Lathe Question's

[Hennessy]

I posted this in the Doosan Thread but i guess it is more of a general lathe question. http://www.cnczone.com/forums/showthread.php?t=73729 any help would be a appreciated

Thanks,

Hennessy

[JDenyer232]

The home position is the safest place to perform your tool changes, but in a production environment where time is money you need to change tools as close as you can without crashing. If I were faceing a part off with say tool #5, and then I needed to profile the part with tool #6 I would do something like this.

G00Z1.0X1.0
T606
ETC.
In doing it this way you don't need to spend all that time sending the machine home, but you must make sure that you have enough clearance from your longest tool in your setup. For tools that are flat with the turret I keep them together on one side, ie tools 1-6. I keep my longer tools like drills and boring bars in the 7-12 slots. When I change to a drill or boring bar, or if a tool callout is going to cause the turret to rotate past a long tool I will use G28 to send the machine home for that tool change. You have to look at the code and see where the tools are going to be when you do a tool change. Parting off is fairly easy, just feed it in, the cutoff tool will do the work. Just don't forget to add the cutoff tool width to the position that you want to place the cut. For example if you want your part to be 0.500" long and your cutoff bit is 0.094" wide, then you would have your z axis position at -0.594" assuming your cutoff tool was touched off the face of the part after any facing was done. If you touched off of the raw stock and faced 0.050" off the part then your new z axis position would be -0.644". When doing the actuall parting off start out slow, ie 1000 rpm and .002fpr, you can adjust your speeds and feeds from there.

One word of advice, go slow while you are learning and getting used to the machine, lathes are actually easier to program and run than mills, but crashes can be rather nasty, nothing makes more noise and does more damage then running your turret into a 3 jaw chuck at 3000 rpm and 1000ipm rapids or more. Hope this is of some help.

[Hennessy]

Thanks for the reply.

I think i will keep it safe for awhile and do all my tool changes at home, at least until i get used to the lathe. I work in a prototype shop so cycle times are not a huge issue. our "big" part runs are 25 to 50 parts max.

I guess the only question i still have as far as parting off is the constant sfm.. should this be on or off for parting off? or does it matter?

the last thing that is still fuzzy is the work offset format. Currently it is set to use g50. The manual is confusing as to the application of the code and how to set the offset. I am assuming you would still face the part with tool #1 and set z0 there. I am also unfamiliar with how this affects the use of the tool setter if at all.

I am going to load a program tomorrow and single block it to see how it looks. sorry for all the questions (i know they are basic) but i would rather ask then crash the lathe. there are only 2 of us in the shop and nether one of us has ever programed a lathe before. so i am kinda flying solo on this. I need all the help i can get .

Hennessy

[JDenyer232]

Originally Posted by Hennessy Thanks for the reply. I think i will keep it safe for awhile and do all my tool changes at home, at least until i get used to the lathe. I work in a prototype shop so cycle times are not a huge issue. our "big" part runs are 25 to 50 parts max. I guess the only question i still have as far as parting off is the constant sfm.. should this be on or off for parting off? or does it matter? the last thing that is still fuzzy is the work offset format. Currently it is set to use g50. The manual is confusing as to the application of the code and how to set the offset. I am assuming you would still face the part with tool #1 and set z0 there. I am also unfamiliar with how this affects the use of the tool setter if at all. I am going to load a program tomorrow and single block it to see how it looks. sorry for all the questions (i know they are basic) but i would rather ask then crash the lathe. there are only 2 of us in the shop and nether one of us has ever programed a lathe before. so i am kinda flying solo on this. I need all the help i can get . Hennessy

I keep constant sfm on, G50 is spindle speed clamp, here is how that works. I specify that I want contanst sfm to be 300 sfm, but I use G50 S3000 to tell the control that I don't want the spindle speed to exceed 3000 rpm, this is useful when you are swinging larger parts and want to clamp the speed for safety reasons. G50 also keeps the speed from going to max rpm when the tool approaches the center line of the part, such as during facing and parting off operations. The following is a program that I have run many times, just use the G28 for all tool changes, until you become familiar with how the lathe is gonna react. Almost all of you lathe programs will be done using G54 as the work offset, just like in a mill. Keep it in mind that lathes are is feed per revolution of fpr, not inches per minute.

