CNC Settings for milling and engraving panels

[Savvy]

After finding the hard way how frustrating it can be getting a cheap chinese CNC machine to cut and engrave panels, I thought I share my settings to-date. I'm still finding better ways to do things so this will be edited when required. It's also a good place to leave this so I can find the info the next time I need to do this Fee free to add any info, it might save somebody losing some hair.

 

Here's a couple of shots of my first completed panel, with a demo of the backlighting which only has 1 strip of led in the demo so will be better when completed.

 

Backlighting pick didn't come out very well, I'll replace it once it's cleaned up a bit.

 

Settings for Milling Acrylic:

First make sure you are using cast acrylic as extruded acrylic will melt on the bit and break it.

 

Starting setup is as follows:

 

Bit: Single flute 3mm end mill

Feed Rate: 200 - 600mm/min (start lower, see more info in below posts)

Plunge Rate: 120mm/min

Spindle RPM: 8000 - 12,000rpm

Depth per cut: 0.25mm (this seems low but it's the only way to stop my bits breaking)

 

If you get chattering, then lower your feed rate. Too low feed rates can increase friction and cause melting.

Sharkfin61 mentioned that setting the Spindle direction to clockwise and set the travel path to anti-clockwise gives the cleanest cuts.

 

Painting the panels:

Spray 1 coat of primer and 2 coats of good quality automotive black spray can. Lightly sand in between and leave to cure for 24hours

 

Settings for engraving panel text:

Make sure text is 'exploded' from Fusion 360 before exporting as a .dxf, otherwise it will come through as a blank box in EstlCam.

 

Bit:So far it looks like a 1mm (non-straight end bit is best). The tip is very slightly 'peaked' which allows different thickness of the font based on the depth of cut.

Alternative Bit: Just use the pointy knife bits that come with the machine and set to 0.08 depth

Feed Rate: 250mm/min

Plunge Rate: 120mm/min

Spindle RPM: 12000

Depth of cut: 0.08 - 0.1 depending on how fine you want the font.

 

Using Estlcam, select Engraving and set the outside line of the font object:

Test examples:

0.1 depth cut: Font height is 4mm so quite small

 

0.08 depth cut: Font height is 4mm so quite small

 

General Tips /Notes:

• Make sure the nuts and bolts on the CNC machine are not loose, especially where the travel rods connect to the X/Y/X motor. As this can cause slipping.
• If the cutting bit is 'Chattering', your travel speed is too high
• When changing a bit, first push the Collet into the collet ring. This will 'click' into place, these two parts can then being installed into the spindle. Not doing this can cause the bit to wobble
• With the machine off, turn the spindle to ensure the end of the bit doesn't 'wobble' due to it being incorrectly mounted into the collet. This will instantly break the bit as soon as it moves in the plastic.
• Using an upward spiral end mill will pull the plastic flakes away better but may pull the sheet up causing problems.

Edited April 18, 2021 by Savvy

[sharkfin61]

Thank you, Savvy.

I think, this is a great write-up of the essentials when s.o. thinks about starting with cutting/milling and engraving.

Wish I had those info a few weeks earlier, would have saved me and the environment from a lot of waste. But the road I went, was incredible educational and showed me also a lot of other things. Most important thing was, it showed me how incredible helpful people we have inside this community!

So, I can only encourage everyone, who thinks about having a more immersive experience with the simulator, with having a haptic feedback when flipping a switch or turning a knob, to start building.

VR might be great for visuals (as long as you can afford the hardware) but panels are a lot of steps closer to the real thing (just my opinion).

 

Just as a small addition to your data, the direction of spindle and direction of the cutting track is also important for the clean edges of the acrylic. Keep in mind that the results may vary from one to another material (cast acrylic in my case).

Test was done this morning with the 20k spindle from Genmitsu @

9800rpm,

3.175 mm "o" flute upcut endmill (Amana Tool - 51410-K) 

plunge rate 150mm/min

feedrate 700mm/min

Depth per cut: 0.3 mm

Complete Depth: 0.6 mm

chips were only brushed away, no filing, no sanding of the edges

 

Turned out that the best result is the upper right square, cut direction counterclockwise, spindle direction clockwise.

