# Feed rates



## IainL (Dec 12, 2012)

Hi all,
I am cnc routing 18mm softwood ply. I would like to cut this in one pass but do not want to stress the machine. We have a Canadian AXYZ 6010 Twin head with ELTE 5 HP spindles.
Could someone please advise what feed rate and stepdown to use. I have tested with 3meters/min in one pass and it seems to work ok but I don't want to do damage over time
Thanks
Iain


----------



## jw2170 (Jan 24, 2008)

Welcome to the forum, Iain.


----------



## neville9999 (Jul 22, 2010)

A bit slower is always better and kinder on the cutter, you will know if you feed it to fast. NGM


----------



## Phil P (Jul 25, 2010)

Hi Ian and welcome

It would be a help if you could say the type and size of the bit you are using as well as the spindle speed and the quality of cut you are looking for. Without knowing those it is impossible to figure out feeds and speeds IMHO. I have run a similar job in the past on 7HP Columbo spindles at a far higher rate, but it was tooling/quality dependent

Regards

Phil


----------



## IainL (Dec 12, 2012)

Hi again
Bit is an 8mm dia. single flute upward spiral. Spindle speed 21500 rpm.
This is for packaging so cut quality is not critical as long as it is decent enough
Thanks
Iain


----------



## Phil P (Jul 25, 2010)

Hi Ian

With a spiral upcut I'd have thought you could get a higher feed rate, somewhere around 5 to 6 metres even with an 8mm cutter. We used to manage 8 metres with 9.5 diameter 1-flute spirals on 12mm fir ply. 2-flutes we ran a bit slower because they tended to clog and break more easily

Regards

Phil


----------



## IainL (Dec 12, 2012)

Thanks for that Phil, I appreciate the response. The reason I asked the question in the first place is 1) Because I'm fairly new ot CNC work and 2) I thought the machine was possibly making a little too much noise and maybe a touch too much vibration. I don't want to ruin bearings neadlessly.
We cut quite alot of 18mm softwood (spruce) ply....can I do this in one pass?
Cheers
Iain


----------



## Phil P (Jul 25, 2010)

IainL said:


> Thanks for that Phil, I appreciate the response. The reason I asked the question in the first place is 1) Because I'm fairly new ot CNC work and 2) I thought the machine was possibly making a little too much noise and maybe a touch too much vibration. I don't want to ruin bearings neadlessly.
> We cut quite alot of 18mm softwood (spruce) ply....can I do this in one pass?


Hi Ian

All over the 'net I see amateur/inexperienced woodworkers saying the same, WRONG, thing when it comes to spiral cutters. They are convinced that slower is better. Well for spirals IT ISN'T. Spirals were designed specifically to allow CNC machines to reach much higher feed speeds than are possible with straight cutters. If you feed a spiral too slowly, especially if the waste isn't being fully cleared from the gullets you end up with "churning" where the waste is cut and recut many times over. Churning generates heat and lads to the cutter blunting and burning. Even solid carbide cutters can burn - expensive. The larger diameter a cutter is, the less it will heat-up (because there is more material to dissipate heat energy). Also the lower the number of flutes, the easier the cutter will clear waste and the faster it can be fed, although that is at the cost of cut quality. In this particular case you'll probably be able to achieve 3 to 4 metres/min with a full depth cut, although I'd consider bringing your spindle speed down to about 18,000 rpm as this will be less stressful on the motor bearings. I'm not sure that with 8mm I'd want to feed much faster than 4m/min as I'd be a bit concerned about cutter breakages

If in doubt why not take a look at the info on the Onsrud Cutter site?

Regards

Phil


----------



## fixtureman (Jul 5, 2012)

limacrouter said:


> It is not always good to be slow, material might start burning if speed is too low. Recommends 2 pass


He is correct about slow look at the chip load and start at their recommended speeds. Remember a screaming bit is a hunger bit you need to either speed your feed rate or slow your spindle speed.


----------

