My Noobness is undoubtedly at work here, but I'm hoping that someone wiser can clue me in to what's happening.

I picked up what appeared to be some soft-ish steel at Home Depot the other day. The intent was to make up a batch of t-slot nuts. The material is 1/2" wide and about 3/32" thick. Cuts pretty easily with a hacksaw - seemed like the perfect material to mill slightly down to width, drill and tap a hole in the center and crank out a bunch of t-slot nuts.

This is EVIL AWFUL HATEFUL CRAP!!! I'm now down 2 ends of a double-ended endmill and one fly cutter bit and I have one little threaded piece of metal to show for it! I've tried light cuts, heavy cuts, slow feed, fast feed, coolant, dry, etc, etc. At one point, I thought I was making progress by standing the piece on edge and flycutting it down to the needed width, but came to find out that the little chips WERE COMING OFF OF MY FLY CUTTER BIT, not the evil awful hateful crap piece of cheap steel that was clamped firmly in my vise.

It would seem that work hardening is going on here, but darned if I can figure out how to avoid or circumvent it. I even tried going at it with my drill press, and got about 1/16" of an inch into it before even the elbow grease that I can apply with the drill press wasn't enough to break through the hard crust that had materialized in the hole. I had the work on a 2x4 block of wood as a backer, and it was burning the wood through the remaining steel under the bit. (oh, and add one drill bit to the list of items incapacitated by this stuff!)

What's the answer here???

Thanks!

Sound like your RPM's are high. What speed were you running it?

Jim - I just bought a piece of still very similar to yours from Home Depot and was able to cut it just fine. I even have a video of it on my blog: http://www.nyccnc.com/Herbie/HERBIES_BLOG/Entries/2007/10/27_Milling_Steel!.html

I, like you, was trying to make t-nuts. HD didn't have the right size for my TAIG, but i bought this piece anyways to expirement. I've seen found the right side piece of steel (had to order from Enco) and will be making t-nuts shortly. I'll be sure to post a video of that as well.

don't buy metal at HD. you'll pay through the nose and you don't know what you are getting. go to a service centre. if it seems like its work hardening, it's either stainless (doubtful) or you were running so fast you wrecked the edge of the tool. you say you are down a flycutter bit? don't waste time and money with carbide tools for flycutters, if its a lathe tool its not ground right for flycutting anyway. use hss, search here, there's stuff on how to grind it properly.

I'll have to double-check my rpms and feed rates this evening, but I believe that my little chart said I should use position "D" for a 3/16" 2-flute end mill. (D is 2900 rpm on the CR machine, I think). The suggested feed rate for the material was .048 inch/sec (which would be nearly 3 ipm), but I wasn't able to get anything near that - I think that the best I got was about .5 ipm. I ended up at a depth of cut of about .005" working the best (though still not well), but it made miniscule chips.

Another interesting thing that was occurring was that the cutter would very obviously load up - it'd get loud, chatter like heck, and then sort of break through and get nice and smooth and quiet, then start loading up again. WD-40 as lubricant seemed only to make this pattern worse. Going completely dry worked best, best being a relative term. The tool obviously overheated, as it was smoking at one point. Hitting it w/ some WD-40 helped that, but then I had the loading problem described above.

Its possible that the end mill was past its prime before I started - I didn't check closely when I mounted it. It was obviously fried by the end.

On the fly cutter - I used the stock HSS bit that came with my Taig fly cutter. I could not believe it when I examined the end of the bit and found the leading 1/3-1/2 of the lower surface was *flat* after attempting to mill the edges of the steel. There was barely a scratch in the workpiece steel itself. I don't recall offhand what feed & speed I used for that. What would be a recommendation for that, assuming the stock taig fly cutter? (2" cutting dia, I think?)

I'm sure the steel wasn't stainless - it was your standard, sort of dark-ish home center steel. I think its hot rolled perhaps? (maybe cold rolled)

What would be a recommended feed, speed and DOC for this material?

I clearly need to get a bit more scientific about my feeds and speeds, but gosh, I didn't think I was that far off. The destroyed tools tell a different story though!

tikka308 - I'm jealous! :-) So that 3/8" 4-flute end mill works pretty well for you? Maybe I should try one of those!

Thanks All

Sounds like you have got some steel (?) re-made from old tram rails and ex army hobnails from boots. In the UK this has been known about mostly in the late 40s and through the 50s when the hard bits had not been properly alloyed into the steel and hard spots were hit with just the results you have described. I hate to think what goes into modern steels that come from sources East of the English Channel.
John.
PS I forgot old bedsteads, nice light steel angle but take the teeth off the saw blade easy as winking.

