What end mill for milling out slots in guards

U

unky_gumbi

Joined
Aug 28, 2009
Messages
7,951
I recently got an old metal lathe, and while I know it isn't the best thing for milling a slot it will be a lot better than drilling a bunch of holes and filing. A lot easier on my elbows too.

What I need to know is what type of end mill I should get for the job and if it could be used for some rough shaping too? I know right off the bat it should be smaller than the width if the slot I want to make, but how much smaller?

In the long run, near Christmas, I plan on picking up a 2X mini mill to do this sort of thing and maybe make the move to making folders along with what I am doing now. So this one bit is just the start to the whole milling thing for me.


Thanks for the help
George.


PS I have been around, just not making much lately so no posts from me:o
 
For slotting you'll want 2 flute. For a less-than-rigid setup you'll want high speed steel. Ideally the cutter is about .010 smaller than the slot so you can finish .005 per side. You might want even more rough stock allowance than that if there is much play in your setup.

Remember, you don't have to take the full cut all at once. You will be better off taking lighter depth of cut and multiple passes if you're milling without very many tons of iron behind the cut.
 
Thanks Nathan, the blade in question here started out life as 3/16" bar not sure exactly how thick it is where it would meet the guard now.

I was thinking a .125" end mill, but I will reassess that once I get the blade closer to finished.
 
Yeah, 1/8" in a 3/16 slot is good. Be aware than cutter deflection and slop in your setup can lead the cutter to plow to the left (relative to the cutter feed direction) and gouge your part. This is a function of rigidity (or lack thereof) and depth of cut. Keep that in mind if you're taking a heavy cut and your cutter is close to your finished wall. This is a common problem when using long skinny cutters such as used when slotting guards.
 
"For slotting you'll want 2 flute."

Will this work for 416 SS? I'll be cutting 3/16" also.

I bought a 4 flute carbide, thinking SS would be hard to cut and 4 flutes would cut better.

Maybe chip removal is an issue? just guessing, this is all new to me.

Great tips, Thank You.

Mark
 
Last edited:
Oh, don't get me wrong, I love carbide. Carbide pays my bills. But I'm hesitant to recommend it because it is expensive and less tolerant of less-then-perfect conditions, and the productivity improvements from the higher SFM is probably of little value to you.

Yes, chip removal is a concern. Re-cutting chips is a good way to quickly dull an endmill, particularly in stainless steel and particularly with carbide. Avoid the coffee grinder sound of doom (air blast is your friend)...

Personally, I would use carbide because it is stiffer and possibly four flute because it can be fed faster. But I'd be blasting it with coolant to clear chips and my setup is pretty well optimized for running carbide.

Stainless steel is weird about being under fed. There is a chipload per tooth you don't want to fall below (and that value is a moving target depending on the sharpness of the cutter) or it doesn't cut, it smears and work hardens. You'll know if you're in that range because it will be prone to chatter. You're gonna have to feed a four flute pretty hard to avoid that. You would probably be better served with a two flute for slotting stainless.

A good feed range for an 1/8" cutter in stainless is a window between .0002" per tooth and .0008" per tooth.

If your length of cut requires you to stick your cutter out more than about four times the diameter you might be better off with carbide because it is stiffer.
 
Excellent, Thank You Nathan

You've given me a lot of info to work with.

I have some 1/8" 2 flutes, and one 1/8" carbide to use on an old BP round ram. Broke a 2 flute feeding to fast in a brass guard ( my first attempt) so I'll study speed and feed and search ebay for some inexpensive end mills.

Thanks again

Mark
 
Nathan the Machinist said:
Yeah, 1/8" in a 3/16 slot is good. Be aware than cutter deflection and slop in your setup can lead the cutter to plow to the left (relative to the cutter feed direction) and gouge your part. This is a function of rigidity (or lack thereof) and depth of cut. Keep that in mind if you're taking a heavy cut and your cutter is close to your finished wall. This is a common problem when using long skinny cutters such as used when slotting guards.
Click to expand...

I work slow and take shallow cuts, it took me close to 5 hours to turn a pommel nut:o Mind you I did start with stock that was twice the size of what I needed because that was all I had on hand. I still need to get the center point un jammed from my index table that came with the free lathe so I can get the nut mounted do do the cuts. Once I get that sorted out all I will have to do is polish it out and its done.

I can see milling the slot in a guard taking me the better part of 8 hours using the lathe. I want a nice tight fit so I can make a take down fighter and not have to solder and epoxy it together.
 
