feeds and speeds Recommendations for belt drive cnc

[marbles]

Howdy,

My belt drive cnc was built for milling foamboard but recently thought it would be nice to cut plywood and acrylic. Basic spec: nema 24, t5 belt, Gecko, Mach 3, 900w spindle (12-26,000rpm)

I was reading this very helpful F&S thread below, which gives a good indication of what i should be aiming for. However as my machine uses, belts and v-groove bearings and is a light weight design for speed I am wondering if there are setting I can use which will at least give me a chance of cutting something denser with multiple passed with reasonable success.

http://www.mycncuk.com/threads/4330-Router-bit-recommendation-spindle-speed-and-feed-rate

I can see from cutting through 9mm ply using 2mm passes that the tip of the single flute cutter is blacking pretty quickly. The timber is not blackening but 20mm/s is not very fast is it ha ha and probably part of the problem.

It could be that the whole machine needs rebuilt to cut more resistant materials but any indication of
where I can look first to at least try to get the machine i've got cutting ply would be useful.

Thanks.

22457

[Ger21]

I can see from cutting through 9mm ply using 2mm passes that the tip of the single flute cutter is blacking pretty quickly. The timber is not blackening but 20mm/s is not very fast is it ha ha and probably part of the problem.


What size tool, and how many flutes?
What feed and speed did you use?

Try 4-5m/min at 15,000 rpm.

[marbles]

What size tool, and how many flutes?
What feed and speed did you use?

Try 4-5m/min at 15,000 rpm.

Hi Gerry,

Thanks for reply. I was using a single flute spiral bit. 4mm dia and 12mm cut length. Spindle set at 'No 6', which i would take to be about 26,000rpm

I'll need to get back to you about the exact feeds and speeds tomorrow. I set the feed rate in Aspire to 80mm/s in 2mm passes but of course this doesnt necessarily relate to the actual rate, which i'll work out tomorrow in Mach3.

I did notice that it was rounding corners again so that'll need a tweak in motor tuning for wood. Currently settings are for foamboard carving.

Thanks

22458

[marbles]

What size tool, and how many flutes?
What feed and speed did you use?

Try 4-5m/min at 15,000 rpm.

Hi,

I set Aspire to profile cut a 400mm square at 100mm/s and timed how long it took to mock cut out the full 1600mm. This took 51.40 seconds. So at 30.9mm/s actual speed, clearly not the 100mm/s set in Aspire. The spindle speed is not set in Aspire but on the actual spindle.

I tried the test again using a faster speed but it gave exactly the same time to travel 1600mm. So it must be that motor tune setting are incorrect or inhibiting speed.

My config settings are 26 stesp- 2000 velocity - 1000 acceleration

(As as side note I recalibrated X and Y axis so they are scaled correctly).

lets say as a rule of thumb I wish to cut out 12mm plyood in forms less that A4 scale with a mixture of straight corner and curved shapes, 10mm slots and 8mm holes etc. So reasonable detail.

I'm a little bit stumped why I couldnt change its speed in Aspire and why 100mm/s does not translate to its actual speed. I'm missing something basic am I not ha!

Any ideas welcome

This is the gcode file.

( Profile 1600mm test )
( File created: Friday, August 04, 2017 - 09:52 PM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 410.000, Y= 410.000, Z= 4.000)
()
(Toolpaths used in this file:)
(Profile 1)
(Tools used in this file: )
(1 = End Mill {3 mm})
N100G00G21G17G90G40G49G80
N110G71G91.1
N120T1M06
N130 (End Mill {3 mm})
N140G00G43Z20.000H1
N150S20000M03
N160(Toolpath:- Profile 1)
N170()
N180G94
N190X0.000Y0.000F6000.0
N200G00X4.620Y4.260Z6.000
N210G1Z-0.500F600.0
N220G2X3.120Y5.760I0.000J1.500F6000.0
N230G1Y405.760
N240G2X4.620Y407.260I1.500J0.000
N250G1X404.620
N260G2X406.120Y405.760I0.000J-1.500
N270G1Y5.760
N280G2X404.620Y4.260I-1.500J0.000
N290G1X4.620
N300G00Z6.000
N310G00Z20.000
N320G00X0.000Y0.000
N330M09
N340M30
%

[Clive S]

Well is sounds like you have a max vel. setting somewhere that will limit your commanded speed. What software are you using?

[marbles]

Well is sounds like you have a max vel. setting somewhere that will limit your commanded speed. What software are you using?

Hmm..i hadnt thought of that i'll have a look in Mach3 tomorrow. Thanks

[Ger21]

Your velocity is set to 2000mm/min, which is about 33mm/sec. The Velocity setting is the Maximum Mach3 will move at.

[marbles]

Your velocity is set to 2000mm/min, which is about 33mm/sec. The Velocity setting is the Maximum Mach3 will move at.

Ah its the max! Of course..better increase it a bit. Thanks!

[paulus.v]

I did notice that it was rounding corners again so that'll need a tweak in motor tuning for wood. Currently settings are for foamboard carving.


Check on the general config page if you have set the "Stop CV on angles > xx Degrees" You can try a value of 50 deg. and reduce it if needed.


To set the velocity and acceleration in motor tunning, increase the values and test by manual jogging and applying some force by hand against the moving axis until the motors will stall to easy. Then decrease a bit the values. You have to restart mach3 for the modified motor tuning settings to take effect.

[marbles]

Check on the general config page if you have set the "Stop CV on angles > xx Degrees" You can try a value of 50 deg. and reduce it if needed.


To set the velocity and acceleration in motor tuning, increase the values and test by manual jogging and applying some force by hand against the moving axis until the motors will stall to easy. Then decrease a bit the values. You have to restart mach3 for the modified motor tuning settings to take effect.

Thanks. All very helpful advice. As I have re-tensioned the v-groove wheels i've noticed it stalling a few times. so will modify and restart.

[marbles]

Seem to be getting somewhere with the 12mm ply cutting after carrying out everyone's suggestions + tightening a slightly slack gantry. Thanks for everyone's help.

Feed 20mm/s
Speed 15,000rpm
3mm, two flute up cutter on 2mm deep passes
Mach3: Velocity 2500 and acceleration 500

I'm not getting the F/S issue of cutting corners i had before and neither is the cutter or timber burnt.
I am however still getting a furry edge, the block of wood was lightly sanded to get rid of the burr edge so they are not so prominent in this image.

I'm going to invest in a 3.175mm down cut and compression cutter to see where those results take me. At the moment i'm only intending to cut smaller parts and perhaps some cabinet doors at a later stage when I upgrade the gantry and whole machine to R&P.

Cheers

22520

[Ger21]

To get rid of the fuzzy top edge, use a downcut bit, and do NOT climb cut.