Lb3000exII c axis feed rate conversion

[rdnck68]

Currently in the process of training my minion operator (button pusher) my okuma lb3000exII myw. I have been using diamond abrasive cutters and rec diamond cut routers with excellent success and excellent tool life. Only thing is this guy can't write his own programs so I have written a series of 10 macro sub programs for him and I can not figure out a good way to calculate feedrates for c axis. Such as a formula I could use in the program as a constant so if he wanted to feed 50 ipm he could could change variable #23 TO V23=50. But have a max feedrate so machine doesn't alarm out with a Mcs max diff alarm.
My machines max deg. Per for subspindle is somewhere around 3000 not sure about main spindle honestly...

My sample code for program looks like

G0 x=v1 z.025

NRUFF
G01 x=v1 z.0 C180. F=v23(math function here)
G01 x=v1 z-.025 C0.

VZSHZ=VZSHZ -.05
IF [VZSHZ GE V25] GOTO NRUFF

VZSHZ=0

GO X=V1+.025 Z.025

Vzshx=vzshx-v27
If [VZSHx GE V29] GOTO NRUFF

Not sure if above is even correct as I am exausted and very distracted with getting children ready for bed but you should get the idea

Thank you ahead of time any help or ideas is greatly appreciated.








BUT what could I put in the program to calculate ipm to degrees per minute using v23 so he doesn't have to try to wrap his head around calculating it.... he has problems calculating surface feet and figuring out angles. Unfortunately I'm having surgery and won't be there to hold his hand for 3 months and would really like to make sure these programs are fool proof (he could f up a wet dream).... I have even set it up where he has barcodes to scan for each drawing number and it automatically calls up programs work offsets and any setup instructions for all existing programs. Just need to come up with a solution to feed rate issue for live tools in New programs otherwise I will come back to a pile of broken tools lol.







Sent from my SM-G930T using Tapatalk

Similar Threads:

• Need Help!- 4th axis feed rate question
• Need Help!- Post processor 4th axis feed rate
• 4th Axis Feed Rate Problem
• Need Help!- Fanuc-mill, Feed rate 4th axis???
• Z-axis feed rate

[deadlykitten]

I have been using diamond abrasive cutters and rec diamond cut routers with excellent success and excellent tool life

hy rdnck so you have experience in grinding ? or something else ? and how did you endup on the lb3000 ? also preparing others ?

But have a max feedrate so machine doesn't alarm out with a Mcs max diff alarm

i dont know about feed limitation; so far i can only put a limit on the spindle ( G50 )

My machines max deg. Per for subspindle is somewhere around 3000 not sure about main spindle honestly

what is max deg ?

F=v23(math function here)

... not a math function but an initialization based on a variable

G01 x=v1 z.0 C180. F=v23(math function here)
G01 x=v1 z-.025 C0.

feed among syncro ZC involves a bit more

at this moment i can only share this without explanations :

    LV05=129600*LV02*LV02
    V15=SQRT[[LV05+250000*LV03*LV03]/[LV05+LV01*LV01*LV03*LV03*9.8696044]]*LV04

pls wait until tomorow, and i will fully explain it to you, since my stuff is @ work ... and i am not there

do you really need to go syncro ZC? it is easier if you can avoid this

as i can see the syncro is looped, so maybe you can avoid it, and use it only for last pass ?

please share image or something, so to better understand your desire

Vzshx=vzshx-v27

vzshx works, but is a tricky variable ... is ok that it is wiped on reset, otherwise you may disaling the entire cnc

i hope you know what you do

Not sure if above is even correct as I am exausted and very distracted with getting children ready for bed but you should get the idea

me neither code is incomplete and i can not figure it out

please share a drawing or something so to see the part / machining that you are tring to achieve

also, you are missing in your post G137 and G95/G94, but maybe they are there inside the main program

... drawing please kindly !

[deadlykitten]

BUT what could I put in the program to calculate ipm to degrees per minute using v23 so he doesn't have to try to wrap his head around calculating it.... he has problems calculating surface feet and figuring out angles. Unfortunately I'm having surgery and won't be there to hold his hand for 3 months and would really like to make sure these programs are fool proof (he could f up a wet dream).... I have even set it up where he has barcodes to scan for each drawing number and it automatically calls up programs work offsets and any setup instructions for all existing programs. Just need to come up with a solution to feed rate issue for live tools in New programs otherwise I will come back to a pile of broken tools lol.

i did not see this from the 1st time

degrees/minute is possible to be coded, but is not a default behaviour

once C axis receives a feed comand, it is :
... angles with feed dependant on X axis position at least, if not Z, or Z&X (G01)
... coordinates with feed constant ( G10* )

degrees per minute is not impossible, but it is dependant on other stuff, like 360degress=500mm and so on

go take your surgery read 1st few pages from the programing manual

i can post them for you ...

