[IlFincoITA]

Hi! i'm working on a generic FANUC PP for my Mill-Turn Machine.

What i cannot understand is that as i press generate G code I get something like this:

"(1)@start_of_file ==> program_number:5000 g_file_name:'MILL_TURN_1.TAP'
..> full_g_file_name:'C:\USERS\MAURO\APPDATA\LOCAL\SOL IDCAM TEMPORARY FILES\MILL_TURN_1\MILL_TURN_1.TAP'
..> part_name:'MILL_TURN_1'
..> part_full_name:'C:\Program Files\SolidCAM2012\User\Getting_Started_Examples\S W\mill_turn_1.prz'
..> path_part:'C:\Program Files\SolidCAM2012\User\Getting_Started_Examples\S W'
..> index_split_file:1 split_name:''
..> rotate_used:false mirror_used:false fourth_axis_used:false
..>
..> first_proc_number:2 last_procedure_number:1
..> inch_system:0
..> home_number:1 home_changed:false
..> clearance_plane:0.000 tool_start_plane:0.000
..> work_upper_plane:0.000 zero_plane:0.000
..> stock_x_plus:15.850 stock_y_plus:15.850 stock_z_plus:1.000
..> stock_x_minus:-15.850 stock_y_minus:-15.850 stock_z_minus:-28.000
..> stock_x:31.700 stock_y:31.700 stock_z:29.000
..> bound_x_external:15.850 bound_z_max:1.000
..> bound_x_internal:0.000 bound_z_min:-28.000
..> clamp_external:1
..> %
> :5000 (MILL_TURN_1.TAP)
(0)@def_turn_tool ==> tool_number:1 tool_position_in_turret:1 tool_position:A spindle_position:0.000
..> tool_id_number:0 tool_id_string:'0'
..> tool_offset_long:1 tool_offset_number:1
..> tool_direction:ccw tool_mode:face insert_face:back
..> tool_origin:T_tangent nose_point:2
..> tool_message:''T tool_type:Ext_ROUGH
..> tool_drill_lead:0.000
..> tool_A:25.000 tool_B:5.000 tool_C:20.000
..> tool_D:55.000 tool_D1:3.000 tool_D2:3.000
..> tool_E:5.000 tool_F:55.000 tool_G:0.000
..> tool_H:0.000 tool_K:0.000
..> tool_ALFA:60.000 tool_BETA:5.000
..> tool_Radius_alfa:0.000 tool_Radius_beta:0.000
..> TurretName:'Spindle' tool_used_in_main_spindle:1 tool_used_in_back_spindle:0
..> number_occur_of_tool:1
..> setup_angle:0.000 tool_tip_z:-60.000 tool_tip_x:-55.000 multi_tool_pos:0"

Is there something wrong with .GPP , .PRP or .VMID files... because it seems that it doesn't compile the G Code...

Thanks a lot...

[glovebox20]

Looks like the 'trace' function is turned on in your GPP file. That would be the first place I would start looking.

The trace function is useful for dubuging the post. Most gpp files normaly have a line something like this:

;trace: 5

Anything after the ';' is ingorned by the postprocessor so if you wanted to turn it on you would change it to this:

trace:5

The number stands for how much info is include in the post file, 5 being the highest. You will normaly find the trace line after all the golbal varibles defintions and user options in the gpp file, but before any gode processes.

Happy hunting

[IlFincoITA]

Oooooo Yes! there were these 3 lines... thanks a lot.

; trace "all":5
; trace"@change_tool":5
; trace "@home_number":5

I'm still have some problem here:

local numeric save_feed xc "it says that variable xc is an internal system variable"

[glovebox20]

I'm still have some problem here:

local numeric save_feed xc "it says that variable xc is an internal system variable"[/QUOTE]

Any idea what that variable is for?

Other than making sure that the variable is define in the being of the post, (or process if local variable?). I not sure where else to go.

You could try removing the varable and see if it makes it better?

Always make sure you keep a backup copy just in case you mess something and you want to go back to a pervious version.

[Aussie_CNC]

"xc" is now used by SolidCAM internally, so cannot be used as a custom variable. Use the Edit>Replace function or similar in your editor to replace "xc" with "my_xc" making sure you replace all instances. This should solve the issue.

[IlFincoITA]

Here we are. Everything works now. Thanks for you invaluable help. Now became the part of trying the code on the machine. Problems coming... he he he. I will start one oparation at a time end see what happens. I've already done in on an old DECKEL CONTROL 2 Milling Machine.

Bye...