I am using a Maxnc 10 CL and don't have a coolant system, so I always manually spray water on the cutting area very frequently,. sometimes mixed with floor wax. Using a Micro100 ARM 250-2, which is a 1/4" 2 flute square cutting mill, I wear these out very quickly in 6062 aluminim. I have tried varying speed rates faster and slower, the spin is most often 8k, and since the machine is broken and will not pwm, I cannot vary that easily (I have attempted to repair it but it is in the logic board, and is a big hassle to have it sent back ans sit around at Max for a week).

After talking to Micro100 they have suggested I slow down the feed rate. In Mach3, I usually run it around F9 cutting at .05 depths notmally. What happens is that after 2 or 3 hours, the tips start wearing or chipping, and at at some point start packing, and then binding. In my location I can't use some odorous oil and have the place smell like a shop, as it is a dual purpose office and workspace. I really could use some suggestions on a water based lubrication that is easy to clean up and not too smelly.
Thanks

, .0005 chip/tooth is pretty light in aluminum , and even so the tool shouldn t wear , it 's probably burning up , try high helix carbides and run at least .004/rev
i don t know much about those little machines but i would think with the right cutter it should perform much better than that ,
tipical water soluble flood type coolant works well in a spray bottle
try snugging up the tool some if you can use a stubby tool you may have less trouble
won t say much about your tool supplier ,though i would suggest getting a second opinion from another supplier

out of curiousity where did you come up with using floor wax for cutting fluid , i had never heard of that before

Hi all , let me relate to you the hazards of using cutting fluids where the tool is allowed to get hot. Some years back I obtained a 25 litre drum of cutting oil, the type that is not mixed with water but is used neat and floods the tools etc.
The oil was used previously on a trial basis, and the unused quantity scheduled to be dumped, whis is how I came by it. I used it on my lathe in a squeeze bottle to do general turning jobs and it worked well. The only trouble is when you turn, the chips come off blue and the oil smokes and the resulting fumes hang around in the air and can be LETHAL if not drawn off by an extraction system.
This problem does not occur on the Mikron Haesler rotary transfer machines that it was trialled on previously as it is used flooded and in an enclosed cabinet.
The oil fumes, once inhaled, caused a flu like symptom, duration two months, and a sore throat with an irritating throat clearing desire that lasted three months.
If this symptom is ignored with prolonged exposure, the sore throat and throat clearing goes away and as the nervous system becomes numb to the irritation, irreparable damage results, and probably throat cancer.
I read of this problem in The Model Engineer Magazine in the '80's by a Canadian subscriber who had experianced the same symptoms. At the time I assumed I was suffering from a seasonal flu bug.
Ian.

I wonder if that holds true for wd-40 fumes as well. I have always been kinda worried about that, but now i am more so. I don't think i will be using wd-40 as coolant anymore.

I think the water may be causing thermal shock to the carbide cutter.
With soluble oil being out of the question, My next choice would be air.
Put a air line pointed on the cutter and see how it works. They make a cooling
nozzle that will supply really cold air to your cutter from a regular air line source. Don't recall what they are called , but they are sold by many vendors.

I used to uise wd40, but the smell was too much. You may have a point about the thermal shock. It is possible that is gets hot, then get rapicly cvol from the occasional spray, the heats again, in a cycle. The company said water should be fine but suggested flood, but I don't have a setup to flood it. I will expliore the air. Thanks

The tool the Ben was talking about is from exair, I think thats how its spelled. That should work good for the application. As far as your speed and feed you are using they are way off. If you look at the tool under a scope it will be rubbed dull. I would run the chip load at .003 to .004. What type of cut are you doing? Are you are milling a full width slot the chip could also be taking out the cutting edge?

The past few days has been primarily pocketing a part out .9 deep, approximately 2.5 wide, 3 long. I run a depth or .05 each pass, overlap of 50%. I don't know how this translates to you guys, but in Mach3 it is F5 today. Prebvious speeds were F9 at around 8k. I started with a brand new bit today, it is chipped already within 3 hours, and will not last more than another 1 hour before it is done. These are the top of the line Micro100 mills, 18.50 each. The whole part isn't worth 18 dollars, but I need it for the project. I have tried it half speeds today, spraing more water and there is no change.

Hi, chipping cutters on ordinary mills is a problem and is often caused by the first point of contact with the job. After that the cutter is cutting in a radiused slot and so the shock loads are carried by more than one tooth.
I would try lowering the feed rate at start until the cutter has got into the cut and then increase it to whatever. Should be only a matter of program control in CNC as opposed to feeling the start of a cut when manual milling and then engaging feed.
The other problem is remilling chips that are a bit harder than the parent metal and tend to wedge between the cutter edge and the job and being a wedge do not allow the cutter to cut but are dragged between the faces and are sheared as in a guillotine, usually putting a side force against the secondary clearance and a chip results. I largeley overcame this by making the coolant flow in a downward jet pattern and forcing the chips to flow up the flutes and so be carried away. I reckon it would be nice to have a hollow end mill and centre feed the coolant to blow the chips out as they are formed like it's done in boring bars on lathes. Not very practical on a 6mm end mill though.
Ian.

How are you moving to each z depth? If you aren't using a ramp/helix, you may want to drill an entry hole.

Your feeds are way too slow. For 8000rpm, you should be feeding at least "F32" (32 inches/minutes).

You should also be cutting much deeper. (like 3 times deeper) By taking such a shallow pass, you're wearing only the very end of your tool rather than using more of your flute length.

You said that your pocket depth is 0.9 inches. Is this also your flute length? If so, I highly recommend switching to a 3 flute. (for tool rigidity) I hope this tool is also a solid carbide tool.

Keep your coolant. If you increase your feed rate, thermal shock isn't going to be a factor with only 8000rpm on a 0.25 inch tool. The benefits of lubricity and chip clearing are worth it.

Justin

Dump the carbide tool. BUE is causing the failure. Buy two flute HSS from OSG or similar with TiALN coating. You will be pleased. At 8000 RPM you should be moving at a min of 16 ipm. Do not be bashful. I promise you will like the HSS cutter better (in this case).

Try Blizzard endmills from OSG they can really hog Try 8000rpm and feed at 75ipm!!!!!!!!!!!!

HSS over carbide? In 30 years I have never seen that work?