Speeds and Feed and DOC

[ctwo]

Seems every time I use my CNC I break an endmill. Only the small ones.

I have 12L14 round that I wanted to run a 3/16, 4-flute, HSS endmill to trace around a shape, so it's making a channel and I got my mister on and manually brushing. I'm running 3ipm, 3500 rpm, and take a 5 thou DOC. Then again 10 thou. It's taking too long so I go for 20 thou and it snaps off.

The online calculators seem to want ME to know the chip load. Isn't 1 thou a good place to start here? I think I was about 1/4 of that. But then DOC would seem to matter DOC, which is not generally addressed on the calculators. Maybe it's less than half or 1/3 the cutter diameter is where it might snap. I know channels are hard.

I can't figure out why the EM snapped though. And the PC running Mach 3 kept locking up. 3 hours to make this and it's too thin because the EM and the PC could not keep thinking it can. I lost my position and decided I want to find a better way. And plunging around makes scallops that seem to grab the EM when you want to finish, and it breaks anyway. That might be the way to go, take 20 thou steps, plunge to full depth, etc... Oh wait, 3/16 EM can't take a 20 thou DOC to work through the scallop. Smaller steps?

[GlennW]

For starters, I believe your speed is about three times too fast for HSS cutting steel.

It may be burning the cutting edges off unit just plows and breaks.

[Harold_V]

I'm inclined to agree with Glenn ----although the reported spindle speed is only a little too fast, but it may well be enough to cause tip failure. I get 171 fpm surface speed, so a reduction if spindle speed may prove to be of value.

I suspect that there's something more going on, though. If your mill isn't very rigid, that's probably the real cause of breakage.

Try slowing the spindle by 20%. Also, examine a broken end for signs of what Glenn described. If that's a problem, the tip will show burning or serious dulling of the cutting edge.

Chip color is often a good indicator of cutting speed. Are the chips coming off discolored? If they are anything beyond a light straw color, speed is part of the problem. Leaded material should cut with relative ease and yield chips that are colorless and shiny on the cut face.

H

Edit: Are you running the spindle in the proper direction? It wouldn't be the first time that has been done if you're not.

[Bill Shields]

Are there chips clogging the flutes in the broken off tool?

Another avenue:

You may have a combination of problems.

Brushing and misting are not the same flood when it comes to chip removal.

And I assume that you are cutting with 180 degrees of the tool?

ALSO:
You say tracing a shape AROUND a bar, which means that you are rotating and cutting.

Some controls use DEGREES/ Minute for rotary cutting, others use inches / minute...others flop back and forth depending on if it is pure rotary or rotary combined with linear....which us what FANUC and others do unless you are in G112 mode.

Is your software calculating the feed rate correctly for what the control wants?

[Wolfgang]

Just a thought.
Check how concentric your cutter is running.
If it is .002" TIR, it means it runs eccentric by .001", which would increase the chip per tooth to twice the .001" you are using, on one tooth!
Further, unless you have a rigid setup, back off on the spindle speed. I'd use 100 FPM cutting speed to calculate the rpm.

[ctwo]

I tried to get some photos, but metal is hard and lighting is poor. Chips look like steel wool to me, feel like sand when I rub them on paper.

I measured cutter runout about a tenth on one side and about 4 tenths the other.

I am using the mister just to blow air for chip removal, and I lead the cut with oil.

I am using 180 deg. of the cutter.

Machine is Bridgport Boss3 and I had replaced all the bearings. Nice Timken spindle bearings with few hours of use.

The 2" solid bar is faced and stood on end in a Kurt vise. I think it's rigid.

There is no fancy software. I export dxf and use f-engrave to figure out tool paths, which are simple point to point.




So I'm hearing to use an RPM anywhere from 1200 to 2800.

I read on another forum to use a feed of 8 to 30 ipm.

I read online DOC for slotting is 0.05 to 0.2 diameter (0.037" max)

This calculator seems to say

2400 RPM
9 ipm

https://www.custompartnet.com/calculator/milling

[GlennW]

Your chips look a bit charred!

I believe you are looking for about .0004"-.0005" per tooth feed.

Try 1900 and 3-3.5 ipm and see how that works.

Are these new or used end mills?

[Bill Shields]

Ah ..ok...not rotating while cutting. I was thinking another direction