The first try of the mill with three axis working was a "ghost" run of a simple program, i.e. the mill quill was not assembled and therefore no metal was being cut. It was really to see that all three axis were working as they should and it gave an opportunity to observe feed rates and motor performance.

The motors were tweaked so their velocity was slightly less and their acceleration a tad more gentle and with a feed rate of around 2.5" per minute all three axis ran quietly and smoothly. The velocity settings were: Acceleration ~2.34 inch/sec/sec and Velocity ~21 inch/sec.

Feed rate is a new sense that has to be learnt as I, like I suspect many, have no idea when manually milling what feed rate is being used as with experience we go on sound and how the cut is performing and adjust the feed for the best finish and speed. All this is done as a second nature rather than consciously computed.

With CNC the feed rate has to be set for the program to follow and it is important to get it right as otherwise all sorts of things will go wrong if set too high with possibly disastrous results to both work and tool. So visually observing feed rates and relating observation to experience is a useful exercise before cutting metal under program control. A help is that in Mach3 despite having preset the feed rate in the G code it can be manually adjusted up or down by a screen button. I found a feed rate of about 2" per minute was about right for a 1/4" diameter end mill.

Another interesting feature is the different spacial awareness that becomes necessary. Initially I had my X and Y table motors wired up so that when the right arrow key on the computer was pressed (under jog control) the X table traveled right and similarly for the left direction. For the Y table the toward operator arrow drove the table towards the operator and again similarly the apposite for the away arrow. For completion the page up key was used to drive the Z axis up and page down key to drive the Z axis down.

The first try at doing a "reference all" operation, i.e. the act of letting the software drive the tables to their home position and automatically zero the machine DRO readings the tables went in the wrong direction. There is a "reverse" facility in Mach3 if this occurs and selecting this to drive the tables to their correct location performed the zero referencing correctly. Of course now the tables travel opposite to the arrow keys on the PC keyboard. However when you look at the Mach3 screen when jogging the cross hairs that identify the tool position move in the correct relationship to the table. So the spatial awareness is the need to think of the jog keys moving the tool to the work not the table to the tool. Now the arrows on the PC keyboard make the correct sense when thinking this way.

I have no idea if this is the "correct way " or not to configure the mill and jog control, but at the moment I have not figured out an alternative. Checking with the Mach3 Forum this arrangement seems to be standard. Perhaps it is because the US users have more gantry machines than vertical mills where such an arrangement would make absolute sense.

The next try of the mill was cutting metal. I devised a test piece consisting of a 3" square contour 0.132" deep having four 1" square islands of 0.100" deep and on top of each island was a 1" diameter circle at 0.050" deep. My idea was that this would show up backlash as the squares would be undersize and the circle not round (and possibly offset from the square) with backlash present.

Setting the work up for machining a contour is worth a mention as when working from stock material it is not necessarily straightforward. The position of the finished job on the raw material needs to be known and its relation to the X and Y edges of the stock material. The X and Y tables need to be first zeroed relative to the tool edge to the edges of the stock material then the table can be jogged by the offset amount that the work is relative to the stock edge. Reset the X and Y tables to zero again and then jog X and Y a second time for half the tool diameter and zero the X and Y DRO readings for the last time. This puts the centre of the tool over the 0,0 point of the work. Finally bring the Z height down so the end of the tool touches the top of the stock material and Zero the Z DRO. This becomes the Z reference from which the depths will be cut. (Slots require a different approach).

The cutting of the test piece immediately showed up the necessity for some form of cover over the front and back of the Y table and also at the drive end of the X table to prevent chips/swarf getting into unwanted places. The arrangement I came up with for these was a simple plate to which spring clip tool holders were riveted and they just clipped over the bars holding the motor mount and ball screw bearing plate.

Using a 5/32" slot drill to cut the work was fine for the squares but the circles were a bit of a disaster and the backlash really showed at the diagonal points where the circle lost its shape. Add to this and the tool had wear at the end giving it a slight taper (yes I should have checked) made the test a bit of a waste.

A simpler test was tried with a rectangle with a 2:1 ratio to its sides lengths. The tool, a 1/4" end mill, was checked and measured for size and found to be 0.002" oversize over both opposite flutes. The cut depth was 0.010" and the width was not over half diameter, so no heavy tool loading, and the total depth set for 0.050" sufficient to measure the edge. The result was an undersize by 0.004" in one direction (X) and 0.005" in the other (Y)

Given the tool was oversize this gave a backlash of 0.002" for X and 0.003" for Y. The backlash compensation was set to these figures and the test rerun and the result was a rectangle of the right dimensions. This may be a bit misleading as with a higher tool loading the backlash may be greater than measured by this test. At least it was a start.

The backlash on the Z axis was thought not to be of concern as it seemed that it would always be going down when cutting. However I did notice variation in surface finish but have yet to ascertain if that was due to the cutter not being sharp or a change in backlash due to larger tool loading when taking a bigger "bite". More to do to understand what is happening there.