[julio_gyn]

my boss bought a doosan lathe wih fanuc 18t, live tools, c axis, subspindle.. i use to program milling machines, but now i have to program that lathe, i have done small works in a cnc lathe, but never used a subspindle, any help? manuals? links?

regards

julio

[olson]

program the sub spindle as you would normally program turning & use the wait (m codes) for that machine. catch up to the other spindle or for transfering to opposite.

[dcoupar]

What model is it? Here's a programming manual that may help. It covers most of the live-tool models.

[julio_gyn]

the machine is a Doosan S310SML

julio

[g-codeguy]

Was it a new lathe? If so there will be a programming manual with it that should tell you everything you will need to know to program it. I am not familiar with the Doosan S310SML, but we have three Daewoo 200MS lathes with C-axis and subspindles.

Most people use the face of the part as zero. On the main spindle you will be cutting in a minus direction. On the subspindle you will be cutting in the plus direction. Swinging a radius from the face to the O.D. on the main spindle is G3. On the subspindle it will be G2.

Think about it a second, and you will see that the direction of cut on the subspindle for cutting a radius from the face to the O.D. is the same as for cutting a radius from the face to the I.D. on the main spindle (G2).

Twin turret, twin spindle lathes are 2 lathes mounted back-to-back. With the face of the part Z0, you will be cutting in the minus direction with either turret. The G3 code would be for the same thing on both turrets.

Transferring a part from the main to the subspindle requires synchronizing the spindles if you are cutting off the part. This is an M203 on our machines. It will require an M-code to allow you to open the subspindle chuck/collet for ejecting an already machined part and going to pick up the new part. I'm not saying this correctly. M169 opens the subspindle jaws. First I have to program an M131 to allow the machine to 'work' with the jaws open.

A word of advice. Our lathes use an M114 to rotate the chuck/collet while giving it an air blast from the side via a copper tube. This is pretty much worthless. You will scrap many parts due to chip marks on the OD. I program a station to wash out the chips at S100. This works.

Now if your machine has a thru-the-spindle air blast, then it should work okay for clearing out the chips.

I will be glad to help you with anything I can. Machines may not be the same, but the methods used should be very close.

[julio_gyn]

is a used machine, year 2000, I am just picking every kind of information before the machine became available for programming (next week) on the main spindle I'm fine for simple programs, on the subspindle I have a doubt, is there an zero shift for the subspindle? do I have to call g54..g59?

regards,

julio

ps. thanks for all replies, it helped a lot...

[dcoupar]

On the newer machines, we use G54 when working on the main spindle, and G55 when working on the sub... might be the same on yours.

Does the machine have a Q-setter for settin the tool geometry offsets?

[g-codeguy]

Our machines are a little newer than yours. Workshifts are set like Mr. Coupar's except I use G54 for the front and G59 for the rear. Ours has a PITA type tooling. I.D holders have to be indicated in every time they are put back on. Or after a crash. I assume the reason we got the lathes at a good price was because they discontinued this method.

Because of the hole pattern in the turret for mounting tools, you can only use the odd numbered stations for the rear spindle. Can use on O.D. tool in an even station if the tool is extended way out. Live tools on the 200MS' can only be used on the even numbered stations. Not saying this will be how your lathe works. Never seen that model.

Don't think you will have much trouble learning to program the sub. Only problem you may have is getting the M-codes set up correctly for the transfer. If there is a manual with the machine, then there should be an example program on transferring the part.

Just remember that the G3/G2 codes will be opposite from how you use them on the main spindle.

[julio_gyn]

dcoupar, i did not see entirelly the machine, but I remember to see the probe arm beside the main spindle, and 1 part catcher'
g-codeguy, I have yet a job that requires both chucks, including milling a square and drill one side and a hole on the other side of the workpiece.

on the manual above i have some gcodes and samples of code, but, how can I have the machine working untill the bar is finished?

[g-codeguy]

On our Daewoos (we have a few others besides the 200MS') you use an M99 to keep the program running. Actually we use /M99. Block skip is off when you want the machine to stop after making one part. On if you want it to keep looping.

Edit: Don't forget the M30 after the /M99. LOL

[julio_gyn]

thanks for the answers, I will read carefully the manual above and wait until the machine is available for setup, then if I still in doubt (i hope not) I will back, thanks for your time again

[julio_gyn]

I started to set up my tools on the machine and I something was wrong, when i checked the turret is on the wrong position, the turret is on 12th and the control shows 11, where can i reset it to the right position?
One more question, we had a daewoo long long time ago, and when the probe was down the control was in the right screen to set the tool geometry, and soon as we touched the sensors the control changed the values, but this is not happening on the doosan, any idea??

thanks...

[dcoupar]

Check parameter #5005 bit 5 (QNI). This controls whether the offset number is automatically selected when the probe is activated.

[julio_gyn]

what value shoud be? one more question, how do i reset the turret to the correct tool? the turret is one position after the control (ie: machine 3 control 2)

[dcoupar]

I'm not sure how to set the tool number to match the turret number... sorry.

[julio_gyn]

no worries, I will keep looking, we have to solve the turret prob very soon... thanks

[g-codeguy]

I started to set up my tools on the machine and I something was wrong, when i checked the turret is on the wrong position, the turret is on 12th and the control shows 11, where can i reset it to the right position?
One more question, we had a daewoo long long time ago, and when the probe was down the control was in the right screen to set the tool geometry, and soon as we touched the sensors the control changed the values, but this is not happening on the doosan, any idea??

thanks...

I posted this on one of your other threads.

I am not a maintenance man, so I asked ours about your problem. If it is indexing to the wrong station when you use MDI, then what I gather is first you index the turret so that station on is up. There should be an encoder under a cover on the side of the turret. Turn the encoder until a red light comes on. This shouold fix it.

However, if it doesn't please don't take it out on the messenger!

[julio_gyn]

g-codeguy the problem with the turret is fixed, but I still with the same behavior with the probe, the machine is not setting the position of the tool when the light show on the probe.....

[olson]

try checking params 5015 thru 5019 for values at the xp,xm zp & zm positions when hit probe.
values are in microns

[julio_gyn]

what do I have to do with them?