Re: [CAD_CAM_EDM_DRO] Two tools on a lathe-programming problem

Ron Ginger wrote:

>I was asked to help convert a large hydrauilc tracer lathe to CNC. This
>is a wood turing machine that generally makes things like porch column-
>up to 10 ft long.
>
>The basice machine would be a simple project, BUT there is one item I
>cannot figure out. It has one carriage driven by a servo motor, but it
>carries TWO cross slides. The slides are about 6 " apart. In tracer use
>the leading cross slide carries a rough cut tool, the following one
>carries a finish tool. In one pass (remember, 10 FEET long) two cuts are
>taken.
>
>It would be simple to put a motor on each cross slide, but how would I
>code it? There is only one controllable Z axis. At any particular spot
>the two X slides need to be in different places. If I could build some
>kind of 'delay line' I could delay all the x steps by the right ammount,
>but that seems tricky.
>
>

This sounds pretty simple. The Z offset between the two tools is constant,
right? So, all you need is to prepare two axes with the correct
offset. So, you'd
have an X and a Y, for instance, instead of just X. For purists, the
extra axis
could be U, which is defined parallel to X. Now, you need to compute
two sets of toolpaths, offset by the known offset between tools. So, if the
finish tool is 6" behind the roughing tool, then when Z is initially set for
100", the X tool is at position 100", but the Y tool is at 106". So, it
needs
to stay retracted for 6" to not hit the tailstock. Once Z=94", the Y tool
is now at Z=100, and can move in for the finish cut. You could do this with
any CAM system by just making up two copies of the part profile, rotating
one by 90 degrees and offsetting it by 6". Then, you have a 3-D surface
that
the tool has to pass down, and the X and Y axes would follow the surface
progressing down it in Z. I think making it look like an inside corner
is what
you need, so that the tool can try to follow where the two surfaces meet at
the inside edge. I think I could even do this in Bobcad/CAM!

Now, of course, this requires some manipulation of the original shape to
dup it, flip it and offset it. I suspect a macro could be set up to do that
on most CAM software.

Another way to do it would be a post processor that starts with a simple
X-Z path, and then computes the Y-Z path for the finish cut. The problem
with that is it prevents the CAM software from fitting the tool definition
to the cut shape for the finish tool.

Jon