I have a job to do in 316 stainless. I have to make the following sizes of tapped holes.
I want to thread mill vs. tapping to avoid breaking taps and trashing out an expensive part. I also believe that I can control size much better with cutter comp. and the finishes should be beautiful. I do not have any hands on experience with thread mills yet, which is why I am posting this.
The job is a small qty. Only 14 pcs. However it would be a repeat job if I quote it properly.
I need to locate reasonably price threadmills that would work.
Any tid bits of helpful info would be great, and very much appreciated.
Also how many threaded holes should I expect to get out of a typical thread mill.
I don't mean to steer you away from how you want to run your job, but if you don't have much experience thread milling, then let me tell ya a few things about it.
There are no really cheap thread mills. Plan on spending at least 100 bucks on each mill. I know you said reasonably priced, not cheap, but you get my point.
If you don't have much experience thread milling, then it may be just as easy to scrap a part using this method, as opposed to tapping. If you were to get real good taps, you would save a lot of tooling costs, and your quote on this job could be cheaper, which it sounds like you need to achieve.
If you insist on threadmilling, I would suggest having someone help you with the programming unless you have a real good understanding of what needs to happen for thread milling to work properly. I'm talking mostly about your lead in to the start of the cut.
When done properly, thread milling can work awesome. Threads come out very pretty, and as you said, size control is in your hands, not the tap.
I'm not sure about the tool life on 316 stainless. Hopefully someone else with more experience will chime in on this. With the right tool and coating, I can't see why you couldn't expect at the very least 100 parts per mill.
Not much help, but hopefully I helped you make some informed decisions.
Advent makes a special tapered thread mill for pipe thread and has the sub on their site I think, not super cheap, but works nice to achieve desired size on holes without much room behind, i.e. water plugs in molds, etc.
I run 316 often with 1/8-27 threads I tap the parts with no problems. with a greenfeield tap. Hole prep is key I us a tapered endmill to bore the hole before tapping. Dave K is correct threadmills are very expensive but work great when programed correctly. I like Emuge threadmills personally. how deep are the 1/2-13 and 3/8-16 holes that need threads? Are they blind or threw? if they are threw I would suggest starting them with a tap and then hand tapping to finish. if blind threadmilling is a good choice. I hope this helps TZ
Yeah man 316 can be a beast, but if you use decent taps like osg or greenfield, you will be just fine,
the main issue is when you are drilling it, dont baby it or it will work harden pretty quickly, and then your taps will have issues. how many holes of each size? and how deep do your threads need too be?
I havent tried it but you may get away with threadforming taps.
Having to buy 3 of them at once for 14 parts can be tough but they would last through many "cycles" if you get the job. I've used Xactform which has the best tech help that i've found but they are pricey.I think it was micro 100 that has a spread sheet program that will generate code for you.Spindle torque doesn't come into play with the mills as it does driving a tap which was a factor on my Haas.
I would recomend getting insert type threadmills. Especially with 316 ss. Much cheaper in the long run. I use Vardex with great success, they have lots of good information on their website to help you get started. Note, there is a learning curve with threadmills and 316 isn't the best to learn them on.
Bluejeep, I could be wrong, but I don't think they make insertable thread mills that small.
Lake Shore Carbide is a very good company to talk to about thread mills:
Do not use carbide thread mills in stainless, they will snap in a heartbeat. Use a powdered metal or cobalt. You'll be much happier.
Just my opinion,
I didn't realize I would recieve this much support so I was vague with the description. I sincerely appreciate the help. I realize thread mills are $100 plus.
1/2-13 threads are thru holes in 3/4" thick 316 ss. There are 4 holes on each part. The part is a cap so I was going to make a quick fix. to clamp to. This would allow for a reasonable thru hole, and for locating quickly.
3/8-16 threads are blind holes 1/2" deep. There is 1 taped hole per part.
1/8-27 npt zert threads. There are 2 per part. One has a lengthy thru hole. The other is perpendicular coming into the same lengthy hole, but it is basically blind.
The 1/8-27 npt scares me the most. I've only taped a dozen or so tapered threads with pipe taps. I normally do it for personal stuff in carbon steel, never in 316 ss for a customer yet, and I haven't used a tapered em.
I would really appreciate info on:
-where to buy the tapered em for a blind 1/8-27 npt.
-a good brand of powdered metal or cobalt thread mills.
