[kvesligaj]

Hi

Okuma OSP-P300L control, which parameter is for setting up range of C-axis 360+ degree; now the range is 0 - 359.99.

I need 0 - ............

If i put for example C=550 degree, machine dont know where to go...


Please help

[deadlykitten]

hi, try to use G91 or MOD function ( also there are other solutions )

range is : [ - u , + u ] where u = 360 - 0.001

input C + MOD [ 550 , 360 ]

how does your part looks like ?

[kvesligaj]

This is part of my code for example when engraving on diameter; you can see here that my cam software (post) gives my coordinates for C axis above 360 degree, and machine dont recognize that, I am asking for parameter which solve that or if i remember there is G-code system variants; I think i solve that on Mazak once with G-code system B.....dont know, dont remember....any suggestions...THNX


Z-43.596 C404.066
Z-43.786 C403.913
Z-44.167 C403.756
Z-44.742 C403.76
Z-45.12 C403.923
Z-45.31 C404.083
Z-45.5 C404.567
C406.033
Z-41.5
G00 X107.
Z-44.549 C407.295
G01 X104.2 F400.
Z-44.922 C407.452 F800
Z-45.304 C407.771
Z-45.5 C408.087
Z-45.505 C408.736
Z-45.318 C409.056
Z-44.939 C409.38
Z-44.559 C409.54
Z-43.984 C409.705
Z-43.035 C409.707
Z-42.46 C409.547

[deadlykitten]

can you output code in G91 ?

[kvesligaj]

I can change post, but I would like to solve this with machine parameter

I didnt have this problem on any other machine, Ouu yeah, I have, Siemens, but I just changed system parameter

[deadlykitten]

i am afraid that there is no parameter

... and your feed is not ok

Z
C
F

-44.922
407.452
800.540

-45.304
407.771
902.526

-45.5
408.087
1022.618

-45.505
408.736
1130.252

-45.318
409.056
1031.588

-44.939
409.38
906.939

-44.559
409.54
800.574

-43.984
409.705
770.798

-43.035
409.707
740.002

-42.46
409.547
769.103

feed = sqrt ( a + b ) / sqrt ( a + c) * d, where ;
... a = ( 360 * dZ ) ^ 2
... b = ( 500 * dC ) ^ 2
... c = ( X * dC * pi ) ^ 2
... d = F for G94, or f for G95

your move now maybe someone has a post for you ? kindly !

[deadlykitten]

and your CAM is not delivering equal discretization ... not on Z, not on C, not on toolpath / nowhere

[kvesligaj]

Ok, i understand what you mean, but this is not an issue, it works fine for my products, thanx for help...

[deadlykitten]

yup, i think is all ok if you fix the C problem ... you can leave the rest for another day

however, sorry, there is no parameter

[deadlykitten]

can you output code in G91 ?

ups, please be aware, that if you output in G91, than full circle may not be complete, because in G91 machine uses only 0.001 precision, while in G90 it goes beyond 0.0001, even if displayed data is only with 0.001 decimals

i am sure for this for my mill, while i have not tested it on lathe

for most cases, it is not important, but when it comes to discretization it may be

also, for engraving, if you toolpath is not periodical with period=360 degrees ( like a helix or spiral or a sinus, etc ), than you can have no worries

if you would engrave a swiss watch dial using G91, than it will show 13 hours

it will stop at 360 - ( number_of_code_lines * truncation_after_3rd_zecimal ); something like that

this aspect can be solved by managing the increasing truncation error

kindly !

[Superman]

This is part of my code for example when engraving on diameter; you can see here that my cam software (post) gives my coordinates for C axis above 360 degree, and machine dont recognize that, I am asking for parameter which solve that or if i remember there is G-code system variants; I think i solve that on Mazak once with G-code system B.....dont know, dont remember....any suggestions...THNX


Z-43.596 C404.066
Z-43.786 C403.913
Z-44.167 C403.756
Z-44.742 C403.76
Z-45.12 C403.923
Z-45.31 C404.083
Z-45.5 C404.567
C406.033
Z-41.5
G00 X107.
Z-44.549 C407.295
G01 X104.2 F400.
Z-44.922 C407.452 F800
Z-45.304 C407.771
Z-45.5 C408.087
Z-45.505 C408.736
Z-45.318 C409.056
Z-44.939 C409.38
Z-44.559 C409.54
Z-43.984 C409.705
Z-43.035 C409.707
Z-42.46 C409.547

Solution is NOT in the machine parameter area.... machine should already be set to travel "shortest distance"
- it is in the CADCAM system that outputs the NC code, so that C axis values don't exceed +/- 359.9999
( if you are at C0. and MDI in G0 C350. -movement would be a -10° move )
( if you are at C350. and MDI in G0 C10. -movement would be +20° move )

[deadlykitten]

hey Super i dont know about the shortest-distance parameter, but only M15 / M16

please, can you share how ? i just found the M960 : i will test it ...

[deadlykitten]

hey kvesligaj, you dont know, but my 1st reply was that you need an option

and i was checking for this option, i failed to find it, so i deleted my answer ...... but now, please find attached

all the best !

ps : the reason why i forget is that i dont have such an advanced cam

[deadlykitten]

i am sure for this for my mill, while i have not tested it on lathe

hello, i just run some tests

    V1 = 7 / 15                     ( absolute mode / G90 )
    V2 = 0
    NLOOP V2 = V2 + 1
          G00 Z300+V1*[V2-1]
    IF [ V2 LT 16 ] NLOOP

( . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . )

    V1 = 7 / 15                     ( relative mode / G91 )
    G00 Z300
    G91
    V2 = 0
    NLOOP V2 = V2 + 1
          Z+V1
    IF [ V2 LT 15 ] NLOOP

... on lathe, both sample delivered 307
... on mill, 2nd one delivered 307.005

---

i chosed 7/15 as an example, because it is a rational number, thus a lot of decimals

7/15=0.4(6)

truncating the number to 3 decimals will lead to a truncation error = 0.000(3)

15*0.000(3) will lead to the 0.005 error, just how the mill displayed

mills with osp300 + G91 may truncate rational values just another team vs team, so a normal day @ the office

real cases that may lead to this behaviour :
... parametric codes
... improper incremental discretizations

FUP error was not enough kindly !

[Superman]

Google search came up with this thread ....link
( for a P200L captain lathe )

[kvesligaj]

Yes, this is solution; i forgot to tell you Okuma dealer told me couple a days agao, but big big thanks


Also it could be done with CAM software; post should be modified.


Thaanks guys