Macturn OSPE100L programming

[Green Button]

Machine:Okuma Macturn 3502SW
(with subspindle & lower turret)


Work done at main spindle, milling at D12
Compensation value 5.95
Okuma Macturn stops at line5, it reads program forward to
line 7 i think. it gives compensation alarm.
This program works at Okuma Multus (OSP200) but fore some reason it gives alarm in Macturn.
Machine have to do small movement in line 7, because there is inner radius R6 and tool in R5.95
This progrman goes throught if i put compensation value to 3...

Could there be some G-code for exact machining.....


G17
n1C0.
n2G00G41 X0. Y4.
n3G01 X2. Y6.
n4X12.726 Y6.
n5G02 X15.637 Y3.728 L3.
n6G01 X17.15 Y-2.325
n7G03 X22.91 Y-12.323 L6.
n8G01 X33.419 Y-9.703
n9G03 X41.Y0. L10.
n10G01G40X-6.C110.

[Algirdas]

N4 X12.726 Y6.
N5 G02 X15.637 Y3.728 L3.
look X values (15,637 - 12,726)*2 = 5,82< Compensation value 5.95
check direction of compensation. Strange, how it works on P200 ...

[Green Button]

Maybe this picture will help.
I'm trying to do this very simple contour into top of hollow bar.
In main spindle with m-axis, tool pointing down.
I'm using 12mm solid endmill, to get as litlle vibration as possible.
To compensation value i have 5.9

I have tried with L and with J& K
Also G18 and XY axis.
This programs works just fine with all Fanuc's & OSP200.
(so coordinates should be correct). I have tried to use accuracy 0.01 and 0.001 but no luck.
Compensation error all time

This example is with J& K:

N0114 G19
N0115 C0
N0116 G41 M13
N0117 G01 X74.75 F120.3 M147
N0118 Y6 Z-2 F24
N0119 Z-12.726
N0120 G02 Y3.727 Z-15.636 J-3 K0.001
N0121 G01 Y-2.325 Z-17.15
N0122 G03 Y-12.323 Z-22.91 J-4.176 K-4.308
N0123 G01 Y-9.702 Z-33.419
N0124 G03 Y0 Z-41 J9.703 K2.419


One glad thing, ATC is working fine

[Green Button]

Solution found.


So problems is that R6 pocket:

Okuma can't handle that as one radius.
There is 2 way to do that:

1) You have to make that R6 in two pieces,so there will be in program:
G03XZR6
G03XZR6

2) Other solution is that you wont do radius at all.
So y have D12 miller and you program just straight lines, there will be automatically R6 of course. But when endmill is end of pocket, you have to make 0.02 straight there. Otherwise y get compensation alarm.

[Green Button]

Solution work on Multus (OSP200) but not in OSP100 !!!
Solution 2 works on both machines.

Man...this Okuma OSP is from outer space....
Why OSP100 wont understand that radius???

[Algirdas]

it's not Okuma. It's DIN CNC standard of arc. The arc with angle close to 180° is problematic allways. You use additional arc command when you need the ark bigger, than 180°. Generally, arc angular size is not clearly described. You can connect two points by defined radius and direction arc in two ways except of exact 180° arc

[budgieW]

Use IJK or break the arcs at quadrants with L

[Green Button]

I have send this programming problem to Okuma's engineer.
I'll let y know result.

OK,I get answer:

Due to the PC base controller Okuma OSP 200 has the possibility to use different algorithm to calculate the intersection points.
OSP100 uses different software and this case is not possible to do with it (using L or I/K)

Case closed.