View previous topic :: View next topic |
Author |
Message |
JoeM Master Poster
Joined: 09 Jul 2004 Posts: 122 Location: Jackson Hole, Wyoming USA
|
Posted: Fri Mar 18, 2005 1:03 pm Post subject: Okuma live tools Code |
|
|
Can anyone please explain to me, what is different between M15 and M16, when M15 or M16 is programmed. _________________ Thanks.
===================
I would rather by Fly Fishing! |
|
Back to top |
|
|
CNCJimmy7 Frequent Poster
Joined: 05 Jul 2004 Posts: 91 Location: Minneapolis, MN
|
Posted: Fri Mar 18, 2005 1:04 pm Post subject: |
|
|
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 |
|
|
franke Master Poster
Joined: 26 Jun 2004 Posts: 161 Location: Indiana, USA
|
Posted: Fri Mar 18, 2005 1:07 pm Post subject: |
|
|
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 |
|
|
JoeM Master Poster
Joined: 09 Jul 2004 Posts: 122 Location: Jackson Hole, Wyoming USA
|
Posted: Fri Mar 18, 2005 1:08 pm Post subject: |
|
|
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 |
|
|
franke Master Poster
Joined: 26 Jun 2004 Posts: 161 Location: Indiana, USA
|
Posted: Fri Mar 18, 2005 1:10 pm Post subject: |
|
|
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 |
|
|
|