PDA

View Full Version : 1018 CRS milling question



dp
01-09-2007, 11:41 PM
I'm trying to clean the hacksawn ends of a 3/4x1.25x2 chunk of 1018 CRS. Regardless of tool choice and a variety of speeds all well researched for S&F, my tools seem only so harden the metal and quickly dull. I've tried with great failure HSS in a fly cutter. Went dull in just seconds. Tried the end of a new end mill with the same results. Tried with the flutes of another end mill and all I get are orange peel surface with bright hardened spots and bits of metal dust when I expect to see chips. What works every time without any precision is a disk sander.

When this has happened with HRS I annealed it and it cut well, but that seems not to work with this stuff. If this were wood I'd be working in the end grain - I don't know what I'm doing wrong but I am consistent. And I'm running out of tooling.

I checked the materials and recommended speeds & feeds and am using a DOC of .005 max and 5 inches/minute so I'm not jamming it by any means which is good because nothing is actually cutting this stuff - the cutters are skidding over the surface and moving molecules from here to there without removing them from the work.

Steve Stas
01-09-2007, 11:49 PM
Sure sounds like it isn't 1018. I've worked with quite a lot of it with just about any tool I have , and it worked fine. Not as nice as some of the other alloys of course, finish-wise, but Ok. 1018 has a little carbon in it, it's possible that it was heated at some point and got hard, but your problems sound like it's a high carbon or alloy and was hardened.

steve

wierdscience
01-10-2007, 12:05 AM
If your hacksaw has cut it,then you should be able to mill it.

What diameter cutter are you using and how fast are you turning it?

J Tiers
01-10-2007, 12:51 AM
What wierd said.....

if it dulls your cutter, almost surely at least one of several things is true.....

1) it ain't 1018

2) you are running WAY too fast.

3) you are not taking a serious cut

I don't know if 1 or 2 is true, but it sounds like 3 is true.....

0.005 DOC and 5 inches per minute is pretty slow. At that you are more-or less just "bothering" the metal with most cutters and mills.

That is a "dusting" cut, and you should with MOST mills be able to crank that along quite fast. I would dust off 5 thou on the side of a piece of 3/8" thick CRS plate at a pretty fast clip using the little Lewis mill (1/4 HP) and running the side or end of a 3/8 end mill at 500 rpm or so (top speed for me).

If you just "bother" the metal, it will respond by heating and dulling your cutter. You may hear it squeaking.

Before you take this as gospel, you better tell us what you are using and cutting with, and cutter rpm, etc.

Paul Alciatore
01-10-2007, 09:59 AM
Sometimes there are "diamond hard" inclusions in even the best, well known alloys. You may have hit one. It happened to me once and the only solution was to get a new piece of stock. It even broke a solid carbide drill.

dp
01-10-2007, 11:10 AM
The mill diameter is .5" and the speed was 950 rpm. The flycutter diameter is .75 and speeds were varied between 300-500 rpm.

I have some 'mystery' metal I've worked with for quite a while and it cuts well with these speeds. The manufacturer's label is still on the steel and it is pretty definitely 1018. I have a dozen pieces of it in various shapes and lengths. The spark pattern from a grinder test does verify it is carbon steel. The hacksaw went through it nicely - not as fast as with the steel I get at Home Depot, but I don't know what kind of steel that stuff is. I have some other steel that the hacksaw just glides over - barely leaves a mark. I have to use a wheel to cut that stuff.

Mcgyver
01-10-2007, 12:28 PM
too fast, cs*4/dia = around 600 rpm. this is the theoretical max beyond which cutter wear goes through the roof, there is nothing wrong with running slower and it will increase cutting life

edit, realized if you are taking a cutting speed of 120, your speed is ok, imo 80 is a safer number. if that doesn't fix it, and its 1018, i'm stumped - presumably its a reasonably sharp cutter to start with?

Mike W
01-10-2007, 01:40 PM
I once picked up a bar of hot rolled from my usual steel supplier. I went to center punch it and the point flattened out. A drill wouldn't touch it.

J Tiers
01-10-2007, 01:51 PM
The way I see it, if you are running that RPM and 5 inches per minute at 0.005 DOC, you have a low chip load.

You have an advance rate of 5 thou per revolution

with a 4flute cutter, that is a chip of 0.0012 thickness, x 0.005 DOC.


I would have NO difficulty suggesting a doubling of the feed, and more DOC if you need it.

