525,474 active members*
2,688 visitors online*
Register for free
Login
Results 1 to 13 of 13
  1. #1
    Member
    Join Date
    Nov 2013
    Posts
    375

    Countersinking tips and tricks?

    Do you guys have any tips or tricks (Feeds & Speeds) for countersinking?
    It seems like almost every time I countersink, my 770 chatters and vibrates like mad.
    Mostly with 82 Degree countersinks.

    I've tried using single flute HSS, 3 flutes, 4 flutes, 6 flutes, and even my single flute indexable carbide
    Also peck drilling, helical interpolating, plunging to depth then light circle milling....
    High RPM's with the indexable carbide, low rpm's with the HSS.
    The lower rpm's worked alot better, but going too slow causes stalling.

    Can't seem to defeat the chatter and vibration monster.

    Let's hear your expert advise.

  2. #2
    Junior Member
    Join Date
    Apr 2013
    Posts
    1549

    Re: Countersinking tips and tricks?

    What size screws are you using?

    I am definitely not an expert! What works for me is to use a small, 4 flute, carbide chamfer bit with either a 82 or 90 degree angle (imperial or metric screws). I use a helical toolpath that is offset from the edge of the bore towards its centre. Perhaps I'm overly cautious but chatter has never been an issue and it only takes a second per hole..

  3. #3
    Member
    Join Date
    Jun 2015
    Posts
    3143

    Re: Countersinking tips and tricks?

    hy russ give a try to integral carbide tools ( attached )

    hss are ok, they work, but ...

    indexable carbide ? yup, but only if you need to use a large diameter tool

    i use integral types: o4z4 o6z4 o10z6 ... 4000-6000rpm, 0.03 - 0.05mm/z, coolant, helical interpolation; integral tools have better tir, and lower diameter tools have a bigger chance to deliver a smoother surface / kindly

    ps : for longer toollife spam, try to spread coolant all over their circumference; they are pretty fast, and if there is coolant lag, you may burn them if in doubts, get a non-coated version ... cheaper, but should serve you well

    ps2 : if the countersink is deep/big, you may consider to use 2 such tools, one for roughing, and another for finishing
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  4. #4
    Member
    Join Date
    Aug 2009
    Posts
    560

    Re: Countersinking tips and tricks?

    I copied this from website
    https://cnctips.wordpress.com/2010/0...rstanding-g82/

    Calculating Dwell Time

    The P parameter in the G82 command is time in milliseconds so P1000 = 1 second, P500 = 1/2 second and so on. To calculate the correct amount of dwell time use this formula:
    P = Dwell Time
    DR= Desired revolutions of tool at bottom of hole
    RPM = Revolutions per minute of tool

    P = DR / (RPM/60) * 1000

    For Example: You want your tool to dwell for 2 revolutions. With spindle speed is 500 RPM you would program P240 as shown below:

    P = 2 / (500 / 60) * 1000
    P = 2 / (8.3333) *1000
    P = .24000 * 1000
    P = 240

    REMEMBER: Only dwell the tool for the minimum amount of time necessary to insure a good clean counter bore face. Dwelling too long will only dull your tool and possibly work harden the piece. Not to mention that long dwell times increase production times.

  5. #5
    Registered
    Join Date
    Dec 2008
    Posts
    651

    Re: Countersinking tips and tricks?

    I'm with kstrauss. For me a countersink just a circular chamfer. I use 4 flute 90° drill mills and include them at the same time as the other chamfers thereby avoiding an additional tool change (not that it really matters for what I do). I've never liked countersinking by plunging because the 360° contact makes the tools very difficult to control as you've found. I wouldn't expect any issues with a circular path if the contact angle isn't excessive and you use a tool designed for "milling" as opposed to countersinking.
    Step

  6. #6
    Registered
    Join Date
    Nov 2007
    Posts
    1881

    Re: Countersinking tips and tricks?