[deadlykitten]

in attached archive you have manual pages about feeding C axis and my xls file that i use for such things

lately i simply compute those feeds inside a procedure, but it is build and verified with that xls

what surgery do you have ? ... it seems something light, if you worry more about codes than yourself

[deadlykitten]

what surgery do you have ?

i got it : you are replacing a grinding panel with an osp

[rdnck68]

i got it : you are replacing a grinding panel with an osp

My left elbow.... right elbow was last year lol this is actually a running program that runs flawlessly making 1000 parts per month. You are sort of correct in saying grinding.... I work with fiberglass composites.... this material is g11 the harder brother of g10/fr4... and as far as the cz move.... just imagine me using an endmill and using it on the OD of the part using the above code.... would be a ruff od turning cycle using an endmill... I will try to come up with some sort of visual that would not get me in any trouble for industrial espionage lol

Sent from my SM-G930T using Tapatalk

[deadlykitten]

I will try to come up with some sort of visual that would not get me in any trouble for industrial espionage lol

you may not get in trouble by sharing images ... anybody can buy a product-disansemble-reverse engineer

idea is not to protect the product or the location where it is manufactured, but how it is done

one may get in trouble by asking for crafting tips for a protected product on a public forum

good luck with the elbow

[deadlykitten]

pls wait until tomorow, and i will fully explain it to you, since my stuff is @ work

hy rdnck here it is :

OFCZ ( feed 4 syncro C&Z : LV01=diameter LV02=|dZ| LV03=|dC| LV04=f_G95 )

    LV05=129600*LV02*LV02
    LV00=SQRT[[LV05+250000*LV03*LV03]/[LV05+LV01*LV01*LV03*LV03*9.8696044]]*LV04

RTS ( . . . . . . . . . . . . . . . . . . . . . . . . . . . . . )

that procedure returns feed for syncro C&Z, while X is constant; it is ok for your code please note that dC and dZ should be passed away in absolute value; however, even if this is omited, there are no worries, because those values are computed inside calculations at their square value : LV02*LV02 will eliminate dZ sign issues, and same, LV03*LV03 will fix dC sign issues

i can make it deliver feed in degrees/minute ( or rpm ), as you wish to go this way, i may ask for draw and machinig aspects

also, you are missing in your post G137 and G95/G94, but maybe they are there inside the main program

also M15 / M16 is not there you may not issue a direct feed on C axis without specifing default rotation, unless :
... default machine state does the job ( that is M15 )
... part is simetrical, and really does not matter if you go one way or another ( your code is like this ); in this case, however, caution to recut, thus chips falling down or in front of the tool kindly !

[rdnck68]

hy rdnck here it is :

OFCZ ( feed 4 syncro C&Z : LV01=diameter LV02=|dZ| LV03=|dC| LV04=f_G95 )

    LV05=129600*LV02*LV02
    LV00=SQRT[[LV05+250000*LV03*LV03]/[LV05+LV01*LV01*LV03*LV03*9.8696044]]*LV04

RTS ( . . . . . . . . . . . . . . . . . . . . . . . . . . . . . )

that procedure returns feed for syncro C&Z, while X is constant; it is ok for your code please note that dC and dZ should be passed away in absolute value; however, even if this is omited, there are no worries, because those values are computed inside calculations at their square value : LV02*LV02 will eliminate dZ sign issues, and same, LV03*LV03 will fix dC sign issues

i can make it deliver feed in degrees/minute ( or rpm ), as you wish to go this way, i may ask for draw and machinig aspects



also M15 / M16 is not there you may not issue a direct feed on C axis without specifing default rotation, unless :
... default machine state does the job ( that is M15 )
... part is simetrical, and really does not matter if you go one way or another ( your code is like this ); in this case, however, caution to recut, thus chips falling down or in front of the tool kindly !

Imagine a ring that is what the part looks like 90 degree face on one side and 10 degree face on the other 4.375 od and 3.0 id.... starts out as a 4.625 x 4.625 x .625 thick square blank loaded in subspindle in an expansion collet with custom made jaw pads to hold the part securely. A 90degree live facing tool with a .500 rec diamond cut router with 18 "flutes" comes in roughs od and id. With code similar to what I shared above using x shift or z shift with an if then statement. Finishes face and od with 55 degree dcmw pcd diamond insert. Subspindle then transfers to custom made jaw pads for main spindle finishes ID with dcmw pcd boring bar and puts the 10deg face using a .375 4flute endmill in an adjustable live angle tool. PART then is pushed into the part basket and machine is ready for next part.

Sent from my SM-G930T using Tapatalk

[rdnck68]

Imagine a ring that is what the part looks like 90 degree face on one side and 10 degree face on the other 4.375 od and 3.0 id.... starts out as a 4.625 x 4.625 x .625 thick square blank loaded in subspindle in an expansion collet with custom made jaw pads to hold the part securely. A 90degree live facing tool with a .500 rec diamond cut router with 18 "flutes" comes in roughs od and id. With code similar to what I shared above using x shift or z shift with an if then statement. Finishes face and od with 55 degree dcmw pcd diamond insert. Subspindle then transfers to custom made jaw pads for main spindle finishes ID with dcmw pcd boring bar and puts the 10deg face using a .375 4flute endmill in an adjustable live angle tool. PART then is pushed into the part basket and machine is ready for next part.

