CNC Milling

I've noticed when watching videos of CNC milling that the technique involves small cuts but repeated many times.

Is this determined by the program itself or does it need to be programmed in by the operator and, if so, are there any rules for depth and width of each cut?

Brian

All of the above!

they are hobby machines and some are lighter router machines meant for wood and light materials. A full size cnc mill will remove high levels of metal, removal rate is dependant on spindle power. There is a big difference between a 500 watt powered spindle and a 20kw one.

Sorry for my cryptic reply earlier, which was factually accurate but absolutely useless!

The machine controller has to be supplied with "G Code" to make it move. This can be generated manually, by a wizard in the controller itself, or by a CAD/CAM system. For the first and second, the width, depth and speed of cut generally have to be set manually (though there might also be "wizards" to set them for a particular material and cutter). CAD/CAM systems such as Fusion 360 will probably have tool & material libraries to largely automate feeds and speeds. If you look around the web there are online tools to recommend feeds and speeds.

The principle is the same whether it's a light "hobby" or a huge industrial machine - with the hobby machine you would use a smaller cutter and slower feeds (though still a high spindle speed).

If the material being cut is aluminium 6082T6 or 7075 the maximum DOC I use is cutter diameter with a width of cut at 1/4 of cutter diameter, feed rate adjusted between 40 and 400mm/min with a spindle max speed of 2000rpm from a DC 400W output motor.
Rate of material removal will depend on whether the part is securely fixed as many will know flimsy parts need much care when machining, if job secure the rates stated above would be used as a starting point but if the machine was not happy then the width of cut would be reduced to lighten the load.

I really need to get some cutters designed for aluminium to take advantage of the increased cutting performance, I am only a hobby user so if a job takes longer than industrial rates that's not a problem.

The width and DOC are set in the cnc program by the programmer writers choice when selecting the tool parameters, that choice stays with the tool for the program.
My machine uses manually written G and M code programs and has a 210 line of code limit so CAD/CAM programming is not possible.

You can see the mill cutting at the link  https://youtu.be/udDhZlu53e0

Emgee

Edited By Emgee on 26/01/2020 10:12:05

The current thinking is to use as much of the side of the cutter as possible with a shallow stepover and high speeds and feeds. This means the cutter wear is spread over all the cutter not just the end and the hot chips dissipate the heat.

These methods work best with heavy machines but just as suitable for hobby ones provided machines ability is taken into account, it is known as trichodial cutting. The program will work out where the tool move but the person setting up will have entered feeds, speeds, depth and height of cut to suit the material and cutter chosen though most manufacturers will publish guide figures or the CAm will have them already.

Toolpaths are selected by the programmer, but the program sorts out the movement details. The programmer also selects speeds, feeds, DOC and WOC. Although of course tool manufacturers give guidelines. I've never found the online speeds and feeds calculators very useful, I prefer to use a mix of experience and calculation.

When I started using my CNC mill (same horsepower as my Bridfgeport) I eventually learnt that it was happier running smaller cutters at higher speeds and feeds to achieve the same metal removal rate. I rarely use a cutter bigger than 10mm on the CNC mill in contrast to the Bridgeport.

Using CNC is a slightly different mindset. I run mine at much faster spindle speeds than I run the Bridgeport and I often run a roughing pass and a finish pass with different cutters. Another useful feature of the more advanced CAM programs is the ability to re-machine. Let''s say we need a recess 70mm by 50mm by 10mm deep with 1.8mm radii in the corner. The 'simple' approach would be to machine the whole recess with a 3mm cutter. But using re-machining one can machine the whole recess with, say, a 10mm cutter. Then one swaps to a 3mm cutter and the CAM program knows that only the radii in the corners need tidying up.

Andrew

The other thing that you may have seen are very fine finishing cuts, if there are complicated angles and curves than the final passes will be done in very small stepovers to get the smoothest finish possible.