Fanuc boring problem

[Scott Bond]

Hi all

We have a bridge machine with a fanuc control,, the post hasd been recently made by our dealer, and has been working fine. But houston We Have a problem with the reamer plunging into the work instead of feeding,,and it's intermitent--some times it feeds correct and sometimes it feeds at what appears to be rapid..??

:

( Here is a sample of my code.

Do any of you see something lame?

Is there something required, that i don't have?

 

T3 M6 ( TOOL - 3 DIA. - .249 REAMER 1.000 LONG )

( "S" HOLES REAMED TO .249-.2495 )

G0 G90 G54 X7.25 Y-3.287 S1100 M3

G43 H3 Z2. M8

G98 G85 Z-.45 R.1 F4.

X-7.25

X-24.4 Y-27.5

X-10.4

X10.4

X24.4

G80

M5

M9

G91 G28 Y0. Z0.

M01

T14 M6 ( TOOL - 14 DIA. - .251 REAMER 1.000 LONG )

( "S" HOLES REAMED TO .251-.252 .08 DEEP )

G0 G90 G54 X7.25 Y-3.287 S1100 M3

G43 H14 Z2. M8

G98 G85 Z-.1 R.1 F4.

X-7.25

X-24.4 Y-27.5

X-10.4

X10.4

X24.4

G80

( "P" .251-.252 REAMED THRU )

X-29.5 Y-22.5

G98 G85 Z-.45 R.1 F4.

X29.5

X-8.425 Y-14.6742

X-10.6625 Y-28.614

X-24.5

Y-43.364

G80

M5

M9

G91 G28 Y0. Z0.

M01

[CAM-mando]

The only thing I can possibly see is after the repositioning move

 

G80

( "P" .251-.252 REAMED THRU )

X-29.5 Y-22.5 Z2.

The next canned cycle is not picking up the initial plane (Z2.) and somehow getting confused.

 

I dont really expect this to be the case, but perhaps you could try adding a Z2.

 

G80

( "P" .251-.252 REAMED THRU )

X-29.5 Y-22.5 Z2.

 

What model fanuc control ?

 

CAM teh "stab in the dark"

[Scott Bond]

Control Fanuc 16

I saw it work right once.

Then I saw it work wrong once.

With out a code change,,,

 

but maybe there is a problem with mid-starting

the program. Is it missing some kind of cancle ?

Thanks Com and Doe

I will try your suggestion on tommorows part.

 

[ 08-15-2003, 03:09 PM: Message edited by: Scott Bond ]

[cg777]

quote:

---

( "P" .251-.252 REAMED THRU )

X-29.5 Y-22.5

G98 G85 Z-.45 R.1 F4.

---

try putting a g43 h(whatever)

between x&y line and canned cycle line.

 

you r correct, starting on that p line has no length offset call out. i'm suprised it didn't alarm out.

[cg777]

also,

 

unless you manualy turn spindle on, you will have to repeat this comand also.

 

this is assuming that your trying to start on the p line

[heeler]

Scott,

 

You can create lots of problems on the Fanuc if you stop in a Canned cycle. My suggestion is to add a saftey line at all tool changes. Then always start at a tool change.

 

HTH

Glenn

[Guest CNC Apps Guy 1]

The "P" should have no bearing beacause it is inside parenthesis but better to be safe than sorry so dump the quotes.

 

 

JM2C

[cadcam]

quote:

---

but maybe there is a problem with mid-starting

the program.

---

I would say this is the main facture here. the Faunu control is not like the Fadals that they are using when it comes to a restart.

[crazy^millman]

You have been pointed it hright direction the older Fanuc contraol always required all cancel code and other thing at every toolchange. I hade a lathe one time get a G50 S500 programmed into it and it took me a day to figure out why the spindle would not go over 500 rpms. It is funny how some machine act and how soem things that should stay non-modal and modal get crazy acting sometimes. I would just modify my post at add the needed coeds that are at the beginning to be at every tool so you can insure you are getting no over lap. G98 is going back to your intinal starting z before you call the canned cycle no matter where it is. I have soemtimes seen where a machine will get grazy if there is not like a g1 to z plane that beign the last gcode the machine see verse a g0 like at the g43 height offcall.

 

Well hope that help and sure you will get it good luck.

 

Crazy Millman

[cadcam]

+1 Millman^crazy , I am with you have seen this to.

 

Restarts on some machines can be a little tricky.

[Scott Bond]

Thanks for the replies gang. I will

not be able to get thru this alone,,

I would like to try and add this to

our post next week.

Have a nice weekend

[Greg Williams]

Scott,

 

I have had a problem similar to this with our fanuc 16IM controlled Makino's

quote:

---

M5

M9

G91 G28 Y0. Z0.

M01

T14 M6 ( TOOL - 14 DIA. - .251 REAMER 1.000 LONG )

( "S" HOLES REAMED TO .251-.252 .08 DEEP )

G0 G90 G54 X7.25 Y-3.287 S1100 M3

 

---

I think that you may need to add a "G49" after

the G91g28z0. block and in the first block at the start of the program

 

"G49" cancels the previous tool length offset

I am not sure if this will fix your issue but adding this code won't hurt.

