Newbie- Fagor/Hardinge 8025- G-codes are they all the same?

[Jnice]

Hey guys,
Im a new guy to metalworking and i was hoping i could get some advice and maybe a point in the right direction. Just as some back round info. i was an excavation contractor and ran heavy equipment and recently got a job working in a machine shop, i am a hard worker and would like to do the best and make the best parts i can as fast as possible. I am being trained on a few different sized Hardinge lathes with Fagor operating systems. The guy training me is only showing me how to enter offsets and select programs.

So basically im not expecting to be a tool maker overnight but i would like to take the initiative and try and learn some things that he isnt teaching me via you. There are a few different lathes i have access to and and some times im left to set up jobs on my own. I know on some jobs im told that there isnt a program set for the task im trying to accomplish and that i have to wait (when my boss asked me to get that specific job finished and sent on).


We machine cold head punches for screw pressing machines, and so far ive learned a few tasks such as facing off, cutting leads, indenting and cross-cornering pins for hexing(which im also being trained on).

So i guess my main question is - is there a list any where that can show me all the codes available for this operating system that has any sort of detailed explanation for a beginner like myself? ANY and ALL advice/information would greatly be appreciated!!

[g-codeguy]

All machines come with a programming manual when new. All the codes available for use on the machine will be in this manual. The manual will also give examples of using each code correctly if it is worth anything. Some aren't all that good. Can you borrow one to read? Also please return it if allowed to read it. Many of our manuals are long gone because people wanted to learn, but never returned the books. Actually I can't think of one person who did bother to spend any time reading the manual once they got it home. I no longer allow anyone to take them home because of this. We have but one copy of several manuals only because I kept a copy in my desk.

[Jnice]

yes i do have the programming manual and the operating manual, im not sure if it is for the specific cnc im working on. we have 3 fagor operating systems on three different hardinge lathes. im just having a hard time understanding the programming manual because there seems to be a decent amount of typos. i would imagine the majority of it is okay to submit to memory but there are those thoughts of "what if".

im also having a hard time understanding the parameters of the machine. is there a manual for that? if so i could get ahold of it, i have been studying the programming manual and like i was saying there are some codes that will do certain things depending on the machine parameters, for instance, and dont quote me because i dont have it in front of me at the moment, when P009(1)=1 and P009(0)=1. im assuming this has something to do with the limits of the machine, but i dont know.

also it gives a format for programs but doesnt explain which codes/axese inputs are supposed to be programmed alone, and which get re-programmed on another block.


here is an example of a face off program with a lead.

N0 (7/8 F.O.)
N10 G0 G94 G90 G70 G7
N20 S2500 M3
N30 T4.4
N40 X.900
N50 Z-.200
N60 G1 G95 F.002
N70 Z-.200
N80 G92 S3000
N90 G96 S300
N100 X.890 F.002
N110 X.852 Z-.060
N115 X.757 Z0
N120 X-.060
N130 G0 Z1.5
N140 T0.0
N150 M30


why do lines 50,70 have the same input?

basically i have a very vauge idea of how to make a program like this work for a smaller sized part, by changing the axese. when it comes to understanding what G codes need to be programmed with/work with other codes im lost. tha manual explains what they are. but not where they go, in relation to other codes, however it does list some that are to be listed alone, are these "modal" codes? sorry for the loooong reply. im just very interested.:

[g-codeguy]

