Anyone ever tried cutting cold rolled steel

[tpulley]

I know the shark hd4 says it will cut aluminum and mild metals. I have two pieces of 1/2 x 1/2 x 36" square stock. I wanted to mill down about .125 on both ends so I can then drill and tap them for carbide inserts. I have been given approx 6 dozen carbide inserts of three sizes. I am trying to make my own wood lathe tools.

Anyone tried cutting mild steel? I will be using a 1/4 carbide end mill.

[SteveM]

I think you would be better off taking the 2 pieces to a machine shop to have that done for you.
I am not sure, but with trying to cut steel, I believe you need to keep the cutter lubricated with some sort of oil or cutting fluid.
That would really make a big mess on your table surface.

[Kayvon]

Would a grinder be able to knock that out? That might be a simpler option, provided you have access to one.

[tpulley]

I had thought about trying to grind it, I just don't think it would be as flat as it should be.

[Rando]

What's your spindle situation? Steel typically wants Very slow spindle RPMs. What kind, size, etc., bits do you intend to use, and can you provide a drawing for the area/shape you want machined? What is the requirement for flatness in that area? What method for holding the workpiece being machined do you have available?

Those are some of the questions that go into answering your question of whether its technically feasible.

Whether it makes sense is down to how much you value your time versus the cost of purchased tool holders...and the safety/reliability issues if any.

One thing to caution...steel chips are SHARP, and because of the flexy nature of our sharks, the resulting chips will be tiny...and thus are easy to spread far and wide throughout your home. So, beware

If you can get that information, a numerical solution can be found. Whether the machine can perform those cuts is another thing.

Regards,

Thom

[cjablonski]

Easy hopeful Rando would reply. A guru at metalworking for sure

[sharkcutup]

how about a rough grind first then finish with machine!

Sharkcutup

[Rando]

Easy hopeful Rando would reply. A guru at metalworking for sure

<blush> Nah, man, I'm still new to this stuff too.

Cutting metal on the Sharks deal with all the normal stuff that woodworkers have to, and in some cases it's easier. Where woodworkers come up with cool workholding solutions, we apply 50# hunks of tool steel to the problem . We have vises and parallels where woodworking uses spoil boards and clamps. The concepts are the same, though: don't let it move, and stay out of the way. Same for the movement limitations and GCode actions of the controller. Bit materials and geometries are all in the same family, with variations depending on the particular thing you're trying to achieve. Woodworking calls for a vacuum, whereas metal tends to do better with a chip-blower. I'm somewhat sadistic to all my machines in how I program them, so the fact that I do all that strange toolpath-automation stuff is really just me being my true, cruel self . But, the concepts--and thus the solutions are shared among them.

The main difference with metal all comes down to heat. Cutting metal generates a lot more heat than the same cut in wood. Where that heat goes, and whether it causes a problem, is determined by the cut parameters. Thankfully, due to that whole "industrial revolution" thing, the physics (aka math) behind the cuts has been argued about for a century. Once you start to treat cut parameters like you do your design's vectors and XY coordinates, in that you hypothesize, test, observe, record, adjust, and repeat as necessary, that's when working with metal becomes feasible, and not a worrisome encounter.

So nope, not a guru, in neither the American sense (someone more highly-skilled than others) nor the Hindu sense (a spiritual teacher who gets the initiate started on the path, but does not guide to a destination). My use of metal is really down to being an EE and wanting to make electrical/electronic thingies. A wooden case will look good, but a polished, machined aluminum one will inspire lust. Not merely like, but full-on LUST. That's what I'm looking for in my products, shameful though that might be . Plus, I'm into dimensional accuracy; it's a thing .

Cheers on this gorgeous Seattle Saturday morning!

Thom

[tpulley]

I am using the nextwave water cooled spindle. 1/4 carbide 4 flute cutters. I wouldn't need to be in a hurry so depth of a pass isn't a huge deal. its a profile cut, I wasn't thinking of programming anything in vectric, just using the pendant, lock it down in a vise, set the spindle speed line up the cutter and let er go.

