machining metal with my woodworking router table? what do i need?

first, a reminder of my machine: it is a roughly 4 foot by 4 foot Techno/ISEL gantry router table, with a 5HP/3PH Perske spindle.

so with the understanding, from some i have spoke with, my machine is able to machine metal, but what what do i need to know to machine metal?
lets just assume i have never milled metal before... (not hard to assume). what i plan on milling, is certainly not Titanium. just aluminum or steel enclosure panels, to make openings for switches, LCD screens, whatever.

first on my list of concerns... coolant. do i need it, and what would be some ideas on collecting it from the table?
chatter, i know i need good clamping, but on thin panels, what is the best way to reduce chattering?

so, assuming coolant would be beneficial, my thinking is a tray around the working area that i can simply mount on the table, and drain it into the coolant tank (through a swarf screen i assume). the tray would be tall enough to prevent splashes from flooding my CNC shed, and i may even use a brush around the milling bit to catch spray off the spinning bit.
could be done, cost-wise, not sure yet.
i am assuming the coolant lessens some chatter, and of course extends the life of the milling bit, as well as lubricating.

~Travis

Metal (iron based) machining requires far slower cutting speeds (end mill rpm) and far higher machine stiffness. Up to a million pounds per inch of deflection. High low speed spindle torque also.
So you can’t cut metal with a wood router.
It will chatter and bounce all over the place moments before the bit is destroyed.


Sent from my iPhone using Tapatalk

Within the limitations of your machine, yes, you can perform the tasks you have asked about. Don't expect performance of a multi ton machining center, but aluminum should easily be within the capabilities of your machine, and drilling / etching steel sheet metal as well.

I have minimal experience cnc machining sheet metal, so cannot give any advice there.

My best advice... try it and learn the true capabilities and limitations of your machine, and then, within those limits, you can do any project you can dream of with your machine.

Sent from my SM-G991U using Tapatalk

Hi,
the ultimate limitation of your machine with regards to cutting metals is stiffness, or rather the lack of it.
You may well do aluminum and brass but I think steel is going to be too tough. Aluminum and brass can be cut quite reasonably with high speed/low torque spindles,
especially with coolant, but steel requires low speed high torque spindles. You must stick to the surface speed recommendations for steel or you will turn expensive endmills
into scrap in seconds.

The stiffness required of a steel cutting mill verses one for aluminum is about FIVE times!!! If your machine flexes the tool will not bite into the steel but rather the machine will
deflect so that the tool gives the work material a 'damn good rub'........resulting in excess tool heat and surface work hardening of the material...a disaster.

Whether aluminum, brass or steel, plenty of flood coolant will help enormously, and no BS tray is going to catch it, it sprays all over the place. Coolant is especially useful for
flushing chips out of the cutzone, recutting aluminum chips is a sure way to clog up the tool and get 'built up edge'.

Craig

Hmm, i think i will try HDPE or acrylic, see if that will work for my panels.

my spindle will turn down pretty slow, like 100 rpm, but i don't know what the torque is at that RPM.

at least with plastics, i can get away without coolant. as long as i use my vacuum setup.

Thanks for the responses!

~Travis

Hi,
believe it or not plastics can be quite a challenge to machine, they conduct heat so poorly. Nylons, and polyethelenes tend to form long strings
rather than chips.

My preferred material is acetal, it's hard and rigid enough that it forms chips and yet has enough flex to make usefully tough small parts.
Even with acetal I use flood coolant, not so much for cooling but rather flushing chips out of the cutzone, recutting plastic chips is as
disastrous as recutting aluminum chips.

Acrylic also forms chips but they get very 'sticky' at low temperatures, best used with coolant or maybe compressed air. It's brittle enough that
its a poor choice for small parts.

Some of the glass loaded plastics have useful properties. The fibreglass filler all but requires carbide tools but can usually be relied on to
form chips even in polymers that do not form chips well, and of course can make a genuinely tough part.

If you want to try metals then brass is a good place to start. There is a reason that brass is widely used as small machined parts.....it cuts
beautifully, nice small easy to clear chips without the propensity to built up edge. Even with brass I use coolant, the cut quality is just so much better,
often not requiring any finishing ops, just straight from the mill into the assembly.... I use surface speeds of 150-250m/min with uncoated carbide tools.

Aluminum is a great material and quite probably within the rigidity capacity of your machine. I use surface speeds of 250m/min with uncoated carbide tools WITH coolant.
As I posted earlier recutting aluminum chips is inviting disaster, flushing, blowing or whatever chips out of the cutzone is essential. Its tempting to believe that if you
take a very shallow cut everything will work fine....but with aluminum that can be a trap. The chip carries away a significant proportion of the heat, and if you thin the chip over-much
then it removes little or no heat and invites built up edge. If you want to cut a little faster or maybe some of the 'sticky' grades like 5083 then try di-boride coated tools,
'greasy as a butchers prick' in aluminum.

If you want to try steel then be prepared to be patient. Use surface speeds of say 100m/min with uncoated carbide up to 150m/min with coated tools, coolant very
much preferred. To get those surface speeds you are likely restricted to small diameter tools, 3mm or less. For example 100m/min at 3mm diameter (uncoated) =10,600 rpm
which should be in the power curve of your spindle. You will have to take very light cuts but within the limitation that you MUST actually cut and make chips otherwise all you do
is generate heat.

I have had reasonable success with a high speed/low torque spindle using Destiny Tools Python endmills, usually with a small end radius for max tool life. The trick is to keep them cool
and cutting at a constant and steady chipload, even if the chipload is light.

Craig

here is what i have come up with, from ideas of others, and my own.

rather than trying to make a removable option for coolant control, i can instead enclose the entire machine for dust AND coolant control. i would need to be able to wipe down the machine after coolant, before using wood for carving. other provisions would be i would want to block off the coolant sump from wood dust, turn off the coolant to prevent drips on the wood. for use of coolant, i would have to clean up any wood dust, un-block the sump drain, turn on the coolant valves, and it would be a good idea to have a blast-gate on the vacuum hose, just in case the vacuum kicks on.

i have configured LinuxCNC so that i have three relay outputs. vacuum, coolant-mist, and coolant-flood. mist and flood can be on at the same time, (for whatever reason i ever need to), but when they are on, the vacuum relay is locked out. but if the spindle starts, either forward or reverse, and both coolant signals are off, the vacuum starts automatically. (I LOVE LinuxCNC!!! don't know why i ever considered anything else)

at one time, i considered selling this machine... but i am having SO much fun working on it, i hope i NEVER sell it! it has become like my own child. i bought it in an inoperable condition, added components, and watched it's first moves (back when i used a parallel port interface to control it). i have since watched it grow and evolve into the fine young machine it is today. :) now i just have to be able to get it to move out of the Camper/CNC Shed, and into a to-be-built shed for it, when lumber prices come back down to reasonable levels...

~Travis