from Korloy. They start at 1/2" or 12mm but they do come to a point so you can use them on smaller parts. here is what they look like:
    https://www.toolhit.com/products/cea45-1600r-s050
    https://www.toolhit.com/products/twx16r-kcpc5300

    You could also go with a 2 Flute Drill Mill instead of a 4 Flute Drill Mill to make sure there is enough clearance for chips to evacuate when plunging. But the Drill Mill should work well at the low feed rate.
    www.toolhit.com

  14. #14

    Re: DRILL/MILL for center drilling

    a decent high performance carbide drill doesn't require spotting nor is it recommended

    true that the drill tip doesn't start at the tip when using a 90 degree but this is brief and I've never seen this to cause a drill to wander even on deep holes , or break . Unlike carbide , hss drills are capable handling the cut . Otherwise the same thing could be said for using a center drill
    If you walk through any production shop you will see that 90 degree spot drills are the most common cutters in machines these days . I've spent many years in a variety of production and jobbing shops and never seen the use or need for a different angled spot drill . It's tried tested and true and doesn't need to be over thought

  15. #15
    Member
    Join Date
    Aug 2020
    Posts
    90

    Re: DRILL/MILL for center drilling

    Quote Originally Posted by ToolHIT View Post
    I see, at the smaller diameter a Drill Mill or Chamfer Mill is a great way to go. Their drill points are not the strongest but if you keep your feed rate low when plunging you should be able to make them work. I would be at around .0008" IPR (.02 mm/rev) when plunging.

    The best indexable Spot/Chamfer Drills that I have seen is from Korloy. They start at 1/2" or 12mm but they do come to a point so you can use them on smaller parts. here is what they look like:
    https://www.toolhit.com/products/cea45-1600r-s050
    https://www.toolhit.com/products/twx16r-kcpc5300

    You could also go with a 2 Flute Drill Mill instead of a 4 Flute Drill Mill to make sure there is enough clearance for chips to evacuate when plunging. But the Drill Mill should work well at the low feed rate.
    Cool, thanks for the advice. I hadn't seen your website, I will check it out...

  16. #16
    Member
    Join Date
    Aug 2020
    Posts
    90

    Re: DRILL/MILL for center drilling

    Quote Originally Posted by metalmayhem View Post
    a decent high performance carbide drill doesn't require spotting nor is it recommended

    true that the drill tip doesn't start at the tip when using a 90 degree but this is brief and I've never seen this to cause a drill to wander even on deep holes , or break . Unlike carbide , hss drills are capable handling the cut . Otherwise the same thing could be said for using a center drill
    If you walk through any production shop you will see that 90 degree spot drills are the most common cutters in machines these days . I've spent many years in a variety of production and jobbing shops and never seen the use or need for a different angled spot drill . It's tried tested and true and doesn't need to be over thought
    I hear you. It was more a point of interest. I want only a 90 deg tool so it can be multi use.

  17. #17
    Member
    Join Date
    Aug 2020
    Posts
    90

    Re: DRILL/MILL for center drilling

    My feeling so far is that the best solution for me is to use two tools, one for chamfering and another for spot drilling/countersinking.

    A four flute carbide drill mill or chamfer tool for fast cutting and good surface finish, I will probably stick with the Garr tool from my original post. It is available and works really well (if you don't plunge it!). Chamfering is only a small cut so I don't think chip evacuation with four flutes will be a problem.

    And a 90 deg carbide insert spot drill or two flute spot drill.

    I was hoping to get away with only one tool in the changer, but given my lack of skills and tendency to try push things, having two tools that are strong for each job is a safer option!

  18. #18
    Registered
    Join Date
    May 2017
    Posts
    26

    Re: DRILL/MILL for center drilling

    Quote Originally Posted by metalmayhem View Post
    a decent high performance carbide drill doesn't require spotting nor is it recommended

    true that the drill tip doesn't start at the tip when using a 90 degree but this is brief and I've never seen this to cause a drill to wander even on deep holes , or break . Unlike carbide , hss drills are capable handling the cut . Otherwise the same thing could be said for using a center drill
    If you walk through any production shop you will see that 90 degree spot drills are the most common cutters in machines these days . I've spent many years in a variety of production and jobbing shops and never seen the use or need for a different angled spot drill . It's tried tested and true and doesn't need to be over thought
    You are correct on all of this metalmayhem! This is awesome advice!
    www.toolhit.com

  19. #19
    Registered
    Join Date
    May 2017
    Posts
    26

    Re: DRILL/MILL for center drilling

    Quote Originally Posted by ashes-man View Post
    My feeling so far is that the best solution for me is to use two tools, one for chamfering and another for spot drilling/countersinking.

    A four flute carbide drill mill or chamfer tool for fast cutting and good surface finish, I will probably stick with the Garr tool from my original post. It is available and works really well (if you don't plunge it!). Chamfering is only a small cut so I don't think chip evacuation with four flutes will be a problem.

    And a 90 deg carbide insert spot drill or two flute spot drill.

    I was hoping to get away with only one tool in the changer, but given my lack of skills and tendency to try push things, having two tools that are strong for each job is a safer option!
    That does make the most sense. It's funny with multi-function tooling like a drill mill, it won't drill as well as a spot drill and it won't chamfer as well as a chamfer mill but they are nice to have if you are lacking tool stations. If you can use separate tools they will hold up longer and cut better!
    www.toolhit.com

  20. #20

    Re: DRILL/MILL for center drilling

    one possibility is to helical interpolate your spots with your mill/drill rather than plunge , a .01" radius should do . It requires a bit more coding and your still at the mercy of that fine tip but who knows it may work well with that tool .

    Another option would be to find a better quality mill drill . The last company I worked for used mostly garr until after a few weeks in I brought them a few test tools to show them what they were missing out on . The grinds and quality of garr's carbide is questionable , to put it politely .

Page 1 of 2 12

Similar Threads

  1. Replies: 10
    Last Post: 08-19-2012, 09:57 PM
  2. Spot Drilling/Center Drilling Steel 55 HRC
    By JWB_Machining in forum General MetalWork Discussion
    Replies: 7
    Last Post: 03-11-2009, 07:35 PM
  3. center drill diameter developpement on mazak nexus 640m mill
    By Denis13 in forum Mazak, Mitsubishi, Mazatrol
    Replies: 0
    Last Post: 01-31-2008, 03:56 AM

Tags for this Thread

Posting Permissions

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