Odd alarm R and Z confilct in G81

[Shotout]

I edited a program that we run on our OKK HMCs (Fanuc 310is) for one of the Okuma (OSP200M) and ran the program. 1st part over-riding rapids, feeds etc no problem. 2nd part straight through, no optional stops etc and I got an alarm stating my R and Z conflicted in a G81 cycle. They didn't. I edited the code, adding a G71 Z and tacked on a M53 and it cleared it. What I don't get is why I got the alarm to begin with. Am I over looking something? Any help would be appreciated.
Bold characters are before editing with added code in italics.
Sub calls from a Main defining work offsets.
H12=Actual center of rotation of the pallet.
O5532
(CUSTOMER ETC INFO)
(553 OP 2 PALLET 2)
(G15H12)
RP=2M289
G119 (LIB clear Z then X&Y then B0.)
G0G90G94G20G80
M1
N2012
(30MM DR DRILL)
CALL OCHG1 TOOL=12
G15H12
M120
M50
G0G90B178.
G0G90X-5.975Y8.870S1800M03
G56H12Z9.1T13
G71 Z10.5
G81X-5.975Y8.870Z8.12R9.1F12.M53
G80
M5
M9
Z16.
G119
M1
<SNIP>
G120 (LIB G30P1 M60)
RTS

[Algirdas]

that's right, look:
G56H12Z9.1T13
G71 Z10.5
G81X-5.975Y8.870Z8.12R9.1F12.
You have both Z and R = 9,1 and compensation G56.
make Z=9,2 or more and must be correct. It depends on accuracy of rapid approach to contour

[Shotout]

I checked the 3 other parts of that family that run on that fixture. I am using the same Z coordinate in the tool length line as the R value in the fixed cycle. I did however have the G71 and M53 in those other programs. Why would the inclusion of the M53 return prevent the error but the exclusion of it cause the conflict alarm? Thanks

Originally Posted by Algirdas that's right, look: G56H12Z9.1T13 G71 Z10.5 G81X-5.975Y8.870Z8.12R9.1F12. You have both Z and R = 9,1 and compensation G56. make Z=9,2 or more and must be correct. It depends on accuracy of rapid approach to contour

[broby]

Can not say that I can see anything wrong in your program.
The only thing is, I usually would program the drilling cycle as follows: (Assuming Z0 top face)

N2012
(30MM DR DRILL)
CALL OCHG1 TOOL=12
G15H12
M120
M50
G0G90B178.
G0G90X-5.975Y8.870S1800M03
G56 H12 Z20 T13
G71 Z10.5
G81 X-5.975 Y8.870 Z8.12 R9.1 F12. M53
G80
M5
M9
Z20
G119
M1
<SNIP>

Usually we approach the job stopping 20mm clear of he work face, before the required operations. This way the operators are used to a standard approach distance and can see and expect the same for each tool.

BTW... what is the following statement for?
RP=2M289

Are you assigning the value of 2 to variable RP and then using M289?
Or something else altogether?

Regards
Brian.

[DIFF OVER]

Agree. i do like to do:
G0 G56 Z1.0 HA

[broby]

Yes I agree, I also use the HA, HB & HC along with DA, DB and DC offset registers in the programs as it makes life so much easier, both for the programmer and for the operator.
If your tool numbers are as dynamic as they are here, it really is the only way to program... never have to remember to alter tool offset numbers throughout the program again.
That being said... on our MA600HB, we MUST use these codes as the machine uses tool groups rather than Tool numbers and we never really know ahead of time (as a programmer) what tool number to use, thus we use VC numbers to set the tool group ID number at the start of the program, set and forget.
I also noticed in the program fragment the use of "T13" on the Tool length offset (G56) line.
I am in the habit of calling the next tool on a line by itself, along with a comment describing the next tool. This way the operator can see exactly what tool should be coming in next, rather than looking at just a tool number.
i.e.

Blah
Blah
N100 M6
N102 M1
N104 T=VC41 (NEXT TOOL= 80MM R490 FACEMILL)
N106 G15 H...
N108 G0 X... Y...
N110 G56 HA Z20
N112 M3 S...
N114 M8
ETC...

Blah
Blah
N120 M6
N122 M63 (NO MORE TOOLS REQ)
N124 M1
N126 G15 H...
ETC...

