Need Help!- lynx 200l lathe

[Hennessy]

Hi all, I am in need of some help getting this lathe up and running. It is a lynx 200l with a fanuc 21 I – t controller. I am a mill guy and I am not familiar with this control or running lathes. I have the basics form school but that was 5 years ago and I am kind of rusty.

The first problem I have run in to is setting work offsets. I get all the tools set (it has a tool setter) I face the end of the stock with tool 1, pull out in x and go to set the z offset but this is where I get stuck. The control has a tool measure button but when I highlight the cell for the offset and all I can do is manually enter my current machine z. is there a better way to do this?

My main concerns as far as programming goes are parting off and getting my tool changes far enough away form the chuck. Currently I have the post set to do the tool changes at the home position. As far as parting off goes I have no idea where to start. Any tips or pointers for things to do or to avoid will be appreciated.

Also we only have a few tools so some ideas on what we might want to buy first would also help. (see photos)

Thanks,

Hennessy

[Fanuc Pilot]

G'day mate,

Just in response to your Work setting (Z axis), Forget that tool measure button. Do the same as what you have been doing, eg face the job and move your X axis away. Then go into your work offsets, select what work setting you are using (G54 or G55 etc). Highlight the Z figure. Then type on the keypad, "Z" 0 (zero) and on the soft keys below the screen there will be a button that says (measure). Press this and it will automatically set your Work setting.
To double check to see if you have done this correctly, If you are setting G54, just make sure it is active by entering it in MDI. Then once you have set your G54 in your work offsets, you should be able to go to your position screen and "Z" should read 0.000 (zero).
You can also set the Work setting to what ever value you want. Just do the same as above, but instead of typing "Z 0 measure", type Z 1 or Z 2 etc then measure. Just make sure you check this on your position screen. This should read the same as what you just set your work offset to. If it doesnt, don't press cycle start because it may crash!

I hope this makes sence

Good Luck

[Hennessy]

thanks for the info... i have been getting some help from the general forums to http://www.cnczone.com/forums/showthread.php?t=73731... i think i have it. just need some time to test the program. i will let u know how it goes

thanks

Hennessy

[g-codeguy]

We have 3 Lynx with the 21i control. Not the L model, but I don't think that would make a difference.

I think the G54-G59 can be used on our lathes, but have never tried it. Better to use the G10P0Z/W function. I set the workshift at the beginning of my programs with the G10P0Z- function. If doing multiple parts on the same barstop, I move the workshift between parts using G10P0W. function.

You can't forget the hard Z tool measure button on our machines. You will not get the correct workshift if you do. Face, stop spindle or move up in X so tool doesn't continue to rub. Go to the Z on the right side. type in the geometry of the tool being used to face, press the hard tool measure button, and then press the soft measure button under the screen. The Z on the right side will now contain the tool geometry, and the Z on the left side will change to the needed workshift. You will be able to figure the constant to add to the cut-off position once you have set your first workshift.

I suggest using the Safe Index programs from the Hardinge manual. I use them on all but 2 of our Fanuc controlled machines. Once you have probed the tools, you add whatever clearance you want between the longest tool and the part, and modify the Z in the one subprogram. Now the turret will always index at that position until you modify that Z again. I can post the Safe Index subprograms tomorrow if you would like to use them. They are very simple to understand and easy to use.

I don't know what is concerning you about parting. Care to elaborate?

EDIT: No idea what your work will be, but you should be needing a bunch more boring bars of various sizes. Figure at least 2 of each size. One for roughing, and one for finishing unless all your jobs will be brass, aluminum, plastic, etc. type materials. Even then I prefer a separate finisher if very much is coming out of the bore. Otherwise you may have to stop the machine to remove chips wrapped around the bar before making the finish pass. Not what you want if barfeeding.

[Hennessy]

I would defiantly be interested in the safe index programs. If you can post them that would be grate!!


