| |
| Home Page | Mark Forums Read | Today's Posts | My Replies | Classifieds | Reviews | Photo Gallery | Web Links | Share Files | Advertise With Us | Ad List |
| |||||||
| G-Code Programing Discuss G-code programing and problems here! |
| | |
| This forum is sponsored by: |
 |
| | LinkBack | Thread Tools | Search this Thread | Display Modes |
|
#1
 
12-05-2007, 10:10 AM
| |||
| |||
Could someone please post a couple of simple lathe programs in Fanuc 10T. I have been programming a Tsugami Mercury with a 6T for years and I now have another lathe to use only it has a 10TF. I don't care to learn the convesational side of it but hope to be able to program it with G code. I have been using G50 like a G92 with the tool X and Y position at the beginning of the program and always send the tool back to this position before a tool change and then on the next tool G50 again and so on. This is the way I was shown to program but believe there may be a better way by using the offsets to load my tool home position in and then a G28 at the end of the program? On my new lathe G50 is not for tool presets but for max speed. Any help would be greatly appreciated. Thank you, Keith  |
|
#2
12-05-2007, 01:02 PM
| |||
| |||
| here is a program that will run on a 10t O1586 (SUB PROGRAM# 1200) G54 G28U0W0 G50S1500 G40G20G80G99 M41 N1T0101(ROUGH TURN) G97S559M3 G54 G0X4.65Z0M8 G96S650M3 G1X1.25F.005 G0Z.1 X4.6 G71P50Q60U.015W.002D0500F.014 N50G0X2.75Z.1 G1Z-.1155 X4.44 X4.5Z-.1455 Z-1. X4.65 N60 G0Z.1 M9 G97S1000M3 G28U0W0 M01 N3T0303(FINISH TURN) G97S1107M3 G54 G0X2.71Z.1M8 G96S750M3 G1Z0F.01 G1X2.75Z-.02F.0025 G1Z-.1155F.0035 X4.44 X4.5Z-.1455 Z-1. X4.6 G0Z.1 M9 G97S1000M3 M01 N6T0606(BORE) G97S1385M3 G54 G0X1.3Z.1M8 G71P10Q20U0W0D0500F.012 N10G0X2.14Z.1 G1Z0 G1X1.84Z-.15 Z-2.45 X1.25 N20 G0Z.1 M9 G97S1000M3 G28U0W0 M00 (FLIP PART) N21T0101(ROUGH TURN 2.756 O.D.) G97S559M3 G55 G0X4.65Z0M8 G1X1.25F.005 G0Z.1 X4.6 G71P55Q65U.015W.002D0500F.014 N55X2.756Z.1 Z-1.526 X4.65 N65 G0Z.1 M9 G97S1000M3 M01 N23T0303(FINISH TURN) G97S11136M3 G55 G0X2.696Z.1M8 G96S750M3 G1Z0F.01 G1X2.756Z-.03F.0025 G1Z-1.526F.0035 X4.44 X4.5Z-1.556 X4.65 G0Z.1 M9 G97S1000M3 M01 N26T0606(BORE) G97S1000M3 G55 G0X2.14Z.1M8 G1Z0F.01 G1X1.875Z-.136F.0015 G1Z-2.5F.005 X1.8 G0Z.1 M9 M5 G28U0W0 M01 N2T0202(16-4 B THREAD) M40 G97S45M4 G55 G0X1.8Z.25M8 G04P2000 M98P1200 G0X1.8Z.5 M98P1200 G0X1.8Z.75 M98P1200 G0X1.8Z1. M98P1200 G0X1.8Z1.25 M98P1200 G0X1.8Z1.5 M98P1200 G0X1.8Z1.75 M98P1200 G0X1.8Z2. M98P1200 G0X1.8Z2.25 M98P1200 G0X1.8Z2.5 M98P1200 G0X1.8Z2.75 M98P1200 G0X1.8Z3. M98P1200 G0X1.8Z3.25 M98P1200 G0X1.8Z3.5 M98P1200 G0X1.8Z3.75 M98P1200 G0X1.8Z4. M98P1200 M9 M5 G28U0 G28W0 M01 N36T0606(DEBURR) M40 G97S1000M3 G55 G0X2.14Z.1M8 G1Z0F.01 G1X1.877Z-.136F.0025 G1Z-2.5F.008 X1.8 G0Z.1 M9 M5 G28U0W0 M30 |
|
#3
12-06-2007, 09:35 AM
| |||
| |||
| Thank you for the example. There are some G codes in it I am not familiar with. G54-G55. I assume these are work shift offsets? I ordered a book for my 10TF and it has the conversational programming in it. I am waiting for the 10TA manual to get here. It is supposed to be for the G code programming side of this control. Hopefully it will help me understand these new(to me) codes and show me how to enter them in the control. What is the purpose of the G28 U0W0 block right after the G54 block at the beginning of the program? I know these must be easy questions for you but please bear with me. Thanks, Keith |
|
#4
12-06-2007, 02:39 PM
| |||
| |||
Hi I run a DSG with 10TF control and from memory G54 / G55 are used as additional workshift commands called within the program. If you need more info let me know and I will check my manuals, its not a function I have used in recent times. I would be happy to assist with your questions if i can. I agree with your comments on the FAPT system, nice for a salesman but not much use in the shop, we always program direct with G code. |
