Cnc machining nm09/2

Contour machining using circular interpolation

Download 0.53 Mb.

Page	18/27
Date	28.01.2017
Size	0.53 Mb.
	#9464

1 ... 14 15 16 17 18 19 20 21 ... 27

4.17 Contour machining using circular interpolation

Circles and curves can be produced on both the lather and on a Machining Centre by one of two methods, point to point programming or by circular interpolation.

4.17.1 Point to point contours

This system of programming curves and contours is very much a thing ofthe past and would be used in the case where a machine was not fitted with a control capable of circular interpolation. When using the point to point method the curve is redefined as a series of straight lines within a calculated zone of tolerance. Refer to figure 4.23.

Figure 4.23 Curve high limit

4.17.2 Circular interpolation

Most modem machines (CNC) have a circular interpolation function which will produce a curve or circle in one motion and to a much higher accuracy than the point to point system. With the exception of a fewer minor points, the calculations for circular interpolation for CNC Machining Centres are the same for CNC lathes.

Circular interpolation has three basic considerations.

The direction of rotation
The end point of the curve and
The start point of the curve.

A typical command for circular interpolation

G03 X40 Y30 I -20 J 0

Figure 4.24

4.17.3 Direction of rotation

On CNC lathes and machine centres the commands used to call up circular interpolation are the same.

G02 Calls up circular interpolation in a clockwise direction.

G03 Calls up circular interpolation in an anti-clockwise direction.

Figure 4.25 Directions of rotation

4.17.4 The end point

The second of the three commands must inform the control exactly where the contour being programmed will end. This normally requires a calculation accuracy of two decimal places. Another important consideration is that the end point is an ‘X’, ‘Y’ or ‘Z’ axis co-ordinate defined as an absolute dimension.

Using the mill sample above you will see that the end point follows the circular interpolation command, ego G03 X40. Y30.

4.17.5 Arc centre offsets

Put simply, an arc centre offset tells the control the point at which the centre ofthe arc is in relation to the start point of the curve.

This distance is always expressed as an incremental dimension accurate to two decimal places. To identify an arc centre offset, the dimensions are prefixed with a letter code; ‘1’ values ‘J’ values and ‘K’ values, these can be positive (+) or negative (-).

4.17.6 ‘I’ value statement

An ‘1’ value statement is the incremental distance from the starting point to the centre ofthe arc measured parallel to the ‘X’ axis.

Figure 4.26 Figure 4.27

4.17.7 ‘J’ value statement

A ‘J’ value statement is the incremental distance from the starting point to the centre of the arc measures parallel to the ‘Y’ axis.

Figure 4.28 Figure 4.29

4.17.8 ‘K’ value statements

In the case of CNC lathes where the ‘X’ and ‘Z’ axes are the primary axes, a ‘K’ value statement is used to define the incremental distance from the starting point to the centre of the arc measures parallel to the ‘Z’ axis.

Figure 4.30 Figure 4.31

4.17.9 General rule for circular interpolation

CNC lathes operate in the X and Z axis only, therefore, the offsets applicable are ‘I’ and ‘K’.
All programming for the machining centre in this course will be for circular interpolation in the X and Y axis therefore the offsets applicable are ‘I’ and ‘J’.
Offset values can be singular or double values ego J1 0 or J1 0 15. If an offset has a value of zero it need not be written into the programme. Example, 120. KO. can be simply written as 120.
To determine the arc centre offset is to be positive or negative and a cartesian quadrant should be constructed at the start point.
A clear plastic overlay of the cartesian quadrants as shown in below will be of great assistance in defining arc centre offsets. This overlay is of particular value in establishing if the offset is to be (+) or (-).

Figure 4.32 Lathe Figure 4.33 Mill

4.18 Programming examples

Example 1: When programming a full circle the end point will be at the same point as the start of the circle. For this reason you need only to define the direction of travel and the applicable arc centre offset.

Figure 4.34

Program

G00 X125 Y60

G01 Z-5

G03 I-42

Example 2: In this next example you will note that the end point is 84mm along the X axis therefore the value I will be + 42 mm.

Figure 4.35

For a semi-circle the programme could read:

G00 X0 Y0

G01 Z-5

G02 X84. Y0. I42

In the case where the arc only forms part of an arc it is often necessary to apply some basic mathematical principles in order to calculate all the coordinates required to define the machining of the arc or curve.