[trampus]

I am having trouble activating g41 on this new machine. There is a rough pass but it's not the same as I need for the finish pass on a casting. I am wondering what am I missing? Thank you for looking.-----
NAT11(FBORE 3/4 CICRLE.015R)
G97 S500 M03 M08
G0 Z3.5 T111111
X2.263
G94
G85 NLAP1 D0 F20.0 U0 W0
NLAP1 G81
G01 G95 Z1.336 F.1
G41 X2.163 Z1.226 F.05
G94 X2.0475 A30 L.005 F1.50
Z.676
G95 X1.3129 F.1
Z.245 F.05
G94 X1.2435 A30 F1.50(*)
Z-.0445
G95 X.960 L.010 F.003
Z-.0695
X.940 F.02 M09
G0 Z3.5
G40
G80
M09
G0 X30 Z30
M05(* VARIABLES)
M30

------------------------------
Also for a really stupid question, (I have brain freeze) How to use or where to place a G90 or G91. Do I need one of these for the use of a G41?

.....:tired:

[littlerob]

I'm going to let someone else address this, since my last few posts have been a little off. (nuts) But one thing I can tell you is that Absolute positioning (G90) and Incremental positionaing (G91) shouldn't have much to do with cutter comp. (G41).

[Algirdas]

I will add a little.
1. G90 and G91 do work untill re-called. Maybe even after reset sometimes. I do always use fragment of part program starting by G91 and closed by G90 to be sure. Fragment is easy readable then and less risk.
2. cutter radius compensation. Easy. First of all, you can change to G42 and see, what happens.
next. You can check the part program in animation in step mode. You will see a movement very clearly, when compensation starts.
third. Rule. Make your shape without LAP first. LAP will work with compensation, defined in program without LAP. Adding LAP, you need to evaluate tool tip retract on each cut. And that's it.
3. Program looks as created by IGF. Is it? go to set IGF parameters properly. It's powerfull tool, it must be adjusted properly first.
one additional question. If M08 works, when defined in the same line with M03?

[trampus]

Thanks for the input. I did put this program together from one that was done on a computer from the "setup tech" who showed me how to use the mahcine. I have been using fanuc for years.(A big change I'll say) With all the options this has, including graghics, I am pushed to make parts. It would be nice to have a "okuma guy" back in our shop and play with it.I did manage to get tnrc working, a couple of costly oops runed my day. But I'll remember what NOT to do. now on snippets you talked about. Do you work on okuma's?
Thanks.

[littlerob]

now on snippets you talked about. Do you work on okuma's?
Thanks.

Uhm no, I'm a professional furniture salesman. :bs:

And AL is a Mime artist (chair) rofl

I couldn't resist, the door opened and I was standing there. Sorry Al.

[Superman]

Uhm no, I'm a professional furniture salesman. :bs:
And AL is a Mime artist (chair) rofl
I couldn't resist, the door opened and I was standing there. Sorry Al.

Saw the 1st one coming,--new kid on the block,,,,, but not the 2nd :cheers:

[budgieW]

LittleROB that is GOLD

[kawarta]

do you have a kind of scketch? on okuma control u can use G97 S1000M03 M8 M42 with out problems, I am attaching one programe made with ADMAC or IGF

[littlerob]

Trampus, sorry about the distraction had a little fun. What exactly is the problem? You say "activating G41", but what is happening? Are the linear or arc dimensions off? Does it alarm "unusable gcode", or "data word calc"? Does it accept the canned cycle at all?

Robert

[Algirdas]

Thanks, littlerob, for nice jokes
Trampus, You don't need to waste money on training. Here we are to help You. Check, if Your lathe has IGF. IGF is dialog for part programming. You do step by step (IGF one touch I would recommend) and You will be satisfied with a result. Okuma OSP is much more powerfull than Fanuc and much easier.
Do You have IGF manuals?
The problem with G41 can be in many places at this case - tool tip radius compensation set, for instance. It's easy to diagnose where the fault is.

[OkumaWiz]

I'm not sure what you mean by having "trouble" - could you be more specific?

I think that based on your program, tnrc is activating. You need to remove the G0 Z3.5 just before your G40.

Also check to make sure you have the correct values in your nose comp registers and the "P" values to make sure they are correct in TOOL DATA.

Best regards,

[Algirdas Basher]

?