|
#5
12-07-2007, 02:22 PM
| |||
| |||
And here it is with a few liberties taken. Don't know your machine, but it should still run. Your 2nd rough turn should have alarmed because you need a G-code in the N55 block. G54-G55-G1 are modal. U0W0 are understood. Also many machines will run with a G1 in place of the G0 in the canned G71-G72 cycles, and that is what I use because of the shallow DOCs I take (similar to your cuts). Assumed material 4.6 diameter based on your 1st approach. Personally I wouldn't finish face with my roughing tool. Can you depend on your operators to maintain the .1455 depth? I can't. What kind of material is it, and how critical is the finish on the face? I also swing a small radius on all chamfers to push the burr ahead of the insert. Looks like it is a thru bore. No idea what your 1200 subprogram looks like. Although I have threaded using a subprogram, I have never seen anything like your cycle. A 4 inch start is a lot of lead. I would be interested in seeing your 1200 subprogram. M3s on G96 blocks aren't needed unless you eliminate the G97 block. Added G96 to your rough bore. I see the chamfer move at the 4.5 diameter is .03 x 45 deg. & that the front chamfer is a nice round .02 move. Did you allow for tool compensation? O1586 (SUB PROGRAM #1200) G28U0W0 G50S1500 G40G20G80G99M41 N1G54T0101(ROUGH TURN) G97S559M3 G0X4.65Z0M8 G96S650 G1X1.25F.005 G0X4.6Z.03 G71P50Q60U.015W.002D500F.014 N50G0X2.75 G1Z-.1155 X4.44 X4.5Z-.1455 N60Z-1. G97S1000M9 G28W0 M1 N3T0303(FINISH TURN) G97S1107M3 G0X2.71Z.1M8 G96S750 G1Z0F.01 X2.75Z-.02F.0025 Z-.1155F.0035 X4.44 X4.5Z-.1455 Z-1. X4.53 G0G97Z1.S1000M9 G28W0 M1 N6T0606(BORE) G97S1385M3 G0X1.3Z1.M8 G96S600 Z.03 G71P10Q20D500F.012 N10G0X2.14 G1Z0 X1.84Z-.15 N20Z-2.45 G97Z1.S700M9 G28U0W0S50 M0 (FLIP PART) N21G55T0101(ROUGH TURN 2.756 O.D.) G97S559M3 G0X4.65Z0M8 G1X1.25F.005 G0X4.6Z.03 G71P55Q65U.015W.002D500F.014 N55G0X2.756 N65G1Z-1.526 G97S1000M9 G28W0 M1 N23T0303(FINISH TURN) G97S11136M3 G0X2.696Z.1M8 G96S750 G1Z0F.01 X2.756Z-.03F.0025 Z-1.526F.0035 X4.44 X4.5Z-1.556 U.004W-.02 G0G97Z1.S1000M9 G28W0 M1 N26T0606(BORE) G97S1000M3 G0X2.14Z.1M8 G1Z0F.01 X1.875Z-.136F.0015 G1Z-2.5F.005 X1.8 M9 G0Z.1 G28U0W0M5 M1 N2T0202(16-4 B THREAD) M40 G97S45M4 G0X1.8Z.25M8 G4P2000 M98P1200 G0X1.8Z.5 M98P1200 G0X1.8Z.75 M98P1200 G0X1.8Z1. M98P1200 G0X1.8Z1.25 M98P1200 G0X1.8Z1.5 M98P1200 G0X1.8Z1.75 M98P1200 G0X1.8Z2. M98P1200 G0X1.8Z2.25 M98P1200 G0X1.8Z2.5 M98P1200 G0X1.8Z2.75 M98P1200 G0X1.8Z3. M98P1200 G0X1.8Z3.25 M98P1200 G0X1.8Z3.5 M98P1200 G0X1.8Z3.75 M98P1200 G0X1.8Z4. M98P1200 M9 G28W0M5 M1 N36T0606(DEBURR) M40 G97S1500M3 G0X2.14Z.1M8 G1Z0F.01 X1.875Z-.136F.0025 Z-2.5F.008 X1.84F.03M9 G0Z1.S100 G28U0W0M5 M30 |
| Sponsored Links |
| |
|
#6
01-01-2008, 08:04 PM
| |||
| |||
mosesooi, I have a moriseiki cnc c/w Fanuc 10T controller,could someone tell me which parameter to change,so that i don't have to key X-axis in negative sign after work coordinate had been determined. Thanks. Last edited by mosesooi; 01-01-2008 at 09:25 PM. Reason: wrong spelling |
|
| | |
| Currently Active Users Viewing This Thread: 1 (0 members and 1 guests) | |
| Thread Tools | Search this Thread |
| Display Modes | |
| |
Similar Threads | ||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| Sample Fanuc Tool change macro | dpuch | G-Code Programing | 6 | 06-01-2011 08:13 PM |
| Any Sample programs with live tooling for Daewoo 700 with Fanuc 18i | bdyenter | Daewoo/Doosan | 2 | 11-02-2007 08:55 PM |
| Sending programs FROM Fanuc 0-PC | scottsr60 | Fanuc | 3 | 01-02-2007 07:07 AM |
| Any One in need of cnc Lathe programs? | tiroler537 | Mastercam | 15 | 08-14-2005 02:08 PM |
| Lathe CAM Programs, help choosing | djshop | General CAM Discussion | 4 | 07-30-2005 10:11 AM |
| | |
Linear Mode
