g-code mystery....any ideas?

[bellyup]

here is an abbreviated version of the file run on a makino vmc/fanuc. please scroll to the bottom to see the problem. i don't think the problem is in the code, but more likely something else. machine error, etc.(???) i didn't program it, but watched it run, and the control showed the same code you see here, but did what i have edited in.

is this breadwinner getting senile? hope you can help.

 

gone for the weekend now. thanks in advance.

 

quote:

---

%

O1000

(10364-101-10)

(21-03-06 - 07:41)

( 6 MM FLAT ENDMILL TOOL - 20 DIA. OFF. - 21 LEN. - 1 DIA. - .2364)

(INSIDE POCKET(15-17))

G20

G0G17G40G49G80G90

T20

G0G90G54X-2.8882Y2.8882S15000M3

G43H1Z.1M7

G5 P10000

Z-1.089

G1G41D21Z-1.191F5.

Y3.1118F50.

X-3.1118

Y2.8882

X-2.8882

Z-1.091F150.

G0Z.1

X-2.7482Y2.7482

Z-1.089

G1Z-1.191F5.

Y3.2518F50.

X-3.2518

Y2.7482

X-2.7482

Z-1.091F150.

G0Z.1

X-2.6082Y2.6082

Z-1.089

G1Z-1.191F5.

Y3.3918F50.

X-3.3918

Y2.6082

X-2.6082

Z-1.091F150.

G0Z.1

X-2.4682Y2.4682

Z-1.089

G1Z-1.191F5.

Y3.5318F50.

X-3.5318

Y2.4682

X-2.4682

Z-1.091F150.

G0Z.1

X-2.8882Y2.8882

Z-1.091

G1Z-1.193F5.

Y3.1118F50.

X-3.1118

Y2.8882

X-2.8882

Z-1.093F150.

G0Z.1

X-2.7482Y2.7482

Z-1.091

G1Z-1.193F5.

Y3.2518F50.

X-3.2518

Y2.7482

X-2.7482

Z-1.093F150.

G0Z.1

X-2.6082Y2.6082

Z-1.091

G1Z-1.193F5.

Y3.3918F50.

X-3.3918

Y2.6082

X-2.6082

Z-1.093F150.

G0Z.1

X-2.4682Y2.4682

Z-1.091

G1Z-1.193F5.

Y3.5318F50.

X-3.5318

Y2.4682

X-2.4682

Z-1.093F150.

G0Z.1

X-2.8882Y2.8882

Z-1.093

G1Z-1.195F5.

Y3.1118F50.

X-3.1118

Y2.8882

X-2.8882

Z-1.095F150.

G0Z.1

X-2.7482Y2.7482

Z-1.093

G1Z-1.195F5.

Y3.2518F50.

X-3.2518

Y2.7482

X-2.7482

Z-1.095F150.

G0Z.1

X-2.6082Y2.6082

Z-1.093

G1Z-1.195F5.

Y3.3918F50.

X-3.3918

Y2.6082

X-2.6082

Z-1.095F150.

G0Z.1

X-2.4682Y2.4682

Z-1.093

G1Z-1.195F5.

Y3.5318F50.

X-3.5318

Y2.4682

X-2.4682

Z-1.095F150.

G0Z.1 (apparently a good move)

X-.8882Y2.8882 (made an x positive move, no y move.)

Z-1.089 (made a good move)

G1Z-1.191F5. (made a good move)

Y3.1118F50. (made what appears to be an x pos. move)

X-1.1118

Y2.8882

X-.8882

Z-1.091F150.

G0Z.1

---

[Mike-T]

Looks like a cutter comp issue.

[Guest SAIPEM]

It's not a smart idea to turn on cutter comp during a Z only move.

 

You are also not turning it off before rapiding to the next cutting position. This is a major no-no.

 

Change the toolpath to include perpendicular lead-ins and lead-outs and turn comp on and off during these moves.

 

Fanuc is very particular about G41/G42.

[bellyup]

thanks.

[bellyup]

now i'm trying to find out how this happened, and cannot get MC9 to output any code that does the same thing. i asked the programmer how he did it, and he can't seem to remember. (he's changed the mc9 file since then, so it's not the same.) it was a 2d contour with multi passes and depth cuts.

 

are there any circumstances where mc9 would output this type of code?

[gcode]

My guess is that your programmer entered G41

by hand.

[toolall1]

My guess is that your programmer entered G41

by hand

[bellyup]

quote:

---

My guess is that your programmer entered G41 by hand.

---

i had thought of that, but it doesen't seem likely, simply because he reposted the program a few times after the problem first occurred and would have had to edit the same thing right back into the program each time.

[Charlie Pierson]

I would only dare to use one Z-only move while cc is on.

What is in the cc offset D21 ??

Which Fanuc ??

 

I backplotted the code in MC9 , looks standard to me.

 

Is the path ok w/ cc off ??

 

 

cp

[bellyup]

d21 is the register for t20.

 

fanuc is 'professional A'.

 

whatever was happening has been resolved, and the part was successfully machined, using another program. but i'm still trying to determine what caused the bad code in the first place.

 

what i was told was, it was originally a 2d contour toolpath cutting the outside walls of a cluster of pockets (transform copied), with lead ins and outs. worked fine. copy/pasted the toolpath and made adjustments so that it then removed the center area of the pockets without the lead ins and outs. the results of this amended toolpath are the first part of this thread.

 

i realize the most logical answer is a manual edit, but what sense would it make for someone to do that on this program? since it isn't machining the outside walls(the first program did that), if you didn't want cc on, you would just turn it off in the parameters, not go to the trouble of a manual edit.

[PeterM]

Perhaps the switch (enter on first depth cut only) was checked in error. This in in the lead in/out page. Peter

[bellyup]

thanks peter,

it does look like that was on. now if i can only figure out how the comp was being generated on a Z move, i think that will be very close. i've been changing parameters and rechecking the code and it keeps coming in on the first lateral move no matter what i do.