As far as parting off, the thing that concerns me is the constant ipr.. i don't want to fling the part and have it bounce all over the machine.. or over load the part off tool. I think i have this figured out but it leads me to my last problem. I know their is a code to limit the spindle rpm but in the manual i have g50 is listed as both work shift and rpm limit depending on the format you are in. Form what i can remember (i am at home rite now and don't have the book) it says with pramater #### set to # you use g50ip# for your work shift... if it is set the other way you use g54-g59 and then g50 is the rpm limit. I will bring the manuals home tomorrow and correct or clarify this.

I think I have been running a fadal for to long and my brain has rotted

Thanks,

Hennessy

[dcoupar]

G50 is used for RPM limit. G54 - G59 are Work Coordinates. Usually G54 Z is used for the main spindle and G55 Z is used for the sub spindle (if so equipped).

When parting off, you can use G96 down to within 1/8 or so of cutting through, the give it a G97 S1000 or whatever feels safe. You may need a dwell to make sure the spindle has slowed sufficently before the final cutoff move.

As for indexing, I've had good luck with programming a G30 U0 W0 (2nd zero) at the start and end of each tool. Find a good safe place to index and set those machine coordinates in the parameters for G30 X and Z. Here's a nice little macro that does the math for you and stores the values. Store this in the memory, move X and Z to where you want to index, and run the macro.

O9010(G30 AUTO SET)
#101=#5021*25400.
#102=#5022*25400.
G10L50
N1241P1R#101
N1241P2R#102
G11
M30

[g-codeguy]

Mr. Coupar is a good man. He wouldn't steer you wrong. I part off the same way. My G50 is always limited to S3000 or less depending on the size of the part. I never cut-off that last little bit at more than F.002 (depends on whether the part has a hole thru it or not) to keep from throwing the part too badly and to keep the pip small as possible. I do the same thing for facing. I may be rough facing at F.01/F.012, but at X.2 I slow down to F.004. Easier on the insert.

Here are the Hardinge Safe Index programs. I keep 2 of them in protected program numbers so the operators can't modify or accidentally delete them. The 999 program is the one where you modify the Z to the longest tool plus whatever clearance you want. I keep the X at whatever the geometry is on that machine for a drill. Mainly run small parts and this saves on travel time.

:9001 (SAFE START)
G0G40G97G99
M98P999
M99

:9002 (SAFE END)
G0G97Z.5
G40
M98P999
M99

:999 (SAFE INDEX)
T0
X5.62Z4.
M99

I take it a step further. I put 92 in parameter 6071 and 92 in parameter 6072. Then I call P9001 with M91 & P9002 with M92. Here is a sample operation. You will notice there isn't a G97 for the spindle speed or a G0 on the rapid approach. Not needed thanks to the Safe Index sub.

I was criticized for ending my programs this way. Said it was bad practice. Notice that the first move in the ending sub is G0Z.5. I have never had a crash in almost 24 years. Never will. Course if you type the wrong number in all bets are off! But then there is the possibility that you might forget to type in the G0Z.5. So....


N400M91 (BORE)
T0404S3500M63
X.888Z.5
Z.02
G1X.8Z-.024F.005
Z.03F.015
X.92
X.8929Z.01
Z0F.002
G2U-.048W-.01R.034
G1U-.0214W-.0107
G2U-.02W-.024R.034 (X.8035)
G1Z-.16F.008
U-.01
M92
M1

Notice that I am always swinging a radius on the chamfer corners to eliminate any burr.

I think this way is just as easy as using the G30 with less typing. However either way will work, and I thank Mr. Coupar for the example. I will have to give it a try on one of the machines that I don't use the safe index programs on.

Comment on using G54 vs G10. Our Lynx lathes use G10 while the Puma S200 and Puma 200MS lathes with 18-T controls use G54-G59. We run a lot of washers. Usually in multiples of 5. On the Lynx I set the workshift and use G10P0W. to increment the workshift for each part. For the G54-G59 lathes I specify in the program header what to set the G54-G58 to, and hope that the set-up guy doesn't forget to make the changes.