# Hogging steel question



## Bill Kahn (Mar 18, 2018)

I have chowdered up several end mills now.  Probably time to actually learn something...

I am using a PM25 mill.  I have a 1" cube of cold rolled steel.  Need to take a 1/2" x 1/2" bite out of it.  (End up with a fat "L" shape).  Being a beginner I set up my 3/4" hogging carbide end mill for 1/2" down and 1/2" in.  I mean, like how hard can this be?  Just go slow and zip-po bang-go I have my bite taken.

Well, as you all can imagine, that doesn't work.  A few more naive tries and I am reduced to having to ask.

How best to make this cut?  What end mill? What rpm? What feed rate? Do I go down to the 1/2" depth and then across a bit at a time?  Or across 1/2" and then down a bit at a time?  Should I do both at the same time? How much is "a bit?"  If I can't do 1/2" cuts, should I be able to do .1"? .01"? As I actually have about 20 such bites to take if each takes 50 slow runs, it is doable.  But would prefer to have some sense there is not a factor of 10 faster way to do it. (Factor of 2 or 3 inefficiency is not problem--I'm just a hobbiest.  Time is not money.)

"In theory there is no difference between theory and practice.  In practice there is." Once I have my bite no one (I mean other than on this board) will see it was actually hard.  The idea is so simple.  Thanks for helping me figure out how to make in practice.

-Bill


----------



## T Bredehoft (Mar 18, 2018)

To remove a cut 1/2 wide and 1/2 deep on my PM25, I would use a rough cutting 3/8 or 1/2" end mill. I'd make a pass .050 deep and .240 wide, nine times. Then I'd put in a 4 flute end mill (not a rougher) and take the .050 out of the bottom, then the .010 out of the side. 
What you are attempting would probably pull the part out of the best vice on a Kearny & Trucker No. 4 (heavy duty) Mill.

Speed would vary, HSS or Carbide, feed rate no more than .002 per flute.


----------



## Old junk (Mar 18, 2018)

Agree with T you can't go at it 1/2 inch at a pass.


----------



## BFHammer (Mar 18, 2018)

I think Tom gave good advice.  I have a PM932 and would approach that cut it steel much the same as Tom.  
If you’ve tried to dig (or hog as the case may be) in on that full cut - you might want to double check the tram on your mill head now. Don’t ask me how i know...


----------



## wendell (Mar 18, 2018)

Some layout dye, a vertical bandsaw and a 4 flute HSS endmill.


----------



## Bob Korves (Mar 18, 2018)

wendell said:


> Some layout dye, a vertical bandsaw and a 4 flute HSS endmill.


If you have a vertical band saw.  If not, hack saw roughing cuts would probably do the job just about as fast as a bunch of cuts with the mill, and you would save wear on the end mill and also get some exercise...


----------



## woodchucker (Mar 18, 2018)

With that little mill you cannot possibly take that much in one bite as said.
I like to use roughing end mills on my mill. It would take me 4 or more passes depending on the material.


----------



## Jimsehr (Mar 18, 2018)

I think the fastest way to remove stock is with a drill. I would drill down with a 7/16 drill two places then use an end mill.


----------



## mikey (Mar 18, 2018)

Bill, your question is something we all struggle with in the beginning. Just so you know, a 1/2" deep profiling cut is a big cut on a small mill but not that ambitious with the right feed, speed and end mill.

For profiling cuts in steel, it is better to use a 3-4 flute roughing end mill to debulk the stock, then take a finish cut with a finishing end mill to clean it up. For slotting cuts, a 2-3 flute clears chips better. I prefer coarse pitch roughing end mills for slotting and fine pitch for profiling; again, this is about chip clearance. Big chips can be ejected from a slot easier than fine ones, while in profiling cuts fine chips just fall out of the way so are not a problem.

If you think about it, the more cutter surface involved in the cut, the slower you have to go, right? There are two kinds of "depth" we're concerned with. Have a look at this diagram:




One is the *Axial* depth; this is the *length* of the end mill surface in contact with the work. Maximum Axial depth is about 1.5 times the diameter of the end mill. The second depth is the *Radial* depth of cut; this is *how much of the cutter is buried in the cut*.

Speeds and feeds will vary with the type of end mill, roughing or finishing, the material and the radial depth of cut. How do you know what speed to use? *Look at the guidelines attached*. Pick an axial depth of cut and limit it to 1-1.5 times the OD of the cutter at most; less is better here. Then decide how much of a radial depth of cut you think you want to bite off at a time (personally, I try not to go beyond 1/4 the cutter OD on a small milling machine). Then look at the table to get the recommended speed. If you don't have variable speed then just get close, and a bit slower is better than faster. Feeds on a manual machine is more difficult unless you have a DRO. The answer to that is to feed manually so that you feel a slight resistance to the feed. Do not try to push the cutter; let it cut. The slight resistance to feed that you feel allows the leading edge of the cutter to cut continuously without deflecting the cutter excessively. Crude, yes, but it is what we have.

This all sounds more difficult that it is. For your 1/2" X 1/2" cut in mild steel with a 3/4" finishing end mill, you can use the 1/2" axial depth. Say we wish to limit our radial depth of cut to 1/4 the cutter OD (0.1875"). The recommended speed is 140 SFM so set your speed at or near 713 rpm (140 X 3.82 / 0.75 = 713 rpm) and conventional cut the material so that you feel a slight positive resistance to the feed. Repeat as needed.