Jim - I'm new at this whole endeavor.. I was going to use a 2-flute, but I use my 2-flutes a lot, so I thought "hey, if I break one of my 4-flute HSS, then I won't sweat it..." As you can see in the video, I was quite conservative with my DOC & F&S... I can't wait to do some more experimenting to see how much more aggressive I can get (if at all...).

The steel that I did mill came out SILKY smooth - which tells me there's no vibration/chatter in the mill. I was quite pleased with the finish quality.

What kind of a mill are you using? I'm using a TAIG - which has got to be one of the least-rigid mills out there (at least when compared to the X3's, IH, Tormach's, etc for cutting steel)...

I think you should give it a try again with a new end mill and see if that solves the problem...

I have used the HD stuff before. I think it is just cheap hot roll. It welds pretty decent though. HD used to sell small brass rounds but I have not seen it at my stores anymore.
I found some really lousy steel to turn this weekend. I needed some 1" steel and spotted an old weight lifting Bar in the garage. Sliced a chunk off with my chop saw and proceeded to turn it on my 9x20. After killing a couple of ccmt inserts I was left with possibly the most horrible looking finish I have ever done with any of my machines.... (chair)

Ahh well that's the way it goes with mystery metal sometimes.
Steve

Just to add my 2 pennys here I never use 2 flute endmills for anything except soft metals with stringy chips where loading in the flutes would be a problem. Steel, Stainless all 4 flute. If its super hard use a carbide endmill. I milled the untapped holes out of a set of 1-2-3 blocks with a carbide endmill and those things are seriously hard.

BTW, mystery metal concerns aside, I fully suspect my end mill and my lack of general knowledge in this problem. The stuff cut quite easily with a hacksaw, so there clearly weren't any chunks of Kryptonite or anything in the bar, as they would have denuded my hacksaw blade in an instant. Also, the first little bit of the hole (1/32-1/16") seemed to go ok, but then it all went to heck from there. (The fly cutter thing I'm still mystified and amazed by, but that was likely a feed/speed thing, too - it, literally, barely even marred the surface of the steel, but teeny chips were flying off of the HSS cutter bit like gangbusters - really pretty funny to think about in hindsight now!)

I just ordered a handful of new end mills from Enco. 3/16" and 3/8" HSS, in 2 and 4 flute. (BTW, they're having a killer sale on some of their 3/8" endmills - $2.99 ea for a double-end! Hope they're not total junk...)

Hey Jim, this may be silly, but it sounds like your spindle is running the wrong direction. I have seen it happen many times in the shop.

cheers,
Michael

I'll have to double-check my rpms and feed rates this evening, but I believe that my little chart said I should use position "D" for a 3/16" 2-flute end mill. (D is 2900 rpm on the CR machine, I think).

I clearly need to get a bit more scientific about my feeds and speeds, but gosh, I didn't think I was that far off. The destroyed tools tell a different story though!


too fast. its not about being more scientific, but machining isn't like knocking a deck together, you do need some theory. you newer guys to metal cutting naturally want to make chips, so sorry for sounding like your mom's :D, but get some theory under your belts ....it'll make everything sooo much easier. Even the old army machining manuals that are online for free will give you a good basis....but read 'em!

Cutting speed, or surface speed, is a distance per unit of time - feet per minute. Imagine a chart where as cutting speed goes up, tool wear goes up mostly in a linear relationship until at some point the line gets steeper - that's the theoretical maximum cutting speed - above it your cutting life starts dropping.

there is a cutting speed for each combo of materials - type of work piece and type of cutter. for example, HSS and 1018 (mild steel), is say 80-100 fpm. look up for each combo. you can work it out from there, or use the simple formula rpm = (4*cutting speed)/dia. in this case rpm = (4*80)/.1875=1500.

it doesn't matter whether its milling, drilling, lathing etc - you want the speed relationship between tool and material to be less than the cutting speed for that combo of tool & material, got it?

Now, this is a theoretical max. slow this down a bit and you increase tool life. point is, don't try to hit the max - a lot of these mills sell for less than the spindle bearings of a full size mill - you can do great work on them, but don't push to perform as if they're a new Bridgeport using theoretical speeds. A machinist has to figure out how to work with the machine at hand, and doing so rarely means running full tilt.