Edited April 18, 2021 by sharkfin61
Picture and additions

[Savvy]

Great point regarding the spindle direction! I was actually wondering if that might have an effect. Fortunately mine just happened to be set to clockwise rotation and the path was going anti-clockwise so I was already getting pretty good results.

[amido]

finally a post where to deal with CNC cutting.
thank you very much for your considerations, as soon as the work allows me I will do some tests.
thanks thanks thanks

[ctytler]

Thanks for creating this post. I have an alternate way I ended up going for engraving on CNC, that may be especially helpful for anyone looking to engrave very small text (but it works for large too).

 

I used a spring-loaded Diamond Drag bit, I got one off eBay that's still pretty pricey - but cheaper than a laser at least.

 

I used Fusion 360 for the CAM profile and to represent the Tool I just said it was a flat endmill with 1 thou diameter, the rest of the settings don't really matter that much. Since it's a drag bit, I run the gcode without turning on the router, so the spindle speed doesn't matter. Also since it's just dragging the tip across the surface the cutting rate doesn't matter much for the material. You should be able to set it as high as your machine can accurately move.

 

 

I designed using the "Text" tool directly in Fusion 360 sketch, and extrude (cut) them -1mm into the material. The depth doesn't really matter since the bit is spring loaded, but providing a significant depth makes sure there's always solid contact with the surface.

 

 

 

I engrave the text using two operations, first a 2D Face operation:

 

 

Followed by a 2D Contour operation to clean up the outlines:

 

This obviously takes a long time to run (about an hour for this full panel), but comes out with good results.

 

Posted a clip of the engraving here: https://imgur.com/gallery/sgssKEy

 

Final results (majority of text is 3mm height, some set to 2.5mm):

[Mr_Burns]

9 hours ago, ctytler said:

Thanks for creating this post. I have an alternate way I ended up going for engraving on CNC, that may be especially helpful for anyone looking to engrave very small text (but it works for large too).

 

I used a spring-loaded Diamond Drag bit, I got one off eBay that's still pretty pricey - but cheaper than a laser at least.

 

I used Fusion 360 for the CAM profile and to represent the Tool I just said it was a flat endmill with 1 thou diameter, the rest of the settings don't really matter that much. Since it's a drag bit, I run the gcode without turning on the router, so the spindle speed doesn't matter. Also since it's just dragging the tip across the surface the cutting rate doesn't matter much for the material. You should be able to set it as high as your machine can accurately move.

 

 

I designed using the "Text" tool directly in Fusion 360 sketch, and extrude (cut) them -1mm into the material. The depth doesn't really matter since the bit is spring loaded, but providing a significant depth makes sure there's always solid contact with the surface.

 

 

 

I engrave the text using two operations, first a 2D Face operation:

 

 

Followed by a 2D Contour operation to clean up the outlines:

 

This obviously takes a long time to run (about an hour for this full panel), but comes out with good results.

 

Posted a clip of the engraving here: https://imgur.com/gallery/sgssKEy

 

Final results (majority of text is 3mm height, some set to 2.5mm):

I bet its easier on the ears too?

[obious]

What machine are people using to mill out their panels? I'm thinking of buying this but not sure if its any good?

[sharkfin61]

I think that depends strongly on how much you are willing to invest. I also use a 3018 (from Saintsmart Genmitsu) but, as I only have it for milling panels, I should have rather sticked to a K40 Laser Cutter/Engraver. The CNC can do the work too, but I feel it would be faster, easier and cleaner to lasercut the acrylic.

FYI, I upgraded the Spindle to a 20k rpm spindle, put a dragchain on it to sort the cables, installed some end-stops and a fume extractor, and finally built an enclosure for it.
After all, it was a lot of fun, but also blood, sweat and tears to get it up running as a CNC and an engraving laser.

[Vinc_Vega]

Since almost 5 years I'm using my Stepcraft 420 2nd edition https://shop.stepcraft-systems.com/stepcraft-2-420-construction-kit, controlled by WinPC-NC and am happy with it.

EstlCam is a really good post processor to prepare all the traces.

