Manufacturing Information Solutions Forum Index Manufacturing Information Solutions
Your Place for Support and Discussions
 
 FAQFAQ   SearchSearch   MemberlistMemberlist   UsergroupsUsergroups   RegisterRegister 
 ProfileProfile   Log in to check your private messagesLog in to check your private messages   Log inLog in 

Okuma live tools Code

 
Post new topic   Reply to topic    Manufacturing Information Solutions Forum Index -> G-Code Programming
View previous topic :: View next topic  
Author Message
JoeM
Master Poster


Joined: 09 Jul 2004
Posts: 122
Location: Jackson Hole, Wyoming USA

PostPosted: Fri Mar 18, 2005 1:03 pm    Post subject: Okuma live tools Code Reply with quote

Can anyone please explain to me, what is different between M15 and M16, when M15 or M16 is programmed. Confused
_________________
Thanks.
===================
I would rather by Fly Fishing!
Back to top
View user's profile Send private message Send e-mail
CNCJimmy7
Frequent Poster


Joined: 05 Jul 2004
Posts: 91
Location: Minneapolis, MN

PostPosted: Fri Mar 18, 2005 1:04 pm    Post subject: Reply with quote

M15 is to programming the C axis in positive direccion and M16 is to programmiong in negative direccion.

And I recomend you use M15 you only have increment the degrees you want to programming

Example if you are programming without can cycle and need to make 4 holes in a given part 90 degrees each just programming like this

M15
G00 C0
G00 C90
G00C180
G00C270

(IS NOT THE WAY TO PROGRAMMING JUST EXAMPLE)

Hope help you
Back to top
View user's profile Send private message Send e-mail
franke
Master Poster


Joined: 26 Jun 2004
Posts: 161
Location: Indiana, USA

PostPosted: Fri Mar 18, 2005 1:07 pm    Post subject: Reply with quote

This is the example you want to program in negative direccion do not have any special fuction just some programers like to program in negative I put in red color the M16 and the start poin in C.

You can try this example and check the "C" axis when it changes the position this part of the program make two holes.

And after you run this just change the M16 to M15 and see what happen.
Code:

( .500" HOLES X 2 TMS AT .8"LOCATION )
(DELTA DRILL DIA .500")
(      R411.5-16032  )

       M05
 M110
 G94 M146 M16 M08 (after you run M16 Change to M15 )
 G00 Z-0.8 T0404 SB=1100       

G00X6.36
G00X2.7
G183 X1.5 Z-.8 C0 I0 F4.50 Q2 D1.50 L1.50
G180
G00 X3.50
G00X6.36
G95
M09
M12
M109
G00X50
G00Z50
Back to top
View user's profile Send private message
JoeM
Master Poster


Joined: 09 Jul 2004
Posts: 122
Location: Jackson Hole, Wyoming USA

PostPosted: Fri Mar 18, 2005 1:08 pm    Post subject: Reply with quote

On some program running with live tool, sometimes i see M146 and M147, but the program you give me for example i see only M146 but no M147, what is the function of these two? And sometimes G181 and G183 for drill cycle, can you tell me when is G181 or G183 is used for live tool drill cycle. Thank your for your help.


Here is program example I want to mention to:

N200 M05

N210 M110

N220 G94 M146 M15 M08

N230 G00 C345 M16

N240 M147

N250 G00 X2.550 Z-.5 T0404 SB=700 M13

N260 G181 X1.920 Z-.5 C345 I0 F08

N270 G180

N280 M12

N290 M146

N300 M109

N310 .....

N320......

N330 M02

Can anyone please help me to modify this progam, which code can be kept, and which code better to be deleted.
Back to top
View user's profile Send private message Send e-mail
franke
Master Poster


Joined: 26 Jun 2004
Posts: 161
Location: Indiana, USA

PostPosted: Fri Mar 18, 2005 1:10 pm    Post subject: Reply with quote

When you select the mill mode M110, M146 is to unclamp the C axis often we use in the start of the program M146 in case you have to rerun the program if the C axis is clamped do not come in alarm. Now the G181 is a drilling cicle this mean holes can do make only one pass,the G183 is deep hole drillind cycle and this is use when you have deep hole and you need cheap control or in other words peek drilling you have in the G183 line D where you put the amount per peek

Example:

Code:
M110
G94 M146 M15 M08
G00 Z-3.17 T0707 SB=1080     

G00X6.36
G00X2.500
G183 X-.98 Z-3.17 C0 I0 F3.80 Q4 D.125 L.250
G180

below you find what i change in you program


N200 M05
N210 M110
N220 G94 M146 M15 M08 (C axis Unclamp M146)
N230 G00 C345
N240 M147 (C axis clamp M147)
N250 G00 X2.550 Z-.5 T0404 SB=700 M13
N260 G181 X1.920 Z-.5 C345 I0 F08 (G181  drilling cycle)
N270 G180 (cancel drilling cicle)
N280 M12
N290 M146 (C axis unclamp again  M146)
N300 M109
N310 .....
N320......
N330  M02
Back to top
View user's profile Send private message
Display posts from previous:   
Post new topic   Reply to topic    Manufacturing Information Solutions Forum Index -> G-Code Programming All times are GMT - 5 Hours
Page 1 of 1

 
Jump to:  
You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot vote in polls in this forum


Powered by phpBB © 2001, 2005 phpBB Group