Feed rate on Denford microrouter

[andy_con]

I'm sure feed rates have been discussed 100s if not 1000s of times.

I've got a microrouter and I always seem to get burning when cutting.

Spindle is a 23k rpm 1.5hp, I'm currently cutting mdf from B&q. Doc 2mm feed rate 450mm a min with a standard length 6mm end mill.

Is this to slow?

[Clive S]

I'm sure feed rates have been discussed 100s if not 1000s of times.

I've got a microrouter and I always seem to get burning when cutting.

Spindle is a 23k rpm 1.5hp, I'm currently cutting mdf from B&q. Doc 2mm feed rate 450mm a min with a standard length 6mm end mill.

Is this to slow?

Miles to slow how many flutes? try 3-4mtr/min. B&Q mdf is not the best

edit: depends on how rigid the machine is as well I think 3-4 is slow

[andy_con]

2 flute, machine is pretty riged

[andy_con]

So no further tips from anyone...

[AndyUK]

So no further tips from anyone...

I think they're all waiting to see how 3-4m/min goes :)

[andy_con]

I think they're all waiting to see how 3-4m/min goes :)

LOL so am I, does someone have a machine they can test that on for me? Maybe film it

[andy_con]

what calculators do people use for speeds and feeds when cutting wood.

I have cnc cook book for metal but dont think it does wood

[JAZZCNC]

Andy speeds n feeds are difficult to advise because of lots of variables come into play and nearly all the calculators are based on much Stiffer machines with much higher Spindle power than what you have so are pretty much useless to you.
Every machine is different, every material and tool is different so Trial and error are the best way to learn.
Material to be cut, Cutter size, Cutter material, # flutes, flute length, flute type along with machine stiffness and spindle power all factor into the speed you will cut at.

In all honesty, no one unless using the same machine with same tool and same material can accurately advise you on cutting parameters. Any suggestion will just be a baseline guide that you will need to adjust up or down based on your setup.

The Sad truth is the Denford machine you have cannot reach the feeds required to cut MDF correctly so you'll always have to compromise.
Clive's suggested 3-4mtr/min is still on the slow side for 2F 6mm cutter. 5-6 Mtr/min would be more like it and that's using HSS cutter. use carbide and you are even higher.
Your Denford machine will probably top out at 3-4Mtr/min Rapids which means you'll have very little torque left and if try cutting at these feeds you'll get stalling motors. So at best you might be able to cut at 3mtr/min so wouldn't go above that.

Also, note that even if you do set high feed rates that doesn't mean your actually achieving those feeds.? I've seen lots of machines like the Denfords, Boxfords etc meant for schools running code with high feeds and the user thinks they are getting those feeds because machine works ok. But in reality, they couldn't possibly achieve those feeds because the machines Max velocity is lower than the programmed feed rate.

The reason they don't realize is that often the machine is De-tuned for the School environment so it will happily cut at Full Velocity without stalling motors. But that velocity is much lower than programmed feed rate so even thou the screen will Show the Programmed feed set in G-code the actual true velocity is the Max velocity set in Motor tuning setup.

This my starting suggestion knowing this type of machine based on 6mm 2F HSS cutter.
DOC 3mm
RPM 18,000
Feed 2500mm/min

This will cut ok but you could get some burning in corners etc.
I would start with this and then try increasing just the feed rate until either maxed out or get stalled motors. This will give you an idea of Max velocity can achieve and when found Limit back of 20%

Next, I would increase DOC, 50% cutter diameter is a good starting point with cutters above 4mm Dia, below 4mm use 30%. But in MDF it's not uncommon to use 80 or 100%. If using Carbide tooling then 100% Dia is easy done in MDF.

Next and in conjunction with both suggestions above you can tweak the RPM based on how it sounds and looks regards the cut.

Try this and see how it goes.