[gcamlibel]

I am interested in milling 7075 T6 sheet material at 4mm thickness. I have some experience on milling aluminum alloys. for example I milled 5086 H32 alloy with 3mm endmill at 2000rpm and 70mm/min feed. result was perfect.

However with 7075 T6 I brake my endmills even if I cut as slow as 10mm/min. my endmills are HSS with 8%Co and I think the problem is to be worn out.

I start cutting 7075 T6 with 10mm/min feed and 2000rpm, after about 5cm cutting endmill brakes.

What should the feed and spindle speed for 7075T6 material? Is there anyone have som experience about milling this material? Should I use carbide endmills?

[IJ.]

Are you using coolant?

If you don't have a flood setup try a spray of CRC or WD 40 while it's cutting each minute.

I find I lose cutters from buildup if I don't use coolant with a large DoC.

Coated cutters help reduce this effect.

I've machined a bit of 7000 series in the past and treat it much like 6000 but it has the avantage of not creating stringy swarf like 6000! (comes off in nice chips)

[Ken_Shea]

To add to what IJ. said, do use flood coolant to keep the chips flushed away as these are a killer especially on tiny cutters. You might also shorten up on how much of the cutter is sticking out of the tool holder, you should also increase the RPM if you can, in my limited experience I find that carbide cutters always seem to out perform the HSS.

[JRoque]

Hi. I've done a few Fortal and other alloy cuts - not exactly 7075 but very close. Follow this link to my post on what I used: http://cnczone.com/forums/showpost.p...0&postcount=19

I highly recommend the end mill used there. It performs great even on my makeshift machine and you can see the video cutting through just fine. No coolant needed other than the occasional water spraying to keep -me- cool.

Cheers,
Julio

[gcamlibel]

I ordered some carbide endmills today. I will try them and write some feedback here.

I used boron oil and water mixture as coolant. I mixtured boron oil with 1oil 3 water ratio. is there any one know if it is true or not?

thank you for all replies...

[Ken_Shea]

Gunol
I am unfamiliar with Boron oil, what is that?
In your case I would think the most important need here is not so much lubrication but to flush out the chips and keep the cutter cool so the aluminum does not weld itself to the cutter. Carbide cutters can take quite a bit of heat but what you want to do is keep the cutter cool and not suddenly cool it after it gets hot as this can cause tiny thermal shock cracks leading to a chipped cutting edge. You can also increase the rpm even more over the HSS cutters.
In IJ. case my thinking is at 30,000 rpm it would just blow the chips away

I am sure you will love the carbide.

[gcamlibel]

I am not sure about english name of boron oil. It is a machining fluid that is used by mixing water. It looks like engine oil, after mixing water it goes into white color.

I tried 3mm cabide endmill TiCN coated at 20mm/min feed and 2000rpm. It works. however there is very high vibration and poor surface. I think these are becouse long tool and wrong cutting speed. however tool brake problem didn't occour with carbide tool.

Thanks for all supporters. I will post other feedbacks

[Ken_Shea]

Your Boron oil description sounds exactly like what I am using only it calls for a 5 percent dilution. I used 4 cups lube with 4 gallons water.


I take it that 2000 RPM is your limit?

[gcamlibel]

my mill can turn 3200rpm max. It has PWM speed control. therefore I can control speed continuously from 100 rpm to 3200 rpm.

I will try 5% solution

What is the name of your coolant?

[ESjaavik]

That may sound like the problem I had with a small milling machine. The spindle bearings had a bit of play. In my case they could not be tightened as it was a needle bearing.
Try to use a heavier milling chuck, or fasten a flywheel to it. It must be in good balance of course.
And go to the max speed your mill can do. 3000 RPM is probably a zero short as already indicated by some. You may need to go back to HSS, as carbide tools hate vibrations. Look at your cutting edge in a microscope or with a good magnifier. If there are tiny particles broken off, you probably have a vibration problem causing it.

Look at your endmill with a magnifier. Is there a lump of aluminum on the tips. Try to wipe it off with your finger. Does it stick? Then you see the problem.

When milling a part out of a sheet, do multiple passes creating a wider trace, and do it in several depths. Leave 0.1-0.2mm to be cut only in your last pass on final depth, I'd prefer a climb-cut assuming you have 0.00mm backlash. If you cut 4mm depth with a 5mm cutter, you're asking too much from it. Try 1mm deep cuts, and you can go much faster than your 0.05mm/tooth. Don't mill straight through even on your last pass. Leave 0.1mm or so. You can cut through that with a knife afterwards. Try this with 5-8% soluble oil, and I bet you'll have a mirror finish.

The multiple passes will make the loading on your bit and the sheet metal lower. The cutting of a wider track will leave the chips somewhere to go without re-entering the ongoing cut. If it does, it will at best ruin your finish, at worst clog and break your bit.

[gcamlibel]

I will go to my workshop and try your suggestions. thank you

[gcamlibel]

I bought some carbide endmills and tried them. one of them give best result. I cut 7075 at 3000rpm 50mm/min feed and 4mm depth with 3mm 3 flute. result was good, chips are uniform.

The manufacturer of tool is WNT. it is written on tool. also "95 202 030" "3.0 27/01*" are written on tool.

Is there anyone know about this WNT brand tool?