Fanuc boring problem

[crazy^millman]

Yeah scoot I think you are getting a ladder conflict or a parameter that may beed to be changed to get it to realize the code. The only other thing I could add which sucks is to put the G85 at every position. We have the ability on the machine we have it to read the code once or on every line code so it may be something that simple.

 

I will throw something out there that may seem out in left felid but have seen it effect a machine tool. Do you have a grounding rod for the machine. I have seen electrial interfence make machines do crazy things and with the grounding rod it seems to keep it from effecting the machine. Just a crazy thought from the crazy millman.

 

 

Good Luck,

 

Crazy Millman

[Scott Bond]

Good idea ,,I have heard of that..I will look for the rod in the morning.

 

Scott

[Hardmill]

+1 Crazy

Golf clap for the grounding rod.

Also Scott do you do any welding anywhere near

the mill? For some machines definetly dislike

that.

 

PEACE

[cadcam]

Scott, Do you remeber we had the trouble with the Fadal years back at SC and they had not put the ground rod in?

 

I have seen this a other palces to with the Machine doing funny things.

[Jack Mitchell]

Scott,

 

Just a thought - please analyze this small manual part program.

 

O0099

N005 G00 G90 G94 (08/20/03**Coding test**Mitchell)

N010 G54 X0 Y0

N015 M06 T01 (#3 C-Drill T01/H01)

N020 G43 H01 X-1.0 Y0 Z2.0 S2000 M03

N025 G99 G81 X-1.0 Y0 Z-.25 R.1 F3.0 M08

N030 X0

N035 X1.0

N040 G80 G49 Z2.0 M09

N045 G91 G28 XYZ

N050 M02

%

....

G54 by itself only changes the display counters

G54 X0 Y0 will also cause a rapid above part zero prior to the tool change (sometimes this is desirable)

G80 returns the function to rapid traverse G00 afterwards is redundant

G49 Cancels all active tool lenghts

G80 G44 Z2.0 M09 is fair game as well - depends on the shops historic preferance

The intial Z2.0 is healthy practice since it gives a operator enough time to react to a potential crash

This can also be single blocked - reset button - then checked with a 123 block

I realize there are those that would frown upon the restatement of positioning in line #25; this is what I would call one of my bad/good habits - for there are many.

 

 

Regards, Jack

 

[ 08-21-2003, 01:49 AM: Message edited by: Jack Mitchell ]

[Greg Williams]

scott,

 

Now I am stumped, Perhaps a G49 at the start of the program as well would not hurt. But all should be cancelled in the reset key is pushed.

 

%O0001

G90G80G40G17G49---Add this

G91G28Z0---And this

T1

M6

G0G90G54X0X0S2000M03---Only restart here

G43Z150.H1

G98G85X-10Y-10R5.F50.

 

AND SO ON

 

If this doesn't do the trick it is a parameter issue, You will need to contact Fanuc.

[heeler]

Budgie,

 

When you push reset a Fanuc control will reset certain functions as defined by parameters. So it may of may not reset the G49 Tool Length offset.

 

HTH

Glenn

[Scott Bond]

And Finally today it works.

Thanks for all the replies.

Glenn your personal attention was great.

Jack this is what was missing,,

""N005 G00 G90 G94 (08/20/03**Codingtest**Mitchell)

""

I had put G95's in for the tapping, and the G94 must be written before the use of a G83.

 

Thanks all the help.

[crazy^millman]

Scott oh yeah them cancel codes for the tap cycles are independent of the drilling cycles. I am glad you got it worked out.

 

Good Luck Crazy Millman