[tbaker2500]

I don't do a lot of steel work, but I've done some. However, my experiences this afternoon confused me, so I thought I'd ask you experts.

Material: 1018 Cold rolled. Mcmaster, claims rockwell 70B.
Cutter: 1/4" carbide 2fl uncoated square center cutting EM. 1.25" stickout
Cut: 45 thou deep slot, ramped plunge. 5.8ipm 4500rpm, flood coolant. (Conservative setting in G-Wizard.)

I got no more than 1-2 inches in this cut before the EM snapped. Not knowing if the bit was dull to begin with, I put another brand new EM. It made it through the cut (4 inches long), but the cutting edges were completely gone, just fractured off the EM.

Laster investigation shows that this was probably a aluminum cutting carbide. I know for sure it came from McMaster, it was an OSG I think. (At home now)

I proceeded to mill the next path, which is a 1/32 carbide EM, ultratool. It had no problem at 1.8ipm 4500rpm 5 tho DOC. Cutting edge intact after 30 minutes of cutting.

So, was it my cut or the tool? Is an aluminum helix EM unsuitable for steel? Is it that this type of carbide is too brittle? Is carbide too brittle for 1018? If so, why does a 1/2" and a 1/32" work fine?

Thanks for the help guys!
Tom

[underthetire]

Too far stick out on a 1/4", and coated tools work better with steel. You also don't say how your holding it, taper type, run out etc.

[zero_divide]

Gwiz does not care about how long your flute is.
I am guessing its around 0.75" long which is too much for going 45 thou deep.
Try 4200 rpm , 13.0 IPM and 0.017" deep.
This is what you should get.

[tbaker2500]

Too far stick out on a 1/4", and coated tools work better with steel. You also don't say how your holding it, taper type, run out etc.

It was held in a TTS set screw holder, which is an R8. I'd have to check the runout. Both flutes were destroyed.
So both of you were saying that I'm getting serious deflection?

Zero, yes the flutes were .75". In terms of load on the tool, isn't that similar since you are saying 13ipm vs the 5.8ipm I was running?

[zero_divide]

It was held in a TTS set screw holder, which is an R8. I'd have to check the runout. Both flutes were destroyed.
So both of you were saying that I'm getting serious deflection?

Zero, yes the flutes were .75". In terms of load on the tool, isn't that similar since you are saying 13ipm vs the 5.8ipm I was running?

Yes, the load is almost equal, but the problem is: you need to keep some sort of ideal chipload.
And if your endmill is too long, the best choose is to reduce the depth of cut, rather than reducing feedrate.
If chipload is too low, the endmill is not cutting but rubbing, pressure builds up and snap!

Also you need to make sure the endmill is at least general purpose, or designed for steel.
Aluminum-specific endmills are designed to remove ships well, but their core strength is not enouh to cut steel effectively.

IE: I was slotting a36 hot rolled with a hi-performance endmill at 8000rpm and 40 IPM 0.170" deep.
The endmill stuck out 1" and it had 4 flutes.
Had I used general purpose endmill, it would have been impossible to pull out 0.170 cut

[tbaker2500]

Thanks.
My chipload was 0.6 thou. Low, but not in serious rubbing territory. I'm starting to lean in the direction of this being an aluminum geometry EM, and the rake angle was wrong?
Learn something new every day. I have some general purpose EM's coming in Monday, I'll try them out!

[kevinro]

Thanks.
My chipload was 0.6 thou. Low, but not in serious rubbing territory. I'm starting to lean in the direction of this being an aluminum geometry EM, and the rake angle was wrong?
Learn something new every day. I have some general purpose EM's coming in Monday, I'll try them out!

I would be looking for a 4 flute end mill myself. I have had poor performance/luck with most of my 2 flutes on steel. 4 flutes I do much better with.

[dertsap]

So, was it my cut or the tool? Is an aluminum helix EM unsuitable for steel? Is it that this type of carbide is too brittle? Is carbide too brittle for 1018? If so, why does a 1/2" and a 1/32" work fine?

