[jprobst]

any6 suggestions on a good countersinking bit to counter a 5/16" flat head in 304 stainless?

[rbest27]

82 deg carbide c'sink will work fine if you don't have one high speed will work also

[DSL PWR]

Just remember to use a high feed and DO NOT PECK!!!

[jprobst]

Don't peck? thats what i've been doing with a hss countersink and one last for about 60 holes and the other lasted one hole, i'm trying to find a bit in a catalogue that will last the remainder of the job, my boss is already flipping on the two bits, so i shouldn't peck? right now i have it going .3 deep at .020 pecks at 420 rpm, this wrong?

[jprobst]

i also have it going 1 i.p.m

[Newby2]

seems your speed is a bit to fast for stainless. try 150- 200 RPM and as others have said, high feed, no pecking
Steve

[gizmo_454]

150 to 200 rpm? That sounds a bit on the slow side. We run jobs on our 1940's screw machines drilling holes bigger than that in 304 at 500+ RPM. I would think that your 420 is all right if the outside diameter of the c-sink is 5/16. If it's for a 5/16 flat head cap screw, it may be too fast. The peck sounds like the main problem. 300 series stainless work hardens, so unless you continually remove material, you will work harden it. So the next time the tool comes into contact, it will either break, or cause it to wear prematurely.

When it comes to stainless, it seems people will more than likely under-do something in fear of breaking something. Unfortunately, it causes more harm than good. Obviously, you don't want to go the other way either. Stainless is somewhat picky that way, don't you think?

Good luck!:cheers:

[Newby2]

Gizmo is correct about 300 series stainless being a RPITA. But it is interesting to note that 303 machines much better than 304.
Also, as with any machineing job, the tools that are used can make the difference between a profit and a loss. I did on job where the boss handed me a box of tools to make the parts with. The result was a 66% scrap rate. I talked him into a carbide bullet drill and the scrap rate dropped to less than 3%.
There are times when, in this day and age of advanced machining methods, some of the bosses just don't want to grow up and listen to those that make them the money!
Steve

[joecnc1234]

If you're having that much of a problem rough c-sink than finish the depth with another tool. The feeds and speeds don't seem that far off other than the fact you are probably burning the tool up at 1 ipm.
Joe

[PBMW]

I have a job where I make 15k parts a month. They have two countersunk .411 holes. 82 deg. this is in 304.
I got tired of buying carbide countersinks. I now drill and interpolate the minor hole dia. (It's close tol) then I interpolate the ocuntersink with a carbide countersink. I stopped plunging them as the chips would turn into a rats nest where the operator needed to stop the machine to clear the chips ftom the cutter. I'm doing 40 pcs at a time. I tried pecking and that worked pretty well. I was getting about 500 holes out of a countersink. I was running 200sfm and .006 per rev to plunge. I started interpolating the countersinks and the cycle time went down a bunch over pecking and the tool life went to over 6k holes.
Worked for me.

[jprobst]

this might be a dumb question, but what does interpolate mean and how do i do it?

[joecnc1234]

lol

[jprobst]

lol

hey thanks for the support man

[rbest27]

what type of tool are you using first of all. High speed or carbide? I've got c'sink's that I've had in my tool box for years. If it's a high speed c'sink try 50 surface feet calculated at the max diameter of the c'sink. My best results have always been just plunging it right in...no pecking. I wouldn't run too slow...you want a nice chip coming off the tool that way there you don't get a rat's nest. Carbide you can run a bit faster...chip load on either one I would estimate at about .005 per rev.

As for the boss freaking out, that's what they do. Sounds like your shop has limited experience with stainless so you'll have some growing pains. Countersinks don't cost that much that he should be freaking out.

[AMW]

Hmmmm how can i put this??????

ok,ok: program a circle= interpolate= go from one pole to the other pole=make a circle


I think

LOL me too

[jprobst]

well the customer came by yesterday and needed his parts this morning, so after hours i broke my last muliflute countersink, thought i was dead in the water, then i found a single flute hss 3/4" countersink i ran it at 250 rpm with a plunge rate of .5 and it ran very well, got the job done, billed customer double for the rush and didn't break anymore bits, so thank you all for your help, as fas as interpolate question, i'm fairly new at this vmc stuff so i'm gonna ask any question i can, no matter how stupid the question is, not only am i the only programmer in the shop, i run the shop to and don't have the time i need to sit down and learn about this stuff, so i learn as i go and ask what some might feel as a stupid question.

[PBMW]

Jprobst
To interpolate is to consider the hole as a profile and drive the tool around the ID to generate the angled countersink.

[jprobst]

thank you

[dertsap]

with using interpolation you should be able to accomplish a consistantly clean surface finish , i would cut it in two passes or
you could helix in so you can save from any air cutting and prevent any lead in and lead out marks