Drilling 316 Stainless Steel 3

[vikin9]

We have a project to improve the yield of a drilling process on an older CNC machining center and I'm looking for some knowledge sources of current best practices on drilling 316SS.

Our biggest defect is a .1874+/-.0004 ID hole that sometimes ends up oversized. The drilling steps for these holes are: center drill, mill, turbo drill, ream. We use a recycled (filtered) Moly-D cutting oil that has been drawn from another CNC machine used for tapping. The oil is not pressure fed.

We have made these parts for years and have considerable experience at it, but haven't paid much attention to advancements outside our company.

So, what are my questions?

I would like to know some good sources of knowledge of drilling 316 stainless (i.e. vendor catalogs, associations, handbooks, etc.)?

Also, I want to test the validity of using recycled oil that is uncontrolled, but our "experts" believe to be more than adequate for the application. How can we test cutting oil? What are the best practices in PM of oils?

If anyone can give me some guidance or advice I would be grateful. Thanks.

 

[TVP]

Authoritative references on machining:

Machinery's Handbook Twenty Sixth Edition

http://www.industrialpress.com/mh.htm

ASM HANDBOOK Volume 16 Machining

http://www.asminternational.org

Good on-line references on machining:

Manufacturing Center

http://www.manufacturingcenter.com/online_book/default.asp

American Machinist

http://metalworking.penton.com/

Production Machining

http://www.production-machining.com/

Modern Machine Shop

http://www.mmsonline.com/

Cutting Tool Engineering

http://www.ctemag.com/

Society of Manufacturing Engineers

http://www.sme.org

I recommend you perform a search for "stainless steel drilling" on the SME site (

http://www.sme.org/cgi-bin/storefront/search/2///)--

between their Manufacturing Engineering magazine and the journal articles, transactions, etc. there will be quite a bit of information. Also, SME has several books on machining-- I don't how they compare to Machinery's or ASM Vol 16:

http://www.sme.org/cgi-bin/storefront/prodgrp/B/B11000/MEMBNUM/SME/

 

[Viktor]

Although the sources provided by TVP are a good beginning, you probably will not find the proper answer to your questions there. The problem is that these recommendations are toooooo general and thus do not account for you particular case.

I would recommend the following sequence to combat the problem:

1. Check your re-sharpening practice. The key issue here is that the drill should have exactly the same angles and length of both lips. It this is not the case, the drill drifts so you have an oversized hole.
2. Since you CNC machine is old, the excessive spindle runout might be the case. Even small runout results in hole oversizing (drilling and reaming).
3. Check you drill holder. The drill holder may contribute a lot in the mentioned runout so its runout adds to that of the spindle.
4. There is no simple method to check the quality of the cutting fluid (coolant). The rule of thumb is to keep it clean (particle size should be <20mictometers). In any case, the coolant for your application should have high percentage of sulfur and chorine – this is mandatory.
5. You have not mentioned the depth of drilling. If it is >5D, you have a problem with chip removal and coolant access to the cutting lips.
Viktor

http://viktorastakhov.tripod.com

 

[vikin9]

Thanks TVP and Viktor for your helpful replies!

On the cutting oil:
We do filter it periodically, however, I'm concerned that other substances are added to the solution over time (i.e. parts cleaning solvents, lube oils from gear boxes, etc.). There must be some point where the fluid reaches a point of ineffectiveness. Is this simply a case of needing a steady source of cooling liquid, or are there other important properties, like viscosity?

On the hole size:
The holes we have the most trouble with are just over 5D and they're through holes. We've suspected chip removal as an issue. Is the solution a matter of programming the the drill to come out more often? Or how is this problem best approached?


Please forgive my ignorance (not stupidity) on this subject. I'm a mech engr and Six Sigma Black Belt, but new to CNC machining.

Again, thanks for your great help!

 

[TVP]

As Viktor mentioned, chip removal becomes a problem at larger depths, especially with stainless steel, due to its tendency to gall. One solution is to program the drill to &quot;come out more often&quot;.

The quality of the lubricant is a more difficult question. You should definitely be using a sulfochlorinated cutting oil if you want the optimum performance. Viscosity is recommended to be less than 300 SUS at 38 C (100 F) in order to permit the necessary flow. I am not an expert when it comes to lubricants and the degree to which contamination becomes an issue.

 

[Drazen]

Viscosity is really good signal of (potential) chemical degradation of oil.

You can measure it periodically, and acceptable tolerance range should be obtained from oil manufacturer.

The other occasion : inter-reaction of oil additives with surrounding chemicals is far too complex for this purpose.

 

[sprintcar]

In an earlier life we did a lot of small, deep drilled holes stainless parts in a twin drill machine (Snow). The biggest problem w/ Stainless is heat - get too much and you're done. I modified the oiling system with a larger flood nozzle where the drill entered the part, and a smaller flow on the drill tip while it was retracted. This increased drill bit life about 10x and allowed changes to drill geometry to combine operations. Worked fine until somebody in the shop decided it didn't need that much coolant and went back to one small line.... drill bits failed in a day again. There was also a programmed chip clearing stroke as the bit got deeper into the part, which retracted the drill just out of the hole (into the large oil flow) for a second to clear chips.
For hand drilling there was a product called Anchor Lube that worked very well. Don't know if its still around. Keep the wheels on the ground
Bob
showshine@aol.com

 

[daveaberle]

In most general maching applications, recycled oil works as good as any 1980's oils. Also to be considered is the source of the recycled oil; no one wants to end up with old PCB cooling oil in the system. However; Rocool has several tapping compounds that work great on 304 SS so I assume 316 should work better. I once had expensive synthetic oil verses recycled cheap oil compared with running a race in a jogging suit verses a three peice suit, both will finish but jog suit wins. The finest finished goods are as good as the ingredients.

 

[Yahnozha]

Anothe option when drilling deep holes and having issues with chip clearance is to try parabolic flute(?) drill bits, these have a more agressive spiral for removng chips a lot easier and tend to have a more accurate hole drilled.

They have worked well for us in our dealings with 316 and 316L SS

 

[Viktor]

Dear Yahnozha

As far as I know, a “parabolic” chip removal flute does not form straight cutting edge when intersected with a conical flank surface. The problem is that the flute counter is not a ”flat” curve, i.e. it does not belong to the plane perpendicular to that containing drill axis. Therefore, the design of a milling tool (or profiling a grinding wheel) for the drill flute is not that simple as it seems to be. The problem is that the line of intersection of two curved surfaces, namely, the flute and the flank, should be the straight cutting edge. Unfortunately this issue is not well understood. Would you please elaborate more on the parabolic chip removal flute. Thank you.
Viktor

http://viktorastakhov.tripod.com