This way the preamble is the same for each tool/process and the operator is in known territory. Flip the Optional Stop switch (or push the button as the case may be) and the machine will stop after the tool change. The note alongside the M63 command also lets the operator know that the last tool is now coming up.

[Shotout]

Z is set to center of rotation of the pallet. The approach is .125in from the nominal value of the casting surface which can vary by about .06in.

RP=2M289 is for pallet recognition. On the Fanuc machines at work this is essential for the Okumas they are for my peace of mind. I use a main program that checks the pallet in the machine and calls the appropriate sub for that pallet.

Originally Posted by broby Can not say that I can see anything wrong in your program. The only thing is, I usually would program the drilling cycle as follows: (Assuming Z0 top face) <SNIP> Usually we approach the job stopping 20mm clear of he work face, before the required operations. This way the operators are used to a standard approach distance and can see and expect the same for each tool. BTW... what is the following statement for? RP=2M289 Are you assigning the value of 2 to variable RP and then using M289? Or something else altogether? Regards Brian.

[Superman]

your OKK code in blue
only needs the modification in red to run on Okuma ( method of end cycle required )( like the Fanucs use M98/M99 )
G15H12
M120
M50
G0G90B178.
G0G90X-5.975Y8.870S1800M03
G56H12Z9.1T13
G81X-5.975Y8.870Z8.12R9.1F12. M54
G80
M5

There are 3 modes of return after a "drill cycle"
M52 ( return to initial level )( see example below )
M53 ( return to G71 point) ( G71 Zvalue must be stated before cycle )
M54 ( return to R plane )


G15H12
M120
M50
G0G90B178.
G0G90X-5.975Y8.870S1800M03
G56H12Z20.
G71 Z10.5
G81X-5.975Y8.870Z8.12R9.1F12. M52 ( returns to Z20.)
X-2. Y-2. M53 ( returns to Z10.5)
X-1 Y-1. M54 ( returns to Z9.1)
X0. Y0. P5. M53 ( 5 sec.dwell added + retract to Z10.5 at end )
X1. Y1. Z8.0 P0 M52 ( new drill depth + dwell cancelled + retract to Z20 at end )
X2. Y2. Z7.5 R9.5 M54 (new depth + new retract + retract to Z9.5 at end )
G80 ( Use G0 if you don't want the spindle to stop )( G0 also cancels the cycle)
M5
...
M30

remember, each address is modal until cancelled or overwritten by a new value
my example will run on an Okuma as is.

[Shotout]

What I'm not understanding is why I had to add the M5x to the code. Shouldn't the G81 default to the return to initial point without it? This was a first run that I was rushed into trowing up so the code wasn't clean and I didn't have time to actually sit down at an editor to clean it up. I was using notepad on the controller if you can imagine. I normally will clean the code up and set a long Z value for G71 and edit that to a better value as I run the 1st part but time was critical in this case so I had to go with it. Because I was working outside of my 4 dots so to speak I came across an alarm that I didn't actually understand what the root cause is for it.

[broby]

Re-reading your original post, I realised that you said that only after the first run did you add in the G71 Z9.1 and M53.
Not absolutely certain of this statement... but I think you MUST have one of the retract M codes in your drilling cycle for the machine to know how to retract from the end point of the hole.
As for why the machine never gave you an alarm on the 1st run? No idea! I have seen a few examples of programs that kick up a fuss when running at 100% but are OK on single block... go figure.
Might be one of those issues where you have to accept the requirements and move on.
Regards
Brian.

[Shotout]

Originally Posted by broby Re-reading your original post, <SNIP> Might be one of those issues where you have to accept the requirements and move on. Regards Brian.

I had also done a program restart in there. I snipped the first drill cycle (different tool) out of the program. That had to clear a known point on the fixture so it was easy to set the correct G71 and retract 1in past that point and move to the second hole with the first drill, however I had to stop the machine and do a pallet rotation to B45. after the first tool operation to check that the hole was centered in the boss because if the y offset was too low 30mm would strike a rail on the casting. The drill only has about .08in clearance below it with nominal placement of the 30mm hole.

Your right I might just have to accept it and stick in the back of my mind for future programs, but I was hoping to understand the reasoning behind it. When hand editing something like this and proofing it myself this is easy enough to deal with, but with new work coming in it will be code generated from our cam software so it is something that could and should be fixed before sending the program to the machine.