View Full Version : Using Roughing EM on 6061

05-29-2007, 09:27 PM
I am using a roughing EM on 6061 T6 stock. The stock is 1.5" thick and I remove a lot of material.

I just bought a 1" 3 flute roughing EM (value brand) from JL. I am planning a surface speed of 300 sfpm and chip load of .007" (feed per tooth). The calculations work out to 30 IPM at 1145 rpm.

In the past I was using a 2 flute standard HSS EM at 20 IPM using the same sfpm, rpm, and chipload.

Is this about right for the tool or does a roughing EM allow greater speed or chip load vs. a standard EM?

My machine is a 5hp Acroloc CNC. The spindle is not the most rigid thing in the world and my max RPM is 3500.


05-29-2007, 11:15 PM
You can always start out with the calculation, but there is nothing better than to run, see, hear, and smell the sound of melting metal.
Put the hammer away cnc is here

05-30-2007, 08:19 AM
The SFM sounds way low for aluminum. All of the running capabilities are dependent on the machine and set-up. If you have more RPMs and coolant then Crank up the RPMs and down the chipload I would probably start in the .003-.004 per flute and then achieve at least 600-800 SFM. Then run and dial in a good cut that doesn't produce harmonics and chatter. Don't be afraid to turn the RPMs up in aluminum. Short of many thousand surface feet, your machine's max RPM will run most everything just fine. I run an 8K RPM hurco. I did some more on the production side parts with a 1.25" HSS rougher in 6061. I ran it at 8K and 100IPM or so,full depth everywhere, without trouble. The thing I ran into was the torque at max RPMs is a bit low, and you must always have a good coolant flow. Also, full width cuts or "slotting" is one of the hardest operations on an end mill. Periphery cuts with a step in are more desireable. Those roughers also don't like to plunge. You can helical ramp, simple ramp, plunge outside the material, or drill a hole with a drill before plunging and save yourself some trouble. Hope this helps.
-Greg Beaman

05-30-2007, 09:50 PM
Thanks for the advice! I am not sure why I was so shy about the SFPM.

I took your advice and used 600sfpm, .005 chip load with the result of (2291 rpm at 34.38 ipm for my 1" 3 flute roughing end mill).

The cuts were great and the machine seemed to handle it very well. I even took it to 120% feed and 120% speed for a bit and it did fine so tomorrow night I plan to try 800 sfpm. Everything is peripheral milling with 50% step over.

Each pass tonight was .3" deep and it took 5 passes to go through the 1.5" stock. How much can I increase the depth of cut? I really don't know what the limits are. My machine is 5hp. Generally, how deep can I go per pass with a roughing endmill?

05-31-2007, 06:23 AM
i have had great luck roughing aluminum with an abtools shear hog. its a 2 flute insertable shell mill. if Ø1.250 fits your needs, i would look into one.
i typically take .100 depth of cut, full radial cut at 8000rpm and 100-150 ipm.

05-31-2007, 07:21 AM
Congratulations on trying something new. Many people are afraid to do this and do the same thing over and over again. 5HP is plenty to get lots of work done, but the machine rigidity is the other factor in the equation. Is your mill a Knee Mill or a bed type mill? A bed mill can take more abuse then a knee mill, because of its design. What I have found with corncob type end mills is, that depth is much less a concern then with a conventional endmill. Because of the broken chip the harmonics and stress are significantly decreased. I think you can achieve much more depth at the same cut settings on periphery cuts where the chips can flow out of the way. I would think you could easily double your depth and maybe up to 1 inch, but be more conservative if the cuts are full width slotting, because the problem is getting the chips evacuated in that type of cut. Good luck.

05-31-2007, 12:07 PM
Thanks again.

The shear hog sounds interesting and I checked out their website but I still have some questions.

For removing the bulk of stock around my part I need to cut along the periphery and since I have a lot of material to remove speeding this operating up would be a big help.

My machine has a limit of 3,500 rpm. It is an Acroloc Series 10. The machine does not have a great reputation for rigidity but it seemed to cut well enough last night at .3" per pass and 600 sfpm so I figure I will try going deeper and pushing up to max RPM.

The corn cob style mill with very deep cuts sounds like it has the potential to remove .5" to 1" per pass at something close to 30 IPM with 3 flutes doing the work. Is this the best way to hog stuff out on a mill like mine?

An insert cutter seems like it would have a much lower limit for depth per cut and since I can't get any more RPM out of my machine I figure I would be stuck with more passes and less material removed per pass so it seems that on my machine the insert cutter might not make sense. Am I missing something?

I plan to do lots of roughing this year so I am looking a technique that is both quick and cost effective. Is corncob better then insert cutter for machines that don't have a lot of spindle speed?

05-31-2007, 12:27 PM
The series 10 arcoloc you have is not very rigid at all, it runs a 3.5" spindle , Ive run and owned these machines since they first hit the market in the 80's.
very good choice to rough before a finish on these machines. DONT use carbide even on a .010 finish past cause you will get lots of chatter, highspeed is the only way to go, this will allow you to load up the endmill and keep the pressure of the spindle on the spindle caseing.
make sure you have the head down as far as it will go so you don't extend the spindle that far.

I am suprised your able to use a one inch endmill on that machine, (either you have the head as close to possible to the work piece or you have an extreamly tight spindle. you might be able to go faster using a 1/2 endmill and increasing your feeds and speeds, however on the series 10 fast spindle speed isnt always better.
dont go buy calculated feeds and speeds on this machine cause they just wont work.
IN many cases you will get better finishes if you Dont climb cut, I know it sucks but climb cutting cause's lots of chatter on that machine due to spindle design. you also dont really want to go more than 50% of the dia of cutter for step over pass's ie 1" dia end mill dont step over more than 1/2" usually less is better,

BTW I think I saw some brand New rebuilt tool holders in my shop when I was doing some cleaning last week, you send me an email or pm with your address and pay for shipping there yours. I dont have any more series 10s and I have one series 100 left. I used to make most parts to rebuild these acrolocs for a local guy here in the valley and repaired a ton of them. do you have the actron control?
if you go with a ball spline on the spindle drive you can eliminate the acroloc finish. I always hated that finish. you can also run a highspeed spindle on it for fairly cheap was well.

05-31-2007, 12:27 PM
In my humble opinion, your best bet will be with a corncob. You can probably peg out the spindle and take a deep cut and then up your travel speed until you are uncomfortable, then just a bit more. If you can get a bigger cutter in there that will help too. I would avoid insert cutters for an operation like this for the reasons you mentioned. The corncobs are relatively cheap, and so insert cost is not an effective comparision. HSS will flex all over the place and not break. For lower RPM machines like yours that probably has plenty of torque I would proceed as you are but start turning it up. You will probably be impressed when you get where you are going at the capabilities of the machine and tooling. Take care.