Cutting Steel - what am I doing wrong?

CNC Machines Shapeoko 5 Pro
1

So our shop purchased a 5 pro w/vfd spindle about a month ago. We bought it to cut some 1/8" steel plate so we could make brackets. However, coming from an SO3 at home that only has seen wood & plastic, so cutting metal is a new beast. I’m busting bits like crazy on this thing.

The part I have is approx 9"x6". The plate steel grade is unknown; it’s been powdercoated & is magnetic is all I can tell you. It’s 0.11" thick according to my calipers.

I’ve been getting F&S rates from FSWizard, but I think it’s WAY off on what I’m doing. Sometimes it’ll give me crazy results (like 0.1094" doc… that just sounds way too deep; change a setting and it’ll say 0.0294" doc. Other times it sounds “good” but will take 3+ hrs for one part).

All 1/16" bits were at 16k, 0.002 doc, 8 ipm. 4 flute. No coatings.
The 1/8" bit was at 9500rpm, 0.059 doc, and 18 ipm. 4 flute. No coatings.

Bits were ordered from Grainger: No specs are available other than what’s on their site.
Carbide, 4 Flute, Square End Mill - 19LE90|206-001020 - Grainger

[WIDIA HANITA, Carbide, 4 Flute, Square End Mill - 48HD91|I4S0125T050R - Grainger] (Whoops, we couldn't find that.)

Boss is thinking we bought a $5000 paperweight at this point. What am I doing wrong?

Here’s the history; sorry, I’m wordy, but smarter people might be entertained by my plight.

Bit 1’s life was short; I followed the f&s settings from FSWizard, and it bore a hole right where it started and the bit lasted about a second until it snapped. 0 inches of travel.

Bit 2’s life was much better; It was doing some pocketing out some holes for a carriage bolt. Worked great until it hit the hole where Bit 1 died. I think there was some carbide fragment left in the hole, and it took all 4 teeth off of bit 2. It finished the hole, chattering like crazy, and died about 3 passes around the perimeter of the part. It turned into a ball mill. Maybe 100 inches of travel on this bit. No curls of metal; looks like iron powder.

Bit 3. It cut a long time. After about 2.5 hrs of going around the perimeter, I went home. A coworker texted me later and said it started chattering and snapped. He hit the stop button and I checked it out this morning. It was in 5 chunks laying on the steel. I can see where it started dulling and was no longer a nice shiny groove. Only a guess but I’m thinking 1000 inches of travel. Still never made it through the metal. Maybe 3/4 the way through. Ain’t going to be good, since I need to cut 10 of these pieces. More iron powder.

Bit 4… After reading a million forum posts over the weekend, I stepped up to a 1/8" bit. Slowed the speed down and increased the doc according to FSWizard. My thinking is I was burning up the bits, losing temper in the teeth and making them break. I got the opposite reaction with this bit. It bore into the metal, chewed its way about an inch, over torqued the spindle, decided to move the gantry using the bit to steer, and ran across the metal making a nice furrow before it sent shrapnel. At least these bit pieces are easier to find.

2

I think you need to determine what grade steel you are trying to mill?

1 Like
3

I’d love to, but these are leftover steel plates (36"x12") from the back of vehicle divider partitions from an aftermarket partition company. We have about 3 dozen of these around the shop. We can drill through them with a power drill fairly easily. No curls, but I get chips with a regular HSS drill bit.

4

Look for posts by Vince, he’s done some good steel work on an older machine. I imagine there are plenty of lessons to be learned from his posts.
Example: Steel plate - sink or swim

2 Likes
5

Sorry, I can’t help you much as I have only cut wood on my S5 Pro. I know the guys cut aluminum with O flute bits and crank up the feeds and speeds. It’s possible that the bit speed is too fast using 4 flute bits. I’m used to seeing these types bits in a milling machines and much slower RPM’s.

Perhaps send Winston a message and he can help you out.

6

Indeed! Not knowing the grade of material is a crapshoot.

