Sensible Flycutting Size

Sometime in the next few weeks I may have a need to do some fairly
wide flycutting on some Aluminium plates. Depth of cut won't be really
large, just enough over a few passes to get it quite flat.
The problem is these plates will be about 10"-12" wide and around 18"
long.
I have a cheap import R8 clone flycutter, but this won't do any more
than around 6" wide safely, as I don't really fancy hanging a great
long bit of HSS off the side of it.
So for those of you who do face stuff off around this width, what is
the best way to do it? Any special/favourite designs for a cutter, and
do you clamp it to the spindle or rely on the taper/drawbar? And what
about tool orientation - should I go with a cutter on a shallow angle
to the surface like the current one, or mount one vertically down in
whatever is used?
Bear in mind that I have to do this on a Bridgeport, with R8 probably
being the limiting factor.
Peter
Reply to
Peter Neill
Loading thread data ...
Dunno mate
I've seen flycutters that are a ten inch alluminium disk with an arbour
Then you would only have to let 1 inch hang out .
You could soon knock one of them up.
Cant see much going wrong with the above if you take light cuts.
and you balance it
or a peice of steel sort of ten inches long and 2x1. arbour in the middle..with a small peice of hss in the end of it.
all the best.mark
Reply to
mark
How well is the mill head trammed? Wide cutters make it harder to get a flat finish according to St. George. If you really want it flat, use a smaller cutter and go up and down more.
Mark Rand RTFM
Reply to
Mark Rand
The tram is pretty good, thanks to some very large parallels in a lot I picked up at an auction. They are 300mm x 70mm x 35mm and make it a doddle to swing the clock around on them. I thought about doing a couple of passes but I really want that nice uniform finish *and* flatness too.
Peter
Reply to
Peter Neill
There are plans in "The Shop Wisdom of Philip Duclos" for a 10" fly cutter to fit an R8. He recomends about 160rpm for aluminium. Drop me an email off-list if you want me to send you a copy.
Regards Kevin
Reply to
Kevin Steele
Even if you have a cutter to cover the width in a single pass your table travel would need to be at least the length of the workpiece plus twice the diameter of the cutter if you want to clear both ends to get that "nice" finish - somewhat more than available on a Bridgy for your quoted sizes.
Bob
Reply to
BobKellock
I use a 12+ inch flycutter. I turned a ring that clamps around the mill spindle. There is a 2" slot across the face of the ring so when it's on the spindle a bit of 2*1 can be bolted to the ring. I made an insert holder to go on one end of the 2*1 and I balanced it by having a central hole to hang it from then adding weight to a stud on the oppostite end to the cutter. I tend to run it with a 12" cutter at ~200 rpm and with a 10" cutter at 400 rpm.
Reply to
richard
You can get around this by canting the head over a thou or so, just enough so the cutter doesn't drag it's heels.
Reply to
richard
Sounds similar to my flycutter for cylinder heads and blocks.
I took a length of 4" mild steel bar a touch shorter than the protusion of the spindle from the quill - about 30mm I think. I bored that out to just slip over the spindle leaving a ring with about 1" wall thickness. I put a 1/8" slot through it at 12 o'clock and drilled and tapped across that for a 3/8" unc clamping bolt. Actually I did the threading first then slotted it. At 3 and 9 o'clock I put two more 3/8 threads in the underside of the ring for the bar to screw to.
The bar is a 10" length of 2" x 1" mild. I slotted that right through with a 3/8" milling cutter for about 7" leaving 1.5" of solid metal at each end. I then opened up the slot to about 1/2" depth to a width sufficient for the heads of 3/8" unc capheads to sit under the surface. That means the cutting tool doesn't need to stick out more than a tad which adds rigidity. The bar can then be adjusted for cutting diameter by sliding it relative to the ring it clamps to. Clamped centrally it's cutting at about 9" diameter and it can move out to about 12".
To remove the whole apparatus from the spindle I only need to loosen the clamp screw. The bar stays clamped to the ring at all times and there's enough spring in the slotted end of the ring for it to slide off the spindle. To refit I just push it up until the bar hits the bottom of the spindle and tighten the clamp screw again.
At either end there is provision for the cutting tools. One end has a 3/8" hole with a grubscrew intersecting it to take a 3/8" brazed carbide tipped bar. The other has a little fixture which takes a DNMG non-ferrous carbide lathe insert held at the correct angle to the work. To be honest I only ever use that one.
Most heads/blocks are about 6" to 7" wide so I run the bar clamped centrally at 9" cutting diameter which gives me 1" to 1.5" overhang each side which is ideal. I don't like to run less than 1" for reasons explained below.
In use the bar is trammed down a tad at the leading end so it doesn't cut on the backstroke. I clamp a dial gauge to it so that just registers on the front and rear edge of the mill bed which is about 9" wide. I then adjust the head so the dial gauge is reading 5 to 6 thou more at the leading edge than the trailing so about 0.6 thou per inch of cutting diameter. In theory this gives a slight dish to the work and that's why you need some overhang on diameter. The bigger the overhang the smaller the arc the tip sweeps out on the job and the shallower the dish. If you could imagine an infinitely large cutting diameter the cutting strokes would be straight lines across the work and there would be no dishing at all.
If the cutting diameter is exactly the same as the width of the work the tool sweeps out semicircles and you dish by half the trammed amount which is clearly unacceptable. At 1.5" overhang you get arcs about 1" high and the dish is only a fraction of a thou. Not visible with a straightedge held to the light anyway.
If you don't tram down then you need to sweep the whole tool over the length of the job and that's too much travel for a small mill on a cylinder head. My way you need the job length, say 18", plus the cutting radius, another 5" plus another inch or two for the tool to clear the trailing corners of the job. Total is about 24" which is fine. I think I have 30" travel on my Bridgeport clone.
For aluminium I run the cutter at 500 rpm and for cast iron I run 180 rpm. I might drop those both a tad if the tool is out at a very large diameter.
In use it's sturdy as hell and gives a mirror finish on good material. I can also slow the feed right down and take 1mm deep cuts if I'm trying to shift a lot of metal. It's the most used tool in the workshop because every job gets a skim at some point. I guess over the years it's shifted hundreds of pounds of metal. It doesn't owe me anything that's for sure.
If I had to flycut something 18" long and as wide as 12" I think I'd start with a bigger bar. Maybe 3" x 1.5" and it would need to run at about 15" cutting diameter ideally. That means about 28" mill travel so it might just be ok for a Bridgeport clone. I'd check your table travel first and do some calcs before making up tooling you find you can't use. Rpm would be 350 with carbide tooling on aluminium. -- Dave Baker Puma Race Engines
formatting link
Camp American engineer minces about for high performance specialist (4,4,7)
Reply to
Dave Baker

Site Timeline

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.