Once you've got a comfortable cutting speed, DOC and feed are more a matter what can the mill handle. depth of cut can be a max of 1/2 cutter dia (a rule of thumb i break all the time) and feed rate should .0005-.002 tho per tooth, depending on the size of the cutter. There is no point in machining at 1/2" per minute feed at 2700 rpm - all you're doing is making dust, thats less that 1/10,000" chip load per tooth. If you aren't taking a decent chip, you're just spinning your wheels and dulling the cutter.

think of it this way There is some removal rate, cubic inches per minute, that the machine is capable of. Its basic to the machine, this can't be exceed - horsepower, structure, spindle etc create a constraint. In most cases the machine will not handle the combined theoretical max spindle speed, full chip load per tooth and full DOC. So the machinist creates a balance. As an example, if the machine can't remove more material than it is already doing, keep the feed the same and lower the spindle speed until the chip load is reasonable.

I've probably just confused things for you, but start off understand what the maximum spindle speed is, then so long as its under that play with speeds, DOC & feeds understanding the objective is to get the best removal rates while also having a decent chip load. I say play because that is part of the process, learning what the machine can handle.

Lastly, get some free machining steel, say 12L14. find a local service centre, online service centre or even mail order industrial supply - it will make a huge difference. you are likely paying a massive premium for that mild steel and it machines poorly.

wisp - double-checked, and the spindle is running the right direction - something really screwy would have had to have happened to reverse suddenly though, as its cut very nicely prior to this particular, horrid, episode! :-)

Mcgyver - Wow - thanks - that was a mini education right there - I really appreciate it! That gives me the big picture, and it helps a lot! I'll seek out some online manuals as you mentioned, too.

Bummer about the Home Depot steel - its *so* tempting because its so convenient (and I'm sure its expensive for what it is, but it was nice thinking I could go walk out of there with metal for a few bucks, even if it was ridiculously overpriced for the quantity). Oh well, free lunches and all that! :-)

Perfesser Mcgyver, thinking this stuff through a bit more, and just want to be sure I understand the point about the feed rate.

You say the feed rate should be ".0005 - .002 thou per tooth" - by that you mean, literally, .0005 - .002 inch per tooth, is that correct? Next, if I'm using a 2-flute cutter running at 1500rpm (just numbers I'm pulling out of thin air for the moment), then that's 1500*2 'teeth per minute', and .0005 inch per tooth would be:

.0005in/tooth * 3000 tooth/min = 1.5 in/minute (feed rate)

Is that correct?

If I'm on the right track on this, then as far as the .0005 - .002 range for feed calculations, you say that's "depending on size of the cutter". Is there some guideline for correlating a particular-sized cutter to some point in that range? (like a 1/16" dia endmill would be the .0005 end, and a 1" cutter would be the .002 end, with sizes between those two distributed linearly in the range - something like that.

Incidentally, you're spot-on as far as the 2700rpm and 1/2 ipm feed rate making dust - that's just about literally what was being produced!

Thanks Again!!

Yeah Jim, a lot of people get the wrong idea when milling or drilling steel. 550 to 650 should be your rpms and that goes for a lot of different steels with the exception of stainless which I haven't had a chance to mill it yet. 2700 rpm way too fast unless you have a 1/4 million dollar VMC. 2 flute not recommended as a cutter for steel. I find carbide is sweet and probably what you bought at home depot I would have used 1/4 to 1/2 " diameter 4 to 6 flute cutter. For carbide dry no coolant but heat strength cutters at least wd 40. Good luck and live and learn.

try heating it to cherry red and letting it cool (anealing)
run about 700/800 revs to cut using a hss cutter and a bit of coolant/oil

Or, just do what I did for my taig. Go to little machine shop and buy them. Isnt more than a buck or two a piece. $1.50 for the taig I think. Or they have bulk packs for less per nut. For the labor, materials and frustration..........this way you can get to work on the stuff that makes money :).

Believe me I am all for making tools when either a commercially purchased one is so unreasonable or there literally is not anything that fits your needs in existance. But when it is readily available and cheap enough.....:)

You say the feed rate should be ".0005 - .002 thou per tooth" - by that you mean, literally, .0005 - .002 inch per tooth, is that correct? Next, if I'm using a 2-flute cutter running at 1500rpm (just numbers I'm pulling out of thin air for the moment), then that's 1500*2 'teeth per minute', and .0005 inch per tooth would be:

.0005in/tooth * 3000 tooth/min = 1.5 in/minute (feed rate)

Is that correct?

If I'm on the right track on this, then as far as the .0005 - .002 range for feed calculations, you say that's "depending on size of the cutter". Is there some guideline for correlating a particular-sized cutter to some point in that range? (like a 1/16" dia endmill would be the .0005 end, and a 1" cutter would be the .002 end, with sizes between those two distributed linearly in the range - something like that.

