Contents - Index - Previous - Next

t Emco choose 1/100mm?). It only resolves into something sensible at ¼, ½ and ¾ of a millimetre. The result is that, when WELmill calculates the machining steps from the co-ordinates in the NC code, it has to round the figures up or down to get the best approximation to the required size of the machined part. Dimensional errors are only the equivalent of one, or possibly two, steps.

Because a cutter moves in steps, the only profiles which will be completely smooth will be those cut directly along the X, Y or Z axes. With one exception, cuts in all other directions will be stepped. The best comparison is with an inclined bit map line displayed on a PC screen and enlarged so that each square pixel can be seen: the line is stepped. WELmill computes from the NC code the best path for the least stepped result. The exceptional direction for a smooth profile is 45 degrees: WELmill moves the relevant axes simultaneously to achieve this result.

Cutter Diameter
An enemy of accurate machining is a cutter which is under size because of wear. Worse still, the wear may be uneven, more worn at its end than higher up. This will produce a step on the side of a deep cut, near its bottom. Because the cutter is worn, the surface finish on the work may be poor. Where a high degree of accuracy is necessary, machine with new cutters and replace them frequently. Use cutters which are suitable for the material being machined. For example, high speed steel (HSS) cutters soon deteriorate when machining abrasive materials: carbide cutters are more suitable.

The fact that a cutter is marked as diameter 6mm does not mean that it is. It could be 5.9mm diameter. If the cutter diameter is recorded in the WELmill Tool Data Table as 6mm and the NC code is for a 6mm cutter, an external profile is likely to be machined 0.1mm over size.

Accurate cutter diameters must be recorded in the WELmill Tool Data Table and the NC code created for those specific cutters. WELmill cannot compensate for cutter wear.

Other Cutter Problems
If a cutter is running slightly off centre, its effective diameter is greater than the nominal value and a profile will be machined under size. The tool holder and collet should ensure that a cutter runs true. If eccentric running is suspected, check the tool, the tool holder and the collet. Ensure that all mating surfaces are clean, that the collet and holder are correctly assembled and that there are no burrs on the cutter shank.

Never use a bent, chipped or otherwise damaged cutter.

If the best precision of which the mill is capable is required, the following suggestions may be helpful in achieving this.

Measuring Cutter Diameter
This can be done with a micrometer but it can be difficult to get the micrometer anvils right on the full diameter. With a cutter with an odd number of flutes it is well nigh impossible. One solution is to cut what looks like a tenon.

                              

The green line on the drawing shows a tenon 10mm wide and a convenient length to be machined on a billet (white line). A 6mm cutter machines round the profile starting from front left, going to front right, then back right and finally to back left. It is important that the cutter enters the material at the start of the cut with a positive Y movement so that any mechanical backlash cannot influence the outcome.

                              

The picture shows the finished tenon. If the cutter is exactly 6mm diameter, the tenon will be 10mm wide. Any difference over or under size is the amount by which the cutter diameter is under or over the nominal value. From this, calculate the actual cutter diameter and enter it in the Tool Data Table. Before you can run the test again, you must create new NC code based on the actual cutter diameter. The tenon should now be the correct size.

If the sides of the tenon are not parallel and/or have small step at the bottom, this indicates the condition of the cutter and how it is worn. It might also point to some misalignment of the milling head.

Example Code for the Cutter Diameter Test
This code will cut the tenon described above.

To use the code, copy it into the WELmill NC code editor and save it in the MillData folder.

Important: adjust the feed, speed and depth of cut, as required, for other materials. If in doubt, create your own version of this code. This code assumes a 6mm diameter cutter. The ideal material is the hard blue modelling wax used for proving tool paths.

