[maximusek]

Hi!!

Maybe some smart head is able to help me - I work at nakamura tw-10 - first operation face off then I have to engage c-axis (left turret) so I use M91. Next operation milling c0, c90,c180, c270, part is quite simple.
the proplem is after turning chuck is in "nobody knows" position, I write M91 and g0 c0 to rehome chuck but it takes time, sometimes after turning I see c axis in 450deg. I cannot wait 3-4 sec. until chuck will be back in 0. Maybe someone knows how M91 works, I need details or some way to fix the problem and make it shorter.
Thank You Guys

[slavetothemetal]

Is there a setting in your control for the rewind of your C axis? What is the code to send your C axis to machine zero? G28 maybe?

[maximusek]

G28 allows me to rehome turret G28U0V0W0, I was using G0C0.0 to rehome c axis, maybe G28 that is the solution; first question - I have no idea whatsoever, I guess You are talking about parameters, but I'm not "so deep"; I think M91 - c-axis engage should rotate chuck to machine zero...anyway I'll try G28 maybe that is going to be faster, thanks Slavetothemetal...

[dcoupar]

Try this:

(engage c)
G0 G28 H0
G50 C0
(cut)
(cut)
(cut)

[g-codeguy]

Try this:

(engage c)
G0 G28 H0
G50 C0
(cut)
(cut)
(cut)

Didn't work for me. Main spindle turned instead of live tool.

I also would like to minimize the dwell time when the live tool is initiated. Best I could tell with a stop watch is the M91 is taking slightly less than 5 seconds. A 4 second cut in cycle time adds up when you have been running the same job for over 3 years.

[maximusek]

Didn't work for me. Main spindle turned instead of live tool.I also would like to minimize the dwell time when the live tool is initiated. Best I could tell with a stop watch is the M91 is taking slightly less than 5 seconds. A 4 second cut in cycle time adds up when you have been running the same job for over 3 years.

- that is the idea to turn the main spindle to correct angle and do it in short period of time; live tool works when U use M89 - just want to remain I would like to talk about TW-10 Nakamura - that is the main subject

[g-codeguy]

- that is the idea to turn the main spindle to correct angle and do it in short period of time; live tool works when U use M89 - just want to remain I would like to talk about TW-10 Nakamura - that is the main subject

I am talking about the TW-10. Well, TW-20 in my case. You only want the spindle to turn enough to reach the programmed C-code. What happened for me was the main spindle ran at the RPM programmed for the live tool. And then the tool tried to move in the Z-minus direction into the part per the program. Not good for the tool, don't cha know.

My program is

M91
G50 C0

and runs fine, except for sitting there doing nothing for almost 5 seconds. This is the exact same thing as your original post.

I tried the solution 'dcoupar' offered. Maybe you didn't read my comments closely enough. I am not trying to change the question, but find the EXACT SAME SOLUTION AS YOUR ARE.

[maximusek]

I am talking about the TW-10. Well, TW-20 in my case. You only want the spindle to turn enough to reach the programmed C-code. What happened for me was the main spindle ran at the RPM programmed for the live tool. And then the tool tried to move in the Z-minus direction into the part per the program. Not good for the tool, don't cha know.

My program is

M91
G50 C0

and runs fine, except for sitting there doing nothing for almost 5 seconds. This is the exact same thing as your original post.

I tried the solution 'dcoupar' offered. Maybe you didn't read my comments closely enough. I am not trying to change the question, but find the EXACT SAME SOLUTION AS YOUR ARE.

- I didn't want to be rude but that the problem is, tw-20 is a little bit different then tw-10, somebody else started talking about Mori NL, the point is I'm trying to get some answer and wait for details, I don't need to develop the subject from tw-10 to milling/turning centers If You know what I mean; I do know You cannot compare cnc's and use the same solutions for all of them, mine is quite old, I last much time to figure out connection between Y-axis knock, spindle break and c-axis, program was getting crazy so I wrote the post to get some info; dcoupar wrote M91 calls macro, I use this code for left and right turret and effect is the same in my machine nothing happens, maybe U can put hole block of the program, I belive not M91 is the problem but something before or after, use single block and try to find critical line. Sorry If I was being rude, but that problem absorbed me so much and really needs to know how to fix it... :cheers: 4 Ya g-codeguy

[maximusek]

Try this:

(engage c)
G0 G28 H0
G50 C0
(cut)
(cut)
(cut)

I saw G50 somewhere but I don't know much about that code, I was using G50 with G96 but I know G50 can be a big problem because of the offsets, if U know some good website with description written using language for normal people without PCHD, please send me a link, for this moment I don't want to use Gcode I'm not 100% sure how it works, thank You 4 your post dcoupar :cheers:

[slavetothemetal]

Is there a setting for direction? On our Mori NL, I say M45(C axis engage) then G0G28H0. Is M91 your command for C axis engage?

