[fordav11]

yeah it will be. If I were on a Fanuc I would put txx00 at the end of each tool but on this machine I haven't done that and it seems to work fine running normally. The reason is so I can rapid the 2nd chuck to a Z-position and it will be relative to the previous tool to speed things up so the chuck is not needlessly rapiding in and out between tool changes.... the machine isn't the fastest thing I've seen

[budgieW]

"If I were on a Fanuc I would put txx00"
You should do this on your OKUMA as well

"the machine isn't the fastest thing I've seen"
As it has a 7000 control it is probably the best part of 15 years old

[OkumaWiz]

ah ok will try it.

Maybe you can help with another restart-related issue

Check the same program I posted before.
On restarting from the transfer (N110) the sub spindle goes into overtravel. It moves back about 2". Its not random, it does it every time when restarted from N110. When the program is run from start to finish it works fine. If I restart from any other place it works fine. I suspect it has something to do with the G00 Z50 lines from previous tools. Normally it would just go to maximum Z (which is the intention of that line) but on the transfer restart it seems to be trying to physically go to Z50 (max Z travel is about 20"-25"). Thus going into Z-overtravel :/
If this were a Fanuc I would use G28 etc but this doesn't seem to have a 'go home' command?

You may have a G30 command available on your machine for home positioning.

I think your main issue is that you are doing a restart with multiple axis movements which are "not in sync" when restarting. ALL axes will move at a rapid rate to their "restart point" (previous coordinate) after the sequence restart button is pressed. This may cause your coordinates and limits to shift for the Turrets as the W-axis repositions to it's restart point thus generating your alarm.

One solution is to make your transfer cycle into a sub program and design it fro the get go with valid restart points in it. We use NPASS line numbers on both turrets with G140/G141 commands on those lines. That way we can number search to the lines (jumps directly there with no waiting) Interlock + cycle start and do a transfer. We use block delete to ignore the call statements for the transfer sub, so we can run parts and stop before transfering and make any needed adjustments. Then transfer if needed by "jumping" to NPASS. We also have OP stops at the beginning of the transfer cycle to make a "check stop" possible without having to do the restart.


Code , code, code, is key!

Best regards,

[fordav11]

[QUOTE=budgieW;994802]"If I were on a Fanuc I would put txx00"
You should do this on your OKUMA as well/QUOTE]

I tried this today and it doesn't work as expected.
For example if there is a boring bar extended 8 inches and I stop it at Z2.0 at the end of the process then put T0100, on reading it the turret moves 8 inches minus! It cancels the offset and puts the turret in a position as if there is no tool length.
That's a potential crash situation. I recall now that's why I don't cancel the offset at the end of each tool. I don't know if that's correct Okuma behavior or if it's just another Okuma controller software bug... errr... I mean 'a special Okuma feature' ;-)

[OkumaWiz]

That is normal behavior on your Okuma. That's also why I typically never cancel it. It will also make your graphics suddenly "jump" by the amount of the offset. You are OK if you account for that and re-command your X & Z positions in a rapid move as you cancel the offset. Sometimes you need to do this in order to position the turret to a specific spot regardless of tool offset, such as during a Main-Sub part transfer. If there is no offset, the turret will always go to a predictable spot.

In your case, it is trying to maintain your X & Z positions, so canceling out the offset makes the turret try to maintain the same positions thereby moving the length of the tool in the "non-preferred" direction. Easy oops is correct!

;-)

Makes sense once you have the logic explained.

Best regards,

PS> Now why would they want RESET to cancel the offset??? Never have figured out that one!

[fordav11]

PS> Now why would they want RESET to cancel the offset??? Never have figured out that one!

They? If you mean Fanuc, reset is typically used in MDI to cancel geometry offset after doing a manual operation.
For example I might have a boring bar in the machine already set and I want to bore the jaws with it for the next job.
I go to MDI type G0 T0101; [INPUT] then press start. The XZ changes to proper values for this tool. I can then switch to manual and bore out the jaws using actual tool coordinates and I can also go to POS and zero the numbers in incremental mode (usually in Z/W) to make it easier to know how deep to go. (the same actual tool position can be had on Mazaks simply by indexing the tool in manual, which is even easier)
Its a real pity Okuma has none of this. I have wished to at least zero out the POS display a million times. Fanuc had this basic function in 1978 on the 3000C, and possibly earlier than that. This Okuma machine was built in 1994-95. On this Okuma POS stands for something else with a completely different meaning
It's pretty funny really. 1st thing I asked the Okuma installer guys was can the position be zeroed in manual mode. Answer: no.
2nd thing I asked, where are the wear offsets? Answer: none, you have to change the geometry plus/minus an amount to adjust wear.
My reply... LOL! Fanuc had this in 1978.

[budgieW]

Change your code

G00 x50 z50 T0100

[Algirdas]

1st thing I asked the Okuma installer guys was can the position be zeroed in manual mode. Answer: no.
It is "MID auto manual" mode on Okuma and works very well. You can use a "zero offset" tool also.
where are the wear offsets
many ways to apply the wear offsets, Okuma provides separately

[fordav11]

1st thing I asked the Okuma installer guys was can the position be zeroed in manual mode. Answer: no.
It is "MID auto manual" mode on Okuma and works very well. You can use a "zero offset" tool also.

huh? Mid Auto Manual is used to stop the machine in the middle of the cycle to check something or move tool away from part to change insert. etc. The actual position can not be changed. I prefer not not create a crash situation by messing with the zero offset, especially if the machine is already set and running. My point was Fanuc have this by simply pressing one button on the relative position page, Okuma does not.

where are the wear offsets
many ways to apply the wear offsets, Okuma provides separately

not on this machine. Okuma told me directly there are no wear offsets on this control.

[Algirdas]

move tool away from part to change insert. etc.
"etc" is exactly what I told about: You can control the tool path by pulse handle or arrow push buttons, and have work coordinate displayed regarding selected tool offset.
The actual position can not be changed
something wrong with the machine in that case.
especially if the machine is already set and running.
Sure, no need to play with offsets at this stage.
Fanuc have this by simply pressing one button on the relative position page, Okuma does not
there are many more controls and solutions with different approach. Okuma still uses OSP floppy format. Does it makes Okuma worse than Fadal or Fanuc?

[fordav11]

move tool away from part to change insert. etc.
"etc" is exactly what I told about: You can control the tool path by pulse handle or arrow push buttons, and have work coordinate displayed regarding selected tool offset.

I'm talking about where there is no tool offset. just current display zeroed out.

there are many more controls and solutions with different approach. Okuma still uses OSP floppy format. Does it makes Okuma worse than Fadal or Fanuc?

there are quirks with every system. none of them are perfect.
let's not get into a Fanuc vs Okuma vs whatever discussion

[Algirdas]

I'm talking about where there is no tool offset. just current display zeroed out
sorry, I misunderstood. My comment was aimed to:
can the position be zeroed in manual mode
if You want to have 0,0 coordinates in desired location, You can use either zero shift (it works temporary only, until reset or mode change) or zero offset (remains permanently). There are no restrictions on manual mode. Just go to zero offset and calculate zero. It's more than one button push on OSP and it is right, because:
- Your zeroing is just a small piece of all coordinate system management on Okuma. It is good to know and understand that
- it is dangerous. It is good to achieve by deliberate action, not single push button, which could be accidental
- it is good to have zero offsets in one mode, one control window. This is done by Okuma
I like Okuma concept, that the function is accessible from single place only.