RE: [CAD_CAM_EDM_DRO] feeds and speeds.

I disagree with regards to the tool insert life. Properly cared for inserts
give much longer life than 20 minutes. Shock loads, both thermal and
mechanical, are the prime destroyers of carbide tooling. Carbide will
certainly wear out, but after quite a bit longer than 20 min. Also note
that there is a MINIMUM chip load to be observed when using carbide. Since
carbide is so brittle, even ground and honed inserts have a slightly rounded
edge. The sharpest carbide inserts that I use require a minimum of 0.0015
chip load and can take up to 0.017 IPR. Non honed or non ground inserts
have a higher minimum chip load.

6061 aluminum is not too fun to machine. It is pretty gummy, and coolant,
either mist or flood, is quite necessary for any useful metal removal rate.
I much prefer 7075 aluminum for its machining properties as well as its
superior mechanical properties. The drawback to 7075 is that it has lower
corrosion resistance, although this is not a problem in most applications.
I mill 7075 at up to 75 IPM using mist coolant with Valenite's water
soluable coolant and a Cool-Mist sprayer. The shop does get sorta foggy
after a few hours of cutting though. I use flood coolant for all materials
on the lathe an this works well and doesn't have the fog up problem.

Thanks,

Ward M.

wardmerk@... <mailto:wardmerk@...>



-----Original Message-----
From: Sven Peter, TAD S.A. [mailto:peteryco@...]
Sent: Friday, June 01, 2001 8:43 PM
To: CAD_CAM_EDM_DRO@yahoogroups.com
Subject: Re: [CAD_CAM_EDM_DRO] feeds and speeds.


Hello friends,
in relation to the speed and feed recommendations for mill and turning
inserts you must keep several aspects in mind:
These numbers are made for stiff production machines.
At least on turning inserts they are calculated for maximum metal removal
rate during 20 minutes!!!!!
Afterwards they have to be changed.
So first if your machine is not as stiff as a high volume production machine
go drastically down with speed and feed.
Second If you not want to break a lot of tools then go even more down with
speed and feed. Because only in proved batch programs and rigid set ups you
are able to use them.
Third tool life is directly depending on the cutting speed. The curve is
like a hyperbola. As slower you go as longer it will last.
But you must select your
carbide grades according to the material you want to work.

My lathe is very rigid and stable but still as a rule of thumb I start for
batch
production with 75% of the recommended cutting speed and for roughing with
a feed of half nose radius. 75% of the cutting speed gives you normally 1
hour 20 minutes of tool life. And half nose radius feed
for roughing is a safe approach from where I start playing. for best
performance.

So for what you should force your tools and machines if you want to make
a nice hobby job?
Better tinkle a lot with your machine, try out for what it is good and where
are
its limits and then make your own rule of thumb for to apply the tooling
manufacturers recommended values.

Lets give you an example. The didactic ENCO lathes I know are small and weak
I would start with a positive insert with not more than 0,4 mm nose radius
at 40 percent of the recommended speed (4140 =
bonificated chrome molly steel 140m/sec*0,4=56m/sec (which is still above
the critical build up speed of 40m/sec)), make narrow cuts
not deeper than 2 mm diameter and start with only a forth of the nose radius
0,1 mm/rev.

The tread started with the the question for speeds and feeds in aluminium.
Aluminium is normally very nasty to work with. It gums up and makes
frequently a great mess. For production and everything else I
always use 6061-T6511 or 6064-T6511 aluminium. because even with the H34
grades I had big troubles.

I hope this gives a notion.

Good Luck.
Sven Peter