Originally Posted by Jnice yes i do have the programming manual and the operating manual, im not sure if it is for the specific cnc im working on. we have 3 fagor operating systems on three different hardinge lathes. im just having a hard time understanding the programming manual because there seems to be a decent amount of typos. i would imagine the majority of it is okay to submit to memory but there are those thoughts of "what if". im also having a hard time understanding the parameters of the machine. is there a manual for that? if so i could get ahold of it, i have been studying the programming manual and like i was saying there are some codes that will do certain things depending on the machine parameters, for instance, and dont quote me because i dont have it in front of me at the moment, when P009(1)=1 and P009(0)=1. im assuming this has something to do with the limits of the machine, but i dont know. also it gives a format for programs but doesnt explain which codes/axese inputs are supposed to be programmed alone, and which get re-programmed on another block. here is an example of a face off program with a lead. N0 (7/8 F.O.) N10 G0 G94 G90 G70 G7 N20 S2500 M3 N30 T4.4 N40 X.900 N50 Z-.200 N60 G1 G95 F.002 N70 Z-.200 N80 G92 S3000 N90 G96 S300 N100 X.890 F.002 N110 X.852 Z-.060 N115 X.757 Z0 N120 X-.060 N130 G0 Z1.5 N140 T0.0 N150 M30 why do lines 50,70 have the same input? basically i have a very vauge idea of how to make a program like this work for a smaller sized part, by changing the axese. when it comes to understanding what G codes need to be programmed with/work with other codes im lost. tha manual explains what they are. but not where they go, in relation to other codes, however it does list some that are to be listed alone, are these "modal" codes? sorry for the loooong reply. im just very interested.:

I'm not at work where I can check in the manual for what each code means so I could be wrong on some of the following comments.

First I assume you know what 'modal' and 'non-modal' mean by now. The lathe has defaults that will always be in affect when the machine is turned on. Naturally these pertain to Modal settings only. I believe G90/G91 switch from absolute to incremental although I never use them since I, and the operators, are use to Fanuc controls.

Ex:
G0G90X.875Z0
G1X.2F.005

In this example the tool will move from X.875 to X.2 (a facing move). Change the G90 to G91 and the tool will move from X.875 to X1.075. A slight difference in the results. Default will be Absolute.

G94/G95 are IPM or IPR if I remember correctly. Default should be IPR (G95 I believe). As a general rule there are only 2 places where I use IPM, 1. Barstop operation and 2. Live Tooling...neither of which are available on our Fagor controlled lathes. A 3rd place is when I don't want to use a G0 command, but what a fairly fast move. Most times I only use this method when drilling.

Ex:
G0X.875Z.03
G1Z-1.F.005
X.9
Z.03F.03

Time to reach the front of the part at F.03 will vary greatly depending on RPM. Will take a lot longer if spindle is running at S500 versus S5000. This is where I would use IPM. IPM does not depend on spindle RPM.

You will notice that just about everyone programs lathes in IPR. Try this with a drill:

G97S1000
G0X0Z.03T4.4
G1Z-.5F.005

VERSUS

G97S1000
G0X0Z.03T4.4
G1Z-.5F500

Actually don't try it with a drill in the holder because in the latter example the drill will feed into the part even tho the spindle is not turning (no M3). The first example will rapid to the front of the part and stop. Why? Because spindle is not turning.

Block N70 does nothing. Here is a better way (IMHO) to program this operation. I may modify it later as I can't recall what G7 and G70 do...having never used them on our Fagor controls.

N0 (7/8 F.O.)
N10 G97 S1273 M3
N20 G0 X.9 T4.4
N30 G92 S3000
N40 G96 S300
N50 Z-.2
N60 G1 X.89 F.002
N70 X.852 Z-.06
N80 X.757 Z0
N90 X-.06
N100 G0 Z1.5
N110 T0.0
N120 M30

A bit cleaner and easier to understand, wouldn't you agree? S1273 is the correct RPM for S300 SFM at X.9 diameter, and G97 insures it will always start at that RPM. I like to start my spindle at the RPM it will be running at for the sfm/dia used. I always set max rpm and sfm after my 1st X move.

You absolutely shouldn't touch a machine Parameter. Not knowing what you are changing could cause the machine to crash or quit working entirely. You need to understand the machine and its parameters VERY well before changing any of them.

I'm glad to help when I can as are many others. Just ask. Giving an example you are working with is always a good idea. It helps us help you.