Thanks Again!!

OK
You are getting it.
A 1" cutter would be .005 - .008/ tooth.
Feedrate = chipload*#FL*RPM
.002*2*1500=6IPM

There are some free apps on this site that will assist your calculations.

Also RPM is NOT an arbitrary # it is based on surface feet per minute. There are general "rule of thumb" numbers like Mcgyver used but each cutter manufacturer has their own recomendations (remember that coated cutters run faster than non-coated).


Here are a couple of references for you.
http://www.speedsandfeeds.com/PDF%20Files/EndmillsDrillsSaws.pdf
http://www.niagaracutter.com/techinfo/millhandbook/speedfeed/index.html

Here
Download this (ME consultant free)
http://www.freedownloadscenter.com/Business/Misc__Calculators/ME_Consultant.html
I almost never use the numbers as this generates them, but they are close and I am usually using specialty cutters.

Jim Stoll, guys,

Is it not the case that Home Depot and such may supply hot rolled as well as cold rolled steel? If that is so, keep in mind that hot rolled usually has a very hard scale on it, which some folks pickle or abrade off somehow. But it sounds, Jim, like you penetrated the surface and were still having difficulties.

An observation.
-Mark

Ok, armed with the education from this thread, and with a new 5/32" end mill (the largest I have left at this moment), I went at the demon steel with my Taig again last night.

This time, I used the slowest pulley position (allegedly 1100rpm) and went for a still-conservative but more sensible feed rate (1.5-3 ipm, depending on my DOC) and it machined, well, I guess how its supposed to machine! Actual chips were coming off of the work (the work, NOT the tool! :-). The cutter was going through it not quite like butter, but perhaps like a block of hard cheddar. It was actually fun to watch. No smoke, no squeals, grinds or shudders. I even used the end mill to mill the hole for tapping (it was the right diameter, it was mounted on the spindle, I was caught up in the moment). This was cool. I could get used to this!

I think that my first mistake (of several) was that I incorrectly positioned the belt on the pulley system. The pulleys are referred to by letters from A-F, and I'd been thinking that A was on the top, but in reality, I think that A is on the bottom. (At one point, I had a diagram that showed the positions and their proper labels, but darned if I can find it anywhere at home, and I can't find it anywhere online either - anyone know where this is??) I have a little 'speed by diameter' chart that shows pulley position (A-F) by material and end mill diameter in a grid, so when it said to use position 'B' (which I now think is 2nd from the bottom, or 1900rpm), I think I actually had it in position 'E' (which was a near-supersonic 6500rpm). Its a wonder my mill didn't take off for the moon. Anyway, I'm abandoning the A-F chart, as my new knowledge has me believing that I'm better off figuring where in the range a particular cutting speed lies, and erring toward the slower vs the faster - the letter labels sort of hide that subtlety.

BTW, under-dog, I have a few of the LMS t-slot nuts for my table, but I was actually making this batch up for the little t-slots on my headstock. I needed to mount my new mist sprayer and those slots are much narrower than anything that I already have or that LMS sells.

Thanks for the links to the charts and the cool-looking software (unfortunately, that link doesn't seem to lead to the software any more - if anyone has this and can send it to me, PM me - I'd love to see it in action). Another helpful link with that type of info, but tailored a bit for the Taig, can be found at http://www.super-tech.com/root/grp.asp?p1=micromill-tooltips

I appreciate everyone's help!!

Jim

Jim, i just threw out the .0005 - .002 numbers. a .001 - .002 thou chip per tooth is kind of textbook, but you can snap a small dia cutter this way, fine for 1/2", but it'll kill a 1/16 end mill....however the sideways force on the cutter will of course also dependent on DOC. As Darebee points out, larger cutters can handle a bigger load.

i laughed at the Professor part, can't help but help the new guys out - it make me feel so bloody smart :D :D :D


and let us know how it works

Here
Download this (ME consultant free)
http://www.freedownloadscenter.com/Business/Misc__Calculators/ME_Consultant.html
I almost never use the numbers as this generates them, but they are close and I am usually using specialty cutters.

Love to get a copy to try out... but the link to the actual D/L is dead. Do you have a copy you can upload somewhere or email me? I can pm my email if you perfer that. Thanks!

