Need Help!- help on fanuc

[RAInB]

i have a fanuc controler on a revolver head milling and i want to change the parameters from:


this is now: G03 X20. Y45. R65.
to this: G03 X20 Y20 R65


i want the dots to dissapear, i just want the dots to go away

[fordav11]

that is impossible on a Fanuc control. The point must be there.
X20.0 without decimal would equal 20 in the least increment
least increment is 1 micron so 20 = X0.020 or 20 microns

There is no reason to not want decimal points. Just accept it and move on (and forget Okuma with its non-standard no-decimals)

[angelw]

Originally Posted by fordav11 that is impossible on a Fanuc control. The point must be there. X20.0 without decimal would equal 20 in the least increment least increment is 1 micron so 20 = X0.020 or 20 microns There is no reason to not want decimal points. Just accept it and move on (and forget Okuma with its non-standard no-decimals)

Actually, not so. The parameter number depends on the control model of course, but using a Series 10,11,12 for example, bit #2400.0 (DPI) will select decimal point by either Conventional Method (bit set to 0), or Calculator Method (bit set to 1). In Calculator method X20 = X20.0. Understandably, X20.25 still has to be written as X20.25

RAInB,
What model Fanuc control do you have?


Regards,

Bill

[yours_prabhat]

there is one possibility If you can send the program from PC to machine. But Why you are doing this and What is the Use for removing the decimal I am totally not understand.in 8 years of my service life of CNC i met first time this type of Q.

[angelw]

Originally Posted by yours_prabhat there is one possibility If you can send the program from PC to machine. But Why you are doing this and What is the Use for removing the decimal I am totally not understand.in 8 years of my service life of CNC i met first time this type of Q.

I personally prefer to use the Conventional form. However, this question has been asked numerous times in this and other forums, and one of the most prolific and knowledgeable contributors to this forum uses the Calculator method. Further, I've been asked about this many times by clients, many of whom were using a Fanuc control for the first time after many years using Okuma controlled machines; it all comes down to preference. There are more than just Okuma controls that use the Calculator method as a default.

There is no requirement to send the program from a PC to attain what the OP desires. If the DPI bit is set to 1, as discussed in post #3, then X20 will be evaluated as X20.0, no matter how the program is registered in the control.

Regards,

Bill

[RAInB]

fordav, i got several controlers that are using fanuc: 0i-MD, 0i-TD, 18i-TB, 18i-MB the only one that uses the dot, is one of the ones with 0i-MD, that revolver,

[angelw]

Originally Posted by RAInB fordav, i got several controlers that are using fanuc: 0i-MD, 0i-TD, 18i-TB, 18i-MB the only one that uses the dot, is one of the ones with 0i-MD, that revolver,

The DPI bit for the 0i control is #3401.0. Set this bit to 1 and integer values will be considered in units of mm, inches, or second, referred to by Fanuc as Pocket Calculator type decimal point input.

Regards,

Bill

[fordav11]

Originally Posted by angelw .....as Pocket Calculator type decimal point input.

ha ha. A pocket calculator just about sums up the 0-series

[RAInB]

Originally Posted by angelw The DPI bit for the 0i control is #3401.0. Set this bit to 1 and integer values will be considered in units of mm, inches, or second, referred to by Fanuc as Pocket Calculator type decimal point input. Regards, Bill

Thx Bill, I`ll try this monday, and i`ll come back with the result

[stevo1]

I set all of my machines up to use calculator method. As Bill has stated it is all preference. My largest reason is that if someone is typing in a clearance plane of 5”and forgets to put the decimal in I don’t want the machine reading it as .005”

Stevo

[g-codeguy]

Originally Posted by angelw There are more than just Okuma controls that use the Calculator method as a default.Bill

I believe our Fagor 8025 controls are set this way, but I use decimals out of habit since all our other lathes are set to use decimal points.