%
O00500
(CLR0006 REVA FASTER VERSION)
(1.2" FROM CHUCK FACE) (NOTES FOR SETUP)
T808(STOP BLOCK) (THIS MOVES THE STOP BLOCK OUT OF THE WAY PRIOR TO A TOOL CHANGE)
G00 Z1. (RAPIDS AWAY ON THE Z AXIS)
X1. (RAPIDS AWAY ON THE X AXIS)
G28 (SENDS MACHINE HOME FOR TOOL CHANGE)
(END FACE)
(55 DEG INS.)
T505
G54 (WORK OFFSET)
G50 S2500 (MAX SPINDLE SPEED ALLOWED)
G96 S300 M03 (CONSTANT SFM)
G00 X0.3625
G00 Z0.05
/ M08 (COOLANT ON, I USE BLOCK SKIP TO AVOID BATH WHEN VERIFING WITH DOOR OPEN)
G72 P101 Q102 U0 W0 D0.025 F0.002 (CANNED FACING CYCLE)
N101 G00 Z-0.05
G01 X-0.05
N102 G01 X-0.05 Z0.05
G00 X0.3125 Z0.
M09 (COOLANT OFF)
M01 (OPTION STOP, ALLOWS ME TO VERIFY PROGRAM ONE SECTION AT A TIME)


(OD TURN)
T505
G54
G50 S3000
G96 S300 M03
G00 X0.3875
G00 Z0.
M08
G71 P101 Q102 U0 W0 D0.02 F0.002
N101 G00 X0.11
G01 X0.11 Z-0.689
N102 G01 X0.3875
G00 X0.3875 Z0.
M09
M01


(OD TURN)
T505
G54
G50 S3000
G96 S300 M03
G00 X0.185
G00 Z0.
M08
G71 P101 Q102 U0 W0 D0.015 F0.002
N101 G00 X0.0505
G01 X0.06 Z-0.3
N102 G01 X0.185
G00 X0.185 Z0.
M09
M01
(OD CHAMFER)
T505
G54
G50 S3000
G96 S300 M03
G00 X0.16
G00 Z-0.2
M08
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 X1.
Z1.
G28
M01

(OD THREAD)
(PARTIAL PROFILE THREADING TOOL)
T606
G54
G97 S1000 M03
G00 X0.21
Z-0.165
G04 P1.
/ M08
M24
G76 X0.0805 Z-0.5725 K0.0347 I0. D0.01 F0.025
G00 X0.21 Z-0.165
M09
M01

(OD THREAD)
T606
G54
G97 S1000 M03
G00 X0.21
Z-0.165
G04 P1.
/ M08
M24
G76 X0.0805 Z-0.5725 K0.0347 I0. D0.01 F0.025
G00 X0.21 Z-0.165
M09
G28
M01


(PART OFF)
T707
G54
G50 S1500
G96 S300 M03
G00 X0.16
G00 Z0.05
/ M08
G00 X0.16 Z-0.584
G01 X-0.05 Z-0.584 F0.001
G00 X0.16
G00 X0.16 Z0.05
M09
G28
M05
M01
T808 (STOP BLOCK, A BLANK ALUMINUM BLOCK THAT I CAN PULL MY BAR TO)
G00 Z0.
X0.
M30
%

Please note that this was written for a Haas control, the codes should be the same but double check your manual. I don't have a tool setter so I can't give you any advise there, but you would touch the facing tool to the end of the stock and call that your zero point, if you removed .050 from the face then you would need to add that .050 to the length that you turn down if you are using the same tool for facing and turning, if a different tool is used you would set it to the new face, don't forget to set your x axis offsets, and then add the stock diameter or radius to it, most lathes are based on the centerline of the part being program zero. On my lathe if I set my x offset and its -10.000 and my stock is .750 in diam, then I would change my offset to -10.750. Be careful here, your control may want the radius instead so have a look at the manual. Run your program in the controls simulator prior to verify with the machine running. When verifying a new program turn your rapids all the way down, drop your feed rate overide way down, and run it with no stock in the chuck, keep finger on the feed hold button, and yes use single block. Hope this is of some help.

