Water cooled spindle speed and bit type question.

[Ollie78]

Hi

I have been trying to run my cnc router better and taking more notice of the recommended chip load settings for the bits etc.
In doing so I have already decreased my spindle speed for many bits to 18000 rpm and increased my mm/min on X and Y, still very conservative at 5000mm/min but I might add more gradually.
However, I have a specific bit which is a 3 flute engraving bit, in order to get a respectable chip load at 18000rpm it wants me to run at over 10,000mm/min.
I have a little trepidation about running my machine at this speed though it might be fine.

So maybe I can slow the bit rpm down, does anyone know or have experience of a sensible minimum for a 2.2kw water cooled spindle with VFD, I have heard they do not perform well at lower speeds.

Secondary question, I am running a single flute compression bit for plywood and laminates and it works really well but it has about 7 mm of upcut, this can be annoying for pocketing when shallow and I dont want to keep changing the bit. I am looking for a single flute compression with a shorter upcut section maybe 4mm or something, does anyone have a favourite bit for birch ply and laminates.

Ollie

 

[Chief Sawdust Maker]

I do a lot of CNC batch work in British oak and also birch ply using a 2kw liquid cooled spindle with ER20 collets and a VFD
My current setup has evolved over the last 2 years
I run at 19,000 for pretty much all cutters usually at around 110 inches/min or 3,000 mm/min usually using a 1/4 compression with 1 x D depth of cut
What sort of chip loading are you looking for?
I always avoid single flute as i feel they are unbalanced. For shallow pocketing I use a down cut and lower the chiploading with a jet of compressed air to aid chip evacuation.
Hope this helps

D

 

[Ollie78]

I do a lot of CNC batch work in British oak and also birch ply using a 2kw liquid cooled spindle with ER20 collets and a VFD
My current setup has evolved over the last 2 years
I run at 19,000 for pretty much all cutters usually at around 110 inches/min or 3,000 mm/min usually using a 1/4 compression with 1 x D depth of cut
What sort of chip loading are you looking for?
I always avoid single flute as i feel they are unbalanced. For shallow pocketing I use a down cut and lower the chiploading with a jet of compressed air to aid chip evacuation.
Hope this helps

D

Hi Darren

This is similar to my speeds at present, I have found the single flute or 1+1 bits to be excellent ( currentlly using a CMT one 6mm ) .

I was previously running too slow and getting more sawdust rather than chips, been doing some birch ply today single compression at 18000 rpm and 4800 mm/min and its making nice chips and zero fine dust, doing 3 passes (18mm ply) with the final pass reversing to conventional for better surface finish (leaving 0.4mm for last pass allowance). This gives a chip of 0.26mm.

To get performance like this from a 3 flute I will either have to slow the spindle a lot or speed up the feed, probably a combo of both.

I should probably use a downcut for the shallower pockets but I dont have an ATC on this machine, I will have on my new one but still waiting for it.
I swear I have seen a bit somewhere with a very small upcut part.

Probably over thinking it but having seen improvement I want to improve more.

Ollie

 

[worn thumbs]

The original question mentions engraving and normally engraving involves a comparatively tiny amount of material removal and a small diameter cutter.The small diameter leads to a lower peripheral speed and a different approach to cutting outlines.In fact,with a V engraving tool there is a variation in chip load across the engaged portion of the cutting flute as a result,so which segment would you apply a chip load calculation to?I have happily run a 7Kw spindle at 10,000 mm/min but it had ample power to cope with the feed rate and I was certain the workpiece wouldn't move.The only time I ran a 2,2Kw spindle,I used 7500 rpm and 5,000 mm/min to take a light skim (0.5mm) on a new spoilboard-the spindle coped but the machine was flexing and I won't bore you with the evasive actions of the company responsible for the construction of the machine.

 

[Ollie78]

The original question mentions engraving and normally engraving involves a comparatively tiny amount of material removal and a small diameter cutter.The small diameter leads to a lower peripheral speed and a different approach to cutting outlines.In fact,with a V engraving tool there is a variation in chip load across the engaged portion of the cutting flute as a result,so which segment would you apply a chip load calculation to?I have happily run a 7Kw spindle at 10,000 mm/min but it had ample power to cope with the feed rate and I was certain the workpiece wouldn't move.The only time I ran a 2,2Kw spindle,I used 7500 rpm and 5,000 mm/min to take a light skim (0.5mm) on a new spoilboard-the spindle coped but the machine was flexing and I won't bore you with the evasive actions of the company responsible for the construction of the machine.

Interesting point about the variation in the speed of the cutting edge at different points in the cutter, I would say that perhaps what I am doing is more "V carving " than strictly engraving.
I wonder how vectric software calculates this, it might be an interesting experiment to program the same project and cutters in different CAM options and see if they agree with each other.
I ran the v bit at 16000 rpm and 5000mm/ min today and it performed nicely but I think it could go a lot faster on the movement or slower on the spindle.
I will do more tests when I have time.
The more I find out about this stuff the less I know, it is a deep subject with much to learn. I have learned however, that there is no way a machine should flex cutting half a mm.

Ollie

 

[Sideways]

Based on some reading around this, I'd say don't drop your spindle speed below 50% as motor torque is typically going to roll off somewhere below this. Sometimes gradually, sometimes precipitously, it depends on the motor.
Keep an eye on motor current. In the region that the motor is supposed to work, motor current is fairly constant, torque is roughly constant and motor power drops as speed drops. Half the speed, half the power.
You want to avoid increased current which will lead to increased heating in the spindle.

You have the advantage of water cooling which is good.
You should look at how your vfd is programmed to handle overloads.
Remember, these spindles have low torque and rely on speed to achieve their rated power. You don't get any extra torque at lower speeds so half the speed, half the power - take care not to stall the spindle.

 

[worn thumbs]

The point about not stalling the spindle is very,very important.You may have a data sheet with the makers recommendation for a minimum speed and if so,you should follow it.I have pushed speeds below this kind of limit when using a drill and I don't want to be in the building if anybody tries using a drill bit at 18,000 rpm.