[peaceandcalm]

Hi, I got Miyano BND 51s5 with Fanuc 21i-T controler
been keen to do ridgid tapping
I performed the command

G97 s1000 M3
G84 z-10 F2.
G80
G0 x100.0 z100.0

and wha happend is acually the tool went right in M3 and right out with M4
but what was missing is that when the tool reached to z-10 the sppindle took a long time to stop thus breaking the tool and didnt syncronize the feed with the spindle speed usually with proper ridgid tapping it should slow down when it starts reaching the z-10 then turn to M4 but what happend is the tool reached to z-10 first then the spinde stoped after reaching to z-10 ...is that paramerts problem? or its simple missing hardware piece on board?

i tried to put M39 (the 2200 parameter is set to 39, so I tried using
M39 s1000
g84 z-10.
etc..
but the spindle refuses to turn on M39 command..
anyone can help?

[fordav11]

Parameter 2200 is not relating to Rigid Tapping.

Generally to set Rigid Tapping Mode you should put an M29 S*** before the G84

M29 S1000
G84 Z-10 F2.
G80
G0 X100.0 Z100.0


From the manual.....

The M code used to specify rigid tapping mode is usually set in parameter
No. 5210. The M code is judged to be 29 (M29) when "0" is set.
To use an M code whose number is greater than 255, Specify the code
number with parameter No. 5212.

[dcoupar]

Per the 21iT-A and 21iT-B Parameter Manuals:

If prm 5200 bit 0 = 0, then the M-code for Rigid Tapping is set in prm 5210. If 5200 bit 0 = 1 then Rigid Tapping mode is not set by M-code.

[peaceandcalm]

thank you for your reply
I have 2 main coolants on M08 and M28 for turning on and M09 and M29 to turn it off..
so how can i use M29 to turn the spindle on when its for coolant?

My 5210 says 39...
so i assume M39 s1000? if so the spindle doesnt turn on M39 command..
and 5200 bit 7 is set to 1, i can set it to zero if i wish but M39 doesnt turn the spindle on it just sits there dong nothing...

[angelw]

thank you for your reply
I have 2 main coolants on M08 and M28 for turning on and M09 and M29 to turn it off..
so how can i use M29 to turn the spindle on when its for coolant?

My 5210 says 39...
so i assume M39 s1000? if so the spindle doesnt turn on M39 command..
and 5200 bit 7 is set to 1, i can set it to zero if i wish but M39 doesnt turn the spindle on it just sits there dong nothing...

If you're testing your program in single block, the block containing the synchronize code (M39 in your case) does not start the spindle. In all cases of rigid tapping I've seen, the spindle starts when the G84 block is executed and stops upon its return to the R level after completing the tapping operation on the current hole.

Are you confusing bit 0 and bit 7 of #5200, or are you just making the observation that bit 7 is set to 1.


Regards,


Bill

[peaceandcalm]

If you're testing your program in single block, the block containing the synchronize code (M39 in your case) does not start the spindle. In all cases of rigid tapping I've seen, the spindle starts when the G84 block is executed and stops upon its return to the R level after completing the tapping operation on the current hole.

Are you confusing bit 0 and bit 7 of #5200, or are you just making the observation that bit 7 is set to 1.


Regards,


Bill

hi, first i tried without single block still the spindle wont turn on M39 command
and as far as i know Bit 0 is on the far right like this?

#7 #6 #5 #4 #3 #2 #1 #0
so in this case bit 7 on mahcine default is set to 1
i can change that to 0 ofcourse but what would that do?
all i know if i put that to zero then i have to use M39 if i leave it to 1 then i dont have to use M39 s1000 is that correct?

in anycase regardless if that is set to 1 or 0 spindle wont more on M39 command..

[Al_The_Man]

Not sure about the i series, but do you have an encoder on the final spindle shaft?
Al.

[peaceandcalm]

what is encoder?

[angelw]

hi, first i tried without single block still the spindle wont turn on M39 command
and as far as i know Bit 0 is on the far right like this?

#7 #6 #5 #4 #3 #2 #1 #0
so in this case bit 7 on mahcine default is set to 1
i can change that to 0 ofcourse but what would that do?
all i know if i put that to zero then i have to use M39 if i leave it to 1 then i dont have to use M39 s1000 is that correct?

in anycase regardless if that is set to 1 or 0 spindle wont more on M39 command..

Yes you're reading it correctly, bit 0 is the right most bit in the byte. However, its bit 0 of #5200, not bit 7, that determines if an M code is used for rigid tapping, and should be set to 0 if the M code defined in #5210 is to be used.

Regards,

Bill

[Al_The_Man]

Feedback device to synchronize the Z with the spindle revolutions.
The earlier Fanuc also required an option parameter for rigid tapping.
Al.

[peaceandcalm]

yes bit 0 is set to 0
and i am not sure if i have this feedback device on main spindle, how can you tell?
My G84 works perfect except for that suncro problem, so by the sound of it i might not have that device installed? is that a chip on board? or accual hardware?

[Al_The_Man]

Most lathes DO have an encoder, you need it for CSF and Feed/rev.
But I know the older Fanuc's required the option parameter for rigid tapping.
Al.

[peaceandcalm]

when you talking about an encoder, is software? or a chip hardware?
can i edit any paramerts to fix this? i do have all the usuall parameters from 5200 all the way down but somehow they all set to zero..except 5210 which is 39...

[Al_The_Man]

It is a hardware item, but I would be surprised if you did not have on that make of lathe.
http://www.google.ca/search?q=rotary...w=1481&bih=938
The option parameters are accessible by password on the i series, these are 9000 series options which Fanuc charge for.
(PM sent)
Al.

[sinha_nsit]

If 5200 bit 0 = 1 then Rigid Tapping mode is not set by M-code.

and G84/G88 would always work in rigid mode, provided rigid-tapping option is available.

[hitachibos]

ok here is something to think about. this is a lathe. Most Lathes do NOT have rigid tapping on main or sub spindles. most are belt driven. not knowing if you have a 3 jaw, 4 jaw, collet nose or face plate. how does a machine builder know what kind of acceration/deceleration needed based on the weight of your part and how your holding it to stop a slippery belt in time to reverse. if you get it right once it wont be the same on the next part.

get yourself a floating holdder and use it.

If it is a live tool then dont forget about Plane selection G17-(z axis depth of hole) G18-(y axis depth) G19-(x axis depth)

Without proper plane selection the tap will just sit at the R-plane waiting forever
(almost always without alarms)

IF you really want to continue on the main or sub spindle you still have to change to G17 so it can drill along the Z axis. a lathe is defaulted to G18

Good luck

[peaceandcalm]

i know i use floating holders there is no way around it...
thanks all for your help.

[fordav11]

the key is the option. rigid tapping is an option. if you don't have it then you can't do rigid tapping.

[underthetire]

Agree with hitachiboss. Most lathes won't rigid tap unless they have live tooling.

[hoi.le]

you should change parameter #911