1 Introduction In the process of using the CNC lathe, in order to reduce the roughness of the surface of the workpiece to be processed, reduce the tool wear and improve the tool life, the blade edge of the tool is usually ground into a circular arc shape, and the radius of the arc is generally between 0.4 and 1.6 mm. CNC lathes with tool nose radius compensation function (G41, G42), as long as the workpiece size is programmed directly in the machining program, there will be no machining error caused by the tool nose arc; and the CNC lathe without this function is processed. It will be affected by the arc of the tool tip. In severe cases, the workpiece will be over-depleted. This problem is now discussed with respect to the machining of the SR10 - 0.04 spherical surface in the workpiece shown in Figure 1.
2 Processing error analysis
In the use of economical CNC lathes, we usually use the trial cutting method to match the knife. Thus, the machining point described by the machining program is point P (Fig. 2), and the actual cutting is the cutting edge arc (where the knife is used) The radius of the pointed arc is 0.4 mm) and not the point P, because this point P does not actually exist. Therefore, there is a different degree of error between the trajectory of the P point described by the machining program and the actual machining contour. However, this error is zero when turning the outer circle, the inner hole and the end face. This error is evident when machining curved and tapered surfaces. The machining error analysis of the SR10
-0.04 spherical surface is shown in Figure 2. In the figure, the M line is the trajectory of the P point described by the machining program, that is, the ideal size of the workpiece, and the actual processed contour is the N line, and the shadow is the solid part of the less cutting, that is, the machining error. We use the "element attribute query" function in the CAXA electronic plate to find that the N line is a circular arc with a radius of 9.6mm. The maximum error is about 0.17mm. If this error is within the tolerance range, we can ignore it, otherwise we It is necessary to take measures to eliminate it.
3 error elimination method
Method 1: Change the programming size
When programming, adjust the path of the tool tip so that the actual machining contour of the arc-shaped tool tip matches the ideal contour. Take SR10
-0.04 spherical processing as an example. When programming, we only need to change the finishing block as follows:
| Before change | After the change |
|---|
...
N100 G00 X0 Z50
N105 G03 X10 Z42 R10 FO.1
... | ...
N100 G00 X0 Z50
N105 G03 X10 Z42 R10.4 FO.1
... |
Method 2: Program the tool point with the center of the tool nose
The steps are as follows: draw the workpiece sketch → draw the tool nose arc motion track based on the tool nose arc radius r and the workpiece size → calculate the arc center track feature point → programming. In this process, the drawing of the center of the tool nose arc and the calculation of its feature points are a bit cumbersome. If you use the drawing function of the CAD software medium distance line and the coordinate query function of the point to complete this work, it is very convenient. In addition, when processing by this method, the operator should pay attention to the following two points: 1) Check whether the r value of the tool nose arc radius of the tool used matches the r value in the program; 2) When setting the tool, it is necessary to put r The value is taken into account, ie if the tool offsets obtained for the tool are x (X-axis) and y (Z-axis), the tool offsets that should actually be entered are x-2r and yr.
4 Conclusion This paper mainly discusses the processing of the outer edge convex arc as an example. Other types of arc surface and cone surface also have similar problems, which will not be repeated here.
