OKUMA - POST

[Lathe-Mill]

Hello peeps, post question:

I need a G00 or cancel (G80) after each drill and tap cycle, G81,G83 and G284.

how can I make that happen?.

thanx peeps.

[crazy^millman]

Explain better after each operation how? Do you mean each hole or after each operation called in Mastercam then posted to the NC code? Do you mean it will do some and not the others drilling operation?

Details Details and we can help you out more.

[fboike]

Is there a pcanceldc section in your post?

You may need to add one. or make sure its being called.

[Brendan P]

You should have something like this in your post:

 

 

pcanceldc #Cancel canned drill cycle

result = newfs (three, zinc)

z = initht

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

pxyzcout

!zabs, !zinc

prv_gcode = zero

pcan

pcan1, pbld, "G80", strcantext, e

pcan2

 

If you want to cancel after every hole,then I'm stumped!

[Lathe-Mill]

ex:

G83 Z-3.904 R-3.604 Q.05 F5. M53

G80 or G00 -------->>> RIGHT HERE

 

REASON:

when i have a drill or tap cycle, and using diferent depths, it moves X and Y then Z

tool breaks, or if i use an endmill to drill and then move for a milling op, same thing

so i want to cancel with a g80 or g0

[chris m]

Carlos

 

If you're using MPOKUMA I edited mine to look like this:

 

pg80_out #Cancel canned drill cycle

result = newfs (three, zinc)

result = newfs (15, feed)

z = initht

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

if initht > refht, ret_ht = initht

else, ret_ht = refht

pxyzcout

!zabs, !zinc

prv_gcode = zero

pbld, n, "G00", *ret_ht, e

g80_out = zero

 

I used 'G00' instead of 'G80' because G80 stops the spindle in my Okumas [which I hate]

 

C

[Brendan P]

If you want the G80 after every hole,then I think if you used seperate operations for each one,then it would work.

But this sux

[Lathe-Mill]

the post is custom made, so i will look thru it and see if i can find those values. thanx guys

[Lathe-Mill]

ok, here it is

 

pcanceldc #Cancel canned drill cycle

#G80 Must Appear in SUB program before RTS

#if g80_out = 1, pg80_out

 

pg80_out #Cancel canned drill cycle

result = newfs (three, zinc)

result = newfs (15, feed)

z = initht

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

pxyzcout

!zabs, !zinc

prv_gcode = zero

pbld, n, "G80", e

g80_out = zero

[chris m]

quote:

---

REASON:

when i have a drill or tap cycle, and using diferent depths, it moves X and Y then Z

tool breaks, or if i use an endmill to drill and then move for a milling op, same thing

so i want to cancel with a g80 or g0

---

This sounds more like a Mastercam prob than a post problem; if you have a safe clearance height set in your ops and nobrk set to 'no' in your post your machine should move safely from one hole or operation to another...

 

C

[Lathe-Mill]

here is a example

 

NT26 G0 G90 G15 H1 X0. Y.67 S3500 M3

N33 G56 H26 Z.25 T27 M8

N34 G81 Z-.035 R.1 F10. M53

N35 X.4738 Y.4738

N36 X.67 Y0.

N37 X.4738 Y-.4738

N38 X0. Y-.67

N39 X-.4738 Y-.4738

N40 X-.67 Y0.

N41 X-.4738 Y.4738

( SPOT 2 PLC. )

N42 X-.375 Y-1.3132 Z.25------->>>

N43 G81 Z-3.739 R-3.604 F10. M53

N44 X.375

N45 M9

N46 G0 Z40.

[chris m]

Carlos; why don't you email me a sample mc9 file and let me post it with my post and see what she does

 

C

[chris m]

Check your Inbox, I think I got it

 

C

[Mick]

Something appears to be missing there. M53 is "return to initial Z position after hole machining", but for that to work, there needs to be the "Initial Z Plane" line, which would look something like this:

 

G71 Z40

 

between N33 and N34. There shouldn't be any need for the breakup of the drilling into two cycles (the two G81 lines) when all that is different is the Z depth and the R height.

[chris m]

Mick

 

I have a copy of Carlos' post from awhile back and it has been modified extensively [in somewhat unusual ways] in the drilling area so the G71 line is actually hard coded in the beginning of the program (since G71 is modal you can just call the M53 later on as many times as you wish) instead of being posted as needed. The post has a lot of hardcode in it that shouldn't really be there, but, if it works....

 

 

In this case, I think his problem was the # in this area:

 

pcanceldc #Cancel canned drill cycle

#G80 Must Appear in SUB program before RTS

======> #if g80_out = 1, pg80_out

 

With that removed, all should be fine

 

C

[Mick]

Ah.. heh... yes, hashed

 

Hardcoding has its merits, and sometimes it doesn't

[Lathe-Mill]

Chris, got your e-mail, thanx alot man, it does work fine. about that G71, it sux when I', doing rotary work, i inherited that post, I try to tweek it as i go.

as you can see that g71 is set at z.25, and that is on all 4 axis, so when i program the rotary that line comes G71 z.25 always, althou i work from centerline of the part, so manually i need to change it to what ever i need to.

thnx

[chris m]

Carlos, in your post someone commented out the line that generates the G71 line where it is really supposed to be. You should try it the way it was originally set up and see what you think:

 

1) Comment out the G71 Z.25 hardcode line

 

2) Remove the pound sign from this line in pdrlcommonb:

 

# pbld, "G71", *initht, e

 

This should tidy things up, I think, but take a close look at the code because there are some funky variables and other things going on in your post that could possibly be affected by this

 

I'm looking into the other question you emailed me

 

C

[chris m]

Carlos, check your inbox

 

C

[Lathe-Mill]

the G71 always output in the beginning of the program like " G71 Z.250 "

How can I make it to output .250 incremental from the starting hight?

[chris m]

Just set the clearance plane where you want it in MC, that's what determines the G71 height in the code

 

C

[Mick]

Chris/Carlos

 

What kind of machine is this post for?

 

If its for a 4 axis Okuma vertical, the MPMaster Okuma post will work great

 

I'm a big fan of it

[Lathe-Mill]

thanx mick, 4 axis vertical, chris really is good help on this post, he guide me very well and post is working good now.

[Mick]

We have a Okuma MX55VB with a 4th axis.

 

Thats great Chris has your sorted

[chris m]

Hey Mick

 

I'll show you mine if you show me yours...

 

C