%
*Name of Part - TOOL DIAMETER TEST
*Material - MODELLING WAX
*Billet Length X - 60
*Billet Width Y - 18
*Billet Depth Z - 25
*Top of billet at least 10mm above the vice jaws
*Cutter T6 is a 6mm slot drill
N10 T6
N20 S2000
N30 G0 Z6
N40 G0 X0 Y0
N50 G0 Z2
N60 G1 X0 Y1 Z-7 F75
N70 G1 X58 Y1 Z-7 F300
N80 G1 X58 Y17 Z-7 F300
N90 G1 X0 Y17 Z-7 F300
N100 G0 Z6
N110 G0 Z50
%

When the machining of the test piece is complete, click on "More" to make the cutter run round the same profile again. This

Backlash Compensation), it is suggested that you do the tests described below to see how the machine actually performs.

Z Axis Backlash Test

                              

Before the test is done, the top of the billet must be machined flat and parallel to the mill table. This is because accurate depth measurements will need to be made later. To make depth measurements use a depth micrometer. This is preferable to a vernier or digital caliper.

In the test, a 6mm slot drill cuts the groove, pictured above, from left to right. The first third of the groove will be 2mm deep. The second third will be 2mm deeper (4mm total). The final third should be back at 2mm deep.

It is not the actual depths which matter. The important thing is that there should be no difference in depth between the first and final thirds of the groove. If there is a difference greater than 1/72mm (0.0139mm) then backlash compensation is required. Remember that 1/72mm is the resolution of the mill so do not try to compensate for depth differences less than this. Check that the performance has been improved by repeating the test after a compensation figure has been entered.

Example Code for the Z Axis Backlash Test
To use the code, copy it into the WELmill NC code editor and save it in the MillData folder.

Important: adjust the feed, speed and depth of cut, as required, for other materials. If in doubt, create your own version of this code. This code assumes a 6mm diameter cutter. The ideal material is the hard blue modelling wax used for proving tool paths.

%
*Name of Part - BACKLASH Z TEST
*Material - MODELLING WAX
*Billet Length X - 60
*Billet Width Y - 60
*Billet Depth Z - 25
*Top of billet at least 10mm above the vice jaws
*Cutter T6 is a 6mm slot drill
N10 T6
N20 S2000
N30 G0 Z6
N40 G0 X0 Y10
N50 G0 Z2
N60 G1 X0 Y10 Z-2 F75
N70 G1 X20 Y10 Z-2 F300
N80 G1 X20 Y10 Z-4 F75
N90 G1 X40 Y10 Z-4 F300
N100 G1 X40 Y10 Z-2 F75
N110 G1 X60 Y10 Z-2 F300
N120 G0 Z6
N130 G0 Z50
%

X and Y Axis Backlash Test
This test is best performed with a brand-new, unused slot drill. A used slot drill may not be of consistent diameter over its length and will produce test piece sides of inconsistent width from top to bottom. It will then be difficult to make accurate measurements with a micrometer.

                              

The drawing shows a profile to be cut on the top of a billet (white line).

                              

The picture shows the finished profile. Measurements made on the horizontal arm will indicate if there is a need for Y axis backlash compensation. Measurements made on the vertical arm will indicate if there is a need for X axis backlash compensation.

There should be no difference in the widths of the nominally 10mm wide sections either side of the 5mm cut-ins: the actual widths do not matter. If there are differences greater than 1/72mm (0.0139mm), backlash compensation is required. Repeat the test, with compensation, to check that the mill's performance is improved.

If backlash compensation is correct and the actual tool diameter, with matching NC code, has been used, the machined dimensions should match exactly those stated in the drawing. Any error should be less than 1/72mm (0.0139mm).

Example Code for the X and Y Axis Backlash Test
To use the code, copy it into the WELmill NC code editor and save it in the MillData folder.

Important: adjust the feed, speed and depth of cut, as required, for other materials. If in doubt, create your own version of this code. This code assumes a 6mm diameter cutter. The ideal material is the hard blue modelling wax used for proving tool paths.

When machining of this test piece is completed, click on More to make the cutter run round the same profile again. This