I would still drill a series of holes to hog off as much material before milling, if using a less than ideal set up.
I use key way cutters a lot which are end mills undersized .001" from 3/16. They allow for a press fit of 3/16 key stock
into a shaft.
 
I don't use carbide on any cutter below 1/2" on my mill currently, even though it's a big old rigid machine (K&T Milwaukee no 2 Vert; 50 taper, 4500lbs), because my spindle speed maxes at 1400 rpm. It simply can't make the necessary SFPM needed to run them adequately, in it's current config, hell any 1/8th cutter for example even at max spindle speed is really too slow, and there are advantages, as Nathan mentions, beyond price, for not running carbide cutters if you can't make the required feeds and speeds.

Most bridgeports and smaller mills, even if they run faster than mine, still don't have the spindle speeds required, and that leads to less than optimal cuts, and cutter life.

Just like the 2 vs 4 flute deal (more has got to be better right?), it seems obvious to go for carbide, since its seemingly higher end, but without the right conditions, you can not only spend more, but actually get worse results, and much lowered cutter life. Milling isn't really intuitive that way, in my experience.


Soon as I find a good deal on one, I'll be mounting a secondary high speed spindle to my mill, specifically for the purpose of being able to run smaller cutters at the necessary speeds. It should ideally give me a highly rigid and accurate platform, with the ability to run tiny cutters the way they need to be, without investing in an expensive new high speed mill.
 
Thanks Javand, Carcara, and Nathan and you too George for posting the question
This is the kind of info you can't find in a book. I guess it's there but who could dig it out when you need it. Not a beginner like me.
Thanks
 
hepclass said:
Unky G , did you ever find out the maker of your lathe?
Click to expand...

Heck I don't even have the book to look the answers up yet;o, but I know from past experience that if you ask the right question there are enough knowledgeable people here willing to share that i would get the answer before I head to the store on Monday to but the end mill:thumbup:

hepclass the maker of the lathe will remain a mystery I guess. The best I can do is that it is European and made sometime in the early to mid 1930s. After I get my mini mill I will start saving to buy a more modern lathe, but I will keep this one and do my best to restore it. I have to do a major overhaul on the auto feed setup, right now it is not working and I had to remove it just so I could move the carriage back and forth.
 
I have always had better results in slotting guards with a slotting saw.I use a mill but it can also be set up on a lathe.
 
unky_gumbi said:
I recently got an old metal lathe, and while I know it isn't the best thing for milling a slot it will be a lot better than drilling a bunch of holes and filing. A lot easier on my elbows too.
Click to expand...

From that, it sounds almost as if you are milling a slot for a hidden tang knife- otherwise you could just drill one hole and rough cut a slot from the top with the bandsaw.

In the case of a hidden tang guard slot, I like to take an undersized cutter- as said above, say 1/8" for a 3/16"ish slot. I mill most of the tang slot pretty fast and rough, a little oversized for the tang thickness, then mill the last 3/32" or so of the bottom of the slot a little bit undersized.

This way, the bulk of the milling goes quickly since I don't have to be finicky about it. Then, after breaking through with the narrower pass(es) at the bottom, if the guard is correctly under sized, it can be driven onto the tang cold for a press fit, filed to fit a bit better if necessary, or even lightly peened on the face to snug up, then ground flat again.

It's all about isolating the fit to the face of the guard, much like the technique for doing it by hand in which the back of the guard slot is filed wider than the tang to make fitup easier.

Not really cutter related advice there, just thought I'd add it since you are getting into milling now.
 
unky_gumbi said:
Heck I don't even have the book to look the answers up yet;o, but I know from past experience that if you ask the right question there are enough knowledgeable people here willing to share that i would get the answer before I head to the store on Monday to but the end mill:thumbup:

hepclass the maker of the lathe will remain a mystery I guess. The best I can do is that it is European and made sometime in the early to mid 1930s. After I get my mini mill I will start saving to buy a more modern lathe, but I will keep this one and do my best to restore it. I have to do a major overhaul on the auto feed setup, right now it is not working and I had to remove it just so I could move the carriage back and forth.
Click to expand...

If you can ID it, more info will help with parts and such.

Try joining the Practical Machinist forum and asking in the antique section, like you say, somebody will know.
 
Thanks for the input Salem, you are right, it's for a through tang knife.


