Haas CONTROLLER crash

[Chris Rizzo]

So I've been utiltizing the highfeed lately, and having problems with my Haas CONTROLLER crashing while DNC-ing. The controller completly locks up in mid-cut, spindle still on, screen still showing code. Reset button doesn't work, have to do an e-stop to reset the thing.

 

I've DNC'ed 10mb prgrams without highfeed and never had an issue before. Any ideas?

[Jimmy Wakeford from Barefoot CNC]

I've seen fanuc's pause when reading a line with a G08 long enough to run through internal macro, but it also quits reading code till done and takes back off when finished.

 

Are you using a gcode to invoke highspeed? Could be maybe the look ahead is emptying buffer?

 

We have customers dnc'ing to haas machines with highspeed with no problems. What are your baud settings?

[Chris Rizzo]

thx Jimmy,

 

My baud is 115200 (full blast on the Haas). My controller is circa 2000, without the highspeed/extended look ahead. I'm just using the Mastercam highfeed (g0-g3) feature. What's strange to me, is that I've never had this arise before with regular programs, even crunching lots and lots of code...

[Jimmy Wakeford from Barefoot CNC]

Look at your feedrates. I suspect a feed of F0. or close to it.

[perfecseal mankato]

if you are using the highfeed in mastercam

only on FINISH TOOLS, it will output "F0."

alot. (logged bug)

to over come this a post modification is required until the bug is fixed.

also the set up sheet needs to be modified to get correct run times, due to the "F0."

[Jimmy Wakeford from Barefoot CNC]

so in the pfr postblock

 

pfr

 

if fr_pos <> 0,[

(whatever is there)

]

 

DOes that sod right PM?

[perfecseal mankato]

Jim,

what I did was to go and create

the following in the post I use

 

pfeed

if feed = 0, feed = 20.

feed, e

 

then everywhere in the post where feed is encountered direct it to pfeed.

The post I use I wrote just for the type

of machining we do here, so the post change may not be quite the same