[OkumaWiz]

Love the screen name "Algirdas Basher" :banana:

[trampus]

Thanks for all your help. There is no IGF in the machine. The owner didn't want to buy it.What I mean by trouble with the g41 is this. I do alot of detail work on our parts. Like a radius at the break outs on any given angle, alot of groove breaks, etc. I am sure you all know the routine. But as a ex-fanuc user I got spoiled. I usually do rad. comp on a cad system g02 g03. Fanuc is very user friendly on the fly though. I have user frustration and just plain not enough time to "learn by playing". My favorite thing to do is "well lets see if we can do this, or that. No matter just having FUN. I did mess around with changing quadrants etc. I really do know better than to do this while working...oops. Again thanks all. I really do appreciate the program examples also.

[trampus]

"P" values A ok. 3 for od and 2 for id. The reason to delete "You need to remove the G0 Z3.5" is a rule?
I will post a picture tomorrow night to show my problem areas.

Thanks you.

[littlerob]

But as a ex-fanuc user I got spoiled.

That's not spoiled bro. thats hammered. Okuma is job shop equipment, IGF or not. If you give it the time you will love it.

[trampus]

"P" values A ok. 3 for od and 2 for id. The reason to delete "You need to remove the G0 Z3.5" is a rule?
I will post a picture tomorrow night to show my problem areas.

Thanks you.

I have #1 as an eyeball test of the g41 working or not ! should have a radius on the corner of the bore of .010. #2 the breakout on the 30 deg. angle were too deep by about .010 or so. This is an idea of what I am trying to do. G41 just makes such perfect parts.
Thanks for the helping hand.

[IMG]D:\My Docs\Text files\Okuma\623014.jpg[/IMG] this is just not working well.
I'll figure it out.night.Been a long day.

[OkumaWiz]

P values look good. The reason to remove G0 Z3.5 is that it is automatically done by the LAP cycle and could cause problems if it goes outside the reference point.

Okuma rapids to a "reference point" and begins all of it's LAP calculations from this point. Depending on the start point, end point in shape definition, it determines how to retract off material when pulling away and it determines what direction to do the depth of cut.

What you MUST do in order for it to work correctly = on normal OD cutting, all shape definition points should be left and down from reference point (x minus z minus from reference) on normal ID cutting all shape definition points should be left and up (x plus z minus). Points "outside" of the reference point can cause such things as pulling into the part instead of away and calculating comps wrong or other funky moves.

If your start point is equal to your reference point in Z, the control will rapid down in X on the next pass. If it is minus from the Z reference, it will feed down in X for the next pass.

I agree with littlerob, once you get used to the Okuma, you'll realize what spoiled is. Try using G75 (auto chamfer) and G76 (auto radius ) with L value for radius size an you'll like it even better. A commands are helpful too to make angles.

If you want to fake out nose comp, you can use imaginary next vectors to get it to do most anything you want regardless of actual next move. Use I and K with sign on your G40 lines to fake it out.

Hope these tips help you.

Best regards,

[Algirdas]

once again. It's evident, you not used my advice. It will be usefull information after that kind a test:
1. Make Your part program without LAP. One pass shape only.
2. Lock the machine. Animation only, no machanical movement.
3. one block (step) mode on
4. Go step-by-step until problematic block (untill error message)
5. Magnify the area where tool tip is - on animation. You need to see approx 20mm on scale as (40 ... 60) mm on screen
6. reset, start the program again and see tool tip movements.
check remaining distances on problematic block.
It will indicate, where tool tip is commanded to go next. It givs much more information regarding thr trouble and wil take just about 10 minutes to do.
6.

[trampus]

once again. It's evident, you not used my advice. It will be usefull information after that kind a test:
1. Make Your part program without LAP. One pass shape only.
2. Lock the machine. Animation only, no machanical movement.
3. one block (step) mode on
4. Go step-by-step until problematic block (untill error message)
5. Magnify the area where tool tip is - on animation. You need to see approx 20mm on scale as (40 ... 60) mm on screen
6. reset, start the program again and see tool tip movements.
check remaining distances on problematic block.
It will indicate, where tool tip is commanded to go next. It givs much more information regarding thr trouble and wil take just about 10 minutes to do.
6.

I will use the graghics when I have the time to experiment, and not worrying about rate for the day. Yep, I work in an aerospace job shop. Time i$ money to these guys. But I do play when I get a chance.