Need Help!- g83 question

[simpy]

can someone pls explain to me this code ... the depth for drill is -4mm but i cant see it between the g83 and g80 code ... so im wondering why?? this program is for vertical mill hurco vmx24
%
N100 G54 G17 G71 G75 G90
N102 G0 T2 M6
N104 G0 X0. Y0.
N106 S1273 M3
N108 Z10.
N110 Z2.
N112 G83 X0. Y0. Z17.3519 Z2. Z2. F38.2
N114 Y20. Z17.3519
N116 Y55. Z17.3519
N118 Y95. Z17.3519
N120 Y135. Z17.3519
N122 Y175. Z17.3519
N124 Y210. Z17.3519
N126 Y230. Z17.3519
N128 X22. Y210. Z17.3519
N130 Y175. Z17.3519
N132 Y135. Z17.3519
N134 Y95. Z17.3519
N136 Y55. Z17.3519
N138 Y20. Z17.3519
N140 G80
N142 Z10.
N144 M5
N146 G0 M25
N148 M2
E

[JWK42]

This is for a Haas VMC
I think this is the same as a Fanuc style drill cycle


G98 in N110 causes the drill to retract to the initial point of Z2. in N100 between holes. This is used to clear clamps or other obstructions
Change G98 to G99 and the retract is to the R.1 in N110 or Z.1 between holes.
The Z-.75 in N110 is the bottom of the hole.
The Q.245 in N110 is the peck amount.


%
O5555 (TEST 123)
N10 ( WRITTEN 06-16-2008 10:44:32 )
N20 (MODIFIED 06-16-2008 10:46:54)
N30 G17 G54 G90
N40 G40 G49 G80
N50 G53 G00 Z0.
N60 G53 G00 X-16.0 Y0.
( TOOL 1 IS A DRILL )
N70 T1 M6
N80 S3000 M3
N90 G54 G00 G90 X0. Y2.
N100 G43 Z2. H1 D1 M8
N110 G83 G98 X0. Y2. R.1 Z-.75 Q.245 F3.
N120 X2.
N130 X4.
N140 X6.
N150 X8.
N160 X10.
N170 X12.
N180 X14.
N190 Y4.
N200 X12.
N210 X10.
N220 X8.
N230 X6.
N240 X4.
N250 X2.
N260 X0.
N270 G80
N280 G00 Z2.
N290 G53 G00 Z0. M9
(UNLOAD HERE)
N310 G53 G00 X-16. Y0.
N320 M30 (END OF MAIN PROGRAM)
%

[chrisryn]

Originally Posted by simpy can someone pls explain to me this code ... the depth for drill is -4mm but i cant see it between the g83 and g80 code ... so im wondering why?? this program is for vertical mill hurco vmx24 % N100 G54 G17 G71 G75 G90 N102 G0 T2 M6 N104 G0 X0. Y0. N106 S1273 M3 N108 Z10. N110 Z2. N112 G83 X0. Y0. Z17.3519 Z2. Z2. F38.2 N114 Y20. Z17.3519 N116 Y55. Z17.3519 N118 Y95. Z17.3519 N120 Y135. Z17.3519 N122 Y175. Z17.3519 N124 Y210. Z17.3519 N126 Y230. Z17.3519 N128 X22. Y210. Z17.3519 N130 Y175. Z17.3519 N132 Y135. Z17.3519 N134 Y95. Z17.3519 N136 Y55. Z17.3519 N138 Y20. Z17.3519 N140 G80 N142 Z10. N144 M5 N146 G0 M25 N148 M2 E

Since you Z depths are a positive number and there at 17.3519 I would assume that the program zero for z is below the surface in which your drilling. eg. All the tools have been touch off the table and the program is not utalizing the g54 z fixture offset. I have worked for companies that program that way. If you don't realize that aspect of the setup the numbers can throw you off.

[extanker59]

but he's rapiding to Z10. and Z2. before starting to drill so the numbers aren't adding up to me.
Simpy, is that a working program? I see a lot I'd change but I've never run a Hurco. What's with the multiple Z commands on the same line? Why call the same Z depth line after line? Where's the tool length call? Hurco sees the tool and so knows the offset?

[chrisryn]

Originally Posted by ccordova@atlass but he's rapiding to Z10. and Z2. before starting to drill so the numbers aren't adding up to me. Simpy, is that a working program? I see a lot I'd change but I've never run a Hurco. What's with the multiple Z commands on the same line? Why call the same Z depth line after line? Where's the tool length call? Hurco sees the tool and so knows the offset?

I didn't look that closely. I saw the positive z moves and took that as the first problem. Your right. Is this a proven program?

[simpy]

hmm i must say i only run 3d programs on hurco whitch i create in mastercam and everything goes just fine .... i never did a drill,, it is nothing special in dialog, but now i wanted to do drill cycle in mastercam i have set the z-4 but when i post i dont see any z-values. i will attach also a mc9 file so if anyone knows where is my mistake i would be happy becouse i cant find it. The job can be done but i just want to do that with mastercam.

[simpy]

here is the mc9 file

[simpy]

Originally Posted by chrisryn I didn't look that closely. I saw the positive z moves and took that as the first problem. Your right. Is this a proven program?

and btw i will test this program tomorow so we will know is it a proven program

[dpark1]

I posted with fanuc post and this is what I got.



(PROGRAM NAME - PLOCICA GINEX)
(DATE=DD-MM-YY - 16-06-08 TIME=HH:MM - 17:56)
N100G21
N102G0G17G40G49G80G90
/N104G91G28Z0.
/N106G28X0.Y0.
/N108G92X0.Y0.Z0.
( 5. DRILL HSS TOOL - 2 DIA. OFF. - 2 LEN. - 2 DIA. - 4.5)
(RUPA FI4,5)
N110T2M6
N112G0G90X0.Y20.A0.S750M3
N114G43H2Z10.
N116Z2.
N118G99G83Z-7.352R2.Q2.F50.
N120Y55.
N122Y95.
N124Y135.
N126Y175.
N128Y210.
N130X22.
N132Y175.
N134Y135.
N136Y95.
N138Y55.
N140Y20.
N142G80
N144Z10.
N146M5
N148G91G28Z0.
N150G28X0.Y0.A0.
N152M30

[Mike Stevenson]

But this is how a hurco G83 works:

T1M6
G0 G90 X0 Y0
Z.1
G83 X0 Y0 Z.5 Z.1 Z.05 F5.0
X1.Y1.
etc.

What it means is this:

from X0 Y0 Z.1 go Z minus .5 with .1 the first peck and .05 as the last.

Very reminiscent of the bridgeport boss series coding.

[simpy]

Originally Posted by Mike Stevenson But this is how a hurco G83 works: T1M6 G0 G90 X0 Y0 Z.1 G83 X0 Y0 Z.5 Z.1 Z.05 F5.0 X1.Y1. etc. What it means is this: from X0 Y0 Z.1 go Z minus .5 with .1 the first peck and .05 as the last. Very reminiscent of the bridgeport boss series coding.

heyy that is what was confusing me the two values z in line with g83 ,,,, i believe the same way and we will try this program in practice today on hurco wmx24 and i will reply what happened thx u all for u'r reply