Simple HAAS example

[Fairlane6t9]

Hi all...new to the community and have a question about HAAS lathe programming. Can anyone give me a simple example of a lathe program. For instance, something like a simple punch with say maybe 3 steps on it? Just looking for a place to start as I don't have any experience on a CNC lathe with manual programming. Any help is appreciated.

[Geof]

Provide a sketch, as a jpg, with dimensions and I can show you the program that would do it.

[JDenyer232]

Originally Posted by Fairlane6t9 Hi all...new to the community and have a question about HAAS lathe programming. Can anyone give me a simple example of a lathe program. For instance, something like a simple punch with say maybe 3 steps on it? Just looking for a place to start as I don't have any experience on a CNC lathe with manual programming. Any help is appreciated.

Here ya go, this is for a threaded part with 2 different diameters. There are some repititions on the diameter as this part is only .060" in diameter at its smallest section, being fairly long and me not wanting to set up the tailstock for it I corrected the tappering issues by machining the small section several times at slower and slower feedrates. I only needed 10 of these, if I needed more then I would have programmed it differently to reduce my cycle time.

%
O00600
(CLR0006 REVA)
T808
(.375 360 BRASS)
(1.2 IN. FROM CHUCK FACE) G00 Z2.
X2.
G28
T505
(80 DEG INS) G54
G50 S2500
G96 S200 M03
G00 X0.424
/ M08
G00 Z0.05
G72 P101 Q102 U0 W0 D0.015 F0.002
N101 G00 Z-0.03
G01 X-0.025
N102 G01 X-0.025 Z0.05
G00 X0.374 Z0.
M09
G00 X2.
Z2.
M01

(OD TURN)
T505
G54
G50 S3000
G96 S300 M03
G00 X0.449
/ M08
G00 Z0.05
G71 P101 Q102 U0 W0 D0.025 F0.002
N101 G00 X0.11
G01 X0.11 Z-0.665
N102 G01 X0.449
G00 X0.449 Z0.05
M09
G00 X2.
Z2.
M01
(OD TURN)
T505
G54
G50 S3000
G96 S300 M03
G00 X0.185
/ M08
G00 Z0.05
G71 P101 Q102 U0 W0 D0.025 F0.0005
N101 G00 X0.11
G01 X0.11 Z-0.665
N102 G01 X0.185
G00 X0.185 Z0.05
M09
G00 X2.
Z2.
M01
(OD TURN)
T505
G54
G50 S3000
G96 S300 M03
G00 X0.185
/ M08
G00 Z0.05
G71 P101 Q102 U0 W0 D0.015 F0.002
N101 G00 X0.06
G01 X0.06 Z-0.25
N102 G01 X0.185
G00 X0.185 Z0.05
M09
G00 X2.
Z2. M01
(OD TURN)
T505
G54
G50 S3000
G96 S300 M03
G00 X0.135
/ M08
G00 Z0.05
G71 P101 Q102 U0 W0 D0.015 F0.0005
N101 G00 X0.06
G01 X0.06 Z-0.25
N102 G01 X0.135
G00 X0.135 Z0.05
M09
M01
(OD TURN)
T505
G54
G50 S3500
G96 S300 M03
G00 X0.135
/ M08
G00 Z0.05
G71 P101 Q102 U0 W0 D0.015 F0.0002
N101 G00 X0.06
G01 X0.06 Z-0.25
N102 G01 X0.135
G00 X0.135 Z0.05
M09
(OD CHAMFER)
T505
G54
G50 S2500
G96 S200 M03
G00 X0.16
/ M08
G00 Z-0.2
G71 P101 Q102 U0 W0 D0.01 F0.002
N101 G00 X0.06
G01 Z-0.25
N102 G01 X0.11 Z-0.3075
G00 X0.11 Z-0.25
M09
G00 X2.
Z2.
G28
M01
(OD THREAD)
T606
(ON EDGE INS.)
G54
G97 S2000 M03
G00 X0.21
Z-0.175
G04 P1.
/ M08
M24
G76 X0.0805 Z-0.515 K0.0347 I0. D0.01 F0.025
G00 X0.21 Z-0.175
M09
M01
(OD THREAD)
T606
G54
G97 S2000 M03
G00 X0.21
Z-0.175
G04 P1.
/ M08
M24
G76 X0.0805 Z-0.515 K0.0347 I0. D0.01 F0.025
G00 X0.21 Z-0.175
G00 X2.
Z2.
M09
G28
M01
(PART OFF WITH PECK)
T707
G54
G50 S1500
G96 S300 M03
G00 X0.161
/ M08
G00 Z0.05
G00 X0.161 Z-0.584
M36
G75 X-0.05 Z-0.584 I0.005 F0.001
M37
G00 X0.161
G00 X0.161 Z0.05
G00 X2.
Z2.
M09
M05
G28
M01
T808
(STOP BLOCK)
G00 Z0
X0
M30

%
Hope this helps.