Hand crank it and see what the cutter load feels like. I'm betting you won't notice it at that slow rate.

If the cutter isn't cutting something serious in the way of a chip, especially at higher speeds, it will get dulled. They like to cut, not rub.

Either speed up the feed, slow the cutter, or increase the DOC AND slow the cutter....

Check the surface where your cutter dulled itself, and see if the hacksaw or file has THAT much more trouble with it.... You'd expect a bit from work-hardening, but not much with 1018.

I don't HAVE power feed (I'll probably add it someday) so I hand crank it, and believe me, it is an education on speeds to do that..... you can FEEL what the cutting is like (unless you have a really big honker of a machine).

dp
01-10-2007, 02:55 PM
Because the intent was to make a light cut to clean up after the hacksaw, I tried a shallow doc. The cutter walked right up on top of the work and pretty much stayed there even when increasing the cut to .015. The endmilll was brand spanky new but needs dressing now.

The flycutter uses a round HSS tool. The first try was with a standard round nose form. That dulled in a few thumps. Then I gave it a 15 degree rake and that too dulled in a few thumps.

The part is ruined now for what I'd like it to have been so I tried a deeper cut with another endmill and got it, but the surface of the work looks like it had been dragged down the street. No chips are forming - only dust. It's like the material is made from some kind of granite :)

This is supposed to be a carriage stop when it's done but at the tool burn rate I could have bought one!

I might look around from some 12L14 or what ever is equivalent and legal.

wmgeorge
01-10-2007, 03:45 PM
Because the intent was to make a light cut to clean up after the hacksaw, I tried a shallow doc. The cutter walked right up on top of the work and pretty much stayed there even when increasing the cut to .015. The endmilll was brand spanky new but needs dressing now.

The flycutter uses a round HSS tool. The first try was with a standard round nose form. That dulled in a few thumps. Then I gave it a 15 degree rake and that too dulled in a few thumps.

The part is ruined now for what I'd like it to have been so I tried a deeper cut with another endmill and got it, but the surface of the work looks like it had been dragged down the street. No chips are forming - only dust. It's like the material is made from some kind of granite :)

This is supposed to be a carriage stop when it's done but at the tool burn rate I could have bought one!

I might look around from some 12L14 or what ever is equivalent and legal.

What are you using for a machine? You said one time it you were using a milling cutter. And then adjusting the rake. It is possible that you have something other than CRS, or it could be a bad piece of steel?
If you have a light machine or one with loose gibs or both, could be you are just riding over the top of what you are trying to cut, especially if you are taking shallow cuts with a not so sharp cutter.

J Tiers
01-10-2007, 05:51 PM
HEY THERE>>>>>>>>>>>>>>>>>>


I see a clue........



I tried a shallow doc. The cutter walked right up on top of the work and pretty much stayed there even when increasing the cut to .015. The endmilll was brand spanky new but needs dressing now.

Is the cutter turning in a direction to roll over the work? That is "climb milling" and most regular and worn out machines cannot do it successully.

Or is it turning in a direction so that the edge is moving AGAINST the feed?

It should be doing the latter.....

DO NOT CLIMB MILL

If your mill would successfully climb mill, you would already know that..................

JCHannum
01-10-2007, 06:21 PM
There is something strange here. You mention having had the same problem with HRS as well, only that it was corrected after annealing.

Work hardening should not be a problem with either material, and a simple milling or face cut should remove a minimal amount of material with no problem. When faced with a similar cut, I usually put the part in the vise and skin it off with whatever mill or flycutter is at hand with little regard to speed or feed, just what feels and sounds right.

Since you are using a fly cutter, I assume you are using the end of the end mill. What is the material of the mill, and who is manufacturer? Can you post a photo of your set-up? That might help us see something we are missing.

pcarpenter
01-10-2007, 06:29 PM
The "walking up" on the work sparked another thought.....but I don't want to insult your intelligence either. This isn't a case of perhaps engaging back gear (which usually reverses a mill spindle) and forgetting to start the motor running the other direction? Turning the cutter in the wrong direction will certainly let it ride up on the work...and dull it very quickly while not cutting the metal.

Paul

dp
01-10-2007, 07:40 PM
The equipment is lamentably a 3 in one Grizzly. I'll post some pix later of the setup and tools, and of the earlier successful work. All the tools are new and (were) sharp. The end mill I tried were purchased either at Grizzly or Harbor Fright. The fly cutter is shop made.