Count I joined a machinist forum when I got the lathe home and that is where I got the info I have on the lathe now. It wasn't till a gentlemen from Holland spoke up that anyone could say anything about it. Most where saying it was homemade or put together from parts.
 
unky_gumbi said:
I am not really sure if you would call it an indexing table or a dividing head. Either way if I can figure out how to get the tapered center out of it with out causing damage I could mount a small vise or chuck to it. I will post some pictures of it tomorrow if I get a chance. It is small but it will do what I need, I think:o It is basicly one of those things that has a plate with a bunch of holes on it and a handle that will key into the holes locking the rotating head in one position. It takes 40 turns of the handle to make one rotation, and the holes in the plates start a 15 on the inner ring, going from there its 20, 22, 24, 26, and 28 holes per ring. Lets say I wanted to make 6 holes around a circle, being that it is a 40:1 ratio I just do a little math. 40/6=6.666666, so full turns and 0.666666 of a turn. .66666*18=12 so 6 turns and 12 holes on the 18 hole index will give me 6 equally spaces holes on my circle. I am sure you knew that already because you knew what tool I was talking about to make knurling wheels:p

No gears with the lathe:( but once I get this table thing sorted out I can make some:thumbup:
Click to expand...


If you need change gears once you figure out what you need, have a look at Boston Gear
You can buy premade gears cheaper than the materials to make them.
http://bostongear.com/litportal/pdfs/P-1482BG_pg05-50.pdf
http://www.bostongear.com/smartcat/...cSrch=-1&from=&vid=15,100,3,0&code=bostongear
As far as getting a taper loose, a hammer and brass punch should usually do it- knock it out from the back.
 
Last edited:
12345678910 said:
If you need change gears once you figure out what you need, have a look at Boston Gear
You can buy premade gears cheaper than the materials to make them.
http://bostongear.com/litportal/pdfs/P-1482BG_pg05-50.pdf
http://www.bostongear.com/smartcat/...cSrch=-1&from=&vid=15,100,3,0&code=bostongear
As far as getting a taper loose, a hammer and brass punch should usually do it- knock it out from the back.
Click to expand...

I got the taper out but I had to make a brass punch first:p I spent most of yesterday working on the dividing head only to find out that it is a little loose:( I got it all setup and mounted on the same carriage that the machinist vise was on and did a few test holes. The thing drifts .16" total deflection, not even close to what I want, a little deflection is OK, but when I was working on something that would have a finished diameter of .5" I have to much wobble. At first I thought it was the way I mounted my part, then the chuck itself. Both were true, so I put a dial indicator against the dividing head itself and gave it 40 turns to make in full revolution. It has a worn bushing or something is out of alignment, but I would have to take it apart to find out for sure, and I just have too much on my plate this week to give it the time, so it will have to wait till next week.
 
Dude---- 8 hours to slot a guard?!?!? :eek:

And people like to poke me about being slow! :eek: :p

Now if you're just talking about to get this all set up and learn the process.... then what they hay, go for it.

But if you mean just a general time to slot a guard, then I would have to SERIOUSLY rethink the validity of the idea.

Obviously Nathan is IMHO the top machining go-to guy on this forum, so I'd read his words carefully. And Salem's post is a great one too.

A 50 cent tip: The difficulty in achieving a visually ridiculously clean fit is exacerbated by surface area. I think that's a fancy way of saying the smaller your guard shoulder is, the smaller the area that you have to get a "perfect" mating fit.

Guys that are cutting their guard shoulder in really deep are (aka making a pencil wide tang), IMHO, doing a double negative. They're creating a weaker tang, and well as increasing the surface area that they have to fit a guard up to.

If you want a quick and dirty machining method that will give you a GREAT fit, with a, let's say 0.250" thick blade. I like to mill the slot to about 0.003 undersize, so 0.247 in this case.

Mill the handle side of the guard stock with a 9/32 endmill, to a depth that is .030" from going all the way through.

Flip the stock over, and mill the face side of the slot with a 7/32 endmill. That leaves you 0.02825 too narrow. Divide by 2, and that means you need to go back and mill another 0.014 per side. IMHO, the best way to do that is to conventionally mill 0.010-0.011 off each side, and then climb mill the remaining couple/few thou.

That will give you an super nice, clean cut that will be right on the money for your desired dimension.

When you go to do a drive on fit... you are only trying to drive on a 0.030" thick area that is just a tad undersize. It will drive on, and be a really nice, tight fit.

Some additional "drive off, sand guard face clean, drive back on, check fit" will be required.


Now of course there are a hundred ways to change up what I typed. Like those endmill sizes aren't absolutes! You can always change that, you just need a dollar store calculator, an abacus, or just be good with numbers to calculate how many thou need to be removed here or there.

The real "key" is that you are fitting a small amount of guard shoulder to guard face, and you are fitting a thin area of the guard rather than the entire thickness.


Just some random thoughts about this thread. :)
 
You must log in or register to reply here.
Back
Top