I'm in Okuma Hell....

[jmjftw]

I just started at a new job and I get the Okuma vertical with a 5020M control.

 

WTF....No home position? No G54 fixture offsets

 

What's up with the H numbers? Is the G15 H* used for the fixture offset and the other H value used for tool lengths? It feels like it wants to be programed incrementally or in pieces with a fixture offset for each tool.

 

What's up with the gage length? How do you set Z zero, with one of the tools?

 

I'm sweating bullets....

[Colin Gilchrist]

Okuma uses a different interpretation of Gcode from Fanuc. Personally I've always hated the way they setup their machines. That being said I have run and written posts for them. This will get you started:

 

Okuma uses G15 H## for its work offsets,

G56 H## for its tool length offsets,

and G41/42 D## for its diameter cutter comp.

 

The Machine Home command is G30 X,Y,Z, BUT!! Z 0.0 is with the gage line of the spindle 4.0" (or something like that) off of the machine table.

 

 

When you send the spindle to machine home it plunges toward the table in Z. Most programmers that I know use a retract of G30 Z30.0 (or something like that). BE CAREFUL!!

 

As far as setting offsets are concerned, I'm familiar with the older style of machine control. You will want to get some help from the Okuma guru's in here. The way we used to do it was to jog the machine to the Z offset location, go to the machine coordinates display page, write the number down and then enter it in the tool offsets page.

 

Are you programming for this machine or just running it?

 

HTH,

 

Colin Gilchrist

The Boeing Company

MR2 and Beta test site

[Colin Gilchrist]

If you are programming for the machine you will need to add some special codes in the psof post block to have the machine check and see if the first tool in the program is already in the spindle. If it is and you don't have:

 

IF [VATOL EQ Txx]NATO1

 

you will get an alarm.

 

HTH

[Jack Neelands™]

Evening jmjft

You will find that G15 H* addresses the work offset...H is the number of offsets you can use up to how many the machine can hold

 

G56 H* is used for the length offset

where as the H is for the tool number for up to how many the machine can hold in its parameters

 

If you have a base tool ie a wiggler in the the machine ...define that as number one tool and set that to zero in the tool offset ....look for a tool in the height offset directory first to find out if one is allready there

[Jack Neelands™]

beat me to it Colin

+1000

[Jack Neelands™]

anyways to to find these tool directories and height directories they are to the left of the soft MacMan button

...the first to the left is the tool heights

the second is the work locations

[Jack Neelands™]

under the screen once you have chosen the either work location or tool height you have soft buttons as well that let you calibrate the tools and offsets by pressing calculate

[Jack Neelands™]

you must hit the enter button once you push the calculate softe key

sorry bout that ...tis one of those reflex things

[Keith @ Solid Code Solutions]

I will put a nice little parameteric utility for doing Okuma fixture offsets on Monday.

 

I always set any unused tools to 20" to ensure safety if you are to call a tool with no offset, Z is just going up.

[elbro]

A couple things about Okuma's. They don't forget where they are even if you shut the off, unplug them move the ball screw by hand. The machine still nows where it is. When you turn the machine on you will never have to home it. You can not send it in to an over travel, the machine will just stop when it get to the limit, no alarm it just stops. So i have always just sent the Z to Z50. at the end of the program. I have never sent it to a home postion. there was never a need.

 

Okuma is a very nice machine. Things will start making sence just give it alittle time.

[Keith @ Solid Code Solutions]

quote:

---

Okuma is a very nice machine. Things will start making sence just give it alittle time.

---

+1000

[david]

G30 P1 will send spindle to tool change position.

 

Our warm up programs for 5020 and U100 controls include going to preset positions for G30 P7 and G30 P8. I dont remember off the top of my head where you go to calibrate these positions.

 

Set your zero set page for z with reference tool, "calibrate" the other tools on tool data page.

 

I can understand your confusion, until about 2 years ago we had all okuma's then miltronics showed up. Now we have a new mazak set up and ready to learn how it wworks.

 

 

Good Luck

David

[jeff]

quote:

---

You can not send it in to an over travel, the machine will just stop when it get to the limit, no alarm it just stops.

---

Only in rapid mode will you NOT get an alarm.

If in G01,2 or 3 you WILL get an overtravel alarm.

HTH

[chris m]

Okumas ROCK!

 

Any specific questions email me and I'll do my best to help you out

 

C