Okuma Thread Milling Code Sample Needed

[Mickey_D]

I am trying to get my cam package post updated to get thread milling working reliably for our 560V (OSP200Ma control). The post guy wants actual code and not the equations provided in the Okuma book. Anybody have a sample that they could post so that I can get this working?

 

[Edster]

Here's code generated from FeatureCAM for a 1/2-13 blind hole with a solid carbide TSC thread mill. The thread mill is long enough so it's only making one pass.

G0 G17 G20 G40 G80 G90 G94
G111 T21 Q28
(OPERATION - Carmex 13 TPI Thread Mill)
(TOOL NO - 21 DIAM - 0.362)
(TOOL COMMENTS - )
M1
G15 H1
S2848 M3
G0 G90 X0.5 Y-0.5
G56 Z1.03 H21
M50 <<<<<< Turns on TSC
G4P1
Z0.
G1 Z-0.6941 F11.2
G41 X0.5423 Y-0.5362 D21F2.8
G3 X0.5785 Y-0.5 Z-0.6769 I0. J0.0362
X0.5785 Y-0.5 Z-0.6 I-0.0785 J0.F5.6
X0.5423 Y-0.4638 Z-0.5828 I-0.0362 J0.
G1 G40 X0.5 Y-0.5 Z-0.6
G0 Z1.03
M5
M9
G4P1
M339 <<<<<< Turns on Through Spindle Air Blast
G4P5
M9

IIRC I didn't have to do anything special to my post FeatureCAM just worked.

Good Luck

 

[Edster]

Here's another one but the Hole is too deep for the threadmill I'm using so it makes multiple steps, but still only one pass.

G0 G17 G20 G40 G80 G90 G94
G111 T22 Q28
(OPERATION - Carmex 13 TPI Thread Mill Mini)
(TOOL NO - 22 DIAM - 0.362)
(TOOL COMMENTS - )
M1
G15 H1
S2848 M3
G0 G90 X1.53 Y-0.5
G56 Z1.0 H22
M8
Z0.
G1 Z-1.0941 F11.2
G41 X1.5723 Y-0.5362 D22F2.8
G3 X1.6085 Y-0.5 Z-1.0769 I0. J0.0362
X1.6085 Y-0.5 Z-1.0 I-0.0785 J0.F5.6
X1.5723 Y-0.4638 Z-0.9828 I-0.0362 J0.
G1 G40 X1.53 Y-0.5 Z-1.0
Z-0.8634 F11.2
G41 X1.5723 Y-0.5362 D22F2.8
G3 X1.6085 Y-0.5 Z-0.8462 I0. J0.0362
X1.6085 Y-0.5 Z-0.7693 I-0.0785 J0.F5.6
X1.5723 Y-0.4638 Z-0.7521 I-0.0362 J0.
G1 G40 X1.53 Y-0.5 Z-0.7693
Z-0.6327 F11.2
G41 X1.5723 Y-0.5362 D22F2.8
G3 X1.6085 Y-0.5 Z-0.6155 I0. J0.0362
X1.6085 Y-0.5 Z-0.5386 I-0.0785 J0.F5.6
X1.5723 Y-0.4638 Z-0.5214 I-0.0362 J0.
G1 G40 X1.53 Y-0.5 Z-0.5386
Z-0.402 F11.2
G41 X1.5723 Y-0.5362 D22F2.8
G3 X1.6085 Y-0.5 Z-0.3848 I0. J0.0362
X1.6085 Y-0.5 Z-0.3079 I-0.0785 J0.F5.6
X1.5723 Y-0.4638 Z-0.2907 I-0.0362 J0.
G1 G40 X1.53 Y-0.5 Z-0.3079
Z-0.2482 F11.2
G41 X1.5723 Y-0.5362 D22F2.8
G3 X1.6085 Y-0.5 Z-0.231 I0. J0.0362
X1.6085 Y-0.5 Z-0.1541 I-0.0785 J0.F5.6
X1.6085 Y-0.4981 Z-0.1538 I-0.0785 J0.001
X1.5714 Y-0.4628 Z-0.1366 I-0.0362 J-0.0009
G1 G40 X1.53 Y-0.5 Z-0.1538
G0 Z1.0
M9

 

[Mickey_D]

Thanks Edster, I will test these out as soon as this run is finished and then send them to the cam post guy. This is for our legacy Visual Mill parts, have been using it for about five years and have a lot of parts done up in it that are not worth migrating over to mastercam but are worth tweaking a little.

 

[Jamie Fritz]

Don't have any on hand, but sometimes they throw them up on their site. CNC Machine Tool Solutions, Solutions, Productivity, Okuma, check there first to see if you can find some.

 

[Dadger47]

Can this be achieved on a non Y axis machine using X and C axis? Cheers

 

[litlerob1]

Mickey, tell your post guy to pop his head out of his ass. There should be an Audible sound when that happens POP.

The code for the actual path is no different than any other RS-274 code. The difference will fall into Tool callout, TLO, Work offset and other random commands, the actual path is no different. Uses the same Comp. codes and Linear, Arc, Rapid and motion control as Fanuc or Haas or Mazak or anything else. The code that Edster posted is identical below the 'coolant on'(M8) command.

If you use the 2D toolpaths> Threadmill and you have Control def, Machine Def and P.P.file correct, it will give you the Toolpath you want.

It sounds like your post guy is full of shit to me.

R

 

[brian.pallas]

Lol, that's funny Rob, and you are right, switching to Okuma is no big deal at all. Buuuut...it seems most of the post people that do the support for cam companies have a computer background, not machining, so you really are better off giving them a text file and a cam file and say "I want this to make this".

 

[litlerob1]

Lol, that's funny Rob, and you are right, switching to Okuma is no big deal at all. Buuuut...it seems most of the post people that do the support for cam companies have a computer background, not machining, so you really are better off giving them a text file and a cam file and say "I want this to make this".

Unfortunately, I am forced to agree with you. I learned to edit my own .pst files for that reason.

But if other Toolpaths are working for that machine, he should not need to send in a working copy of a Threadmilling Toolpath to make it work. Errrr>>>CC>>

R