Looking at your numbers, you’re chiploads are 0.0001" and 0.0005" respectively.

I notice FSWizard seems to recommend DOC & WOC for HSM. Try swapping them.
I.e. you’re getting a 0.1094" DOC, the WOC is probably really small, like 0.003"
Try DOC 0.003" and WOC about half the dia. of the cutter or just a bit smaller.
i.e. end milling rather than side milling.

What cutting strategy are you using? And which CAM software?
I don’t like CC for cutting metal. Straight plunges are rough on the tool, and CC’s ramping is crude. Fine for wood & plastic, Meh/OK for soft metal.

I have the privilage of Siemens NX (I work for Siemens). So I use that for most of my metal cutting. I haven’t tried any steel, but I did cut some counterbored holes in a cast iron machine vise.

I have the HDM, I think the most rigid machine of this lot, and I still baby it when cutting metal.
With the steppers energized, I can move the axes by hand if I really lean on them. A commercial grade machine for cutting metal, you would not be able to do this.

Hopefully Winston chimes in. I believe he’s had some luck with harder metals.

2 Likes
7

Thanks @HuristicBishop. I read through that sink or swim posts and that’s why I’m banging my head. It sounds like I’m in the ballpark with his numbers, but he’s using a 1/4" roughing bit where mine are 1/8" or 1/16" finishing bits.

I looked at the datasheet from the 1/8" bit as I know what company makes those bits. It’s funny because it shows numbers that more than what I typed in, and it was the most spectacular failure of them all.

Widia says 13k rpm. I did 10k.
Widia says 34 ipm. I did 18 ipm.
Widia says 0.062 doc. I did 0.05.

FSWiz says 9495 rpm/18.83 ipm,0.0589 doc/0.125woc because I’m technically slotting (through cuts to punch out pieces vs milling and carving).

I’m using CC, as the boss doesn’t want to spend more to get better software until I can show that it cuts steel.

8

The SO5 will definitely cut steel. I look closely at the cutting force number from FSWizard. I like to see numbers in the ~2 lb (~1kg) range with small cutters. So with slotting, reduce the depth of cut. And lubricant (eg. WD40) doesn’t hurt.
BR

1 Like
9

A question and a couple random suggestions in no particular order:

  • How are you generating your gcode? Do you know if you’re using conventional or climb cutting?

  • You should try coated endmills. They don’t cost much more and every marginal advantage you can get will help.

  • Stubby (short flute) cutters will help if you’re cutting thin plate or doing shallow cuts. Less flute length = stronger tool overall. Example: Stub End Mills | 2 Flute & 4 Flute | Stub Altin Coated & Uncoated

  • You should be using compressed air to get chips out of the cutting zone ASAP. Not sure if you have that on the machine, but letting the cutter grind through previously cut chips will drastically shorten the bit’s life.

  • If you’re cutting a deep slot (more than ~1.5-2x the bit’s diameter), that can make it difficult for chips to be flung away from the cutting zone. It might take a little longer, but if you cut a wider slot at the top of the material for even just 0.04" (let the cutter take 2 passes), the remaining 0.07" would go much better.

  • It wouldn’t hurt to get a small plate of a known steel alloy just to try.

  • The machinability of steel can vary wildly, even for just “carbon steel”. See: https://www.carbidedepot.com/formulas-machinability.htm. Even if a drill press can make a clean hole in it, there’s no guarantee it will cut okay on a milling machine. When you drill a hole, you’re often using a bit of cutting or tapping fluid which can help a lot. But that’s not something you can do over an MDF spoilboard. But the point is, cutting “mystery metal” is the single worst thing working against you. It wouldn’t be fair to declare the machine a paperweight due to your boss’s ignorance. There’s just too much unknown.

  • I haven’t done it on the S5 platform yet, but I’ve felt that 3/32" was a good sweet spot in terms of endmill size. Lets you make bigger chips than the 1/16" bit, lets you run at a higher RPM than a 1/8" bit (the VFD torque curve prefers this).

