Parameter number out of range

Hi Mr CS Kilian,

In line 128 :
Z10.

Just remove the dot .

Line 110 same issue. So check your code good !!

It looks like you use H codes outside of G43 :
G43 H1 (set tool offsets using the values from tool 1 in the tool table)

Good luck !!

I made your routine running, didn't test the grooves. But that's the easy part for you. I kicked out G41 cutter compensation, used #5410, diameter of current active tool. Now diameter registered in the tooltable is used: T2 and T3 . #<_fingerbit_dia_mm>=20
#<_ball_end_dia_mm>=12 are commented. I made some changes in your code, so you need to test, if the coordinates are ok. At least it is running now, ready for you to finish.


Edit
It was a bit late yesterday, following changes needed in the file:
(The entry for tooldiameter must match in the tooltable and the parameter)

uncomment:
#<_ball_end_dia_mm>=12

replace #5410 by #<_ball_end_dia_mm>:
#<_groove_start_right_x>=#<_right_mm_to_basin_centre>+[#<_sink_hole_mm_lr>-[2*#<_required_oh_mm>/2]-[#<_ball_end_dia_mm>/2]]
#<_groove_move_right_x>=[#<_grooves_length_mm>+[#<_ball_end_dia_mm>/2]]
#<_groove_start_left_x>=#<_right_mm_to_basin_centre>-[#<_sink_hole_mm_lr>-[2*#<_required_oh_mm>/2]+[#<_ball_end_dia_mm>/2]]
#<_groove_move_left_x>=[-#<_grooves_length_mm>-[#<_ball_end_dia_mm>/2]]

Thanks for you effort to assist!

Please confirm that the program which you have attached is the one that you got running? I have copied it as is and opened the file but got error message "Radius to end of arc differs from radius to start....." near line 82.

As you said, if I can get the routine to tun I will be able to finish it and check coordinates.

meant to say "get the routine to RUN...."

curtkilian@gmail.com wrote: "Radius to end of arc differs from radius to start....." near line 82.

That will happen if you have a radius that does not have a start point, or use to big of a tool diameter for the radius to be cut, or you have some type of tool compensation active.

Thanks, I will check that out.

Thanks for the G code changes. After a bit of tweaking the simulation follows the paths perfectly on the XY axis.

Only 2 small problems:
1. I have commented out the M0 pauses but it still pauses between some of the G90 and G91 instructions? Unless I click twice on the "Execute next line "T" arrow button, then it continues to the next instruction without pausing.
See code below:
G91 G1 Y#<_left_bf_move> (Incremental Mode)
(M0 Temporary Position Check)
G90 G3 X[#<_left_rad_x>] Y[#<_front_rad_y>-#<_cut_radius>+[#<_fingerbit_dia_mm>/2]] I[#<_cut_radius>-[#<_fingerbit_dia_mm>/2]] J0
(M0 Temporary Position Check)
G91 G1 X#<_front_lr_move> (Incremental Mode)
(M0 Temporary Position Check)
G90 G3 X[#<_right_rad_x>+#<_cut_radius>-[#<_fingerbit_dia_mm>/2]] Y[#<_front_rad_y>] I0. J[#<_cut_radius>-[#<_fingerbit_dia_mm>/2]]
(M0 Temporary Position Check)
G91 G1 Y#<_right_fb_move> (Incremental Mode)
(M0 Temporary Position Check)
G90 G3 X[#<_right_rad_x>] Y[#<_back_rad_y>+#<_cut_radius>-[#<_fingerbit_dia_mm>/2]] I-[#<_cut_radius>-[#<_fingerbit_dia_mm>/2]] J0.
(M0 Temporary Position Check)
G91 G1 X-#<_back_final_move> (Incremental Mode)
(M0 Temporary Position Check)

This also happens between the milling of each groove? see code below:
#<_i>=1
o<cutgrooveone_r> sub
#<_i>=[#<_i>+1]
G0 Z3.
G1 Z#<_groove_start_z> F60. (Start Depth)
G91 X#<_groove_move_right_x> Z0.
G90 G54 G0 Z5.
o115 IF [#<_i> LE #<_qty_of_right_grooves>]
G91 X[-#<_groove_move_right_x>] Y#<_grooves_spacing_right_y>
(M0 Temporary Position Check)
o115 ENDIF
o<cutgrooveone_r> endsub

2. When a tool change is done, machine first moves back to HOME before moving to the work start position?
G53 G0 Z0. Y#<_tool_change_position_y>
(DRILL START HOLE)
T1 M6 (msg, Fit Core drill with 20mm dia and 118mm Height. M6 Tool Change Pause. Then start cycle)
G0 X#<_right_mm_to_basin_centre> Y#<_start_point_y>

Overview of the changes done so far.

Change in the most recent file #<_tool_change_position_y>=-500, if required, and take a look at Toolchange_position in your .ini file, or use G30 G30.1.

Thanks! this is now resolved .