G98~G99 Okuma OSP-P200 Control

We just got our Hardinge GX1000 with an Okuma OSP-P200 control up and running the other day and I've done a couple jobs already without a problem. Today I was drilling some holes in the bottom a of a c'bore and I came across a problem. My Z zero was the top of the part and my Z starting point is Z-1.000 and then I drill a hole 7/8 deep. I use GibbsCam to program, all my other machines will output a G98 or G99 when I'm below the the Z zero plane. What does the Okuma use in this situation? I looked in the manual but didn't find much info on this, it was towards the end of the day so I didn't have much time. Does Okuma use a different G-code for this type of application? I did see something about a G71 but didn't have enough time to read up on it. One more question, I was using a G73 drill peck cycle and I was wondering if there was a parameter setting somewhere to tell the machine to stop a specific distance when the tool rapids back down into the hole? I broke a couple small drills today and was wondering if the tool was stopping on the rapid before it hit the bottom of the hole.

Okuma doesn't use g99 and g98 for return to rapid plane or clearance plane. I don't remember the format off hand, but it is in the manual. I usually set that in my cam software and it will post a separate canned cycle for each hole.

How do you like the new machine so far?

This one thing that Okuma tried to "improve" that leaves me scratching my head.

To do a G98 on Okuma, you need to use this format:


T1 M6 (or G111 if you use a tool change macro)
G0 X0 Y0 M8
G56 H1 Z1.0 M3 S5000
G71 Z1.0 (SETS THE CLEARANCE PLANE AT 1.0)
G81 Z-1.0 R.1 F30 M53 (M53 IS THE SAME AS G98)
G0

Basically, you use G71 to set the clearance plane, and M53 to tell it you want to return to the clearance plane. I can't recall if M53 is modal, I think it is. M52 should turn it off. The other weird thing is that the G71 is modal. So if you called another canned cycle later in the program and used the M53, the control would return to whatever value was last set for G71. This can get you in trouble!

Notice that I used a G0 to cancel the canned cycle. G80 will turn off the spindle on Okumas. Man that's annoying.

It's a little tricky to get the post to spit out the G71 and M53. I wrote one for EdgeCAM to do it. I had to have some help.

I'm loving the new machine Ed! I'm getting familiar with the control but I have to admit Okuma is in their own little world....... I have the tech in today to install my probe, tool setter and my 4th axis, now it's going to get fun!

Thanks for the help ewlsey, at least I can look in the manual for it now that I know what to look for. I have a post that I'm using right now and making notes for them to change a bunch of things. I use GibbsCam and they have a great post department and will modify the post exactly how I want it. I hope they will be able to add the G71 and M53 without too much trouble.

ewlsey said:

Notice that I used a G0 to cancel the canned cycle. G80 will turn off the spindle on Okumas. Man that's annoying.

Click to expand...

Say What??? I've never seen that happen before on any Okuma... You need to ask your service/apps guy about that.

I've used a U10M, P100, and P200 control, and all turn of the spindle with a G80. G0 cancels the canned cycle but leaves the spindle running.

So does anyone know where the parameter setting is to set the distance to rapid to before feeding in the high speed peck drill cycle? That's going to be my first job in the morning, have to get this job going and I don't feel like starting my Monday breaking any more drills!

I don't know the number, but parameters are easy on the P200.

FYI, you can combine high speed and peck drilling cycles. I can't remember the code exactly, but you add another variable in the G83 cycle and it does a mini high speed drilling cycle between the pecks.

The only thing I don't think it can do is decreasing peck depth like Fanuc.

ewlsey said:

I don't know the number, but parameters are easy on the P200.

FYI, you can combine high speed and peck drilling cycles. I can't remember the code exactly, but you add another variable in the G83 cycle and it does a mini high speed drilling cycle between the pecks.

The only thing I don't think it can do is decreasing peck depth like Fanuc.

Click to expand...

Thanks for the tip ewlsey, I'll check the manual in the morning for the parameter settings.

All went well this morning, parameter settings were fine. Chose a different drill geometry and it cut a lot better. I found another weird and annoying problem today with the control, I even had the tech there today and he took a look at it and couldn't figure it out either. If someone could tell me what the hell is going on here that would be awesome!

When I'm running the machine the door interlock button will only automatically unlock at the end of the cycle every 4 cycles??? I've checked work counters and a bunch of parameter settings to no avail. So I have to push the door unlock button 3 times and then it will work on the 4th cycle. Anyone have a clue as to what this could be?

I personally hate the door lock/unlock button.

Mine locks and unlocks the door by itself in auto mode if the key switches are set to production and to the little picture of the control (not sure what the name is).

Edster said:

I personally hate the door lock/unlock button.

Mine locks and unlocks the door by itself in auto mode if the key switches are set to production and to the little picture of the control (not sure what the name is).

Click to expand...

It's a little annoying but I wouldn't mind if it worked properly...... It's strange though, I have it in Auto mode and the key set to Production but it will only auto unlock 25% of the time. I will be calling support tomorrow if I can't get it figured out.

What about the other key? The one near the lock/unlock button, it's got a picture of a control on one side and a picture of what looks like a wheel on the other.

Mine will only lock and unlock itself when running a program in auto mode with the key set to production, and the other key set to the pic of the control.

Edster said:

What about the other key? The one near the lock/unlock button, it's got a picture of a control on one side and a picture of what looks like a wheel on the other.

