Hi
I don’t have experience in writhing or modifying post processor for mastercam v9.1, so I am asking for help now.
#1 How to modify mpfan (generic Fanuc mill post) so do not post tool numbers and tool change any more.
#2 And in circular motions to post I & J instead of R
Any other tip regarding post processors for mastercam is more then welcome to
Thank you

for answer number 1 try this...
first back up your post.... then under your ptlchg find this line..
pbld, n, *t, "M6", e
and change it to...
#pbld, n, *t, "M6", e

then under the psof find this line..it should be the last line that I have pasted here where the editing is done..
psof #Start of file for non-zero tool number
pcuttype
toolchng = one
if ntools = one,
[
#skip single tool outputs, stagetool must be on
stagetool = m_one
!next_tool
]
"%", e
*progno, e
"(PROGRAM NAME - ", sprogname, ")", e
"(DATE=DD-MM-YY - ", date, " TIME=HH:MM - ", time, ")", e
pbld, n, *smetric, e
pbld, n, *sgcode, *sgplane, "G40", "G49", "G80", *sgabsinc, e
sav_absinc = absinc
if mi1 <= one, #Work coordinate system
[
absinc = one
pfbld, n, sgabsinc, *sg28ref, "Z0.", e
pfbld, n, *sg28ref, "X0.", "Y0.", e
pfbld, n, "G92", *xh, *yh, *zh, e
absinc = sav_absinc
]
pcom_moveb
c_mmlt #Multiple tool subprogram call
ptoolcomment
comment
pcan
#if stagetool >= zero, pbld, n, *t, "M6", e

notice the last line I have here... put a # sign in front of the if stagetool that will get rid of your toolchange, BUT you still will have a H for a height offset in there.

answer for #2
And in circular motions to post I & J instead of R
find this in your post.. yours is set prolly at 1 right now.. change it to zero and it should start coughing out I and J's

arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

under your general output settings in your post.. find this
force_wcs : yes #Force WCS output at every toolchange?

more then likely your is set to no