[RMR]

Does your HAAS Lathe have quick codes

[hardcore]

Check out www.cncci.com they sell a turning center programing,setup, and operation learning book. It's pretty good if you are trying to learn on your own about fanuc controls like your haas is. Also Haas has a online class www.learnhaas.com the class runs a grand the book was 60 bucks. If your still having troube look into mastercam.

[RMR]

If you had a dwg or dxf file or pdf I could program it in master cam for you.

[RMR]

Just for fun to see if the program is smaller or bigger.

[Geof]

If he showed up again all of the above maybe could be done. One post and he evaporates.

[Fairlane6t9]

Sorry for the delay. Trust me, I have not evaporated into thin air. I've programmed with Mastercam X3, but it wants to post out the LONG version of turning. This may be due in part to not having the proper post for the HAAS lathe. I'm interested in canned cycles for some of the turning etc. I've got a HAAS lathe programming workbook, but honestly, some of the things in there don't give the reasons for doing what's there. I like to know why I'm doing something, not just taking it for granted. Anyway, thanks for the replies.

[JDenyer232]

Originally Posted by Fairlane6t9 Sorry for the delay. Trust me, I have not evaporated into thin air. I've programmed with Mastercam X3, but it wants to post out the LONG version of turning. This may be due in part to not having the proper post for the HAAS lathe. I'm interested in canned cycles for some of the turning etc. I've got a HAAS lathe programming workbook, but honestly, some of the things in there don't give the reasons for doing what's there. I like to know why I'm doing something, not just taking it for granted. Anyway, thanks for the replies.

There is nothing wrong with the long version, after all the software is writing it, not you. If you have a cam package then by all means let it do the work for you. I thought the work book combined with the owners manual did a pretty good job of explaining canned cycles. Did your machine come with vqc templates? If so it will write out the canned cycles based on answering a few dimensional questions that it asks you. The intuitive programming system works in much the same way as the vqc templates. Hope this helps.

[Fairlane6t9]

I agree, there is nothing wrong with the long version MasterCam generates. I'm actually a new CNC Instructor at a local community college, and 99% of my training/experience is with mills and milling aircraft parts. This is why I didn't want the long version. I want my students to be able to program some things manually using canned cycles. I'm just not used to some of teh stuff on the lathe. When I went through the program, we used software to generate the code, but didn't go over what it was or what it was doing. The lathe does have VQC, but I don't want my students to get into the quick code until they understand what the G-code is actually doing. I'm coming in behind an instructor that left at the end of last semester and I along with the lead instructor have been having a hard time getting things back together. Thanks for the help.

[JDenyer232]

Originally Posted by Fairlane6t9 I agree, there is nothing wrong with the long version MasterCam generates. I'm actually a new CNC Instructor at a local community college, and 99% of my training/experience is with mills and milling aircraft parts. This is why I didn't want the long version. I want my students to be able to program some things manually using canned cycles. I'm just not used to some of teh stuff on the lathe. When I went through the program, we used software to generate the code, but didn't go over what it was or what it was doing. The lathe does have VQC, but I don't want my students to get into the quick code until they understand what the G-code is actually doing. I'm coming in behind an instructor that left at the end of last semester and I along with the lead instructor have been having a hard time getting things back together. Thanks for the help.

No problem, glad to help. I would suggest getting some books on cnc lathe programming, while the canned cycles are easy to use you will need the definitions of the variables in the cycle. The Hass manual does an excellent job of explaining this. For example G76 X=minor diam Z=thread end point I=thread taper amount if any K=thread height D=first pass cutting depth etc. Most controls use the same format among the different canned cycles, and in fact these canned cycles are very similar to canned cycles used in drill and milling operations. I first learned G-code on the mill, once we got a lathe having the knowledge of programming the mill made learning the lathe fairly easy. What are you using for text books in the class? Maybe changing to different more up to date books would help your class out? Just some ideas to ponder.