G60 - single direction positioning

[kccadcam]

Where's the best place to insert this?

The postion move before the canned cycle? (G81,etc.)

Would the misc. integers be the easiest way to call this? Do I need G64 to cancel? Never dealt with it before.

[Quickmike]

I believe this is not modal; it needs to be inserted at each location, HTH

[specv]

Actually G60 is modal, G64 cancels it.

insert it on the positioning line then G64 before you start the next op.

[specv]

oops I was thinking G61, disregard my last statement

[kccadcam]

I found more info,

G60 is modal, same as G61.

G64 cancels both.

Must turn on at first position and off at G80.

 

What will be the easiest way to invoke this?

[Quickmike]

On a fanuc 11m I believe it is just one time shot per entry. This can be checked by trying it with the rapid rate down all the way. Better yet try turning single block on. I think this is how I figured it out when I needed some accurate bore locations relavent to each other on a older machine. Please post the results when you find out. Inquiring minds want to know. Then maybe I'll be able to remember better this time.

[crazy^millman]

Yes Kevin this is easy to do. Have to decide if you want this as a call it when you need it or hard coded in the post to always come out. I will try to show you the Misc way. Look here in the post:

code:

---

pdrlcommonb #Canned Drill Cycle common call, before

if sav_dgcode = 81,

[

result = newfs (two, zinc)

if drillcyc = three, drlgsel = fsg1(-ss) + drillcyc * two

else, drlgsel = fsg2(dwell) + drillcyc * two

if initht <> refht, drillref = zero

else, drillref = one

prv_refht_a = c9k

prv_refht_i = c9k

prv_dwell = zero

]

if cuttype = three, sav_dgcode = gcode

else, z = depth

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

pcom_moveb

feed = fr_pos

comment

pcan

#5 axis must map the true Z, correct Z calculation here

if cuttype = three,

[

prv_zia = zabs + (-depth) + initht

zia = fmtrnd(zabs)

zinc = zia - prv_zia

]

if mi8 = 1, "M60" , e

 

pcanceldc #Cancel canned drill cycle

result = newfs (three, zinc)

z = initht

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

pxyzcout

!zabs, !zinc

prv_gcode = zero

pcan

pcan1, pbld, n, "G80", strcantext, e

pcan2

if mi8 = 1, "M64", e

---

Do not have at home but think this might work. If you want to get fancy can change the TXT for the post and have the Misc look like a question or something to your liking. If you want this hard coded then you just take out the if mi8 = 1, on both and will be there for all. This way is for all drilling routines and all you have to do it use the mi8 to turn it on or off wit hthe vaules of 1.

[kccadcam]

Thanks Ron, Easy enough... Quickmike I'll let you know how this works out.

[Threept82]

Ron.

Where do I tell MC that mi8 = 1 or mi8 = 0

[Threept82]

Never mind, I got it

[kccadcam]

Ok, have been tweaking on this machine (Matsuura H600 Horizontal) for awhile, and I think I've got it.

 

code:

---

 M6 (#3 CENTER DRILL  TOOL-428)

M22

G90

M21

G60

G0 G17 G90 X-5.8125 Y-4.9199 S1749 M3 T411

G43 H428 Z8. /M8

M50 (SPINDLE COOLANT ON)

G81 Z6.665 R6.84 F3.

G80

G64

M9

G94

G91 G28 Z0 M5

G49

M52 (AIR BLAST ON)

G4 X9.5

M53 (AIR BLAST OFF)

(BREAK CHECK)

G65 P9301 D0.015 H428

M1

M6 (3.3MM MITSUBISHI CARB COOLANT THRU DRILL TOOL-411)

M22

G90

M21

G60

G0 G17 G90 X-5.8125 Y-4.9199 S3500 M3 T426

G43 H411 Z8. /M8

M50 (SPINDLE COOLANT ON)

G81 Z6.59 R6.84 F9.

G80

G60

G81 Z5.7517 R6.84 F9.

G80

G64

M9

G94

G91 G28 Z0 M5

G49

M52 (AIR BLAST ON)

G4 X9.5

M53 (AIR BLAST OFF)

(BREAK CHECK)

G65 P9301 D0.015 H411

M1

---

It's working quite well now other than transform toolpath calls a new canned cycle for every part

[crazy^millman]

Funny I just had to do this again 13 years later. I did a search with google and see what I could find to use G60. I must be slipping not remembering I helped someone so long ago to do this very thing again.

[Leon82]

Do you happen to know if this is a pay for option on FANUC or you just need to enable a parameter?

[crazy^millman]

4 minutes ago, Leon82 said:

Do you happen to know if this is a pay for option on FANUC or you just need to enable a parameter?

For this machine it was an option from the builder. Each MTB does things a little differently you would need to get a hold of your MTB and see what they say. Not an expensive option if it is a chargeable one.

[huskermcdoogle]

Look at parameter 5440.  If they are set to zero it won't do anything on those axes.