Tool Radius Compensation Introduction
The tool offsets explained above are entered assuming that the cutting tip is sharp. But the actual cutting tip has a particular tip radius. The offsets taken in the above manner leads to contour errors whenever a contour machining is done.
Lines passing tangential to the “TIP CIRCLE” meet at point P. Tool tip touching at points 1 and 2 is as good as touching at point P. Keeping this point as reference CNC executes all tool movements. Point P is called as leading tip.
The example shown in the figure is having contour error.
Different programmed positions are attained by leading tip. It can be clearly seen from the drawing that the tool has already crossed point 1 and not yet reached point 2. Because of the leading tip there is profile error at the chamfer portion, i.e. chamfer is short.
Chamfer is less than the programmed value, leading to profile error.
Since the cutting tip is of circular shape, depending on the contour profile, any point on the circumference may touch the component which leads to contour error. To avoid this sort of error tool radius compensation is used.
By programming radius compensation, control calculates and generates a new patch called compensated path parallel to the programmed path, keeping the distance between the two paths equal to tip radius. Then the tool offsets get shifted to the tool tip centre and the tool tip centre follows the compensated path.
Compensated path being traced by the centre point, the counter error is eliminated.
Programming of tool radius compensation is done by the relevant G code. There are two types of cutter radius compensation (C.R.C) like C.R.C to the left of the component G41 & C.R.C to the right of the component G42.
The above codes are decided looking in the direction of cutting, to which side of the component, the tool is existing i.e. if tool is to the left side, code is G41 and if the tool is to the right side, code is G42.
Direction of Cutting
G41 Code Programming
Looking in the direction of the feed if the cutting tool is to the left of the cutting surface code used is G41.
G42 Code Programming
Looking in the direction of the feed if the cutting tool is to the right of the cutting surface code used is G42.
Whenever C.R.C is selected, to initiate the compensation in the proper direction, CNC refers to the tool offset page to identify the tool location code and the tip radius.
G41 and G42 are modal. They are cancelled by G40 or after M30, reset or emergency stop.
Tool Radius Compensation Selection
Tool radius compensation selection (G41 / G42) can only be carried out when G00 or G01 is active. Before selecting the tool nose radius compensation, the tool should have been called earlier (i.e. the tool programming with the relevant offset number is programmed earlier).
Tool radius compensation cancellation (G40) can only be carried out in a block in which G00 or G01 is programmed.
Tool radius compensation cancellation is achieved by function G40. Tool offset memory number 00 corresponds to zero compensation. It can be used to cancel tool radius compensation.
G40, G41 and G42 can be programmed in a block separately with any other function. They are not active, unless a movement command is programmed at least in one axis.
When any change from G00 to G01, G02 or G03 is detected the CNC applies the same process as when the tool radius compensation is initiated.