Thanks for the help guys!
Tom

When you say aluminum helix I'm assuming you mean high helix ? if so then it won't work on steel , if it's rated for aluminum then it's the wrong tool for the job . Also a 2 flute is the wrong tool for the job , use a 4 flute , better yet get a coated 4 flute endmill or go one step further and get a coated variable flute . A quality variable with cost a bit more but the life of the tool will equal to at least a couple of standard mills , and they can handle much greater feed and speed rates .
If your using end mills from quality venders then check their websites for their recommended speeds and feeds , even though you can have 5 different brands of the same end mill style it doesn't mean that they can be run at the same rates .

[tbaker2500]

Thanks guys. I'm always learning...
So why is 4fl better on steel? I use 2fl on aluminum for chip clearing, and I can see that's not as important for a cut like this.

[kevinro]

Thanks guys. I'm always learning...
So why is 4fl better on steel? I use 2fl on aluminum for chip clearing, and I can see that's not as important for a cut like this.

High helix works well on soft materials like AL. The material deforms well and follows the countour of the bit. The chips tend to be longer and curled along the bit. They are also thicker from a higher chip load. Steel does not deform as well and requires a smaller chip load. You can make up for the smaller chip load with more flutes. The geometry of the flutes is different.

Sent from my GT-P5113 using Tapatalk HD

[tbaker2500]

Aha! That's a good explanation.

[dertsap]

So why is 4fl better on steel?

rigidity

[dertsap]

High helix works well on soft materials like AL. The material deforms well and follows the countour of the bit. The chips tend to be longer and curled along the bit. They are also thicker from a higher chip load. Steel does not deform as well and requires a smaller chip load. You can make up for the smaller chip load with more flutes. The geometry of the flutes is different.

Sent from my GT-P5113 using Tapatalk HD

high helix have more of a shearing action than a lower helix . There are many brands available that offer high helix steel cutting mills , but they have a beefier geometry than aluminum mills and they are usually 3 flute or more in order to uphold the tools rigidity . In 1018 they work quite well and they tend to have great chip evacuation , they also leave a great finish which is typical with high helix mills . my preference leans towards the variable flute/variable helix mills which tend to be less prone to harmonics and result in less chatter

[tbaker2500]

Well, interesting update. It turns out that a piece of non-1018 worked it's way into my pile.
I had run another cut with a general purpose HSS EM. It removed more of the endmill than of the stock. So I did a quick hammer test, and the piece I was cutting looks hardened, probably tool steel. Oops.

Well, live and learn, I guess.

[tbaker2500]

Heh. It's amazing how well 1018 machines!! :-)

I'm actually pretty amazed that the 1/32" EM survived that encounter with the hardened steel.
I also found the data on the 1/4" EM, it was actually a sgs series 52, aluminum and non-ferrous, low stress work. Boy, I kinda had everything wrong, didn't I?
Thanks for the pointers, guys!

Tom

[nitewatchman]

Try some 12L14.

nitewatchman

[BNX]

Thought I shared since I started one a while back beginning this year. I'm making engine bracket swap kits using 1/4" 1018cr.

Both 4 v. flute from maritool. Both stickout are less than 1" enough to clear my fixture 1/4" bolt head.

3/6" - DOC 0.028", 2000rpm, 10.5ipm
1/4" - DOC 0.045", 2000rpm, 12.8ipm (might tray .068" next time, I backed out).

As someone mention "Rigidity!" Workpiece and fixture plate is everything.

I do stock 2 flute also but they are not my main cutters (slotting/plunging holes in steel and aluminum uses). Less three flute also as I use my tormach 17mm and 25mm center cutters.

4 flute works wonder and they are only $15 at maritools vs $8 for a two flute.

1018cr tigs right up with a wipe.

[tbaker2500]

Thanks BNX! How long do your tools last doing this?

[BNX]

The 1/4" end mill last me for 3 kit and then I move it to the dull pile for r&d purpose.

[tbaker2500]

Thanks, that helps.