Re: Using a porter cable router to cut aluminum

--- In CAD_CAM_EDM_DRO@yahoogroups.com, Jon Elson <elson@p...> wrote:

>
>
> camfambmw540 wrote:
>
> >Hi all, new to the group...seems like a very excellent group :-)
> >
> >My name is John; I live in the Chicago area. I have a nice

compound

> >milling table that I would like to use in a very simple cnc

setup.

> >My plan is to fabricate a very sturdy z axis for a porter cable
> >router (1.75 hp), use the compound milling table as my x-y axis.

I

> >have 2 nema34 173 oz in stepper motors for the xy, still have yet

to

> >get the z motors. I also have yet to get the controllers or

power

> >supply. I have a 1 GHz pc dedicated to my shop needs.
> >
> >I plan on cutting odd shaped holes (1.5"x2.5") into 1/4 and 1/2

inch

> >6061 aluminum. I also would like this setup to be able to assist

me

> >in making a much better cnc sysem (when wife approved funds

become

> >available).
> >
> >
> I think you are dreaming! I do a fair amount of this sort of work

on

> a Bridgeport, and really would not want to do it on a much lighter

machine.

> We have a 3-in-1 machine at work, and it is an absolute joke! Not

an

> awful lathe, but for milling, it is actually WORSE that awful. It

has

> a Morse #3 taper spindle, too.
>
> >Question: Does anyone see flaws in my idea? Will I be able to

cut

> >holes of this size in aluminum (if I go slow and keep lubricant
> >constantly sprayed on the metal)? Any suggestions on how to
> >fabricate a z axis that will hold a porter cable router (simple
> >plans??)
> >
> >
> >
> Is the router designed to handle coolant getting into the bearings

and

> motor? Assuming it has a brush-type motor, you probably don't want
> to be feeding oil mist into that motor, so you'd better use a

water-

> based coolant! Can the bearings really handle the side loads of
> cutting aluminum? What diameter cutters do you plan to use?
> For a 1/2" thick piece, you can't use 1/8" end mills (which would

be a

> good match for the router's spindle speed). I think you'd need at
> least a 1/4" end mill (maybe 3/16" would do) to get enough
> projection past the collet.
>
> You say "go slow". Well, that's the problem. You CAN'T go slow
> at these spindle speeds (~20,000 RPM). You have to keep the chip
> load per tooth within a fairly narrow range. If you go too thin

(slow), the

> tool skates along the previously cut edge, and wears out very

quickly.

> If you go too thick (fast) then either the tool breaks or the

spindle

> stalls. With these size tools, the range is somewhere

around .0002"

> to .002" per tooth. A 2-flute cutter allows you to go at half the

feedrate

> of a 4-flute, so that would help. But, to put a number on it,

20,000

> RPM on a 2-flute cutter is 40,000 teeth/minute. At .001" per

tooth,

> that requires a feedrate of 40 IPM, which is certainly moving right
> along.
>
> Now, you see that we have the tool cutting (approximately) .001"

for

> every cutter tooth that passes into the workpiece. So, if the

rigidity

> of the ENTIRE machine, from the X-Y table, through the supports,
> up to the head, and including the router mounting and its spindle,
> flexes more than .001" under the cutting loads, then the machine is
> going to vibrate wildly and break tools or just make a lousy cut.
> To some extent, you can make roughing cuts that leave stock to
> be cleaned up by a finishing pass. But, on 1/2" plate, that

finishing

> pass will have to clean up a 1/2" wide face of the material, and

that

> will subject the machine to a torture test. If the vibration

builds up,

> it will leave nasty patterns on the surface. Maybe you won't mind
> that.
>
> Jon