Sub spindle related questions. Primarily positioning.

plutoniumsalmon · Jun 20, 2017

Howdy.
I bough an Okuma LB3000 with a sub and esprit 2 years ago, and due to family issues and lack of appropriate jobs have not really ran the sub that much. My questions are as follows. How do I set the sub origin in relation to the part origin and how do I make a master tool for the sub. I think the second question I can answer as it lies in the second spindle setup but the first bothers me. How is it supposed to know where home is where I have to tell it to pick up in relation to that and so on. I will call gosiger and esprit tomorrow but thought you guys might have a few ideas as well.

Thank you

gregormarwick · Jun 20, 2017

I've never used an Okuma, but on fanuc I set all tools (main or sub facing) on the same origin (using the toolsetter) and use a different work offset for working on the sub.

HYPERTUNE · Jun 20, 2017

plutoniumsalmon said:
Howdy.
How do I set the sub origin in relation to the part origin and how do I make a master tool for the sub.
Thank you

Do you mean the C axis angle, or the position of the sub spindle in Z (A axis on my machine)?

litlerob1 · Jun 20, 2017

plutoniumsalmon said:
How do I set the sub origin in relation to the part origin
Thank you

In manual mode jog the sub out to where you want it, and press "CAL" then "ENTER"

R

plutoniumsalmon · Jun 20, 2017

HYPERTUNE said:
Do you mean the C axis angle, or the position of the sub spindle in Z (A axis on my machine)?

Hello.
Sub in Z.
Thank you

deadlykitten · Jun 20, 2017

plutoniumsalmon said:
how do I make a master tool for the sub

what is a master tool for the sub ?

...you may mirror Z axis

so to run on 2nd spindle programs for the 1st spindle

skywalker4 · Jun 20, 2017

hi,
i to have a lb3000, the cool thing about okuma is you treat the sub just like the main, as far as writing the program and setting up the master tool.
when you are ready to do a pick up, just run the sub down to the part and just touch the bottom of the jaws and as said earlier hit calculate, then back up till you are off the part and put that number in your program, as where to feed from. after you have the part and the main chuck is open just put in a g00 w100. and it will rapid home.

plutoniumsalmon · Jun 20, 2017

skywalker4 said:
hi,
i to have a lb3000, the cool thing about okuma is you treat the sub just like the main, as far as writing the program and setting up the master tool.
when you are ready to do a pick up, just run the sub down to the part and just touch the bottom of the jaws and as said earlier hit calculate, then back up till you are off the part and put that number in your program, as where to feed from. after you have the part and the main chuck is open just put in a g00 w100. and it will rapid home.

Thank you. I now have to figure out how to get Esprit to write it, but I guess I can just go in and edit whatever it puts out.

HYPERTUNE · Jun 20, 2017

plutoniumsalmon said:
Hello.
Sub in Z.
Thank you

In Esprit, set the pickup position to zero and on the machine set the work offset zero location for the sub spindle to the point where you want to clamp the part (for example, 20mm back from the face of the part) To be safe, add a clearance value in Esprit of say, 25mm or so to feed the last bit.

I usually machine the first op in the main, then use a magnetic tool length sensor on the front of the sub spindle jaws. Jog it up to the part, zero the "A" axis then take off the length of the sensor + the amount you want to grab it by.

Posts perfectly out of Esprit, no edits

Orange Vise · Jun 20, 2017

On our Mori NLX2500SY, I set the main chuck face to G54 Z0 and the sub chuck face to G55 Z0.

During part handoff, I'm in G54, so whatever I have in G55 is irrelevant. Mori designates the subspindle position as the B-axis. I set my G54 B-axis offset to where the chuck jaws would be touching at G54 B0. That way the B-axis uses the same Z coordinate values as the turret.

After part handoff/cutoff, the program resumes in G55 with B-axis in the home position.

plutoniumsalmon · Jun 20, 2017

HYPERTUNE said:
In Esprit, set the pickup position to zero and on the machine set the work offset zero location for the sub spindle to the point where you want to clamp the part (for example, 20mm back from the face of the part) To be safe, add a clearance value in Esprit of say, 25mm or so to feed the last bit.

