PDA

View Full Version : G42 Tool nose radius.



al-108
02-27-2008, 03:39 PM
I really need some help with the G42 on my Okuma LR35
i can not seem to get this program to work with the G42 in there it works just fine when i take it out, but i need to control the radius to get a correct part.

Please HELP.


D-300131-1-TEMP.MIN
G13
G50S1000
G0X50Z50
NAT07
T070707 (CNMG .010 RAD)
G0 G90 X12.718 Z3.100 G97 S300 M43 M3 M8
G96 S1000
G85 NODIA D.20 F.01 U.005W.005
NODIA G81
G42 G0 X.030 Z3.000 F.008
G1 Z2.790
G3 X12.2186 Z.184 I-.015 K-8.464
G1 X12.500
G80M9
G40 X12.718
G97S200
G0 X50. Z50.
M2
%

Spaantje
02-27-2008, 03:56 PM
I'm not familiair with this type of machine,
but can you put a G42 in combination with a G00 within a cycle.
On some type of Okuma's it gives you a error message.
(Dit you have a error message?)

littlerobb
02-27-2008, 04:46 PM
I need to know what control it is, but I will be willing to bet that the problem is that you have cancelled the G42 after you cancelled the canned cycle try putting the G40 in the x 12.500 line before the G80. Best of luck
Robert

broby
02-28-2008, 07:47 AM
You definitely need to move your G40 command line to the line before the G80 command


D-300131-1-TEMP.MIN
G13
G50 S1000
G0 X50 Z50
NAT07
T070707 (CNMG .010 RAD)
G0 G90 X12.718 Z3.100 G97 S300 M43 M3 M8
G96 S1000
G85 NODIA D.20 F.01 U.005 W.005
NODIA G81
G42 G0 X.030 Z3.000 F.008
G1 Z2.790
G3 X12.2186 Z.184 I-.015 K-8.464
G1 X12.500
G40 X12.718 <---- Move this line to here!
G80
M9
G97 S200
G0 X50. Z50.
M2
%

al-108
02-29-2008, 06:35 PM
Thanks quys the problem was that the g42 should have after the g80

broby
03-02-2008, 02:39 AM
Actually the command structure is that you specify the canned cycle first with the line name that the start of the shape definition starts on within the line defining the cycle, then you define the shape between G81/G82 and G80.
Any tool radius compensatation actions (G41/G42 through to G40) are then used within the confines of the shape definition!
The only way to access a "Shape" is via canned cycle such as G85 (roughing), G87 (finishing) etc...
for example: (ignoring the usuall startup codes...)

N100 G0 X Z (RAPID TO START POINT)
N102 G96 S(Surface Speed)
N104 G85 NTURN D... F... U... W...
NTURN G81
N106 G00 X(strt point)
N108 G1 G42 Z...
N110 shape
.
.
.
N200 G40 X Z
N202 G80
N204 G00 Xhome Zhome G97 S...
.
.
Rest of program blah blah blah

The Shape defined between line NTURN and N202 is not accessed until "called" by a canned cycle such as the G85 roughing cycle above.
If you take out the roughing cycle and let the program run through, it will get to line N102 and then jump to line N204 (in the above example).
THEREFORE you need to have your tool nose radius compensatation INSIDE the G81/G80 commands.

You can actually do simple things such as defining the roughing cycle and then on the next line define the finishing cycle. I used to do this all the time if I was using the same tool to rough and finish with.

N100 G0 X Z (RAPID TO START POINT)
N102 G96 S(Surface Speed)
N104 G85 NTURN D... F... U... W...
NFIN G87 NTURN
NTURN G81
N106 G00 X(strt point)
.
.
.
N200 G40 X Z
N202 G80
N204 G00 Xhome Zhome G97 S...

In this example the program will rough the shape and when the roughing cycle is finished the machine will return to the Cycle start point, then read the next line which is the G87 finish turn cycle.
When the finish turn cycle completes it will NOT return to the cycle start point so you need to be carefull when doing ID work that you program a correct excape tool path (or have new tools on standby :)).
Once the Finishing cycle is complete it will read the next line (NTURN) see that it is a shape definition line and then jump to the end of the shape definition G80 and carry on from there.

Hope this clarifies your situation.
Regards
Brian.