Drilling Stainless

[cncClintain]

Started a new job today and the bossman showed me a brand new OSG (cobalt I believe) drill that hadn't made it through one part. It was leaving a poor finish and actually wallered out the top of the whole so badly that it scrapped the part. I looked on OSG's website and found little help. I figure the speeds and feeds should be round 60 SFM and .006 to .010 IPR which is about what they were running it at. It is not a Through Tool coolant drill so Im assuming pecking is needed. OSG said it could just be a bad drill but I still wonder. Any advice for drilling and tapping 316 stainless would be appreciated.

[emonje]

I'd try to avoid pecking & drill through in one go as Austenitic stainless steels tend to work harden

[metlshpr]

Use carbide and go fast.

[ObrienDave]

What diameter drill and how deep?

[cncClintain]

Originally Posted by ObrienDave What diameter drill and how deep?

Rarely over a half inch diameter and a couple inches deep, anything bigger and we use inserted drills. Tapping advice would be nice too, that's what the drilling is for.

[knsmilk88]

might want to try a Precision Twist Drill.
IMO, PTD drills have the best grind on them.
Just play with the speeds and feeds.

[littlebrewman]

i have drilled and tapped in 316 stainless with no problems as this is my expertise using titex drills and osg spiral flute taps what size are you tapping and how deep?Is it a blind hole or a through hole? roll tapping or cut tap?when i have this info i can tell u what to use to get the best results.Are you doing this in a mill(vertical or horizontal) or lathe as this can make a difference due to forces involved.

[cncClintain]

Originally Posted by littlebrewman i have drilled and tapped in 316 stainless with no problems as this is my expertise using titex drills and osg spiral flute taps what size are you tapping and how deep?Is it a blind hole or a through hole? roll tapping or cut tap?when i have this info i can tell u what to use to get the best results.Are you doing this in a mill(vertical or horizontal) or lathe as this can make a difference due to forces involved.

Mazak vertical mills. So far Ive seen anything from a 4-40 up to about a 1/2-13. They were using cut taps but I think theyve been using form taps lately. Our most substantial customer is very picky about thread depth and minor diameter so the drilling process needs to be pretty precise. They even want the tap drill to be within a few thousandths usually. I have zero experience with form taps but they seem to be the best route from what Ive seen but this is only my first week on the job.

[littlebrewman]

well to tell you all drilling should be precise.all drills should be indicated in and have little to no runout so a proper holder and tool length as short as possible is a must.when making threads the minor diameter should always be within specified tolerances.for instance a 4-40 thread should have a minor diameter of .0849 to .0939. to use a form tap you should be using #39 drill to achieve 75% thread which is standard for most threads.A high pressure tapping fluid such as moly dee should be used to tap the hole with. as far as speed 22sfm is a good place to start. i usually do all my tapping rigid as opposed to using a floating holder to prevent driftting before it reverses.I hope this is of some help since your question is very vague as far as what size u are looking for.Icant list all of what i use up to .5 inch taps.I would use a titex cobalt drill with a 135/140 degree angle.as far as a tap goes i would use an osg for cut tapping but prefer balax for a form tap.For 1/2 inch threads i generally use thread milling for this so as not to break taps.

[cncClintain]

Originally Posted by littlebrewman well to tell you all drilling should be precise.all drills should be indicated in and have little to no runout so a proper holder and tool length as short as possible is a must.when making threads the minor diameter should always be within specified tolerances.for instance a 4-40 thread should have a minor diameter of .0849 to .0939. to use a form tap you should be using #39 drill to achieve 75% thread which is standard for most threads.A high pressure tapping fluid such as moly dee should be used to tap the hole with. as far as speed 22sfm is a good place to start. i usually do all my tapping rigid as opposed to using a floating holder to prevent driftting before it reverses.I hope this is of some help since your question is very vague as far as what size u are looking for.Icant list all of what i use up to .5 inch taps.I would use a titex cobalt drill with a 135/140 degree angle.as far as a tap goes i would use an osg for cut tapping but prefer balax for a form tap.For 1/2 inch threads i generally use thread milling for this so as not to break taps.

Thanks. Any specific series or coating you would recommend? Also I notice they peck with their form taps. I have zero experience with form taps but this makes no sense to me.

[littlebrewman]

With titex drills i use the cobalt and whatever coating is available from them on that size drill.as far as pecktapping a form tap it is done.i usually only peck when i get above 2times the diameter of the tapped hole.u have to remember when u peck there is a possibility to blow out your minor diameter so be careful us ing this method with either cut or form tapping.form tapping is great because you dont have to worry about chips in the hole or chips binding up and also produces a better thread form.you really are a rookie arent you?

[cncClintain]

Originally Posted by littlebrewman With titex drills i use the cobalt and whatever coating is available from them on that size drill.as far as pecktapping a form tap it is done.i usually only peck when i get above 2times the diameter of the tapped hole.u have to remember when u peck there is a possibility to blow out your minor diameter so be careful us ing this method with either cut or form tapping.form tapping is great because you dont have to worry about chips in the hole or chips binding up and also produces a better thread form.you really are a rookie arent you?

Not a complete rookie, just younger. Ive worked part time in a job shop programming and operating a Mazak lathe off and on for 4 years while finishing my Bachelors in Industrial Technology from Purdue University. Also have an Associates in Injection Mold Making from Vincennes University and another Associates from Vincennes for Advance Manufacturing. The Advance Manufacturing was basically a degree based around an extra two semesters of MasterCam and Haas training. I just don't have much real world experience with this kind of work or stainless at all for that matter. The form tapping is brand new two me and they've been pecking the hell out of everything and it just didn't make sense to me, that's why I asked. Thanks for all the advice.