One common machining operation on the CNC lathes is facing a solid part. Regardless of the operation that follows, it is important to have the front face perfectly flat all the way to the centerline. There are two possible reasons why a small tip is left where the face meets the spindle centerline:
Tool height set incorrectly … setup error Incorrect tool position … program error
A subject earlier in this chapter described the effect of geometry offset on a diameter of the part. With or with out a tool nose radius offset, the part diameter will be machined as per drawing – and that is the exact situation in this case. The solution is simple-change the XO in the program to an X-position below centerline, which will be a negative position. This corrected position should be
just right’ – after all, there will be a certain amount of drag, since the spindle rotation below centerline is oppo site to the one used for cutting.
What is ‘just right”? The minimum amount is the tool nose radius (TNR), doubled for diameter programming:
Tool Height Error
If the tool height is set incorrectly, the only remedy is to change it. This is usually done by placing a suitable shim under the tool holder, if the height is too low. If the height is too high, grinding off the contact surface of the tool holder will be necessary.
In the previous chapter, the wear offset was changed from one to a different one for the purpose of maintain ing dimensional tolerances. In those instances, the direc tion of cutting had not been changed.
Changing offset because the tool has changed cutting direction is much more common on lathes than on ma chining centers. A simple drawing example and a short program will illustrate a possible problem that may oc- cur during the program check stage of the part setup.
This program will not work as presented and has to be changed. During the program check, you will find that the facing cut has started well, but it will not be finished.
The CNC system will follow all program instructions, including the G41 – Left and G42 – Right commands. The program calls the facing cut to start in block N4 and end at X-1.7 in block N5, in the G41 (left) mode. This facing motion is followed by a rapid motion in the opposite di rection, creating a wedge. In order to be to the left, the tool nose radius also has to be to the left of the motion from block N5 to block N6. Since the control does not allow overcutting, it just follows instructions and re mains in the G41 (left) mode. The result is that the face cut will not be completed:
Incorrect Tool Position
If the tool height is correct, the problem is most likely in the program itself. Consider the following program segment:
The next two tables show the minimum X-position and suggested X-position for the three most common corner radiuses:
TNR = R0.8
N1 G21 T0100 N2 G50 $2750 N3 G96 S300 MO3 N4 GOO X33.0 20 T0101 M08 N5 C01 xe F02 N6 …
TNR – Metric
The program starts with a face cut, then the chamfer and continues diameter turning. G41 is in effect for the face, G42 is in effect for the chamfer and the diameter:
In the program, the tool moves to the spindle center line, which is XO, so the program looks correct. The problem is that there is no provision in the program for the tool nose radius. This will be the result of running the above program:
TNR – Imperial
N1 G21 T0100 N2 G50 $2750 N3 G96 S300 MO3 N4 G41 GOO X33.0 ZO TO101 MO8 N5 G01 X-1.7 F0.2 N6 G42 GOO X25.0 22.0 N7 G01 X30.0 Z-3.0 F0.15 N8 Z-..
The updated program will be the same as the last one, except the change of X-position in block N5:
Not in scale
When you evaluate the program, all data appear to be correct. In the following illustration, the enlarged tool motions can be viewed as individual motions (blocks N4 to N7). The control system only interprets the XZ point definitions and defines tool motions based on the prepa ratory G-codes.
N1 G21 T0100 N2 G50 $2750 N3 G96 S300 M03 N4 GOO X33.0 ZO T0101 MO8 N5 G01 X-1.7 FO. 2
Just like cutter radius offset for milling, the tool nose radius offset is also the ‘look ahead’ type that prevents overcutting – and it is the overcutting error message that will be the result of the above program.
The undesired tip can cause problems for subsequent operations, for example, accuracy of a drill position. It can also create problems during assembly, if the face is not flat. The problem can also be esthetic.
| CNC Control Setup for Milling and Tuming TOOL NOSE RADIUS OFFSET
To correct this problem, the program itself has to be changed. The change in the program has to eliminate the wedge between the two tool motions. Just changing the Z-clearance alone will not do it, the angular motion has to be replaced by a rectangular motion:
The previous program used a 2 mm clearance for the tool to move away from the front face. The last illustra tion shows that this amount was sufficient.
The rule of clearance is simple:
Clearance must be greater than double nose radius
N1 G21 T0100 N2 G50 $2750 N3 G96 S300 M03 N4 G41 GOO X33.0 ZO T0101 M08 N5 G01 X-1.7 F0.2 N6 GOO 22.0
(*** BLOCK ADDED) N7 G42 GOO X25.0 (*** CLEARANCE REMOVED) N8 G01 X30.0 Z-3.0 F0.15 N9 Z-..
During machining, it may often become necessary to change the insert and – along with it – its nose radius. When such radius is smaller, for example, changed from R0.8 to R0.4, the program does not need to change.
On the other hand, a change from R0.8 to R1.2 will re quire an increase of the 2 mm clearance, otherwise an overcutting alarm will occur:
R0.4 R0.8 R1.2
R0.0156 R0.0313 R0.0469
As long as the rectangular motion can contain the full circle of the nose radius, the face cut will be completed
Considering the three most common nose radiuses available on lathe inserts (shown in both metric and im perial sizes), it is easy to establish that a clearance that is greater than the largest nose radius of the three will al ways be sufficient for majority of work: