G83 Macro

[hatchmar]

Hi all, We have a shop full of Miyano LE22's turning/milling ctr's and none of them have the ability to do a G83 deep hole pecking cycle. They have G74 pecking cycles but G74 does not do a full retract. our solution to this has been to just write out all the rapids and feeds line-by-line and on some of the holes that are fairly deep, this can be a time consuming as well as memory consuming process. Is there a way to create a Custom Macro that will mimic a G83 full retract cycle? the Miyanos have Fanuc Series O-T controls and judging by the manual, they do have Custom macro A and B ability. Ive tried to understand how these work by reading the book, but anybody that has seen the infamous "Yellow FANUC Book" knows that they arent written well, i guess something getslost in the translation. anyway, does anybody have any ideas on how to do this without taking up alot of memory or time?

[Al_The_Man]

Yeah, the manuals are written in 'Jinglish' , there are a few options, but if you have macro A & B, this allows parametric programming and you could use G65 followed by the values you want to plug into the specified variables in the subroutine that is called by the G65. You would then have to write the subroutine only once.
If you want to do any Macro programming in length, I would recommend getting hold of a 3rd party book on the subject as there is a quite a bit you can do in the way of programming. I believe the canned routines such as G74 exsist in the programs 9000 & up. Hopefull someone here may have done this particular routine to help you get started.
Al

[wms]

Guys,

This was given to me years ago..for this very reason..deep hole peck drilling on a Fanuc OT.

I never used it as I let the cam system output code for this.

See if it helps or you can use it..unfortunatly I will be of no help if you have questions as Macros are not my thing...dumb as a rock as far as they are concerned..but maybe with this Macro and some help from some other user here you can get up to speed.

Below is the Nc program, a hard copy of the nc file, and some instructions.

Please note the program numbers is 9136 and the samples show 9135..must just be a typing error.

[Al_The_Man]

Looking at it, That seems like it might do the trick, anyway if not it is should be almost there and you can fine tune it to your liking.
Al

[hatchmar]

WOW! man, I expected to get some help here maybe pointing me in the correct direction but you guys hit the nail on the head. This Is exactly what I need. I mean exactly! I havent tried it yet because I want to understand how it works but i will take AL's advise and read up on it and ill take WMS's code and put some lipstic on this pig!
thanks very much

[wms]

Hatch,

Your welcome. Glad to help.

Hope it does the trick.

Stop by more often.

OH and Pigs need love too.. : )

[ghyman]

I wrote this macro on a Citizen swiss machine; it allowed me to do a 'regressive' peck cycle... each peck is slightly less than the previous one. This let me keep the bore clear of chips, keep oil on the drill, and eliminated broken drills.
This will work for a 'long-hand' peck cycle without actually requiring 128K of rapid/feed moves to be programmed. Just set the variables and go!

As I said, this was on a Citizen control, so I had to reverse the Z direction, but it should work on any control that has a Fanuc 'look and feel'.

(Fadal users, I can convert it to use V/R variables if need be.)


Set the following values in your program before moving to the first hole.
Set #534 to 1.00 for a 'standard' peck cycle,
Otherwise, it will reduce the length of each peck by a percentage (in this case, 85%)... this is good for really deep holes, where chips, coolant, etc are a concern.
If you do use a regressive peck, make sure #533 is valid for the drill you are using.

(SET-CONDITIONS)
#531=4.361(DEPTH-TO-DRILL)
#532=0.160(FIRST-PECK-DEPTH)
#533=0.010(MIN-PECK-DEPTH)
#534=0.850(REGRESSION-PERCENT)
#535=0.1(Z-START-POSITION)
#536=0(RESERVED)
#537=0(RESERVED)


Then, move to the X/Y hole location, and give it a "M98 H310" on the next line.
Then, for each hole, do an X/Y move, then another "M98 H310"
Finally, at the end of your program, add this:


N310(REGRESSIVE-PECK-CYCLE)
#536=#535
#537=#532
N320(HERE-WE-GO!)
#536=[#536-#537]
IF[#536LE#531]GOTO330(DONE)
G1Z#536F.0016(DRILL-NEXT-DEPTH)
G0Z#535(RETRACT)
G0Z[#536+.005](CLEAR)
#537=[#537*#534](REDUCE-PECK)
IF[#537GE#533]GOTO325
#537=#533(NOT-TOO-SMALL)
N325GOTO320
N330G1Z#531
G0Z#535
M99

Gives you a LOT of control, with no canned cycles, and very little extra code!

