[peps1]

Hi, I hope this is the right place to ask, sorry mods if it is not, just finding my feet here!

I have just been running a whole bunch of pocketing feed speeds/depths on my 3020 and have come to the conclusion I can cut pockets in MDF at 400mm/min with a 5mm depth of cut without bogging down the 300w spindle (with a 40% stepover).


Is there a rough rule of thumb that I can use this information to work out where to start with working out the contour speeds?


I'm working on the assumption with a contour cut much more of the endmill is in contact with the material = more friction, heat, and higher chip load, so will need to slow the feed or depth down?

[Vlod]

It depends on what type and size of the bit you are using.
Check https://www.amanatool.com/products/r...iAAEgJdZPD_BwE

I use vectric software and Amana bits have tool data base file to download that will show all feeds and speeds for specific bit in a menu when i pick a bit from tool data base, then you can adjust it if it needs…
They have the same for Fusion 360.

[joeavaerage]

Hi,
less sure about wood, MDF etc, but a very common figure of merit is 'surface speed'.

The surface speed is the recommended speed for a tool to rotate past a given material. Its dependent on the tool material and the work material.

For instance a rule of thumb for cutting steel with an uncoated carbide tool is 100m/min. You might increase that to 150m/min if the tool had a good AlTiN coating or similar or you might reduce
it for a really tough steel. The point is that if you attempt to go faster than that you risk the tool getting red hot and that's the end of that!.

For the same steel but a HSS tool you'll slow down to about 50m/min.

Lets say you have a 10mm diameter endmill, uncoated carbide cutting mild steel.
Recommended rpm = 100 (surface speed) / (0.01 (diameter in m) x pi) =3183.7rpm

Aluminum has quite a broad range from 250m/min to 500m/min depending on the particular grade of aluminum. So with the same 10mm carbide tool:
Recommended rpm =250 / (.01 x3.141)=7959rpm to 500 / (.01 x 3.141) =15918 rpm.

Most materials and tools have a 'sweet spot'. You can go slower if you wish but risk overheating if you go too much faster.

Now you have to decide on the thickness of the chip.
I tend to use small to very small endmills down to 0.5mm. They are fairly tender so I use another rule of thumb 1% of diameter per tooth per rev.

So a 1.5mm tool spinning at 24000rpm (fastest my spindle goes) with four flutes:

Feed Rate= 24000 (revs/min) x 0.01 (1%) x 1.5 (diameter in mm) x 4 (four flutes)=1440mm/min

This is a good place to start, If you try to take too much material in one pass you'll overload the tool and snap it, as always you can go slower and for a tough material like steel or stainless I'd go as slow as one quarter
rather than break tools all the time.

With bigger tools, they are stronger and say for a 6mm tool you might allow 2% per tooth per rev, and with a 20mm tool you might allow even 3%. With big tools its sometimes less about snapping the tool
but not overheating or blowing the spindle by having it produce such high power levels continuously.

You can go too slow. When that happens the tool is not really peeling off a chip so much as its giving the material a 'good rub' and really only heating it up. That's bad news. You want and need a chip to be taken
and hoping that the majority of the heat is being carried away with the chip. So by all means go slow and gentle while you get a feel for how much a tool can handle but don't be so gentle that you just
heat up and burn your tool or your material.

Plastics are actually quite tough to cut. Its not that they are hard or strong but rather many of them heat up and the chips weld themselves to the tool and make a real mess in no time. I tend to cut plastics fairly fast
(200m/min to 500m/in) but ALWAYS use flood cooling to wash the chips out of the way otherwise you get Built-Up-Edge (BUE) where chips stick to the tool. It'll wreck your day! Acrylics and polyethelenes are
notorious for BUE.

Craig

[Vlod]

I just want to add,
as your spindle is only 300W you might want to make shallow cuts on some materials but be aggressive with feed.