[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.

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

[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

[btu44]

I'm thinking your breaking end mills because the chip load is pretty heavy at .0015 per tooth. Thats typical for for a 1/4 EM. The chip load per tooth I see suggested for 1/8" EM in aluminum is .0005 - .001"

It's also good to check the tool run out for such a small tool. The slotting parameters I listed has a chip load of .0006". If theres something like .002" of run out, that can break EMs.

Here's 2 videos I did on runout if interested.
[ame=http://www.youtube.com/watch?v=2rur6oFaYhY]TTS Runout - R8 Collet.wmv - YouTube[/ame]

[kevinro]

Hmmmm..... I think I would reconsider my position on GWizard! Your speed and feed values are quite a ways off. You should be going much higher RPM and much slower feed.

GWizard came up with 5100 RPM @ 12.24 for the .011 depth and .125 width.

GWizard has been going a pretty great job for me.

[Magnum164]

I think you guys are more interested in selling me on Gwizard than you are helping me to understand how to determine the proper RPM's and settings to select.. Did you notice where I stated I cut back to 12F and had no problems?


So for the Gwizard impaired let me ask the question again...

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?

Any thoughts? I realize I can play with the settings all day long and run analysis in Gwizard. The stress engineers do that at work all day long. But at some point you either have to put the numbers to metal - which can be costly, or you can ask others who have been there and get a starting point and suggestions. Carbide was a good suggestion and perhaps using the higher speed rates. I'll start there and perhaps email the mfg to get some info while I wait for the bits to get here.

[TXFred]

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?

Absolutely. Not only will you decrease your cycle time, you may get better looking parts. Carbide tools make prettier cuts at the right surface speed.

Every cutting tool has an ideal surface speed. This speed is determined by finish quality and cutter life. The smaller the tool, the faster you must run the spindle to get the right surface speed.

If you switch from HSS to carbide, the ideal surface speed increases.

So, look up your work and cutter materials, and find the ideal surface speed. Use that to calculate the ideal spindle speed. Then take that and your ideal chip load, and you can calculate the feed rate.

Frederic

[bobeson]

I think you guys are more interested in selling me on Gwizard than you are helping me to understand how to determine the proper RPM's and settings to select...

I'm not trying to sell GWizard; that's how *I* fiigure out my feeds and speeds, and I think you're hearing a chorus of voices saying "use GWizard!" not because we get kick-backs from Bob, but because GWizard works better than any almost other method for determining initial feeds and speeds. Machinists with years of cutting time have learned how to estimate their feeds and speeds pretty quickly, but unless you have that body of knowledge yourself I don't think you're going to get any better starting points than what GWizard has to offer, and that includes polling cnczone members. For myself, looking up feeds and speeds for a given cut takes only a few seconds; if I want to explore the parameter space I can fool around with optimizers and various "what-if" scenarios, but that all happens in a few minutes tops, certainly not "all day".

[dbrija]

As to the question of endmills, the 3 flute coated carbide from Maritool are nicely priced and make nice finishes.

[Magnum164]

As to the question of endmills, the 3 flute coated carbide from Maritool are nicely priced and make nice finishes.

I might try some, looks like I need to do some experimenting. I ordered some 2 and 4 flute from Monstertool. I could only find a 30DEG Helix so we see how they will do. I also ordered one coated to see how it does.

However, I realized why not do to my profiling what I am doing to the slots inside. I am hogging them out with a 1/4 coated EM then following up with the 1/8 EM just to get the smooth finish and smaller corner radii. It's also a heck of a lot quicker.... So why not profile my parts (actually its slotting) with the 1/4 EM then just follow up with the 1/8 EM for the radii as well. Would mean wasting more material but would cut faster.


Now on to the RPM issue. I can increase my RPM, but the runout issue has me concerned. I am not 100% sure my ER20 holders are balanced. I will have to go back and see what Tormach states about the higher RPMs and how to make sure everything is still in balance. I know they sell balanced ER20 collets for that reason.

And I still have a optical tach on the way.. I have never checked the RPM on my machine... Should get a baseline I guess.

[kevinro]

I think you guys are more interested in selling me on Gwizard than you are helping me to understand how to determine the proper RPM's and settings to select.. Did you notice where I stated I cut back to 12F and had no problems?

You asked a very legitimate question: How to determine the speeds and feeds for the tools. You got a very legitimate answer: With very few exceptions, we all use GWizard.

If you wish to do it without such a software tool, then you will have to spend time doing all of the calculations by hand. There are many variables to take into account that you will need to account for. It is tedious, requires digging through charts and graphs from manufacturers, evaluting the materials you are cutting, calculating tool deflection based on the amount of stickout from the tool, evaluating how much horsepower is available on your spindle, and much more.

You did state that you cut back to 12F and had no problems. If you had started with GWizard, you would have started at 12F and had, well, no problems.

Not trying to sell you anything. You can drive a nail into wood with your thumb, a rock, or a bowling ball. We are suggesting you use a hammer like the rest of us!

Kevin