[hatchmar]

well., i have been trying to get these programs loaded into the machine but i keep getting "004" alarms. this happens when i try to download the code into the machine and it will load only untill it sees a # sign. ive noticed it will load anything that has a letter in front of it such as " Z#532 " evewn if i try to manually type the code in, it wont allow me to put #'s in until i have a letter in front of it. any ideas?

[ghyman]

Maybe my O-T memory is a little fuzzy, but an error 004 is what you get when you try to use a code that does not exist (Like trying to give a Y-axis move on a machine with only X/Z)... I would think that if you did NOT have macro variables available, that you would get an error 115...

Can you call up the Macro Variables in the 'offset' screen? That would be the first place to look and see if you have the Macro A/B functionality.
If you have #501-#531 available, but not any higher, then you just don't have the 'extended' variables... try re-coding the routine using #501-#507 instead of #531-#537. This will use the basic variables instead.

Or, try this:
In MDI mode, type in
#501=1 EOB INSERT
and hit cycle start
If no errors, then type in
T#501 EOB INSERT
and hit cycle start... you should get a tool change to tool 1.

If you DO get an error with the first code, then try using #101 in place of #501.

If the error continues, then it would appear that you do NOT have the Macro A/B capability, or that there is some other problem...

As a last resort, try the same sequence, only use #1 instead of #101 or #501.

If you can get the #501 or #101 to function in MDI mode, then recoding the peck cycle using the #501-#507 (or #101-#107) should do the trick. If the #1 works, then try re-coding the peck cycle subroutine with #1, #2, ... #7 instead of #531-#537

As I said, my OT memory is a little rusty (I've had 18's for the past 3 years), but you should still have some of the basic variables available.

Let me know!!!

[hatchmar]

ok, I really have been trying to get this by reading the *cough* FANUC manual. part of my problem was that I was trying to change the variables in the wrong place.... oops. we do have a macro screen on the offsets page and i am now trying that. I still have the problem where I cant just type #536=#535. It looks like I have to use a G65 followed by an H code (ex. H01 is = H02 is addition ...) then a P,Q,and/or R. It is starting to make a little sense and I did get the machine to move but it only does one peck and the program ends. another thing im not too sure about with OT controls is the GOTO function. it isnt anywhere in any of the manuals and we have never used it here. I cant even MDI it in but if I upload it, it shows up but doesnt seem to do anything. here is how I have coded it:

O0083
G65H01P#515Q#514 (H01 DEFINITION, SUBSTITUTION)
G65H01Z#507Z#511
N320
G65H03P#515Q#515R#507(H03 SUBTRACTION)
G65H86P330Q#515R#510 (H86 IF<=THEN)
G65G1Z#515F0.0016
G65G0Z#514
G65G0Z#515
G65H04P#507Q#507R#513(H04 PRODUCT)
G65H85P325Q#507R#512 (H85 IF>=THEN)
G65H01P#507Q#512
N325GOTON320
N330G65G1Z#510
G0Z#514
M99
%

PS- i do get an alarm right at the beginning- 025(unusable variable) but if i start from N320 there are no alarms. It says unusable var. in the book but we have variables in the macro screen from 500-531

[hatchmar]

OOPS- THAT 125 ALARM IS "unusable address in G65 command" im assuming that something is wrong with my N numbers?

[hatchmar]

ok, got rid of the alarm, it was on the 2nd line- i had 2 Z's where it should have been a p and a q. it runs trrough but only does one big peck