Parameter number out of range
- curtkilian@gmail.com
- Offline
- New Member
-
Less
More
- Posts: 10
- Thank you received: 0
30 Sep 2018 06:55 #118219
by curtkilian@gmail.com
Replied by curtkilian@gmail.com on topic Parameter number out of range
Thanks,
With regards to the Tooldiameter input, I am using tooltables but do not know how to use the tool diameter size from the tooltables in the parameter formulas. Therefore I created the Parameters for tool diameter un the Operators input. I'll fix it as soon a I know how.
I've made the changes suggested, but still gets the same "Parameter number out of range" near line 128.
I have attached the program file for simulation.
With regards to the Tooldiameter input, I am using tooltables but do not know how to use the tool diameter size from the tooltables in the parameter formulas. Therefore I created the Parameters for tool diameter un the Operators input. I'll fix it as soon a I know how.
I've made the changes suggested, but still gets the same "Parameter number out of range" near line 128.
I have attached the program file for simulation.
Please Log in or Create an account to join the conversation.
30 Sep 2018 16:55 - 30 Sep 2018 17:15 #118239
by Grotius
Replied by Grotius on topic 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 !!
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 !!
Last edit: 30 Sep 2018 17:15 by Grotius.
Please Log in or Create an account to join the conversation.
30 Sep 2018 21:47 - 01 Oct 2018 07:27 #118244
by MaHa
Replied by MaHa on topic Parameter number out of range
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]]
#<_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]]
Last edit: 01 Oct 2018 07:27 by MaHa.
Please Log in or Create an account to join the conversation.
- curtkilian@gmail.com
- Offline
- New Member
-
Less
More
- Posts: 10
- Thank you received: 0
01 Oct 2018 14:50 #118287
by curtkilian@gmail.com
Replied by curtkilian@gmail.com on topic Parameter number out of range
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.
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.
Please Log in or Create an account to join the conversation.
- curtkilian@gmail.com
- Offline
- New Member
-
Less
More
- Posts: 10
- Thank you received: 0
01 Oct 2018 14:52 #118288
by curtkilian@gmail.com
Replied by curtkilian@gmail.com on topic Parameter number out of range
meant to say "get the routine to RUN...."
Please Log in or Create an account to join the conversation.
- tommylight
-
- Away
- Moderator
-
Less
More
- Posts: 18524
- Thank you received: 6191
01 Oct 2018 19:44 #118314
by tommylight
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.
Replied by tommylight on topic Parameter number out of range
"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.
Please Log in or Create an account to join the conversation.
- curtkilian@gmail.com
- Offline
- New Member
-
Less
More
- Posts: 10
- Thank you received: 0
02 Oct 2018 09:00 #118336
by curtkilian@gmail.com
Replied by curtkilian@gmail.com on topic Parameter number out of range
Thanks, I will check that out.
Please Log in or Create an account to join the conversation.
- curtkilian@gmail.com
- Offline
- New Member
-
Less
More
- Posts: 10
- Thank you received: 0
03 Oct 2018 15:53 #118414
by curtkilian@gmail.com
Replied by curtkilian@gmail.com on topic Parameter number out of range
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>
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>
Please Log in or Create an account to join the conversation.
03 Oct 2018 18:01 #118418
by MaHa
Replied by MaHa on topic Parameter number out of range
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.
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.
The following user(s) said Thank You: curtkilian@gmail.com
Please Log in or Create an account to join the conversation.
- curtkilian@gmail.com
- Offline
- New Member
-
Less
More
- Posts: 10
- Thank you received: 0
05 Oct 2018 04:55 #118455
by curtkilian@gmail.com
Replied by curtkilian@gmail.com on topic Parameter number out of range
Thanks! this is now resolved .
Please Log in or Create an account to join the conversation.
Time to create page: 0.188 seconds