Mine will only lock and unlock itself when running a program in auto mode with the key set to production, and the other key set to the pic of the control.

Click to expand...

Yes I had that key set to control, that's for the remote hand jog. The machine locked up today with that "ATC Error" and could not be cleared. A tech was coming in today to install the probe (For the second time) so he worked on the machine to clear the alarm and it took him 6 hours to do it! And he still doesn't know what caused this....... He then spent the rest of the day trouble shooting the probe, turns out Okuma needs to update the software in the control so it's compatible with the Renishaw Probe. Not a good day, machine ran 30 minutes today and that's not making my boss very happy. They are close to telling them to pull the machine out of the shop, had it two weeks and it hasn't run for more than one day in a row without some type of error or repair person working on it for the entire day. Too bad, we are very busy and the company will not spend another penny with these guys at this rate. We have had issues with ALL 3 machines that were purchased. Took more than a week for them to get the bar feeder working with the Genos!

I feel your pain. The Okuma control should never have gotten in bed with windows.

On the the ATC alarm, check your tool life management. If the the tool lifes out, the control gives you a wonderfully descriptive error "wrong T command". It doesn't say "T1 tool life error" or "Check Tool Life". Okuma mill tool life management should take a lesson from their lathe control.

I've told this story before, but I worked in a shop that had an MB5000 horizontal. The control would just completely freeze up. The axes would be moving, but the screen was frozen. Replaced the motherboard and life was good. Then the thing wouldn't power up. We had to leave it on 24-7 in case it failed to power up in the morning. That time they replaced the entire control computer.

The wine rack tool changer also had a nasty habit of destroying itself if you tried to put a tool in a certain series of pockets. Of course there was no way to lock those pockets out.

What causes the dreaded ATC error for me is unlocking the door or resetting the machine while the magazine is moving the queued tool into position. It's hard to tell when the magazine is moving so it's easy to do. The easiest way to avoid the error is to not queue tools or make damn sure the magizine is finished before pressing buttons. Every time the ATC error occured for me it was operator error. Not saying this is the case for you but my guess is that it is.

It's not a big deal to resolve the ATC error either. First I try to one step the tool change either forward or backward. Usually that does it, and sometimes after I do that I have to powercycle the machine. One time I couldn't get it to do anything so I found the foward and reverse contactors for the magazine motor in the electrical panel. There is also a main contactor that powers the forward and reverse contactors, so the main contactor and either the forward or reverse contactor should be pushed in momentarily then the magazine will rotate. Make sure the tool pot is not down before you do this. Have someone watch the magazine so you know when it rotates. Rotate it one position one direction than back to where it was. The electrical diagrams have the contactors labeled so it's easy to figure out which ones need to be pushed in.

I should go on service calls for these machines. It only took me about an hour to figure this out and I don't even play a cnc tech on tv.

Sounds like your other issues are with the service guys not being familiar with the machine. Who is the dealer you bought the machine from?

I have caused the error my self twice already and I'm already familiar with clearing the error from within the ATC page and it was easy to clear both times. Had to power cycle both times but the alarm cleared without a problem. Today on the other hand I just loaded 3 tools and touched off my XYZ, I went to the computer and posted my program and threw it on my USB, when I returned to the machine not more than 5 minutes later I got the dreaded ATC error. I went to the ATC page and went back to step one like the tech told me to do and powered down, same error after it powered up. The tech spent almost all day trying to clear the alarm, so this was a fluke thing and I hate those the most. I want something to be broken so it can be fixed! I'm not ready to throw in the towel on the machine but the owners are very frustrated right now and rightfully so......

You wouldn't believe the service (Or lack of) that we have been receiving with all these problems. I don't want to go into too much detail. We bought the machines from Robert E Morris, been in business a long time, we've bought many machines from them in the past but that was about 10 years ago.

Just wondering if your issues have been resolved and how the machine is running.

Start with G1

For the ATC, I have learned to not touch any buttons when the ATC is in operation.
I start all of my programs with something like the following: THE VALUES ARE ADJUSTED.
G15 Hn
G71 Z.5 (IT IS THE STANDARD RETRACTION HEIGHT I USE TO CLEAR ANY HOLD DOWN SCREWS)
G53 (TURNS ON G71)
M6 Tn
G56 Hn
I AM OFF AND RUNNING

Now I have a question. I want to mount a small high speed drill (20,000rpm) to my machine through the CAT40 tooling.
How do I override the machine to allow me to use a G83 or G1 without the spindle turning?

graemeian said:

For the ATC, I have learned to not touch any buttons when the ATC is in operation.
I start all of my programs with something like the following: THE VALUES ARE ADJUSTED.
G15 Hn
G71 Z.5 (IT IS THE STANDARD RETRACTION HEIGHT I USE TO CLEAR ANY HOLD DOWN SCREWS)
G53 (TURNS ON G71)
M6 Tn
G56 Hn
I AM OFF AND RUNNING

Now I have a question. I want to mount a small high speed drill (20,000rpm) to my machine through the CAT40 tooling.
How do I override the machine to allow me to use a G83 or G1 without the spindle turning?

Click to expand...

I solved my moving without spindle rotation problem. There is a DNC button on the panel and a touch screen icon to turn off the condition.

Here is another question. Is there a way to turn off the ATC? My drill has water and electric lines and an accidental M6 could cause problems.

Thank you.