Thread: CNC - Speeds and Feeds

David,

There are two kinds of cnc users on this forum I have seen. Most of us appear to be hobbyist and our machines do not compare.

Mine for instance has a 1.5kW spindle and a max travel rate of 2500mm/min.

My cut depth at max speed is at most 1.5mm on soft wood only.

I ran a 5.5kw vacuum table flat bed (Biesse Rover 24) for a few years at my old work and came to the following guides, all of these are based around 18k RPM, which was max speed for our machine.

Nesting/sheet materials:
8-12000 mm/min
3-flute carbide (either compression or up-spiral, depending on application), 10mm bit for material up to and including 19mm thick, 12mm bit for thicker material up to 33mm (that was the flute length, so can't cut thicker).
Cut full depth unless parts are small and the vacuum can't hold them against the cutting pressure. If that's the case, cut all parts leaving 2mm at the bottom (so the vacuum is still holding a full sheet), then go back and cut the last 2 mm.

Timber:
4-6000 mm/min
16 and 20mm (smaller bits are, of course, not a problem) 3-flute spiral carbide bits, proper roughing (jagged edge to reduce cutting pressure and up spiral for chip evacuation) and finishing bits (smooth edge for smooth finish and down spiral to reduce breakout)
Roughing cut depth generally 1-2x diameter, leaving 1mm to clean up with finishing bit (full depth)

Bits under 5mm:
3-4000 mm/min
Generally single flute straight carbide
I don't like cutting more than 1xD because they're fragile.

6mm 2-flute down spiral in 3mm ply:
18000 mm/min (this was for cutting out shapes for moulded chairs, the finish didn't really matter and this was the best balance of speed and not completely blowing the edges out)

Smaller bits = slower feed or you'll snap them (been there, done that)
Deeper cut = slower feed for the same reason

The biggest thing is don't feed too slow; large chips carry away more heat from the tool and help prevent the edge from burning up prematurely

The manufacture has suggested to me a spindle speed of 18000 rpm and feed rate of 6000 - 10000 mm per min is a likely starting point for 3 to 5 mm vertical passes with a 6mm flute.

That sounds pretty reasonable, but I think you could comfortably go to 8-10mm depth at the slower end of the feed range.

If you've got any other questions, let me know

Amanatool and Whiteside both have Fusion 360 (and Vectric) library downloads for all their tools. I've been using these for my AvidCNC without issues so far (mainly cutting cheap poplar-cored ply). Can be scary - particularly with the 3D adaptive paths. Goes at the wood with an animal yowl and a cloud of sawdust, and 10's of hours of modelling work appears in minutes.

For a paid option, and for tools where you don't have a library download, , CNCCookbook does a cloud-based calculator -seems quite comprehensive. Used to have a Mac version but looks like that has disappeared. There's a free trial, and lots of education/info on the site. I haven't really got into it yet, so not sure how good it is/whether it's worth the $.

Hi
Yes this can be very confronting in the beginning. I teach joinery and CNC machining and this is always a steep and confusing learning curve for my apprentices.

Feeds and speeds is very importantly related to the type of material, thickness of material, finish required and very importantly the type of tooling being used.

The 5.5 kw motor stated is sufficient for most work, but this is directly related to what I have stated above. Just because you have more 'grunt' so to speak does not necessarily mean you can increase the feed speed and just plough through it.

I could write a novel on this subject but I will just write about marine ply, as this is what you need info on.

Marine ply has a different type of glue than standard plywood and is harder. Depending on the thickness of the plywood you will either have to raise and lower the feed speed, or program (in your software) to do more than one pass (2 or more passes). This now depends on your tooling (diameter and number of flutes) as well as type of configuration (compression, down cut, roughing spiral etc) and of course the quality of the tooling. Remember you only get what you are paying for.

As a guide only, say you are machining 18mm marine ply -3 x 6mm passes, 2 flute 8mm compression, 18000-20000rpm, 6000mm/min to start with. The key here is to listen to the machine and tooling. There should be no 'screaming' or high pitch 'chattering' if there is, slow the feed speed down slightly, adjust the spindle speed slightly. As I said in the beginning, this is a steep learning curve, but the real key here is to listen and watch the machining and adjust to suit.

It is really hard to give advice like this without practical demonstrating what I mean, but I hope this has help some what.

Kevin

Originally Posted by kph

As a guide only, say you are machining 18mm marine ply -3 x 6mm passes, 2 flute 8mm compression, 18000-20000rpm, 6000mm/min to start with.

An 8mm bit can quite comfortably do that in 2 passes, I know a 10mm 3-flute does it in one pass at double your feed rate. Don't be afraid to push your tools, you'd be surprised how hard you can actually go.