[Hennessy]

thanks that helps out a lot... I have a basic part programed (its a chess pawn) i just have to get some time to set it up. we just had several emergency's role into the shop so we are puting out fires rite now... i should be able to get to it next week... i will let u know how it goes....

thanks a lot

Hennessy

[JDenyer232]

Originally Posted by Hennessy thanks that helps out a lot... I have a basic part programed (its a chess pawn) i just have to get some time to set it up. we just had several emergency's role into the shop so we are puting out fires rite now... i should be able to get to it next week... i will let u know how it goes.... thanks a lot Hennessy

Glad to help, and yes do let us know how it turns out.

[g-codeguy]

Don't know if you have it set up to receive an email if you get an answer to a post, so I will mention here that I gave you some help on the Doosan/Daewoo forum.

[g-codeguy]

Hennessy: You will not be able to use G28 as shown by JDenyer on your Lynx. You need to add a U0 to send it home in X or a W0 to send it home in Z. Of course you can have both the U0 & W0 in the same block if the tool is in the clear.

JDenyer: Never used a Haas and kind of glad I haven't if you have to have a G01, G00, etc. in every block. These are modal on Fanuc controls. I noticed you programmed the starting position after the canned cycle on the first 2 canned cycles with T505. This would be unnecessary on a Fanuc as the tool returns to the starting position upon completion of the canned cycle. Same goes for when you have the same X value in consecutive blocks. Not needed on a Fanuc. G54 only needs to be called once on a Fanuc for the same reason unless you are using more than one workshift in the program.

Hennessy I think you should be glad you got the Daewoo instead of a Haas.

[Hennessy]

Originally Posted by g-codeguy Hennessy I think you should be glad you got the Daewoo instead of a Haas.

ha ha ... i am just glad to have a Fanuc control in the shop i do like the haas machines but they are a little light imho. Fadal is another animal tho...i don't know why you would ever want to change machine home... eye baling sheetmetal tabs to home the machine just seams like a bad idea

update: i have got every thing up and running... thanks for every ones help!!
i haven't gotten to cut any thing just yet tho just dry run some programs. i don't want to run parts until i can get the lathe serviced.... i ran a worm up program and the spindle got to hot to touch... its like something is to tight. the heat starts in the back and creeps up to the chuck and it gets HOT

Thanks

Hennessy

[Geof]

Have you tried letting it cool down and then running the warm up again? Many times the heat is caused because either oil has built up in the bearings, if they are oil lubricated, or grease has all drained to the bottom side. It is not that anything is tight you just have to run the spindle slowly until all the lubricant is evenly distributed or the excess has been purged out.

If the machine has not been run for a long time it may be necessary to run the warm up until things get hot many times. Each time it should take longer for the heat to build up.

[gthal]

Can somone help me with a simple code to Pgm. a 5/8 - 11 od thread in steel. maybe a G76 or G92 I have Fanuc OTC so I need the code. Thanks

[JDenyer232]

Originally Posted by gthal Can somone help me with a simple code to Pgm. a 5/8 - 11 od thread in steel. maybe a G76 or G92 I have Fanuc OTC so I need the code. Thanks

Well what is the thread length, here is an example of a G76 threading program with a thread length of 1", you will need to ajust this to match your thread length requirments. Also I asume this is OD threading, right hand. Here are both one block and 2 block examples. You may need to tweek these values to give optimum results depending on the material, setup rigidity etc. I usually use the one block format with alternating flank infeed, it gives a superior thread finish and even wear on the insert.

Diameter programming
Inch dimensions
Start point 5.00 pitches clear.
G00 X0.6250 Z0.4545 S1000 M03
Programming example using Plunge infeed.
G76 U0.1115 Z-1.0000 I0.0000 K0.0558 D18 A0 F0.0909

Programming example using Flank infeed.
G76 U0.1115 Z-1.0000 I0.0000 K0.0558 D18 A60 F0.0909 P1

Programming example using Alternating Flank infeed.
G76 U0.1115 Z-1.0000 I0.0000 K0.0558 D18 A60 F0.0909 P2

and here it is in 2 blocks

Diameter programming
Inch dimensions
Start point 5.00 pitches clear.
G00 X0.6250 Z0.4545 S1000 M03

Programming example using Plunge infeed.
G76 P1000 Q3 R3
G76 U0.1115 Z-1.0000 R0.0000 P0.0558 Q18 F 0.0909

Programming example using Flank infeed.
G76 P1060 Q3 R3
G76 U0.1115 Z-1.0000 R0.0000 P0.0558 Q18 F 0.0909

Hope this helps.