Threadmilling speeds and feeds check (I don't do it enough to know)

On occasion I break out the thread mill when doing some one-off threads. I've got a couple iscar tool bodies with the full form thread inserts. Whenever I use them, it seems it takes significantly longer than tapping. And I think that is to be expected.


Although when I see people say "just threadmill it" on here, it seems to come with the undertone of, "it is plenty fast".



So my question is, how fast do you guys run your threadmills? A couple examples:


Lets say I have a 1/2-13 thread, 3/4" deep, in 1018 using one of these: 1/2-13 Variable Flute Carbide Thread Mill

Lakeshore's recommendations seem to be 350-500sfm, .0025-.0035ipt. middle of the road numbers would be about 4600rpm at 55ipm.

Harvey tool's recommendations are about 550sfm, .0016ipt. That is about 6000rpm at 38ipm. But harvey's guide also has an adjustment formula ((major - tool dia)/major), which ends up putting me at 11.4ipm


Are you guys really running these at 500sfm? I have a long running job, running the lakeshore threadmill, and we settled in at 2000rpm at 3/4ipm a long time ago. Tool life is pretty good, is consistant. I remember we tried going faster but settled in on this after a short period of trial and error, settling on the current numbers just because "it worked"




Another example (the real reason I'm asking):


I am running a one off repair job, where I need to mill a 4"-12 thread about 5 inches deep in some sort of steel (seems to cut easy, might be 1018 although the finish I got while boring the hole was nicer than I expected. The part is welded so I don't think it is 12L or similar)

The only tool I have for this is a boring bar from the lathe dept. 1.5" bar, approximately a 2" diameter. So it is basically a single point, single tooth threadmill. I am running 300sfm (573rpm) at about 8.5ipm (.015 per tooth!!!) now. I had started at like .003" but it really felt like it was creeping along way way way too slowly.

Even at this speed it takes about 40 minutes to complete the part (in this case, not a big deal, i wander off while it is cutting) but to you people who do this all the time, how fast can I ramp this up to? Can I expect to gain anything on this part?


Is there another place to look for even different threadmill information?

Well at that depth I would guess it has to be single point, but for shallower threads, say up to 1" deep (depending on diameter) you can get multi tooth mills so you only need to make 1 or 2 revolutions around the ID of the minor diameter.

* I see you linked a multi tooth threadmill. You are only going 1 or 2 revs, yes?

I don't do too much larger than 3/4-16, but I can tell you a lot of machines will have a hard time making a nice circular path at 55ipm at that diameter or smaller.

Lets say you have a Haas VF?, one would want to turn the quality setting up to medium or finish to help with accuracy. The machine will slow itself down as needed when these settings are on.

For me in steel, I start with 70sfm and .005" stepover and at least 1 spring pass. Super conservative, but I have yet to break a threadmill, even in inconel/monel. From there you can speed things up or increase stepover distance. To be the most effective, maybe try a bigger stepover with a slow feed/speed to start, and just increase that until you find your diminishing returns.

I do have the benefit of running 1-offs for prototypes, so taking a little extra time here isn't a huge consequence for me as long as I don't make the thread(pitch diameter) too big on the first cut. If I were running 10+ parts, I would use the first part to try and speed things up as much as I can. But you will either have a larger stepover with slower feed/speed or vice versa. Pretty much always need a spring pass from what I've observed, especially if you are making class 3 threads.

Just my 2 cents.

Mike1974 said:

Well at that depth I would guess it has to be single point, but for shallower threads, say up to 1" deep (depending on diameter) you can get multi tooth mills so you only need to make 1 or 2 revolutions around the ID of the minor diameter.

* I see you linked a multi tooth threadmill. You are only going 1 or 2 revs, yes?

Click to expand...

yes, the 1/2-13 example, I do one depth pass on the rough (doing 2 radial passes, 65%/35%) and do a second circle around on the finish pass. I am climb cutting. I generally use the generated program from SCT (Thread Mill Code Generator – Scientific Cutting Tools, Inc.)

And the iscar threadmills I use are inserted, 14 and 21mm insert lengths, so I can do many threads in 2 depth passes.

I always have a skim pass too (so technically it's 3 passes, with the 3rd the same as the 2nd)

dandrummerman21 said:

yes, the 1/2-13 example, I do one depth pass on the rough (doing 2 radial passes, 65%/35%) and do a second circle around on the finish pass. I am climb cutting. I generally use the generated program from SCT (Thread Mill Code Generator – Scientific Cutting Tools, Inc.)