-is it wise to buy such tooling on ebay.
I occassionally threadmill M6 STI & M8 STI holes in titanium. I threadmill since I can't find stock STI taps for titanium in metric sizes ( no luck from OSG, Emuge, etc.) The trick for me is to make several passes, each pass increases the pitch diameter and to use a TiCN coated, helical threadmills. A straight flute threadmill snapped after a few holes. I use carbide threadmills but powdered metal sounds like a good idea. Who makes them? The M6 threadmill has cut about 80 holes and the M8 about 25 holes. The bigggest disadvantage for me is that threadmilling is a lot slower than tapping with relatively small holes. I've been using threadmills from Scientific Cutting Tools. Their catalog explains multiple passes. They will send you sample code free as will almost every other threadmill manufacturer.
For typical threaded holes, you start at the bottom of the hole and mill up in Z. I have read that for tapered pipe threads, you are supposed to mill down into the hole, since the some CNC's can't cut a tapered helix. I've never done it though.
If possible, I prefer to work with local tool distributor, that way I can get tech support. If they can save me time and shorten my learning curve, that will more than make up for any Ebay savings.
where to buy the tapered em for a blind 1/8-27 npt.
it's usually referred to as a pipe taper reamer....
do you have g84 rigid tapping on your machine?
there are some awesome taps for 3/8 , 1/2 ,1/8npt.
why reinvent the wheel? i suggest greenfield's EM-SS
gun taps , and EM-Tough series spiral flute taps.
YMW ZELX-ss taps are swell too. never broke one
larger than 10-24 .
try interrupted thread for the npt. i have tapped many,many threads for AG applications...thread
milling in ss can take a LONG time compared to a tap.
mmm... Dave I think you are probably right, I was not thinking too clearly this morning :rolleyes:
I use a 1.5 deg. tapered endmill with a 1/8 tip from kenametal.
As for the powdered metal Threadmills I have mixed feelings. I have had great luck using them in stainless. But the ones I have used have been Greenfield. The problem I have had is the cutting diameter was not consistant from 1 mill to the next.
Feel free to use lakeshore carbide thread mills on stainless steel.
We have sample programs with code and recomendations for stainless steel milling
in the speed and feed chart section of our site.
The 1/8-27 NPT thread mill itself is $80.54 and will thread a blind hole much safer than a tap.
Our thread mills run against Emugee all the time with favorable results.
As far as ebay, the tool you buy today may not be available next month.
The best process for Stainless would be to take several passes, especially on the NPT.
You will snap the tool trying to finish in one pass but a rough, semi-finish and finish pass will dramatically extend the life of your tool.
As far as taps....by the time you buy a high performance tap and the tapered reamer, you are close to same cost of thread mill, but you will mill perfect threads with a thread mill and can compensate for size and wear as time goes on.
Thanks for that link, Spencer. They look like good quality cutters, and the pricing is extremely reasonable.
Lake Shore Carbide.
I'm glad you added a post. I was looking at your website a few days back, and I was impressed. Although I'm still a little leary.
I'm not sure if it is out of line or not, but if it is I appologize. If I win the quote, could I buy a 1/8 npt thread mill at a reduced price. I will run it exactly as you tell me to program it. I will pre drill to what you want. In return I will post to tell others of how they worked, good or bad. If your thread mills work as well as you say, I will be a repeat customer and refer you to the other shops I work with.
Please feel free to private message me with your thoughts, I will respect your decision either way.
A good quality thread mill, solid carbide will do a 1/8-27 in one pass and give you about 1,000 holes without taper reaming. You probably wouldn't need to ream a 1/8-27 NPT even in 316SS. Anything larger that that, yes, even in soft material.
I am taking the chance, I ordered thread mills for everything. I realize it isn't cost effective for the 14 assemblies I'm running. If they make it to the 2nd or 3rd batch, they're paid for. If the customer is extremely impressed and it gives me more opportunities with them they are paid for time and time again.
To a certain extent it is a chance for me to evolve with the ever changing tooling. I very much appreciate all the help from every one. I promise I will add a post to say how things worked.
Tapman, If you don't mind could you email me a copy of a 1/8-27 npt cycle you run. Right now It looks like the manufacturer wants me to run a couple rough passes then the finish pass. I plan to run the concept they want on the first order. As soon as I feel comfortable with the thread mills I plan to play a little.