lathe face drill needs to be ipr feed

[Pete Thomson]

I have a fanuc 18i control and using- GENERIC FANUC 4X MT_LATHE.pst

when i use C axis face drill the post outputs the feed in IPM and I need IPR

also my "Dia offset 0" box is greyed in C-axis face drill out so when it post i get T0900 in stead of T0909

 

X7 mu2

puma TT2500SY

fanuc 18i

Thanks

 

G0 T0900

G17

M35

M8

G0 G54 Z.25

X3.74

C180.

G97 S3834 M33

G83 Z-.343 R.1 F15.34

C60.

C300.

G80

M9

G28 U0. H0. M35

G28 W0. H0.

T0900

[Reece L Gibson]

Probably the easiest way is to set up a Misc real to trigger feed per rev.

If it's a drill cycle, might go thru the drill cycle

Declare / format your variables:

 

use_pitch : 0 #0 = Use feed for tapping, 1 = Use pitch for tapping

fmt "N" 4 n_tap_thds$ #Number of threads per inch (tpi)

fmt "F" 2 pitch #Tap pitch (inches per thread)

 

Might capture it in "pdrlcommonb" post block

 

if mi6$, use_pitch = 1

if use_pitch = 1,

pbld, n$, "G95",e$

else,

pbld, n$,sgfeed, e$

 

(Drill cycle post block)

 

mtap$ #Canned tap cycle, mill

pdrlcommonb

if use_pitch,

pitch = 1/n_tap_thds$

pcan1, pbld, n$, *sgdrlref, pgdrlout, pfxout, pfcout, pfzout,

prdrlout,*pitch, strcantext, e$

else,

pcan1, pbld, n$, *sgdrlref, pgdrlout, pfxout, pfcout, pfzout,

prdrlout,pffr, strcantext, e$

pcom_movea

[Pete Thomson]

I couldn't figure out the above solution.

I put " sg98 " into the canned drill cycle below and i seemed to work.

 

mdrill$ #Canned drill cycle, mill

pdrlcommonb

pcan1, pbld, n$, *sgdrlref, pgdrlout, sg98, pxout, pyout, pzout,

pcout, prdrlout, dwell$, pffr, strcantext, e$

pcom_movea

 

 

 

My reseller said - without looking at the entire I can't say if there are anger conflicts but it looks good.

what are anger conflicts?

When I use canned drill cycle it outputs T0900 when i need T0909

the reseller said I needed to edit a math equation in the post

 

would it be something like- toolno = t$ * 100 + zero

Thanks

[Reece L Gibson]

toolno = t$ * 100 + tloffno$

[Pete Thomson]

on the #tool change mill it was

toolno = t$ * 100 + tolffno$ but on my c-axis face drill the Dia offset is 0 and greyed out.

i changed it to

 

toolno = t$ * 100 + t$

 

then it posted T0909

is there any way to get dia offset un-greyed?

Thanks

[crazy^millman]

on the #tool change mill it was

toolno = t$ * 100 + tolffno$ but on my c-axis face drill the Dia offset is 0 and greyed out.

i changed it to

 

toolno = t$ * 100 + t$

 

then it posted T0909

is there any way to get dia offset un-greyed?

Thanks

Nope since a Drill should never have a diameter offset. You can make a mi or mr control this if you need it, but milling toolpaths like this when used in lathe never had the logic built into them that you might need adjustments. It was done along the lines of you would never need them since what would you be adjusting. You can define or do a different type of toolpath and they are not greyed out, but would need to know exactly what you are trying to accomplish.

[Pete Thomson]

Before i changed toolno = t$ * 100 + tloffno$ to toolno = t$ * 100 + t$

it would post T0900 instead of T09?? the last 2 digits are for the tool length.

It would index to tool 9 but would have zero tool length offset

 

toolno = t$ * 100 + t$ works if i want the same tool & length number, but some times i might need T0919

 

is it possible to use toolno = t$ * 100 + ( Len. offset) ?

[crazy^millman]

Before i changed toolno = t$ * 100 + tloffno$ to toolno = t$ * 100 + t$

it would post T0900 instead of T09?? the last 2 digits are for the tool length.

It would index to tool 9 but would have zero tool length offset

 

toolno = t$ * 100 + t$ works if i want the same tool & length number, but some times i might need T0919

 

is it possible to use toolno = t$ * 100 + ( Len. offset) ?

 

Yes, but the problem is the lathe operations do not possess such a thing so not sure how you would make something that is not there work like you are thinking. That was why I suggested the mi or mr process to help control this. Mill toolpaths have the length offset, but not the lathe toolpaths unless I am missing something.

[Pete Thomson]

What are the mi or mr process?

are the in the post?

thanks

[crazy^millman]

These are the misc variables every Mastercam operation has do a search been covered 100's of time and one you get it done sky is the limits to what you can do with them.

 

 

Sent from my iPad using Tapatalk