  • If you get bits with a corner radius, it can help improve their longevity. Even a couple thousandths of an inch will help. The corner is usually the first thing to chip, and then things to downhill rapidly from there. Example: Corner Radius End Mills. These are what I used when I profiled an O1 tool steel blank on a Nomad 883 Pro way back in the day. ( https://youtu.be/G5TYla5x-Nk?si=bj1XyYbmnOzzk7CL )

6 Likes
10

Just did a quick check on FSWizard. Force is 8.39 lbs on .0589 doc. It’s not until I get down to a 0.009 that it gets into the 2 lb area. That’s with the 1/8" bit.

@cajbr1 - what do you consider small cutters? If 2lbs is good for a 1/8", what about a 1/16"? Or (as winston suggests, 3/32")?

I’ve told my coworkers that cutting steel is like baking a cake. If you don’t get it just right, the cake turns out horrible. Wood is so much more forgiving…

2 Likes
11

The facilities guy is supposed to be plumbing in the airline for the air assist. I’m not going to try again until that gets put in.

Another question: How are people doing oiling above an MDF table? I see a lot of photos of people misting, but never get a wide enough shot to see if it’s on MDF, or if they replaced the table with a giant kiddie pool and 30 gallons of oil.

12

For mist cooling I got a commercial sheet pan and drilled holes that line up with the T-tracks. I mount that between the work piece and the MDF slats. Mind you I try to keep the mister set to only put out enough fluid that it evaporates from the heat of the cut and doesn’t pool. However if it does the liquid will got through the holes of the sheet pan and into the T-tracks and not onto the MDF. Mind you I have only cut aluminum and brass with this setup, but its worked quite well. If you only plan on cutting metal with your S5 you should look into getting an aluminum fixture plat to replace the MD5 slats.

3 Likes
13

You can download and run Fusion 360 for free, as long as you’re not using it for commercial purposes. Here, you’d be using it to test out tool paths, so I believe that qualifies. And, if not, you can always do the 30-day free trial.

Winston, as always, has some great advice, but I’d add that you really want adaptive toolpaths with entry ramping. F360 can give you those. Slotting is hard on tools.

.

14

In my experience, cutting force is the limit when cutting metals. These machines are made of Aluminum, after all. FSWizard works well, but it assumes a “standard” end mill length and stickout(unless you override). If you use a cut length 3x diameter, for instance, the feed will be reduced. Try it (I was reminded yesterday when I cut 6061 with a Carbide 1/16"). My strategy for profiling thin plates is a continuous ramp with a maximum stepdown limit in Fusion 360. No plunge. Follow the cut with a vacuum and spray some lube.
BR

15

I’ve used Fusion a while back, but given that this is a gov’t-owned laptop I’ll need to work on getting approval for Fusion to be installed. The IT guy didn’t seem to care much about having to install CC given that it’s free. I’ve used Aspire before at home, and am familiar with ramping and doing 3d carving.

Thanks everyone for your ideas! I knew moving from wood to metal was going to be a challenge. Hopefully once I get the air line put in and stand by with a can of cutting oil it’ll go better.

2 Likes
16

I forgot to mention, look at posts from RichCournoyer as well. He’s been doing work in various steels since the early days.

2 Likes
17

I had some “free” time this morning (while on a conference call) to get in and try again. I’d like to thank all of you because I finally got my first piece! Takes 30 minutes to cut, and 15 minutes to bend, sand, finish and paint, but the boss is happy that he didn’t buy a paperweight. A few tweaks and I think it’s a winner! Thanks everyone!

9 Likes
18

That’s awesome to hear! It will only get better as you tool up and get more familiar with everything :beers:

Good job sticking with it through the stress and headache :slightly_smiling_face:

19

@jdezur

What parameters did you change that got the results you were looking for?

We appreciate the the fact you got your project moving. It would be good info for other folks and help us all out if you shared what you did to get it done that was different from your original post?

:face_with_monocle:

1 Like
20

Here’s my experience, Altin coated endmill was the solution for me.

2 Likes