And the iscar threadmills I use are inserted, 14 and 21mm insert lengths, so I can do many threads in 2 depth passes.

I always have a skim pass too (so technically it's 3 passes, with the 3rd the same as the 2nd)

Click to expand...

He's not talking about depth passes, he's talking about how many revolutions you make around the hole.
For those multi flute thread mills, spiral up twice and done.
For example if it's a 1/2-13 thread you'd have only 2 lines of code after it feeds down into the hole.
G03 X-Y-Z IJK
G03 X-Y-Z IJK
G00 Z retract.
M30

Threadmilling is great for one-offs, short runs, hard materials, when the stock (or previous operation) is very expensive, when a very high quality thread is paramount, or when you don't have enough torque for tapping. For most production in normal materials, I prefer form tapping. It can take some fiddling to get form tapping right (may need to ream the drilled hole), but once it's running it's very fast and reliable.

Mtndew said:

He's not talking about depth passes, he's talking about how many revolutions you make around the hole.
For those multi flute thread mills, spiral up twice and done.
For example if it's a 1/2-13 thread you'd have only 2 lines of code after it feeds down into the hole.
G03 X-Y-Z IJK
G03 X-Y-Z IJK
G00 Z retract.
M30

Click to expand...

Yes, I knew what he meant. That's why i said I do the thread at one depth at 65% (one G3 revolution), and I do 2 revolutions at 100% (2 G3 revolutions).

Same as your code basically.

It also depends on stepover. I tend to treat these like a lathe tool and run a few stepovers. I just did an oddball 15/16"x16 thread in a part using Carmex inserted tooling and with a 0.790" cutting diameter 14mm tall insert, I did 650SFM (3140rpm) and 0.0035" per tooth, so 11ipm. I used three 0.015" stepovers. Material was 1018 cold rolled. I also recently did a 304 job with an M6x1.0 thread and a Harvey single point. That one went 150sfm and only 0.0002" per tooth with a four tooth cutter, so 2.55ipm.

I generally like going faster with lighter cuts and get better tool life and have never had a failure (chipped tooth, etc.). I always just follow the speeds and feeds from the tool manufacturer's website.

dandrummerman21 said:

Yes, I knew what he meant. That's why i said I do the thread at one depth at 65% (one G3 revolution), and I do 2 revolutions at 100% (2 G3 revolutions).

Same as your code basically.

Click to expand...

Sorry about that, I must have interpreted it differently.
No worries.

Fi= (Fl x (R-r))/R

Where:
Fi= the feedrate for an inside arc
Fl= the linear feedrate (in/min or mm/min)
R= the inside radius of the hole to be threadmilled
r= the cutter radius

Fl= r/min x Ft x n
Where:
Fl= the linear feedrate (in/min or mm/min)
r/min= the spindle speed
Ft= the feedrate per tooth of the cutter
n= the number of cutter teeth

Is this the formula you are searching for? This came directly from Harvey Tool

Houndogforever said:

Fi= (Fl x (R-r))/R

Where:
Fi= the feedrate for an inside arc
Fl= the linear feedrate (in/min or mm/min)
R= the inside radius of the hole to be threadmilled
r= the cutter radius

Fl= r/min x Ft x n
Where:
Fl= the linear feedrate (in/min or mm/min)
r/min= the spindle speed
Ft= the feedrate per tooth of the cutter
n= the number of cutter teeth

Is this the formula you are searching for? This came directly from Harvey Tool

Click to expand...

Yeah. I didn't have the formula until I started writing this thread.

Maybe the question is more related to three things:


1: why is the answer often "I threadmill everything" when we're talking about a relatively standard size and depth in a relatively standard material that someone might be having trouble with. When it takes 10 seconds to tap a 1/4-20 or 30-40 seconds, the choice is clear. Plus the tap is often an order of magnitude cheaper.

2: does it seem reasonable for me to spin away at a 4"-12 hole 5" deep for 80 minutes?

3: why does there seem to be a large discrepancy between feedrates and speeds(the example in my OP had lakeshore's tool doing about .003 per flute while the harvey tool was half that. But the harvey SFM was about 40% higher?)