Machine move doesn't match program.

[neil qwerty]

Hi, we have an OKK660 with a Fanuc 16m control. We broke a cutter on the weekend because the control made a change to a rapid move. The cutter lifted to the correct z position and instead of going directly to the next x,y position it appears as though it moved on a 45 degree angle first (this is where it crashed) before going to it's intended destination. I'm assuming it's some type of parameter setting in the control. Anybody have any ideas??

 

Thank,

 

Neil.

[Josh T™]

Look in: Settings - Control Def Manager - Linear - Mill - XY Plane Control - Change to "Break Rapid Moves"

 

HTH

Josh

[neil qwerty]

Thanks for you reply Josh, the control def is already set up to break the rapid moves. The program retracts first then moves in x and y. The problem lies in the control somewhere, it took the one x and y move and broke that into two pieces.

[Dave Ball]

most machines move this way, it's sometimes called "dogleg" moves. It results when the distance to a point is not an equal distance in both axis, since each axis moves simultanisly at rapid the one with the shorter distance arrives first, resulting in a move that is not a straight line. You may be able to find a parameter in your machine to control this.

[MLS]

What Sheffer said.

 

If you can, I would suggest contacting the tech support for the machine. Changing parameters is dangerous if you are not sure what is what.

 

That being said...

I just was looking at this with a Fanuc 15i. Pull out the parameter book and look up the feedrate parameters. In the 15i it was 1400 series, but 16m may be different. Look for a LRP Data type. This tells it to either rapid each axis at max velocity or linearize rapid motion.

 

HTH

[Ocean Lacky™]

[Murray Mold]

You might want to look at your operations also and check to see if you change from absolute to incremental.

[gcode]

This has nothing to do with Mastercam

output, its how a machine tool repsonds to

a G0 (rapid ) command.

Some run in a straight line , on most,

all axis run at top speed to their programmed value.

This results in a dogleg rapid and can get you in

trouble because Mastercam shows all rapids as straigt likes.

If you can't change a machine parameter to fix it,

you have 2 choices.

1. Make sure all your rapid motion is high enough

to miss the part.

2. Force Mastercam to output G01 rapids

like G01 X2. Y3. F500.

[Murray Mold]

If you change from absolute to incremental from one op to the next, all 3 axis will rapid at the same time, possibly causing a crash.

 

I only suggested this because he might not have noticed if his z axis actually did this or not.

[MMT-USA]

PRM 1401.1

 

(0)Non Linear

(1)Linear

[neil qwerty]

Thanks for your input guys! I'll have a look at the 1401 parameter tomorrow. I realise I could have my program retract to completly clear the part, I'm just trying to avoid wasted time in my program.

 

Neil.

[Jack Neelands™]

Thanks MMT...I was going to suggest that he get ahold of Emec tools cause i forgot what the parameter setting was

[neil qwerty]

Thanks MMT, that fixed it!!