Contents - Index - Previous - Next

The following briefly illustrates this topic.

Introduction
With orthogonal machining, ie. cutting only along the X or Z axis, the fact that the tip of the tool is not pointed but has a radius causes no problems. Where cutting is along both the X and Z axes, as when machining tapers or arcs, the tool tip radius can cause a problem: the part will not be dimensionally correct if the tip radius is not taken into account. The larger the tip radius the greater the dimensional errors.

Generally, tool tip radius compensation is not needed for roughing cuts. It is needed for finishing cuts. The roughing cut must leave sufficient material on the part for the finishing cut to produce the required artifact.

The drawing below shows two parts being finished by a button tool tip 5mm in diameter. The Z co-ordinates at the left hand end of the small diameter in each drawing are significantly different even though the lengths of that part are the same.

                    

If you are creating NC code manually and using CAD software to help you, it is probable that the software will allow circles, with a radius equal to the tool tip radius, to be drawn tangential to lines on the part drawing, for example, tangential to a horizontal and an inclined line.The software can then report the relevant X and Z co-ordinates so that the profile is machined dimensionally correct. To get the same figures by manual means is a long-winded process and the trigonometry is complex.

A Deeper Look

                    

The picture shows two tool tips. One is pointed while the other has a tip radius. Two purple orthogonal lines are drawn at each tool tip. The intersection of these lines is the tool tip driven point. For the pointed tip, the tip point and the driven point coincide. For the radiused tip, the driven point is away from the tip.

It is always the X and Z co-ordinates of the tool tip driven point which are required in the NC code.

                    

The picture shows a pointed tool at the junction of a horizontal and an inclined line. Because the tool is pointed, the driven point coincides with the tip point. Therefore the X and Z co-ordindates required in the NC code are the X and Z co-ordinates of the junction of the two lines. In reality, tool tips are not pointed: they all have a radius.

                    

The picture shows a radiused tip at the junction of a horizontal and an inclined line. The tip arc is, correctly, tangential to both lines. The X and Z co-ordinates required in the NC code to bring the tip arc to this position are the X and Z co-ordinates of the tool tip driven point.

                    

The picture shows a tool facing the end of a part. Notice how the driven point needs to go past the part centreline so that a pip is not left on the end of the part. The X co-ordinate for the driven point will be a negative value equal to the radius of the tool tip, eg X-0.4

                    

The picture shows the driven points of right hand, neutral and left hand tools

                    

In the picture, the white line is the profile of a part. Working from right to left, the profile consists of line, first part of arc, second part of arc, line, first part of arc, second part of arc, line, arc, line, line.

The tip (green) and driven point (purple) of a right hand tool are shown at each of the critical points round the profile. These critical points are the start and end of lines and arcs.

The blue line is the path of the centre of the tool tip arc.

The radial red lines are from the centres of the arcs which form the profile of the part. They pass through the start/end of each of these arcs (white) and intersect the path of the tool tip centre (blue).

It is when the tool tip centre is at each of these intersections that the X and Z co-ordinates of the tool tip driven point must be found and entered in the NC code. These co-ordinates give the start/end of arcs and lines.

When programming for arcs (G2 or G3) the radius value entered in the NC code is the radius of the part (white).

Origins and Tool Offsets

                    

Before machining with WELturn can commence, as the picture shows, the right hand tool must be touched on the end and the surface of the billet. Along with measurement of the billet diameter, this locates the centre of the right hand end of the billet, the X=0, Z=0 point. This is the datum point from which the part is measured.

What is less obvious is that touching the right hand tool on the end and surface of the billet declares that the driven point of the tip of this tool is the datum for all cutting movements of this and all other tools. The X=0, Z=0 point and the tip driven point of the right hand tool are coincident.

When tool offsets are measured with the aid of the tool setting microscope, the first tool to be set is always the right hand tool. Its tip is brought into the appropriate quadrant of the microscope cross hairs. The intersection of the cross hairs actually shows the location of the tip driven point of this and all other tools.

When other types of tool tip are brought into their correct cross hair quadrant for offset measurement, their driven points are being established relative to the driven point of the right hand tool. When, in machining, one tool takes over from another, the offset correction movement brings the new tool