It seems logical if it would do mild aluminum and etc it should be able to handle mild steel. Especially if not pushing the chip envelope. . I am thinking I am gonna give it a whirl. I am not expecting any major catastrophes... Expecting...

Looks to me that by the charts 3500 rpm at 28 ipm ought to do it.

http://www.sgstool.com/PDF-speedfeeds/S ... eds-GP.pdf

[Rando]

tpulley:

Cool; thanks for the information. Now we can really start to look at the numbers .

Just remember: the chart-supplied numbers are for machines of substantial rigidity. Using just that table, you don't really have a way to understand the torque and power that a cut will produce, as you choose those numbers. Even a moderate amount of torque on the HDs leads to diving and jutter and jumping.

"Mild" is of course relative. On the Brinell hardness scale (https://en.wikipedia.org/wiki/Brinell_scale), 1040 steel is 187, while 6061-T651 Al is 95. So, the mild steel is actually fully twice as hard, for machining purposes, compared to the aluminum.

On our HDs, cuts like this should ONLY be made in the "pull" direction. That is, the gantry moves in the direction away from the spindle, dragging it across the material, versus forcing it into the material. If you need a back-and-forth cutting motion, then along the gantry width is the best choice. This will help immensely with the success of these cuts.

Remember that, regardless of your depth-of-cut and stepover, if the first cut is a slot, you'll need to use full-slotting F&S, which are much slower than a typical profile cut.

On our machines, one of the things you'll notice is that the exact height-location of the cut surface top is directly related to how much deflection occurs, which is directly related to how "hard" the cut is. How "hard" the cut is varies not only when the cutter changes direction, but also as the cutter enters and leaves the material. What you'll notice by sight and sound is that, there will be odd tool markings on the far end of the cut, right at the moment that the force starts to go down, as the bit comes off the edge of the material. I wish I had a technique to cancel it out, but it's perceptible even on 0.002" deep finishing cuts in aluminum. So, don't freak out if you see that....

3500RPM @ 28IPM only gets you 229 SFM, but 1020 steel (low-carbon, cold-drawn, low-temp relieved) wants 345 SFM. I'd recommend going with 5000 RPM @ 28IPM, for 327 SFM, though myself I'd probably do something more like 4000 RPM and 18 IPM. Note that plunge rates are in the 1.5-1.8 IPPM range, so be wary there. That gives about 1/3 the chipload recommended, so it's a nice easy cut. I used 0.05" DOC and 0.01" step over. If you haven't already, and your VFD has a setting for "low RPM (power/current) boost", you might want to increase it for a little more ability to push through the cut at that 4k RPM.

As a first test, I'd run one at 0.025" DOC and 0.008" step over. If that works, move up to the other, increasing stepover slightly first, then depth, then stepover, etc.

Full slotting F&S for 0.025" DOC are 4500 RPM, 8.1 IPM and 2.0 IPPM (plunge). That seems reasonable, but I could also see it going horribly wrong.

And finally, are you familiar with the "color" test of the chips? (a good chip-reading article is here: http://www.mmsonline.com/articles/read-your-chips) There are cutting conditions that inject so much heat into the cutter that it loses its temper, goes dull and then just starts rubbing. Also, chip re-cutting in steel is a far bigger issue than in aluminum. Steel work-hardens to a much greater degree. When those hardened-steel chips get lodged between the cutter and stock, it is very common to chip the cutting edge. For you, that might mean rigging up the back-end of the shop-vac for a temporary chip-blower.

While you're doing this, stand by with a squeeze or spray bottle of some sort with light motor or machining oil. I wouldn't worry about flooding the cuts, but having misted-drops of lubricant on the surface and the bit can make cuts like this a lot safer. In the real-world, after all, most cuts in steel are done with flood cooling being poured on a rate of multiple gallons per minute. Nowadays, that coolant is delivered by a high-pressure stream that goes through the length of the bit itself: through-spindle cooling they call it. Flood cooling at that volume might be an issue on our machines .

I'm excited for you; I've stayed away from steel on my machine, so I'm interested to see how it comes out. You're a trailblazer, man!

Regards,

Thom