G41/G42 Post question

[stude8]

Simple question that I can't seem to find an answer to.

V25
I'm profiling a part and I turn system comp off and Machine comp G41 on. Why doesn't a "D" and a G41 appear in the program after I post it? Fanuc 11M

Thanks
Drake

Similar Threads:

• New here and don't know where to post my question ...
• Where to post a question?
• where to post my question?
• Post Question

[The Engine Guy]

Really needs you to upload a copy of your Post Processor to get it right.

Normally most PPs default to not having Cutter Compensation active, look in your PP at Blocks 2,3 and 4 for the line n,cc or n,force_cc

Possibly should look a bit like the PP shown below which is a Fanuc 0M PP.


2. Start of file Standard
"(PROGRAM NAME - ",prog_name,")"
"(POST - ",machine_make,machine_model,")"
"(DATE - ",output_date,")"
"(TIME - ",output_time,")"
user_comment_1
user_comment_2
user_comment_3
user_comment_4
user_comment_5
user_comment_6
user_comment_7
user_comment_8
user_comment_9
user_comment_10
user_comment_11
user_comment_12
user_comment_13
user_comment_14
user_comment_15
" "
n,absolute_coord,cancel_drill_cycle,"G40",inch_mod e,"G17"
" "
n,rapid_move,incremental_coord,"G28","Z0."
n,rapid_move,incremental_coord,"G28","X0.","Y0."
" "
system_comment
feature_name_comment
" "
n,t,"M06"
n,s,spindle_on
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xyr_angle,
n,rapid_move,length_offset,coolant_on
output_rotary_angle
n,cc

3. Tool change
n,coolant_off
n,spindle_off
n,rapid_move,incremental_coord,"G28","Z0."
n,optional_stop
" "
system_comment
feature_name_comment
" "
n_forced,t,"M06"
n,s,spindle_on
n,rapid_move,absolute_coord,work_coord,force_x,xr, force_y,yr,rotary_xyr_angle,
n,rapid_move,length_offset,coolant_on
output_rotary_angle
n,cc

4. Null tool change
" "
system_comment
feature_name_comment
" "
n,s
n,rapid_move,force_x,xr,force_y,yr,rotary_xyr_angl e,
output_rotary_angle
n,cc

[COLOR="#000000"]It might need a d_offset inserting as well so it may need to be something like :-

n,d_offset,cc

but I would try just using the line n,cc first

Hope that`s of some help

Regards
Rob
:rainfro: :rainfro: :rainfro:

[stude8]

Thanks very much Rob. I followed your instructions and next I will prove out at the shop. Here is a screenshot showing the "D" and "G41"

[The Engine Guy]

Thanks very much Rob. I followed your instructions and next I will prove out at the shop. Here is a screenshot showing the "D" and "G41"

Code looks fine Drake, as long as the Fanuc control has the Tool Offsets screen correctly set then that code should call up the tool offset OK

Not familiar with Fanuc 11M so not able to help with the settings

Regards
Rob
:rainfro: :rainfro: :rainfro:

[SeanDa]

Drake,

Did you provide a lead in/out other than vertical?

[stude8]

Sean I always do when manually programming with G41/G42, but for some reason the Bobcad program is with the Z axis. I haven't been able to get to the shop for 2 days because of a blizzard and will try it as soon as I can. I found it interesting.
Thanks,
Drake

[SeanDa]

Drake,

You should be able to see an area for selecting lead in/out. I have attached a picture showing what it looks like, its in the new version, but same general area in V25.

[stude8]

Sean you've been very helpful. As soon as I picked a parallel lead in of 1 inch the G41 and "D" were put where I'm used to seeing them. Many thanks.
Drake