End Mill Snapping

[Magnum164]

What's the best end mill for cutting AL plate 7075, mainly profile and slots? I broke so many bits this weekend it was not funny. Granted they were el cheapos as I figured I would break them.

I would get 3 parts profiled out of a set of 4, then the end mills would snap. 2 FL HSS.

I am running a PCNC770 at 4K RPM with a depth of cut of .011 and a feed rate of 19. I did cut back to 12 and I managed to finish all 4 pieces and there is no signs of damage to the end mill.

The parts are taking about 20 minutes each and I need to cut that down some. With the 770 is there an advantage to using a higher speed to increase the feed rate?

[300sniper]

diameter of endmill?

[Magnum164]

Darn it.. Thought I had covered everything

1/8IN End mill...

[drwc]

Thats definitely a speed and feed issue, I think you need to check out Gwizard to calculate your settings.

If you are slotting, your depth of cut is aggressive, and spindle speed too low, but Gwizard will really help you optimize settins and avoid breakage

Wayne

[Magnum164]

Thats definitely a speed and feed issue, I think you need to check out Gwizard to calculate your settings.

If you are slotting, your depth of cut is aggressive, and spindle speed too low, but Gwizard will really help you optimize settins and avoid breakage

Wayne

I am not a fan of Gwizard... Looking for info on what I should be using based on what others have tried and is working.... Not a software to use.

[bobeson]

I found that I break a *lot* fewer endmills when I bother to go into my office and look up my speeds and feeds in Gwizard at my workstation. Hopefully you have found a suitable alternative besides machinery handbook tables - that's a sure fire way to get frustrated until you've broken tools at all the boundary conditions and found your sweet spots. With Gwizard guiding me, I almost never break tools from the feeds and speeds. I haven't explored other calculators much, since Gwizard appears to have such an advantage. I just wish it ran on my machine's control computer natively, without needing a network connection. Other than that, I'm really glad I bought it, and I'm confident that it has paid for itself several times over in savings from the tools I didn't break by following the recommendations it gives.

[dertsap]

.011 depth of cut is peanuts but your feed rate is awfully high for an hss end mill , check the manufacturer specs for speeds and feeds rather than going with generic calculators .
1/8 carbides are dirt cheap and would be your best bet

[Magnum164]

.011 depth of cut is peanuts but your feed rate is awfully high for an hss end mill , check the manufacturer specs for speeds and feeds rather than going with generic calculators .
1/8 carbides are dirt cheap and would be your best bet

That is kinda what I was asking, would the carbides be better at that size and a higher RPM. I use carbides for smaller sizes which also seem to take forever, but I know others can get better times on cheaper machines.

In the video below I know the plunge rate is rather slow was deliberate but if you skip to about 5:10 you can see the cuts with the 1/8EM. I was actually testing a new HD camera.

One thing I did think of is perhaps my spindle is not turning the speed it should be, I am ordering a tach tonight as well so I can check it.

http://www.youtube.com/watch?v=AXdY0IMzUD4]New movie 2 - YouTube

[dertsap]

One thing I did think of is perhaps my spindle is not turning the speed it should be, I am ordering a tach tonight as well so I can check it.

]

higher spindle speed would be good but if you don't have it then just keep the chip load proper and you should be ok , I'd consider the difference of a few dollars for a performance carbide end mill over a standard carbide , a high helix would most definitely be a strong advantage over anything else , I sell and use 55 degree helix end mills and the performance over the standard end mills is night and day , the chip evacuation is incredible , the chips push up the flute and are thrown clear of the part , they can handle heavier cuts , there's less chatter and generally the surface finish is much better due to the shear the tool provides with that much of a cutting angle . overall my preference is to avoid the use of standard end mills for any aluminum cutting .
Anyhow whether you go that route or not I believe that standard or performance carbide will be an major advantage over hss

Btw take advantage of having a cnc and try to ramp your tools , it always makes me cringe to watch a cutter plunge into material ( it just screams trouble )

[Magnum164]

higher spindle speed would be good but if you don't have it then just keep the chip load proper and you should be ok , I'd consider the difference of a few dollars for a performance carbide end mill over a standard carbide , a high helix would most definitely be a strong advantage over anything else , I sell and use 55 degree helix end mills and the performance over the standard end mills is night and day , the chip evacuation is incredible , the chips push up the flute and are thrown clear of the part , they can handle heavier cuts , there's less chatter and generally the surface finish is much better due to the shear the tool provides with that much of a cutting angle . overall my preference is to avoid the use of standard end mills for any aluminum cutting .
Anyhow whether you go that route or not I believe that standard or performance carbide will be an major advantage over hss

Btw take advantage of having a cnc and try to ramp your tools , it always makes me cringe to watch a cutter plunge into material ( it just screams trouble )

Thanks.. I have some ordered, I will look at the 55 degree helix as well. Would there be a concern with them pulling the material up out of the way I hold them with mitee-bite clamps? I can always order the ones with grooved sides.

Actually they were supposed to be ramped. It made me cringe as well I think I missed something in one of my settings.. But getting there..

[dertsap]

not much concern with them pulling the material up if it is well secured , and the mitee bites (one of my favs) will be fine

[BobWarfield]

The old adage is if you snap an endmill, it's too much feedrate and if you dull it it's too many rpm.

4000 rpm is slow, even for HSS in a 1/8" EM. Small EM's like a lot of rpms. The carbide is helpful from a rigidity standpoint to many applications, BUT, when running small EM's on smaller mills, consider another factor: runout.

HSS is less sensitive to runout than Carbide because it is less brittle. If you've never measured your runout, you might be surprised. It's much worse for small cutters as it should be thought of as a % of your cutter diameter or as additive to chipload.

Getting back to where we started, if you snap an endmill, it's too much feedrate. In this case, you're 2x too fast on feed as G-Wizard suggest 9.6. BTW, you're welcome to import the manufacturer's recommendations to G-Wizard. It's easy to do and there are also quite a few available for download within the program. Some will be a bit higher than the default, but I doubt there's any that are 2x.

Last point, in aluminum, make sure you're really clearing the chips well, especially for small cutters. If they start welding on the cutter will be toast in no time.

Cheers,

BW