[RussMachine]

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.

[kstrauss]

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..

[TurboStep]

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

[mountaindew]

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.

[mdpcnc]

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

[deadlykitten]

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

[deadlykitten]

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

[machinehop5]

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.

[metalmayhem]

severance makes the best anti chatter countersinks in the market