[dcoupar]

M91 is probably calling a macro or a sub-program. Check parameters 6071 through 6089 and see if there's a 91 in any of them. We might be able to adjust the macro to improve the performance.

[dcoupar]

Maxi,

Have you ever tried G28 H0 instead of G28 C0?

[maximusek]

Maxi,

Have you ever tried G28 H0 instead of G28 C0?

I use G28 to rehome turrets and I know G28 goes with U V W H, doesn't use X Y Z C, to get corret angled position I use G0 C0.0

[maximusek]

Huge Thanks for dcoupar, g-codeguy, Sump Cleaner for suggestions. In my Tw-10 I don't call any sub, everything is in main program, like below:

N4(MILLING)
G0G40G80G18G98
G54 (work offset)
M87(Spindle unlock)
M8
M91(C-axis engage)
G28 H0.0
G50 C0.0
M86(Spindle lock)
M471(Y-axis knock out)
T0404
(.625 DIA.EM)
S1650M89
(machining)

IT WORKS!!! :cheers: 4all - maximusek 10-4

[g-codeguy]

Huge Thanks for dcoupar, g-codeguy, Sump Cleaner for suggestions. In my Tw-10 I don't call any sub, everything is in main program, like below:

N4(MILLING)
G0G40G80G18G98
G54 (work offset)
M87(Spindle unlock)
M8
M91(C-axis engage)
G28 H0.0
G50 C0.0
M86(Spindle lock)
M471(Y-axis knock out)
T0404
(.625 DIA.EM)
S1650M89
(machining)

IT WORKS!!! :cheers: 4all - maximusek 10-4

Glad it works for you. Only dif between your & my program is the G28H0. I added it, but it didn't work for me. Still losing almost 5 sec. I'm not even using the spindle lock function. We don't have Y-axis either.

Guess I am SOL on reducing my cycle time. Too bad as this job has been running for about 3-1/2 years. If I did the math correctly, a 4 second cut in cycle time would amount to making an extra 4685 parts per year at 85% efficiency for the number of hours we work per week.

[maximusek]

Glad it works for you. Only dif between your & my program is the G28H0. I added it, but it didn't work for me. Still losing almost 5 sec. I'm not even using the spindle lock function. We don't have Y-axis either.

Guess I am SOL on reducing my cycle time. Too bad as this job has been running for about 3-1/2 years. If I did the math correctly, a 4 second cut in cycle time would amount to making an extra 4685 parts per year at 85% efficiency for the number of hours we work per week.

- sorry to hear that; In my opinion only someone who has tw-20 is able to help U, that's why I was so crazy in looking for person with the same model of cnc, to many things are optional in those and a lot depend on who was setting up your machine; one more thing forget about Y-axis, it doesn't change anything, I just posted part of the program (I didn't have time, It was busy day and my boss is not very happy seeing me to long in web), before I had:
M91;
G0 C0.0;
and that was causing delay, I changed G0 to G28 H0.0 and added G50 C0.0. That would be all, Good luck g-codeguy...

[Sump Cleaner]

Naki Guys,

Try this...

Instead of issuing the M91 to change from main spindle to live tooling, try M98P9000. This is a sub that engages the C axis, homes it out (in about 1 second), and engages the live tooling unit. Then use the M41 to disengage after you are done. I don't ever use the M91 command because of the same problem. The only time I have the 5 second engagement now is when the M98P9000 is issued when it the C axis is all ready engauged.

P.S. - mine are TW-10's

JK

[g-codeguy]

I had considered trying the M98P9000 subprogram, but since it contained an M91, I figured it wouldn't be any faster. Might even be slower. However, I am willing to give it a try Monday. Thanks.

[maximusek]

Naki Guys,

Try this...

Instead of issuing the M91 to change from main spindle to live tooling, try M98P9000. This is a sub that engages the C axis, homes it out (in about 1 second), and engages the live tooling unit. Then use the M41 to disengage after you are done. I don't ever use the M91 command because of the same problem. The only time I have the 5 second engagement now is when the M98P9000 is issued when it the C axis is all ready engauged.

P.S. - mine are TW-10's

JK

- Is it a standard sub implemented in every machine?? for me it seems first I have to save it on HDD and then I can call it, same like bar change subprogram...can You write here all , I would like to see into it, Thank You very much for answer...

PS. we don't fight, it's only argumenting, that way we teach each other

[Sump Cleaner]

Hey Guys,

Here is a copy of the sub...

%
:9000(C-AXIS ENGAGE)
M91
M27
G28H-3.M28
G50C0
M99
%

I'm not sure if this sub is standard on all Naki's with C axis. These two TW-10's came straight from Elliott brand new in the mid 90's and the subs were in there. (both machines, both left and right sides)

The only other thing I can offer is the double engagement. The only time I get this condition (where the c axis goes around about 400° slowly before it homes out) is when the call is issued and the C axis is allready engauged. Also, if the axis is disengauged and then reengauged without doing some turning in between it can give a slow result.

Keep me posted guys.

Thanks

JK