Okuma Multus U question.

[crazy^millman]

I am doing some balance turning. I thought I was going along pretty good until now. I can get the machine to rough with Sync Codes no problem. When I get to the next tool call on the lower it alarms out with 2463 Change Timing G140/G141/G142 B Side 4. The PDF says Constant Peripheral Speed Control. I was getting an alarm if the Lower had a G97 so I commented that out and got rid of that alarm, but now I am getting this alarm and the G140 is being called in the tool change.

 

VBNCT=1

G140

VBNCT=0

RTMCR

 

I even put a G140 after my wait code to see if I could alarm it before the tool change and I can. I have tried M05 in a Wait Code sync and still getting the alarm. I am thinking I am going around the approved process to balance cut operations and why I am getting the error. I have attached the code if someone wants to take a look at it. Thanks in advance for any suggestions or help.

 

Sorry I had to remove the file.

Edited May 1, 2015 by 5th Axis Consulting

[crazy^millman]

Okay I figured it out. I had commented out the G97 out of the lower steam because the machine was alarming out as it rolled through both G97 together. Once I wait coded the process to do the G97 with the S command the same as the Upper to the Lower where the Upper goes through everything and is done then wait code through the lower and everything is done then I was able to get through it.

 

Everyday is a learning day. :laughing:

[Mick]

Is it something to do with constant surface speed being applied while the lower turret is being activated? It sounds like you're using both turrets on the main spindle?

 

Sorry, I can't be much help. We've ordered ours but it is going to be a long wait until we get it. (Can't wait though )

[Greg Williams]

Ron,

 

You need to tell the machine which turret is controlling the CSS with G110 (Upper) G111 (Lower)

 

G96 G111 S600

 

Then you need to cancel the CSS on that turret with G97

 

G97 S1500

 

Both turretts should be synced on the G110 line and the G97 line

 

G13
G140
G50 S2000
G00 X2000 Z2000
MT=0101
M321
TL=010101 BT=1 M603
P4 G96 G110 S200 M3 M185
G00 X300Z10
G01 Z-50 F0.5

 

CUTTING

 

P5 G97 S200
G00 X2000 Z2000 M05
P10
P20
 
G14
G140
G50 S2000
G00 X2000 Z2000
P10
T070707
P4 G96 G110 S200 M3 M185
G00 X300 Z10
G01 Z-50 F0.5

 

CUTTING

 

P5 G97 S200
G00 X2000 Z2000 M05

P10
P20
M30

 

If ewe use a LAP4 cycle you will not need any P codes, if you use longhand code or LAP3 there should be a P code om each line for the syncro cutting

[Mick]

I was kind of right. And I haven't actually worked with one of those yet...LOL

[crazy^millman]

Ron,

 

You need to tell the machine which turret is controlling the CSS with G110 (Upper) G111 (Lower)

 

G96 G111 S600

 

Then you need to cancel the CSS on that turret with G97

 

G97 S1500

 

Both turretts should be synced on the G110 line and the G97 line

 

G13

G140

G50 S2000

G00 X2000 Z2000

MT=0101

M321

TL=010101 BT=1 M603

P4 G96 G110 S200 M3 M185

G00 X300Z10

G01 Z-50 F0.5

 

CUTTING

 

P5 G97 S200

G00 X2000 Z2000 M05

P10

P20

 

G14

G140

G50 S2000

G00 X2000 Z2000

P10

T070707

P4 G96 G110 S200 M3 M185

G00 X300 Z10

G01 Z-50 F0.5

 

CUTTING

 

P5 G97 S200

G00 X2000 Z2000 M05

P10

P20

M30

 

If ewe use a LAP4 cycle you will not need any P codes, if you use longhand code or LAP3 there should be a P code om each line for the syncro cutting

 

Greg I was hoping you our Doug would chime in. At this point can not get my Sync codes to come out on every line, but hacked them in like I wanted. I am doing balance turning where I am machining on the OD and ID at the same time. I was looking for the Master and Slave process and that filled it in.

 

Have you done Lap 4 Cycles with OD and ID work? If so have any example code? Yes I know one of the 2 will have to suffer from the difference in SFM, but the idea of putting 2 tools to the part is the reduction reducing the cycle time on the part. 

[YoDoug®]

If you are looking for true balanced cutting (both turrets in cut at the same time for the entire Z length of cut) then LAP 4 cycles may not work. Unless you are running the exact tool path on upper and lower (both OD or both ID) you have no way to specify inside of the lap cycle calculation where to put the sync codes. If the part/process is stable enough to have one turret engage/disengage into cut while the other is in the middle of a cut then just put sync codes at the end of the approach move and at the beginning of the retract move.

 

BTW, Mr.M is our Multus U expert here. When I have a question I go to him. 

[crazy^millman]

If you are looking for true balanced cutting (both turrets in cut at the same time for the entire Z length of cut) then LAP 4 cycles may not work. Unless you are running the exact tool path on upper and lower (both OD or both ID) you have no way to specify inside of the lap cycle calculation where to put the sync codes. If the part/process is stable enough to have one turret engage/disengage into cut while the other is in the middle of a cut then just put sync codes at the end of the approach move and at the beginning of the retract move.

 

BTW, Mr.M is our Multus U expert here. When I have a question I go to him. 

 

Doug thanks. No I have different shapes and types of cuts why I did it the way I am doing it.

 

I forgot about Mr. M., but I have learned a lot about theses machines in the last 6 weeks. We have got the machine environment dialed in good at this point in MT. Sorry I can't share the work I am doing all Confidential, but making some good progress on the projects I am working on. 

[Greg Williams]

Ron,

 

Sorry I did not realise you were doing OD and ID, I thought you had both tools on the OD in which case LAP4 cycles with no P codes works fine. As you are doing OD and ID then Doug is correct you will need P codes but they do not need to be on each line but it will defiantly work better if you do. I always found it easier to use longhand code when cutting OD and ID

[Okumawiz]

Your problem is probably that you tried to change spindle modes with your G96 still active. You cannot change modes if G138, G96, Nose comp, Lap cycle, M110, etc. are active. They need to be cancelled before attempting to switch modes.

 

Best regards,

[Mr. M]

Nice picture

[crazy^millman]

Your problem is probably that you tried to change spindle modes with your G96 still active. You cannot change modes if G138, G96, Nose comp, Lap cycle, M110, etc. are active. They need to be cancelled before attempting to switch modes.

 

Best regards,

Thanks for the almost 10 month late answer, but we figured out and once we isolated upper control and upper control it was easy from that point.

[Mick]

Thanks for the almost 10 month late answer, but we figured out and once we isolated upper control and upper control it was easy from that point.

 

Heh, don't you just love old thread revivals?

 

Hey Ron, I'm headed to Charlotte in just under a months time to do some application work on a U3000. Looking forward to it

[Mr. M]

Going to travel through MN on your way, Mick?

[Mick]

Going to travel through MN on your way, Mick?

 

Unfortunately not

 

I'm doing a bunch of flying in a short amount of time though. NZ -> Houston -> Charlotte. 5 days in Charlotte, then on to Chicago for three days, then on to Irvine for three days, then to San Francisco then home.

 

Ugh...

[Watcher]

What a horrible job Mick.... Ugh...

[Mick]

What a horrible job Mick.... Ugh...

 

Yes, we all have to bear the good with the bad... LOL

 

The Okuma facility will be great. Great learning centre