 

[ 08-16-2003, 03:48 AM: Message edited by: Budgie ]

[Scott Bond]

M5

M9

G91 G49 G28 Y0. Z0.

M01

T14 M6 ( TOOL - 14 DIA. - .251 REAMER 1.000 LONG )

( "S" HOLES REAMED TO .251-.252 .08 DEEP )

G0 G90 G54 X7.25 Y-3.287 S1100 M3

 

We put it here and the machine alarmed out on Z

[Greg Williams]

The "G49" needs to go after the Z return block

 

M9

M5

G91G28Z0

G49

T2

M6

G0G90G54X0Y0

 

[ 08-19-2003, 04:12 AM: Message edited by: Budgie ]

[chris m]

Scott, just to chime in on this, I think that restarting may definitely be related to your problem. I don't know how many Fanuc controls you have but they definitely are not the greatest when it comes to restarting in certain situations so be sure that the operator is doing it properly and that the machine is reading the tool-length offset and the canned cycle call properly. Often it is easier (and safer) to just start at the beginning of the tool and just flip on the 'Z Axis Neglect' or whatever switch the machine has to stop Z axis movement instead of trying to pickup the 2nd cycle of a particular tool.

 

For my .02 on Fanuc program format, the post I just tweaked up for my 18M posts the beginning of the tool like this:

 

N15 G00 G17 G40 G80 G90 G97 G98 G94

N20 G111

N25 T2

N30 M6

N35 G90 G54.1 P3 X-.6695 Y1.0112 S262 T3 M03

N40 G43 H2 Z.250 M8

N45 Z.100

.

.

.

 

And the end like this:

 

N995 G00 Z.25 M09

N1000 M05

N1005 G28 G91 Z0

N1010 G40 G49

N1015 M01

 

 

I like the safety lines in every tool, just personal preference

 

 

Good Luck

 

C

[mayday]

right on the money cris

we always restart at tool change to pick up all info

on our 15m select single block

READ

G00 G90 G54 X0 Y0 B0 S1000 M3

G43 Z1. H1

turn on z neglect

go to edit mode

jump to the line where you want to restart

go to memory mode

single block start to new position

turn off z neglect and let it go

 

CAUTION ON THE Z NEGLECT

wherever z is when you turn it on

MAKE SURE z is there when you turn it off

the z axis becomes incremental when in z neglect mode

go to edit

[Scott Bond]

Thank you gentlemen

 

I will try this when I get to work today, and once perfected I will attempt to put it in the post.

Scott

[Scott Bond]

My code looks like this at the tool change right now

quote:

---

X-20. Y-41.5

G80

M5

M9

G91 G28 YO. Z0.

M01

T2 M6 ( TOOL - 2 DIA. - .281 #K DRILL )

( "CC" .281 ENTRY DRILL FOR 1" DIA. )

G0 G90 G54 X-20. Y-41.5 S951 M3

G43 H2 Z2. M8

G98 G83 Z-.45 R.1 Q.05 F4.3

X-26. Y-35.5

---

So I should change it to

X-20. Y-41.5

G80

M5

M9

G91 G28 YO. Z0.

G49======================only adding this?

M01

T2 M6 ( TOOL - 2 DIA. - .281 #K DRILL )

( "CC" .281 ENTRY DRILL FOR 1" DIA. )

G0 G90 G54 X-20. Y-41.5 S951 M3

G43 H2 Z2. M8

G98 G83 Z-.45 R.1 Q.05 F4.3

X-26. Y-35.5

[mayday]

yes that will cancel the tool lenght offset,sounds like a control problem to me. I have never had this happen

[chris m]

The G49 is a definite must at the end; the location that you have looks OK. The G28 Y word looks like it has a letter "O" instead of a zero in it?

 

C

[Matthew]

G91 G28 YO. Z0.

 

So I should change it to

 

G91 G28 YO. Z0.

 

 

I don't know if this is a typo or a direct cut-paste from the program, but that "YO." doesn't look like a "zero" compared to the "Z0".

 

Could this cause the problem?

[Matthew]

duh, sorry Chris, I didn't read your post before I replied!

[Scott Bond]

My post is still new,, and i'm manually putting the y0. in ,, and yes it was the letter O ,, but it is still the "mid start" and the "g49" will be tried out today.. Then I'm hoping to doctor up the post this week.

Scott

[Matthew]

Another thing to watch out for when mid starting a program, is make sure it is in G91, and not G90. I have had this cause a problem once in the past.

[Scott Bond]

Hi everyone

I tried every opinion--I am now surrendering.

Our machine still rapids into the part where it should pick up the feed.

Also while doing so I am not able to change the feed with either the

feed percentage dial of the rapid percentage dial.

Yet if we reset the program and then cycle start if runs fine great for a

part or two ..

I must call the machine builder tomorrow.

 

Thank you all for your input

Scott

 

[ 08-20-2003, 08:27 PM: Message edited by: Scott Bond ]