I have created a program that uses a VBit in the floating head to create the pattern in diagram. I am using BA intersection where the line hits the larger V in the panel and machining to the base of the V and then returning the tool along the same path to the tip and vice versa on the other side. The code looks good and I have even checked the Zoom in Draw. Unfortnately the tool stray slightly when it reverses back up the path. I am not ruling out mechanical problem but it has no problem returning down path when moving in only one axis. Your thoughts would be appreciated.

Also I would like to know how to to change spped settings in the axis. I have been typing in my changes followed by enter. Exiting out and typing CNI in password but my changes dont register?

If you have engaged cutter compensation, you can not reverse the trajectory 180 degrees. You must program something of that nature on the centerline of the tool. You must enter <CNI> & <enter> and it must occur before and after the Screw Corr. appears in the lower left corner of the screen. For most NC481 / RT480 machines, if anything you would want to reduce the speed settings for age / wear of the machine. I believe most of the older machines were set with a 55-60mpm max rapid.

Hope this helps

Mark Tomlin
CNC Custm Services

I owe you a couple of beers for the password tip as we are only running at a max interpolar speed of 10m/min.:cheers::cheers:

As to the other problem I think it must be mechanical. Looking at the diagram the apex of the 2 triangles don't line up in the X axis. Although the parrallel lines are evenly spaced.

i find that if you slow feed down to f3 or f2 before a reversal where backlash or inertia problems show it helps. just split the line before corner and revert back to f5 or f6 for straights. f10 is a bit fast into corners!

i find that if you slow feed down to f3 or f2 before a reversal where backlash or inertia problems show it helps. just split the line before corner and revert back to f5 or f6 for straights. f10 is a bit fast into corners!

I will give that try for future reference. Although I got round the problem by lifting the the tool and a GO. Instead of using a BA instruction.

I also had to add a couple of mm to get the triangles centred(LPX/2 + (TRI/2)+2).

Can I alter screw correction or something else to resolve this problem?

do you have tool correction on ie g41 or g42? if so tool needs to be measured and set exact in tool table
have you measured your origin of work where the tool starts to see if its correct? (try a single plunge and raise at say x50 y50 to see if its accurate from the edge of the board with a caliper. then try the same at lpx/2 and at lpx. you should then be able to see whats out.
then a line from x0 to lpx at say y100 and a cross line at yo to lpy. depth approx 2mm so you can try again at deeper depths as you change things
my machine was 1.2mm out of square when i had it as back stops had been removed and not set back correctly. now its less than 0.2 all along board.

you should also check similarly with drill head. not lines obviously!

the ba command works really well if feed is set at f5 or below. i use it all the time