G85 / finish cycle with radius compensation

[fomaz]

Hello.
Controller OSP U100L in a lathe.
I normally program my parts manually and therefor I need to use cycles. I need to use the G85 cycle with radius compensation and I am not being capable despite the large numbers of tests that I did. I want to do the following code:

T010101
G96 S400 M4
G00 X115 Z5
G85 N40 D4 F0.2 U4
N40 G81
G00 X101.8 Z2
G01 Z0 F0.12
G01 X99.75 Z-5.4
G01 X99.55 Z-11
G01 X96.55 Z-12.5
G01 Z-13.15
G80
G42
G87 N40


The code runs as expected (if the G42 is commented), but I must run it with tool compensation turned on, at least on the finish pass.
When the machine reaches the line with G87 N40, it complains that the tool compensation is turned on.
Please do not tell me that the control cannot do cycles with tool compensation ON... This would mean a poor controller to me.

Thank you

Similar Threads:

• Nose radius compensation
• Tool Radius Compensation
• Radius compensation
• Radius compensation in G71
• Radius compensation?

[Axce]

Hi my friend .

It actually seems you might be having a few things going on here.

1. G41/G42 activate radius comp while the G40 code turns it off. Looks like you are turning it on after the G80 which means it isn't active during the rough passes but was turned on before the finish..explains why the machine is saying it's turned on, because it is .
(Now on this point I'll add on an Okuma, I've never used radius comp, always gave me problems. Instead I'll draw the profile in my cad system, cam it for a finish pass them take that profile and paste it into my canned cycle).

2. Re-code your G85 to activate rad comp on the line where you feed to Z0 and make sure you are using the right code (G41 = left, G42 = right), then turn it off (G40) before your G80. That should fix the code, but then you must make sure the rad comp in your tool settings is correct (that it's the correct radius and the correct corner for the tool you are using).

Hope that helps!

[fomaz]

It was a good help.
I managed to do what I wanted IF the compensation if only ON inside the cycle, so for now it get me going.
Thank you

[Axce]

No problem

[fomaz]

Although I got the G85 going, there is still one thing that I cannot find and that I need to change.
Maybe due to the control is on a foreign language to me.

The issue is the retract value of the tool that it is currently set to 0.1 (I managed to see it using single block movements), that in my case is too low. At least 0.5mm is needed.
Anyone knows if this can be changed? Some option maybe?

Thank you

[OkumaWiz]

It is in your parameters and is your LAP cycle clearance value. Change it to what you want. It is standard on all Okumas.

Best regards,

[fomaz]

It is in your parameters and is your LAP cycle clearance value. Change it to what you want. It is standard on all Okumas.
Best regards,

What is not clear to me is that if is something that I can call when using for example the G85 (like the U D parameter) and in this case on the same program I would be able to use for example more than one clearance; or if is something that is changed on the controller itself using some configuration and it would remain fixed until another change on the controller settings.
If it matters, I program the cycle manually without using any feature that the controller may have.

[Axce]

As far as I know, this cannot be changed by coding a parameter (ie: U, W, D). So advice is choose an escape value that is acceptable for the entire program. I'm not trying to figure out the relevance of the escape value to the problem you're having, as it is a rapid move in any case. And in a G85 its at the end of each pattern repeat...just seems to me like overkill for a problem that might not exist if you look closer at what you are needing if its holding up production, my friend.

[fomaz]

For future reference this is set in Parameters->Optional Parameters->Another function 1->Line 4 (related with LAP). Value is in um.
I cannot write down the English reference as I do not have the controller in English.

[broby]

According to the documentation I have to hand, the parameter you are chasing for the retract amount is "Parameter, Optional Parameter (Long Word)" number 6.
This is listed as being the "Relieving amount in LAP - Bar turning (µm)"
Also, just to confirm, you must have your compensation for G41/G42 within the G81/G82 -> G80 shape definition section of your program.
Cheers
Brian.