Hogging steel question

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

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.

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

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...

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

wendell said:

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

Click to expand...

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...

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.

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.

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.

Climbing?