when I said that my X axis seems to be in the worng direction, I am talking about the image area, not the axis motor.  Teh tabels moves in teh driection of teh arrows on teh control pendant, so they are going in the right direction. 

OK IF the toolpath on the screen is backwards (mirrored ) then you are programming it backwards.

What type of machine is this Knee mill, Gantry mill, router. Does the spindle move in xy or does the table move XY?

Depending on the type machine as to which way it should move when you use the jog button. Direction is based on which way the perceived tool motion is.

(;-) TP

Teh tabels moves in teh driection of teh arrows on teh control pendant, so they are going in the right direction. 

That is actually incorrect.  In the world of CNC, all motion is defined in terms of direction of movement of the tool, NOT the table.  Clicking on a "right arrow" control should move the TOOL to the RIGHT relative to the workpiece, or move the table to the LEFT on a milling machine.  So, your machine is setup backwards.

Regards,
Ray L.

tool is stationary as this is a BP knee mill.  Let me think about that in my dreams tonight. 

tool is stationary as this is a BP knee mill.  Let me think about that in my dreams tonight. 

Which means pressing the RIGHT arrow key should move the table to the LEFT.

Regards,
Ray L.

Ray is correct with a knee mill if you push X+ the table should go left which move the  tool tip right(perceived tool motion)

With Y push Y+ and the table moves towards  you (away from the column)

Mach3 will DISPLAY the code in the conventional MODE.   

(;-) TP

OK, so the direction that I had my program in cad was right and when I transposed those points into G code that was also right and it displayed correctly on the VRO, but my X and Y is going in teh wrong direction so that means after I get this part made I should switch things around including my homing config screen. 

Mountainman,
If your machine has only a little backlash and can handle climb milling, then I would climb mill the part the whole time.  Conventional milling has the cutting edge sliding over the surface until the material is thick enough to peel a chip.  This wears the cutter much faster.  Climb milling starts with a full chip and the chip thins until it breaks off, which is much better. In most cases the finish is better too.

When programming manually from a CAD drawing I always program right on size and use cutter comp.  I always put the tool path in a subroutine and just set cutter comp, call the sub, adjust comp, call the sub.  I program the subs in incremental.  That way I can always position it anywhere, or even use it in multiple locations.  I also like to use undersize cutters on pockets to sweep the corners with the cut, not crash to a stop and change direction. This got me on good terms with the guy in the tool room because I actually asked for resharpened end mills, and he always made sure I got freshly sharpened ones.  He did a good job too, they always seemed to cut better than new ones.

One of the machinists said I was wasting time with rapid moves back to the start of the tool path and should program it the way you want to.  I pointed out to him that if we had lots of parts to do that would be a good idea.  With batches of ten or less you really can't justify the extra coding and testing to be sure it works.

Gary H. Lucas