Ken

i laughed at the Professor part, can't help but help the new guys out - it make me feel so bloody smart :D :D :D


Heh heh, well FWIW - it makes me feel pretty bloody smart just by association! :-)

Seriously though - those are the kind of insights that help us noobs out immensely. I've stared at my share of feed & speed charts and have actually read parts of various online manuals and docs, but seeing it presented in the 'look kid, this is how it works' manner made it suddenly much clearer, and I can now look at those charts with a new perspective. This will definitely help my machining capability out a whole lot, and multiply the fun quotient by several orders. (Its fun running the mill under any circumstance, but its alot more fun when you're not smoking your tools! :-)

PM me your email and I will email the prog.

Never mind the PM
A few minutes on Google gave me this working link.
http://www.softsea.com/download/ME-Consultant.html
You will need to allow pop-ups.

Here
Download this (ME consultant free)
http://www.freedownloadscenter.com/Business/Misc__Calculators/ME_Consultant.html
I almost never use the numbers as this generates them, but they are close and I am usually using specialty cutters.

Hi DareBee,

When you say close enough; can you give some insight into how you would go about using the numbers for our small hobby mills?

Would I be right to say the RPM’s and feed speeds would be correct for a good finish but the depth and width of cut would need to be adjusted to suit machine/fixture rigidity?

Thanks,
John

EDIT: It might be worth noting there is a Pro version of this software that is worth looking at here http://mrainey.freeservers.com/PurchaseInfo.html

Good thread. Good information. Makes me a wee bit antsy to tackle the aluminum with a 1/64" end mill this weekend.

I do have a question though. How do you guys clamp something down which needs milling on all sides? First pass of what I will be doing this weekend is to mill the square blocks (1/8" thick) into circles. I have read someone said they used Superglue to glue the work to a wood block and then clamp the wood block. Feasible? Better solutions?

Oldman
For tweaking i adjust the SFM to the cutter manufacturers SFM.
I also find that the chipload is often heavier than what I want for profiling or pocketing. The chipload is too light for surfacing and the drilling feed is very heavy.
Remember, these are my opinions and I usually am only doing 1 part so the machining time is negligable compared to setup and programming time.

Skuzzy
Always cut with the largest cutter that you can, up to about 3/4 - 1 inch. Cutting with a HSS 1/64 cutter is like milling with a noodle.
You can clamp the scrap tails down and then dont mill quite through .005 - .010. You will be able to push the part out or cut with knife, then file the flash off.
Mitee-Bite makes a heat activated tape/sheet that works well if that is what you want to play with, or clamp it in the vise and mill out the circles.
If you need a lot of circles a laser will make them for pennies over the price of the material.

I was not clear. I am doing this in stages. I'll be using a 1/4" end mill for punching out the circles. Then move to a 1/8" for roughing and finishing with a 1/64". Unfortunately, the 1/64" will be cutting grooves, so it will be a slow process, I figure.

I am making 10 units. Thought about taking them to get them laser cut, but I am in a pinch for time and all the locals I have called are quoting a 2 week lead time. Guess they are busy this time of year. Not sure why though.

Great suggestion about the partial cut through. I might be able to make that work.

Sounds good.
It is not always possible, but I like to cut serrations with a slitting saw.

Two things I can add here -

When cutting, it's just as important to pay attention to the chips as the surface finish - especcialy when using HSS tools. The chips should look brown or silver when cutting steel. Blue is too hot. You can measure the chips with calipers or a mic - the thickness is your chip load. For begginers, this might be a good, sensible thing to do.

When holding a perimeter cut-out, I suggest the same method as mentioned above in addition to using tabs. I use thinned tabs most of the time - it reduces the amount of clean-up time required.

Scott

Oldman
For tweaking i adjust the SFM to the cutter manufacturers SFM.
I also find that the chipload is often heavier than what I want for profiling or pocketing. The chipload is too light for surfacing and the drilling feed is very heavy.
Remember, these are my opinions and I usually am only doing 1 part so the machining time is negligable compared to setup and programming time.


Thank you DareBee :)

Sounds good.
It is not always possible, but I like to cut serrations with a slitting saw.Unfortunately, the grooves are arcs, some are pretty tight. Not even sure it is going to be feasible to make this, but it looks good in wax so far.

I figure to cut 0.0078" depth per pass to get to the 1/32" depth I need for the grooves.

I like the tab idea. If I understand that concept, I would cut all the through the 1/8" plate and leave connection bridges (as it were) holding the circle in place.

I have a rotary table, but I cannot figure out how to attach a flat plate to it.

By the way, I do really appreciate the input. I have been reading and practicing with this mill for a couple of months now getting comfortable with the software, hardware, and general milling procedures/operations. I feel pretty good right about now, but still lack the practical application of the knowledge.