For engraving the panels I recommend roundes bits with a radius from 0.2 to 0.5 mm https://www.sorotec.de/shop/Cutting-Tools/sorotec-tools/Engraving-bits/Radius-Router-Bit/

My PCBs were engraved by using 30° V-Router bits like that https://www.sorotec.de/shop/V-Router-Bit-30-.html

 

 

Regards,

Vinc

 

 

Edited May 3, 2021 by Vinc_Vega

[Savvy]

16 hours ago, obious said:

What machine are people using to mill out their panels? I'm thinking of buying this but not sure if its any good?

I've got the 3020 version of that one and are quite happy with it. I've managed to get what I would consider pretty good looking panels created just using the knife blade (which comes with the kit) to engrave.

Edited May 4, 2021 by Savvy

[No1sonuk]

Thanks for this info.
Something to consider is the "Bit fan", which is literally a fan attached on the shank of the bit.
It blows air down while it's spinning, cooling the chips and clearing them away (in ALL directions!  )

https://www.bantamtools.com/blog/introducing-the-bit-fan-a-new-othermill-accessory-you-can-make

 

[CorporalCarrot]

Two things to consider when using the "Bit Fan" is that it may affect accuracy, and be a potential source of injury if you are not careful.

 

The idea is pretty sound, but the thing to keep in mind is that the fan will be rotating at whatever speed you set the machine spindle too, which is usually as fast as possible for most people (in excess of 8,000 rpm on basic machines, but higher end hobbyist spindles can reach 20,00rpm or more).  As the instructions are to manufacture them yourself, most people would print them (I guess, the .nc file might not work with anything other than the bantam machine it is written for).  It is likely that the fan won't be very well balanced.  At low RPM this probably isn't much of an issue, but at higher RPM it will start to have an effect on accuracy (i.e. a 1mm slot drill may produce a slot that is >1.0mm).  This will be more noticeable on lower end spindles (with lower quality bearings) and lower stiffness spindle mounts.  Your design/product may not be affected by this effect, as the effect maybe be too small to notice, but if you are milling PCBs with a 20 deg. V-bit and looking for small traces, then it could easily be significant then (although you should not be blowing the debris from a fibre glass copper clad board anyway - the dust is highly irritant if inhaled and will do you no favours! - Vacuuming is the way to go here).

 

The other problem could be that the fan fails at high RPM, sending bits of plastic out like a grenade.  They are unlikely to do any serious damage if they hit a clothed part, but if they ping you in the eye, which could cause some serious injury.

 

I'm am not trying to put people off using them (they seem like an innovative solution for many), but just be weary of these pitfalls and account for them accordingly.  Personally, I have a small shop compressor, which provides compressed air and I've made a small nozzle to blow regulated air on the cutting tip (although mostly to cool it).  If you get into manufacturing bits and bobs, they are worth the investment.  You can pick up cheapish ones for around £100 in the UK, but do your research and make sure it has the necessary rated flow rate (otherwise it won't keep up and run out of air and/or kill the compress by over working it). Mine is rated at 14 cfm, but I do a bit of sandblasting and spray painting too (although it is only just up to those jobs).  9 cfm compressors are probably entry level imho.

 

...having written the above, I've overlooked the more obvious solution, which I use most of the time anyway!   Vacuuming the chips is probably the most straightforward way of keep the cutter clear!  It also means no mess at the end of the run  You could use a domestic vacuum cleaner, but they are not intended to be used for extended periods of time, and can overheat quick easily and burn out.  I have a workshop dust extractor, which is designed to run for longer periods of time and work with clearing swarf and other debris.  This one is not the exact model I have, but very similar.  Just got a hose reducer down to a 40mm hose and have a smaller nozzle on the end to collect the chips.

Edited May 14, 2021 by CorporalCarrot

[No1sonuk]

On 5/14/2021 at 8:05 AM, CorporalCarrot said:

Two things to consider when using the "Bit Fan" is that it may affect accuracy, and be a potential source of injury if you are not careful.

[deleted stuff]

All good points.

 

I milled mine from a solid piece of cutting board.

I don't use one when milling PCBs for exactly the reason you stated - the dust.

And who the hell is operating one of these machines when they're not wearing safety glasses?!? 
Not to mention the ABEK filtered respirator when using a laser.

As for the last comment:  Vacuuming alone may not be enough as it doesn't have the cooling effect blowing directed air does.

[gersonh]

I can only encourage everyone, who thinks about having a more immersive experience with the simulator, with having a haptic feedback when flipping a switch or turning a knob, to start building.