Hello, does anybody know how to get separate moves to stop cutting double depth? if you use canned cycles it cuts the depth that is entered? Thanks
Printable View
Hello, does anybody know how to get separate moves to stop cutting double depth? if you use canned cycles it cuts the depth that is entered? Thanks
The software can post in Radius or in Diameter mode. I wouldn't think that canned cycles vs separate moves would post differently.
Which post processor are you using?
Fanuc 10 T , I have worked on it for a month to get it were it outputs everything my lathe needs. I just cant get this one figured out? you can draw a part create the code in canned cycle and it will output the chosen depth go back and choose separate moves and it will double the depth of cut? Thanks For Any Help
Here is my sample file layout
Separate Moves:
Code:(BEGIN PREDATOR NC HEADER)
(MCH_FILE=LATHE.MCH)
(LTOOL T0101 M0100 S1 O5. I.25 A80 C.0156 H0. D0. N1)
(SCYL S3 X0 Y0 Z-3. D2. L3.)
(HCYL S3 X0 Y0 Z-3. D0. L3.)
(END PREDATOR NC HEADER)
O0001
(JOB 1 ROUGH CYCLE )
(TOOL #1 80 DEG. 1/64 ROUGH TURNING )
G80 G93 G40 G54 G18
T0101 M06
G50
G96 M03
M08
G00 X2.2 Z0.
G00 X1.82
G01 Z-.4901 F.015
G01 X2.02
G00 Z0.
G00 X1.62
G01 Z-.49
G01 X1.82
G00 Z0.
G00 X1.42
G01 Z-.49
G01 X1.62
G00 Z0.
G00 X1.22
G01 Z-.49
G01 X1.42
G00 Z0.
G00 X1.02
G01 Z-.49
G01 X1.22
G00 Z0.
G00 X1.02
G01 Z-.49
G00 X10.
G00 Z5.
G40
M01
M09
M05
M30
Canned Cycle:
Code:
(BEGIN PREDATOR NC HEADER)
(MCH_FILE=LATHE.MCH)
(LTOOL T0101 M0100 S1 O5. I.25 A80 C.0156 H0. D0. N1)
(SCYL S3 X0 Y0 Z-3. D2. L3.)
(HCYL S3 X0 Y0 Z-3. D0. L3.)
(END PREDATOR NC HEADER)
O0001
(JOB 1 ROUGH CYCLE )
(TOOL #1 80 DEG. 1/64 ROUGH TURNING )
G80 G93 G40 G54 G18
T0101 M06
G50
G96 M03
M08
G00 X2. Z0.
G71 U1 R.1
G71 P1 Q2 U.02 W.01 F.015
N1 G00 X1.
G01 Z-.5
N2 G01 X2. Z-.5001
G40
M01
M09
G00 X10. Z0.
G00 Z5.
M05
M30
This posting blocks effects radius or diameter mode:
249. Output X as a diameter or radius (d/r)? d
I changed the posting block from D to R and here is the resulted code.
Canned Cycle:
Separate Moves:Code:(BEGIN PREDATOR NC HEADER)
(MCH_FILE=LATHE.MCH)
(LTOOL T0101 M0100 S1 O5. I.25 A80 C.0156 H0. D0. N1)
(SCYL S3 X0 Y0 Z-3. D2. L3.)
(HCYL S3 X0 Y0 Z-3. D0. L3.)
(END PREDATOR NC HEADER)
O0001
(JOB 1 ROUGH CYCLE )
(TOOL #1 80 DEG. 1/64 ROUGH TURNING )
G80 G93 G40 G54 G18
T0101 M06
G50
G96 M03
M08
G00 X1. Z0.
G71 U1 R.1
G71 P1 Q2 U.01 W.01 F.015
N1 G00 X.5
G01 Z-.5
N2 G01 X1. Z-.5001
G40
M01
M09
G00 X5. Z0.
G00 Z5.
M05
M30
Code:
(BEGIN PREDATOR NC HEADER)
(MCH_FILE=LATHE.MCH)
(LTOOL T0101 M0100 S1 O5. I.25 A80 C.0156 H0. D0. N1)
(SCYL S3 X0 Y0 Z-3. D2. L3.)
(HCYL S3 X0 Y0 Z-3. D0. L3.)
(END PREDATOR NC HEADER)
O0001
(JOB 1 ROUGH CYCLE )
(TOOL #1 80 DEG. 1/64 ROUGH TURNING )
G80 G93 G40 G54 G18
T0101 M06
G50
G96 M03
M08
G00 X1.1 Z0.
G00 X.91
G01 Z-.4901 F.015
G01 X1.01
G00 Z0.
G00 X.81
G01 Z-.49
G01 X.91
G00 Z0.
G00 X.71
G01 Z-.49
G01 X.81
G00 Z0.
G00 X.61
G01 Z-.49
G01 X.71
G00 Z0.
G00 X.51
G01 Z-.49
G01 X.61
G00 Z0.
G00 X.51
G01 Z-.49
G00 X5.
G00 Z5.
G40
M01
M09
M05
M30
Line 249 is set to d. when you turn it to r it will post out with the cut depth that was entered but when you use D it is wrong? my lathe needs to be in Diameter
skippy, your lathe WILL be in diameter, its the post that will change. if you set it to diameter, then when you tell it to cut .1 deep, it will cut the DIAMETER .1 smaller (or .05 per side) if its set to radius, and you tell it .1 deep cuts, it will reduce the RADIUS by .1 (or .2 on the diameter).
I understand all of the diameter verses radius, what I am trying to figure out if you take a ruff cut say at .100 in canned cycle it will post .100 depth of cut, go back to the same thing just choose separate moves and post it will be posting a cut depth of .200? nothing changed just canned cycle verses separate move?
Have you tried doing it with the "System Compensation" on or off ? ?
Also does it actually cut the double depth at the machine ? ?
Take a 2 inch bar stock and draw your geometry at 1.8 as the diameter you want to turn the bar to. Clear all allowances etc so it`s easier to see what is happening with the code.
In the canned cycle if you set a DOC of 0.05 then it will usually show as G71 U.05 R.1 or similar.
This is showing what DOC the canned cycle has been instructed to make, after the two G71 lines there is an X value, this is the diameter you have drawn and this line tells the canned cycle where to go to diameter wise at the DOCs set in the first G71 line.
In the separate moves it will show the first cut at X1.9, this looks at first glance to be a double depth cut but it is not, it is the DIAMETER the machine is being told to cut to, the machine if set in diameter mode will therefore actually only do a 0.05 depth of cut, it should also show on the machine control screen as X1.9, reason for this is you should be working in absolute mode so you are instructing the machine to go to a specific point, in this case a diameter. The control decides how much to cut depending on all your other settings like TNR for example.
In both examples the machine will physically only make two passes to run this program of 0.05 DOC to reach the 1.8 diameter required :D
I don`t have the 10T PP so I can`t check if there might be an issue there, if the above doesn`t help then upload your 10T PP and I`ll give it a try. :D
Probably confused you even more now :D :D :D
Regards
Rob
:rainfro: :rainfro: :rainfro:
IN the seprate moves post abotu from Al, why does it do the same move twice?
G00 X.51
G01 Z-.49
G01 X.61
G00 Z0.
G00 X.51
G01 Z-.49
G00 X5.
G00 Z5.
It goes over the exact same area at the same distance twice, it goes to X.51 then cuts along Z to Z-.49 deep, then does it again.