    Quote Originally Posted by TurboStep View Post
    I'm with kstrauss. For me a countersink just a circular chamfer. I use 4 flute 90° drill mills and include them at the same time as the other chamfers thereby avoiding an additional tool change (not that it really matters for what I do). I've never liked countersinking by plunging because the 360° contact makes the tools very difficult to control as you've found. I wouldn't expect any issues with a circular path if the contact angle isn't excessive and you use a tool designed for "milling" as opposed to countersinking.
    Step
    I was wondering what the problem was. I always used a chamfer operation as mentioned here with more then one pass if required. I do get away with using the chamfer left after spot drilling. But I use a small spot drill. I also found using chamfer operation was the easy way to control the exact results using cam tool paths. And found it less repeatable using a contact point on tool with a centered z plunge in cam anyway. But you end up with lots of machine movements that are not fast for production work. As step mentions many parts are finished with a chamfer op so hitting the holes works well.

    edit I do use very exact cam models for tool path generation. I have always wondered how others handle this in cam setup because of the many ways to do it.

  7. #7
    Registered
    Join Date
    Apr 2015
    Posts
    2

    Re: Countersinking tips and tricks?

    Stefan Gotteswinter

    Stefan Gotteswinter recommended these countersinks on his YouTube channel. I’ve found that they are very good at making smooth chatter free countersinks.


    https://www.guhring.com/ProductsServ...ls?Series=5538

  8. #8
    Member
    Join Date
    Jun 2015
    Posts
    3143

    Re: Countersinking tips and tricks?

    hello again after reading other replies in this thread, i started to think of this ... you may cut the chamfer :
    ... before driling, making also the spot for the drill ( attached is the classical hss spot drill )
    ... during drilling, using some chamfer adapters or a combitool
    ... after drilling :
    ...... by machinining, thus by changing the drill with a chamfer tool of you choice
    ...... by hand, by using a specific tool, which may vary in size from small ( like a pen ) to big ( like 400mm long, designed to be used with both hands, for chamfering big holes )

    i have used all those ... i guess choice depends on real scenario / kindly

    ps: in some conditions is possible to drill without using a spot drill
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  9. #9
    Junior Member
    Join Date
    Apr 2013
    Posts
    1549

    Re: Countersinking tips and tricks?

    The tool pictured is normally called a "centre drill" rather than a "spot drill" and may not be the best choice for spotting. Also, it cannot be used for countersinking since the relevant portion of a centre drill has a 60-degree angle rather than the required 82 or 90 degree (imperial or metric screws) angle for countersinking.

  10. #10
    Member
    Join Date
    Jun 2015
    Posts
    3143

    Re: Countersinking tips and tricks?

    hy kstrauss, you are right, that's a center drill ... my english, my bad

    yes, it is indeed 60*, but it works well for those parts where is only required to have a "chamfer" instead of a sharp corner

    even if 60* is the most common shape, there are also center drills with different angles, or with 2 tapers

    sometimes, if a thread is required, a 60* will be less agressive and allow the tap to guide smoother into the hole, compared to a 90* / kindly

    ps : is it always raining ?
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  11. #11
    Junior Member
    Join Date
    Apr 2013
    Posts
    1549

    Re: Countersinking tips and tricks?

    Deadlykitten your English is fine!

    Rather than a small angle it is often recommended that the spot drill have an angle greater than the usual 118-degree drill point to ensure precise starting of the drill. For example, Guhring (a manufacturer of outstanding quality drills) offers spot drills with a 142-degree angle. See https://www.guhring.com/ProductsServ...omResults=True for some details of their products.

  12. #12
    Member
    Join Date
    Jun 2015
    Posts
    3143

    Re: Countersinking tips and tricks?

    hello , yup, they have to have a greater angle, in order to assure that the following drill will start cutting from it's center towards the exterior

    another condition is that the pilot diameter has to be greater then the following drill, in order to assure that his flutes will avoid contact with the walls when going inside the previous hole

    drills are generally listed inside catalogue as h7; in that link that you shared, pilots are h6 ... it is ' some kind of saying ' that the pilot will deliver a bigger hole / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  13. #13

    Re: Countersinking tips and tricks?

    severance makes the best anti chatter countersinks in the market

Similar Threads

  1. Enroute 5. Tips and Tricks
    By JeepDewd in forum EnRoute
    Replies: 0
    Last Post: 05-03-2018, 11:46 AM
  2. Tips and Tricks
    By cs49230 in forum Momus Design CNC plans
    Replies: 9
    Last Post: 03-04-2013, 07:06 PM
  3. tips and tricks in powermill
    By wizard200097 in forum PowerMILL
    Replies: 0
    Last Post: 11-20-2011, 08:29 PM
  4. Tips and Tricks
    By Smitty911 in forum Dolphin CAD/CAM
    Replies: 9
    Last Post: 03-03-2008, 06:59 PM

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
  •