HELP with drilling cycle

[camgeneration]

can someone please tell me why if i run this code alone the drill goes to the initial height between holes(1"), but if part of a bigger program is stays at final z depth between holes, (scraps centerdrill and part)

N1 G00 G17 G20 G40 G80 G61.1 G90

N9010 M01

N9011 M08

N9012 T1 T3 M06 (DEFINE TOOL NAMES)

N9013 (MAX - Z1.)

N9014 (MIN - Z-1.412)

N9015 G00 G90 G55 X1.375 Y-1.188 S10000 M03

N9016 G43 H1 Z1.

N9017 G98 G82 Z-1.412 R-1.212 F30.

N9018 X.5

N9019 X4.33 Y-1.718

N9020 Y-.588

N9021 X6.017 Y-1.718

N9022 Y-.588

N9023 G80

N9024 M09

N9025 M05

I am running a mazak nexus 510c hs

[Guest]

There is nothing in that code or anycode that I am aware of will make a drill stay at the final Z height. The retract motion is built into the machine canned cycle, you simply define where it goes.

 

Make sure the "use clearance only on first and last holes" is unchecked and make sure your retract plane and clearnace heights will clear the part.

[Thad]

The exact same code does two different things or can you post some code for us when it's in a bigger program?

 

Thad

[Rick Henrickson 65]

depends on G98 or G99 which it picks up with your retract and clearance planes or if you have a jump in the points page

[Hardmill]

G98 will retract to 1.0

G99 will retract to your "R" plane ( R-1.212 )

 

 

PEACE

[jeff]

Camgeneration...what control do you have?

[camgeneration]

here is some of the code from before the drill cycle of the bigger program(it's part of a 3d program so i'm only posting the tail end.

N8995 X5.9211 Z-1.5833

N8996 X5.9029 Z-1.5793

N8997 X5.8849 Z-1.5747

N8998 X5.8671 Z-1.5694

N8999 X5.8495 Z-1.5634

N9000 X5.8321 Z-1.5568

N9001 X5.8284 Z-1.5554

N9002 X5.8246 Z-1.5544

N9003 X5.8208 Z-1.5536

N9004 G00 Z-1.4535

N9005 Y-2.4377 Z.5

N9006 Y-2.4378

N9007 M09

N9008 M05

N9009 G91 G28 Z0.

N9010 M01

N9011 M08

N9012 T1 T3 M06 (DEFINE TOOL NAMES)

N9013 (MAX - Z1.)

N9014 (MIN - Z-1.412)

N9015 G00 G90 G55 X1.375 Y-1.188 S10000 M03

N9016 G43 H1 Z1.

N9017 G98 G82 Z-1.412 R-1.212 F30.

N9018 X.5

N9019 X4.33 Y-1.718

N9020 Y-.588

N9021 X6.017 Y-1.718

N9022 Y-.588

N9023 G80

N9024 M09

N9025 M05

N9026 G91 G28 Z0.

N9027 M01

N9028 M08

N9029 T3 T2 M06 (DEFINE TOOL NAMES)

N9030 (MAX - Z1.)

N9031 (MIN - Z-2.4691)

N9032 G00 G90 G55 X4.33 Y-.588 S2000 M03

N9033 G43 H3 Z1.

N9034 G98 G73 Z-2.4691 R-1.212 Q.25 F10.

N9035 Y-1.718

N9036 X6.017 Y-.588

N9037 Y-1.718

N9038 G80

N9039 M09

N9040 M05

N9041 G91 G28 Z0.

N9042 M01

N9043 M08

when i just pull the code out of the big program and run it by it's self, it does as it should, but as run as above (the same code rember) it stays at z -1.412, the stock starts at z-1.312. I am looking right at the programming manual from mazak and it looks right????

[camgeneration]

fusion 640m, only a year old.

[Matthew]

line N9017, That G82 is to allow the tool to dwell at the bottom of the hole, but you don't have a value specified for dwell. Maybe change it to G81 or add a dwell value, I think it would be 'P'.

[camgeneration]

it was originaly g81, which mazak calls spot drill, and only allows x,y,r,z doesn't even list feed rate as an option. I changed to g82 which is listed as drilling with the options for dwell and feedrate override for a final distance (I). both g81 and g82 do the same thing on the machine, ok by itself, milling across the part untill the tool breaks if part of a bigger program. g82 actually has a extra variable D which is distance from R to start of cutting. It is allowed to be omitted, and since i don't know how to modify the post to add this distance variable, i was allowing the start drilling point and the reference plane to be the same. just set it above the surface .1".

[camgeneration]

found the problem, the filter put in a g18 in the 3d area, and it never reset to g17 before the drilling.

[camgeneration]

I had the support arcs in the xz and yz unchecked in the controll definition, why would it allow it to output g18 and g19(i am assuming the g19) at all?

[Rick Henrickson 65]

hey camgeneration refer to G17, G18, G19 thread

[Allan Brown]

Looks like an mpmaster-based post. I'd like to get your full mcx or Mc9 file to test on our latest to see about ensuring G18 gets set back to G17.

[Fig sign]

N9003 X5.8208 Z-1.5536

N9004 G00 Z-1.4535

N9005 Y-2.4377 Z.5

N9006 Y-2.4378

~~~~~~~~~~~~~~~

The reason is very simple .

G00 cancels the drill cycle same as g80

Beware ..

 

 

Teh oldtimer .

You need to learn coding

[camgeneration]

iskander, the drilling doesn't start untill line 9012. The code you refering to is part of a 3d program. you need to learn to read the posts before you start telling people to learn coding.

[Fig sign]

My fault .

Next time post up 300 lines of code ,PLZ

[Fig sign]

No ,really ,it is my fault .

Sorry .

I was in hurry ,working ,some heavy stuff and very

silly too (designer is dumba$$ )

I had no time to read very nessasary information and replies ,I thought this is a drill code ,why on earth the guy would post nonreliable code .

Next time I would be more accurate .

And cautious .

 

Sorry one more time .

My fault .

Nevermore

[Fig sign]

can someone please tell me why if i run this code alone the drill goes to the initial height between holes(1"), but if part of a bigger program is stays at final z depth between holes, (scraps centerdrill and part)

~~~~~~~~~~~~~~~~~~~

But if this is g18 it will move on Y axis

BTW ,in my deckel-maho you need to call g18 any time after the toolchange due to some parameter ,THAT ALLWAYS RESET IT TO G17 AT TOOLCHANGE (M6 actually macro program ,so no wonder )

May be you have such an option on your MAZAK TOO ?

[camgeneration]

I will look to see if there is a parameter, i kind of doubt it though, it definitly does not reset now. i think the machine gets confused with a g18 and a drill cycle, doesn't do it either way right. Didn't want to be nasty either but after a lot of stress and time getting the post edit free, and to have tools and workpieces scraped i was not a happy camper. it all comes out of my wallet being my own shop, and times for me are hard enough already without extra expenses and time.

[Rick Henrickson 65]

Might want to check your parameter book

 

F92 bit 6

0=G17, G18, or G19

1=z axis fixed

[htm01]

i had a fadal post that left G18 or G19 active,would try to drill in x or y.thats why i put G17 in safe start block

[Rick Henrickson 65]

if it is not resetting the g17 refer to the thread i was talking about earlier g17, g18, g19

may need to add to your post

[camgeneration]

cascadeclimbr, right on the parameter, why it would not be set by default on a 3 axis machine to begin with i have no idea. I was planning to fix the post anyway but i will also change the parameter, can't be too careful.