Re: G-code lesson

Ed,

Cuttter radius compensation and tool nose radius compensation are
essentially the same thing. The first generally applies to milling
with a rotating cutter and the latter applies to turning (lathe) with
a fixed cutter and rotating workpiece. Same concept, in both cases
the the cutter's center point is offset from the work surface by a
distance equal to the radius value specified in the tool offset table
of the controller. For a rotating tool the center point is the axis
of rotation, for a turning tool the center point is the center of the
nose radius.

Note, varying the radius value of the cutter in the tool offset table
can be a useful trick. For instance, in milling with a .500"
diameter end mill the cutter's tool radius offset value should
theoretically be .250". But, if that end mill is getting dull
cutting forces may cause it to deflect away from the work which will
not give correct sizing of the finished part. By lowering the radius
value slightly, to maybe .245", you can compensate for the tool
deflection and get a part that has the correct dimensions.

Likewise, you can use the radius value to create a roughing pass by
specifying a larger than actual radius value. As above, with
the .500" end mill, enter a radius value of .275" and your part will
be cut with .025" left as a finishing allowance. Then, change the
radius value to the actual .250" and make your finish cuts to size.
This method allows roughing and finishing with the same Gcode segment
and may give a more consistent size and surface finish since the chip
load is identical around the part.

From the above, you can see how important a feature cutter radius
compensation is for precision machining. Any controller that doesn't
support it isn't going to be very useful for anything except very
simple work pieces.

Doug

--- In CAD_CAM_EDM_DRO@y..., edwardhall@a... wrote:
> Hi,
>
> Thanks to those who responded to my earlier question about tool
> holder. Didn't express my appreciation earlier to save bandwidth.
>
> Below extracts from Mike Lynch's lessons for radius compensation. I
> alwasy thoutht that cutter radius compensation is the same as tool
> nose radius compensation. Exactly what is the difference the two?
>
> "Cutter radius compensation
> Just as tool length compensation allows the machining center
> programmer to forget about the tool's length, so does cutter radius
> compensation allow the programmer to forget about the cutter's
radius
> as contours are programmed. While it may be obvious, let us point
out
> that cutter radius compensation is ONLY used for milling cutters
and
> only when milling on the periphery of the cutter. You would NEVER
> consider using cutter radius compensation for a drill, tap, reamer,
> or other hole machining tool."
>
> "Tool nose radius compensation
> This turning center compensation type is very similar to cutter
> radius compensation. In fact the same three G codes are used. G41
> instates tool nose radius compensation in a tool left condition.
G42
> instates with a tool right condition. G40 cancels tool nose radius
> compensation"
>
> ED