Again, note that speeds and feeds are slightly faster with roughing end mills. It is always a good idea to debulk the work with a band saw as Bob said, then use roughers to further debulk the work, then use a finishing end mill to clean it all up. 

Hope this helps.


----------



## P. Waller (Mar 19, 2018)

Climbing?


----------



## Asm109 (Mar 19, 2018)

P. Waller said:


> Climbing?



On the last finishing pass yes. Otherwise conventional.


----------



## T Bredehoft (Mar 19, 2018)

Finishing pass, no more than .005 on the side, climb milling. Conventional milling tends to pack chips onto the surface.


----------



## P. Waller (Mar 20, 2018)

If the machine will allow it always climb. On a manual machine this is often not practical so do what works best.


----------



## wrmiller (Mar 20, 2018)

I never used a end mill that large on my PM25. She just won't take it, i.e., not rigid enough. I never used anything larger than a 3/8" end mill in my machine, and if I had to do what you are doing, I'd use a rougher to reduce the loading on the mill for the initial passes. Then a four-flute for the finish passes.

The PM25 is a great machine. If you don't try to overpower it. 

EDIT: Using a 3/8" rougher, I'd take half-width passes with it. But that's just me, as I don't like to push my machines too hard and wear them out prematurely.


----------



## chips&more (Mar 20, 2018)

You should have a VERY ridged machine/set-up when using a Carbide end mill. Or you will just be asking for trouble. And probably destroy the Carbide cutting edges. I would not buy Carbide end mills. Instead, if you want something other than regular HSS, I would take a look at Cobalt. I have a 8 flute 1/2” Cobalt that I grab first and is still good and sharp after several years!!! As for roughing, maybe try one of the corn cob end mill cutters. And don’t try any climb milling unless it’s a VERY light cut and everything is tight. Or it could be unsafe with your type of milling machine…Good Luck & be SAFE...Dave.


----------



## 12bolts (Mar 21, 2018)

I would just use a slitting saw and keep the resulting waste for another purpose apart from swarf

Cheers Phil


----------



## Bill Kahn (Mar 21, 2018)

12bolts said:


> I would just use a slitting saw and keep the resulting waste for another purpose apart from swarf
> 
> Cheers Phil


Have you (well, does anyone) have any specific recommendation for a slitting blade ( and arbor)?  How many tpi? What material? Thickness?  Vendor?  Sensible price?  That is good for steel?  

Thanks. 

-Bill


----------



## Bob Korves (Mar 21, 2018)

Bill Kahn said:


> Have you (well, does anyone) have any specific recommendation for a slitting blade ( and arbor)?  How many tpi? What material? Thickness?  Vendor?  Sensible price?  That is good for steel?
> 
> Thanks.
> 
> -Bill


There are lots of different slitting saws and arbors.  Pick one that will do the job at hand and perhaps also serve for other jobs in your shop.  There are too many variations in machines, projects, and preferences to give a good answer to your question beyond "there are plenty of useful tools out there to do what you want to do."  With slitting saws, do your homework and learn about speeds and feeds with the purpose of achieving a reasonable chip load per tooth, which is important.


----------



## T Bredehoft (Mar 21, 2018)

I've found that my PM25 has problems going slow enough to run a 2 1/2" slitting saw. there's not enough torque to carry it through the cut, I have to hand feed it about .001 per rev. if that much. Otherwise it catches and stalls. That's at whatever its slowest speed is. Any faster is too many surface feet per minute.


----------



## Bill Kahn (Mar 26, 2018)

12bolts said:


> I would just use a slitting saw and keep the resulting waste for another purpose apart from swarf
> 
> Cheers Phil


OP here.  Thank you.  It is a bit of a pain given my HF 4x6, but some jury rig part holding and got the bulk of the notch cut out horizontally and finished up vertically by hand.  In terms of speed, this is the way to go.

But, in terms of easy, figured out a better way.  Using this https://www.ebay.com/itm/5-8-Solid-...e=STRK:MEBIDX:IT&_trksid=p2057872.m2749.l2649 end mill, with .5" in and .15" down at 2000rpm and the slowest x-feed my PM25 could go (about .003"/sec (.2"/min)) just let her run.  Way slow.  But I can putter around the shop while it makes the dust-like sharf.  Seems to work both directions (at that speed I guess makes sense)).  And, yes, I tried a full .5" depth and even at that slow speed, would not work.

Oh, and thanks to an earlier poster on needing to retram.  Yup.  Stalling the machine and cracking a 3/4" carbide end mill. (Yes, I wear eye protection if any machine is running (or I am exerting force)) got my attention.  And when I went to check, the tram was .01" out over 18".  Now is back to .001" over 18".

Thanks for all the advice.

-Bill


----------



## umahunter (Mar 27, 2018)

Don't feel bad I thought the exact same way when I got a mill. then I got a crash course in mill weight horsepower  endmills speeds feeds depth of cut endmill types hss cobalt carbide roughing  finishing  2 flute 4 flute 6 flute and on and on. lol I've watched  a lot of videos asked a ton of questions. the folks on here are very knowledgeable and helpful and I love learning from others experiences especially when it saves me money. I'm sure you realized burning through a couple endmills is exspensive


----------