I usually machine the first op in the main, then use a magnetic tool length sensor on the front of the sub spindle jaws. Jog it up to the part, zero the "A" axis then take off the length of the sensor + the amount you want to grab it by.

Posts perfectly out of Esprit, no edits

View attachment 201624

Perfect. Thank you.

Though one question. How do I set the tools to the sub in this scenario. Or am I overthinking it. IE Where does Esprit think part zero is for the sub and where should the machine think it is? Do I set them to the front of the jaws or to whatever value I had at move to pick up the part, for example in your case zero plus 20mm? Thank you.

HYPERTUNE · Jun 20, 2017

Standard in Esprit is to use G55 for the sub, so you would set G54 to the front face of the part, and G55 to the rear (which becomes the front when transferred to the sub). To set G55 in the machine, I just take the length of the part (say 50mm), minus the amount I'm going to hold it by (say 20mm) an set G55 that amount in front of the sub spindle jaws (30mm in this case).

After running the first part, you might want to fine tune the G55 setting in the machine to get the correct overall length, but I have always fount it to be within tolerance for my parts.

litlerob1 · Jun 20, 2017

Obviously you don't use G54/55, Esprit should kick out G140 for Main work and G141 for sub. Program as if the face of the part is Z zero just the same, OSP doesn't care, as long as it knows which spindle is running. Sorry for my Ignorance as far as Esprit goes (very limited)

R

Per post #11 if you are using a probe to touch off tools it doesn't matter the control calculates all that for you, if you are physically touching off tools using CAL will do the "CAL"culation for you, so yeah you are over thinking it.

deadlykitten · Jun 20, 2017

skywalker4 said:
just run the sub down to the part and just touch the bottom of the jaws

hy walker / skywalker

do you know G22 ? feed the axis until effort raises ?

G22 is there for parts transfer

please, what is a master tool ? kindly !

gregormarwick · Jun 21, 2017

deadlykitten said:
please, what is a master tool ? kindly !

Master tool is usually referred to as the tool used to set the work origins.

In some situations (like if there is no tool setter) the master tool will be set with a Z offset of zero, and all other tools will be set relative to the master tool.

skywalker4 · Jun 21, 2017

deadlykitten said:
hy walker / skywalker do you know G22 ? feed the axis until effort raises ?

G22 is there for parts transfer

please, what is a master tool ? kindly !

I dont use the torque function (G22) , I never really found it necessary.
although if i started, im sure i would find it handy. i dont get out on
the floor much anymore, im programming now. the lathe i ran just sits there.

deadlykitten · Jun 21, 2017

skywalker4 said:
I dont use the torque function (G22) , I never really found it necessary. although if i started, im sure i would find it handy

good to you

in other words, length tolerances were ok ...

G22 is there when length tolerances get lower + safe transfer of heavy parts + etc

skywalker4 said:
i dont get out on the floor much anymore, im programming now. the lathe i ran just sits there

if i may : be careful not to get fat ? sorry

skywalker4 · Jun 21, 2017

i may : be careful not to get fat ? sorry

It is to late, it has already started. lol

Chip Turner · Jun 27, 2017

Programming tips for you
G140 (MAIN SPINDLE)
G141 (sub spindle)

position setting help.
Manual mode, select spindle 1 or main spindle
move the W axis and touch off the end of the finished part and Cal zero (Teach) "W" zero in Work offset for the pick off position if you are going to transfer parts

Teaching the Zero offset for the sub spindle:
Manual mode
Select spindle 2 (sub)
index to master tool and Teach your Zero shift just like you would on the Main side.

Sub spindle related questions. Primarily positioning.

Hot Rolled

Diamond

Cast Iron

Diamond

Hot Rolled

Banned

skywalker4

Guest

Hot Rolled

Cast Iron

Titanium

Hot Rolled

Cast Iron

Diamond

Banned

Diamond

skywalker4

Guest

Banned

skywalker4

Guest

Plastic

Similar threads