CNCzone Network:

# Thread: cutting radius on okuma lathe

1. ## cutting radius on okuma lathe

the line in the program reads G02 x1.51 z -2.9897 k.0808 I.53
The rest of the program runs fine till it gets to this line?
Anyone have a solution?
Thanks

2. Also when it gets to this line it says 2252 alarm b data word circle calculation 3

3. More information may be needed here. Can you give us the two or three lines before and after the one you gave? The problem may be in one of those, or certainly the error can be deduced from them.

4. Originally Posted by clayd-cnc
the line in the program reads G02 x1.51 z -2.9897 k.0808 I.53
The rest of the program runs fine till it gets to this line?
Anyone have a solution?
Thanks
The error you state translates into a problem that can stem from either the start point of the arc, or from the end point of the arc.
The problem is that the machine can not move along an arc between the start and end points, the error is greater than the specified tolerance within the parameters.
So... for you to work out where the error is, you need to check the start point of the arc, which is the end point from the previous line, then recalculate the end point of the arc, which is the X & Z point you mentioned.
The I & K values need to be the incremental distance from the START point of the arc to the centre of the arc.
Once you have the Start point and end point and vector correct, the machine will be fine.
Usually the default arc error tolerance is set to 20microns. (0.020mm)
I always teach the guys that you need four pieces of information to program an arc:
1. Start Point.
2. End Point.
3. Direction
4. Distance vectors to arc centre (or us "L" along with the radius value)

Point 1. is the XZ value of the line before the G2/G3 command
Point 2. is the XZ value stated on the G2/G3 line
Point 3. is the direction you require G2 being Clockwise, G3 Anti-Clockwise.
Point 4. is the IK values (or L)

Hope this helps.
Brian.

5. May even be a forgotten G01 on the next linear move.

Try single stepping the program to narrow down which lines are in error,
when running on AUTO, it is calculating tool moves about 4 lines ahead, or what is being processed through the "Read ahead Buffer"