G71 OKUMA OSP 7000

[Okuma rookie]

Hey there I'm having trouble writing a canned cycle on my Osp 7000 G71 

Just wondering if there are any wizards out there that could help me write a program to turn a m10 threat 1.5 pitch?? 

Cheers Matt 

 

[mkd]

N190 G00 X.5937 Z.2116
N200 G95
N210 G71 X.3298 Z-1. H.0639 B60 I0. D.0248 Q1 M32 M73 F.0591

[Okuma rookie]

Mkd 

 Thank you soo much for that you are the wizard 👍👍👍

[Okuma rookie]

Hey I tried this but not having much luck  with this machine  I think I’ts speed G50 G97 I’ll sus it out but what’s better m33 or G71  and how do you determine how many cuts are taken ++ thanks again for you reply’s very helpful  

I’m only doing basic threads no angles  

 

On 07/11/2014 at 4:28 AM, T_MALENA said:

Welcome to the forum.

Something like this should help.

 

G0Z5.5X24.(20.955??) Start position in X and Z

G71X20.955Z-17.3 B59. D1. W.1 H1. F M34M74   à   X=finish dia (root) Z=fin or end of thread B=angle of thread for infeed calc  D=doc W=finish pass H=height of thread F=pitch or federate  M34 & M74 are different cut patterns on Okuma machines.

Look in the programming manual for a good pic of the M34M74 stuff

Hope that helps.

 

11 hours ago, mkd said:

N190 G00 X.5937 Z.2116
N200 G95
N210 G71 X.3298 Z-1. H.0639 B60 I0. D.0248 Q1 M32 M73 F.0591

 

[mkd]

4 hours ago, Okuma rookie said:

nd how do you determine how many cuts are taken

there is not a direct setting for number of cuts(obviously)

you gotta take H/D into consideration. Cimco does a good job of backplotting number of passes.

yes i usually tweak it to M33, but don't do enough threads to see huge differences

[YoDoug®]

1 hour ago, mkd said:

there is not a direct setting for number of cuts(obviously)

you gotta take H/D into consideration. Cimco does a good job of backplotting number of passes.

yes i usually tweak it to M33, but don't do enough threads to see huge differences

M73/M74/M75 determine how many cuts by formula. Each M code is a different formula. M73 will give the least cuts, M75 will give the most. 

M32 is leading edge cutting, M33 is alternate edge cutting, M34 is trailing edge cutting. 

[Okuma rookie]

Thank you Mrk and Yodoug very helpful reply 

I have a much  better understanding of this now so

I'll giv both methods a go thanks again 👍 

[Okuma rookie]

On 04/06/2018 at 8:37 AM, mkd said:

N190 G00 X.5937 Z.2116
N200 G95
N210 G71 X.3298 Z-1. H.0639 B60 I0. D.0248 Q1 M32 M73 F.0591

Hi MKR I did get this going seems I needed G50 at the start of my program thanks again for writing the code I transferred it to metric;  Thanks again for you help much appreciated 👍