Sent from my SM-G930T using Tapatalk

Also no problems with chips.... it's dust so recut is not an issue

Sent from my SM-G930T using Tapatalk

[deadlykitten]

hy into attached image i tried to draw the stock and the part

i am an mm guy ... i can not full draw the part, because i dont undersand this :

Imagine a ring that is what the part looks like 90 degree face on one side and 10 degree face on the other

so you wish to rewrite the code for the roughing operation with the z18 0.5"dia tool ? pls share full code for this operation, and intermediate dimensions : before and after this operation; i guess that before is the stock, thus no worries, but i need to know the final shape, thus what the code delivers

with exact data i can give you an exact code

---

otherwise, i can give you a generic procedure that delivers rpm_feed for helix cutting, that you simply use as you like; in this case, please provide what inputs and outputs you wish for kindly !

your code so far :

    G0 X+V1 Z0.635

    NRUFF G01 X+V1 Z.0     C180 F+V23
          G01 X+V1 Z-0.635 C0
          VZSHZ = VZSHZ - 1.27
    IF [VZSHZ GE V25] NRUFF

    VZSHZ=0

    G0 X+V1+0.635 Z0.635

    VZSHX=VZSHX-V27
    IF [VZSHX GE V29] NRUF

[deadlykitten]

otherwise, i can give you a generic procedure that delivers rpm_feed for helix cutting

[ variant 1 : this version messes with inputs for a classical syncro CZ cut, so to deliver a desired rpm among C axis ]

code is as follows :

- main headquarter

  ( intro )

    G50 S2000
    M867 ( cas          : off )
    M216 ( rapid ignore : on  )
    LVXP = VPVLX - VBZOX

  ( main )

    NN01    CALL OS01

    G00 X+LVXP-VETFX Z100-VETFZ

  ( outro )

  ( M84  )
  ( G195 SP=1 )
  ( M215 ) ( rapid ignore : off )
    M866   ( cas          : on  )
    M02

- soubroutine :

OS01

G00 X+LVXP-VETFX Z100-VETFZ
M110 T101010 M66 ( M08 )
G00 X100 Z0 SB=100 M13

CALL OFCZ LV01=VSIOX LV02=10 LV03=180 LV04=18*0.085*10 LV06=50 

V1=0
G91
NHERE G01 X0 Z-10 C180 F+V15
          X0 Z-10 C180
      V1=V1+1
IF [ V1 LT 5 ] NHERE
G00 X=VSIOX+0.6 Z=VSIOZ+0.3 G90

M12

RTS

 ( . . . . . . . . . . . . . . . . . . . . . )


OFCZ ( feed 4 syncro C&Z : LV01=diameter LV02=|dZ| LV03=|dC| LV04=f_G95 LV06=desired_rpm < 200 )

    LV03=ABS[LV03]
    LV06=360*SQRT[7615.4355/100000000*LV01*LV01*LV03*LV03+LV02*LV02]*LV06/LV03 ( F reloaded )
    SB=LV06/LV04                                                     ( update live tool rpm )

    LV05=129600*LV02*LV02
    V15=SQRT[[LV05+250000*LV03*LV03]/[LV05+LV01*LV01*LV03*LV03*9.8696044]]*LV04

RTS

(     5 loops in  7.15 seconds )
( 41.96 loops in 60    seconds )

after testing, it did not delivered 50 rpm but cca42 pretty close, considering that C axis does not work like the S axis

i considered a feed of 18*0.085 for that z18 tool ( hope i got it right ), and that feed i have multiplied by 10

this method works, thus numbers get well, but in reality it may spin your live tool like crazy

however, maybe your desired inputs will deliver a normal rpm

if you provide desired feed G95 for the tool + desired rpm for the spinde, than i may simulate and see what rpm will be required for the live tool

if values are high,or as you wish, you may consider M153 ( M-tool spindle interlock release / interlock OFF), which allows the cnc to rotate S and M separated, each one with its own rpm kindly !

[deadlykitten]

[ more variants packed ]

hy pls check attachement

os01 : syncro CZ that delivers rpm on C axis ( same stuff as the one from previous post )

os02 : os01 with less movements : a revolution is no more cut by 2 arches, but by almost a full circle; please notice that feed is calculated for 360 degress, while G01 is issued for 360-0.001; yup, there is a difference, but is not relevant a cnc with less syncro capabilites than an Okuma may deliver things even worse

os03 : uses M153, so to allow spining bought M and S axis, each one with its own desired rpm ( i was told about this trick by mr Wizard )

---

bought os01 and 02 use syncro CZ

gap between expected_duration and real_duration increases when a higher rpm is desired ( encoders cinematics drops in )

anyway, real_duration is always < expected_duration; kindly !