G02 bad arc error or just wanders off into space.

[h2ocean]

ill put the facts up here and the story below so if you don't like to read or don't enjoy laughing at those who do not know what they are doing you can skip the bottom.
ive attached a crude drawing of the part and i want to mill the "u-turn" rounded tip. the code has the .219 tool offset dimensions since G42 i cant make work either. from what i understand the line should read,
G02 X1.812 (where i want to end up on the x plane) Y-0.938 (where i want to end up on the y plane) I0.0 (no change in the x plane) J-0.187 (the incremental radius center on the y plane)

current g-code
%
O01230
(X-0 Y-0 MACHINE SIDE LEFT CORNER)
(MACHINE RUNNING IN ABSOLUTE INCH COORDINATES)
N005 G40 G54 G80 G17 G90 G20 G94
(TOOL#3 7/16 2 FLUTE END MIL)
N010 G0 X-0.250Y0.250 Z0.500
N015 T3 S1800 M3
N016 G01 Y-0.125
N020 G01 Z-0.020 F15
N026 G01 X1.812 F25
N030 G02 X1.812 Y-0.938 I0.0 J-0.187
N035 G01 Y-0.938 X-0.250
M03
%

so i have been attempting this for awhile now and have a TMC1000 bench top mill, it was originally dos and i got a copy of the windows 95 program that came with the later models. I have a full size mill and have in cases like this given up on the little CNC since i can cut the part at full 0.500 depth and round the end with a file, which is so far faster and easier since i could have made 50 of them with the time i spent on the gcode. i am not sure if i am doing something wrong in the code or the machine just does not understand it. right now if i cannot program and use it i may as well just sell it. i tried G42 comp and it never works out correctly, in the tool library it is tool 3 and D3 in the code. the tool diameter is set at 7/16 0.437 and the comp if set to 1/2 like the graphic in the program shows ti just follows the toolpath with no offset, if you set it to full diameter it cuts the tool diameter plus the coordinate. the cutter is cutting clockwise around the part so it should be the right hand offset from what i have read.

anyone that can fix the code if it is wrong i would appreciate it.

Similar Threads:

• Space planning
• mach wanders off after tool change
• Newbie- Space Constraints
• Newbie- Need more space
• Paper space Model space ??

[mcode]

If your setting the tool radius in the tool offset page then I would modify the program like this

O01230
(X-0 Y-0 MACHINE SIDE LEFT CORNER)
(MACHINE RUNNING IN ABSOLUTE INCH COORDINATES)
N005 G40 G54 G80 G17 G90 G20 G94
(TOOL#3 7/16 2 FLUTE END MIL)
N010 G0 X-0.250Y-.094 Z0.500
N015 T3 S1800 M3
N020 G01 Z-0.020 F15
N025 G01 G41 Y-.344
N030 G01 X1.812 F25
N035 G02 X1.812 Y-0.719 I0.0 J-0.1875
N040 G01 Y-0.719 X-0.250
N045 G01 G40 Y-.969
M03


If your setting 0 radius in the offset page then

O01230
(X-0 Y-0 MACHINE SIDE LEFT CORNER)
(MACHINE RUNNING IN ABSOLUTE INCH COORDINATES)
N005 G40 G54 G80 G17 G90 G20 G94
(TOOL#3 7/16 2 FLUTE END MIL)
N010 G0 X-0.250Y-.094 Z0.500
N015 T3 S1800 M3
N020 G01 Z-0.020 F15
N025 G01 G41 Y-.1253
N030 G01 X1.812 F25
N035 G02 X1.812 Y-0.9378 I0.0 J-0.4063
N040 G01 Y-0.9378 X-0.250
N045 G01 G40 Y-.969
M03


Hope that helps

[rcs60]

This is how i would write it
1st one would be with out cutter comp
2nd is with cutter comp
The X1.812 move would take you off the part when doing the radius


No cutter comp
N010 G0 X-0.250Y0.250 Z0.500
N015 T3 S1800 M3
N016 G01 Y-0.1245
N020 G01 Z-0.020 F15.
N026 G01 X1.6025
N030 G02 X1.790Y-.531 I0.0 J-.4065
N032 G02 X1.6025Y-.9375I-.4065J0.
N035 G01 X-0.250
M03
%

Cutter comp
G0X-.500Y.0.Z.500
T3S1800M3
G01Z-.02F50.
G1G41D3Y-.3435
G1X1.6025F15.
G2X1.790Y-.531I0.J-.1875
G2X1.6025Y-7185I-.1875J0.
G1X-.250
G1G40X-.500F50.

[mcode]

This is how i would write it
1st one would be with out cutter comp
2nd is with cutter comp
The X1.812 move would take you off the part when doing the radius


No cutter comp
N010 G0 X-0.250Y0.250 Z0.500
N015 T3 S1800 M3
N016 G01 Y-0.1245
N020 G01 Z-0.020 F15.
N026 G01 X1.6025
N030 G02 X1.790Y-.531 I0.0 J-.4065
N032 G02 X1.6025Y-.9375I-.4065J0.
N035 G01 X-0.250
M03
%

Cutter comp
G0X-.500Y.0.Z.500
T3S1800M3
G01Z-.02F50.
G1G41D3Y-.3435
G1X1.6025F15.
G2X1.790Y-.531I0.J-.1875
G2X1.6025Y-7185I-.1875J0.
G1X-.250
G1G40X-.500F50.

Good catch, overlooked that, thanks

[deadlykitten]

hello i would do something like this :

    intro codes                                                   (*1)
    R                                                   Zsafe     (*2)
    R                X-tool_radius-2.5mm YA+tool_radius
    R                                                   ZA    G41 (*3)
    linear   feed to XB                  YB
    circular feed to XC                  YC
    linear   feed to X-tool_radius-2.5mm YD
    R                                                   Zsafe G40

(*1) ( work_coordinate , tool_length , tool_radius , rpm , coolant , check seat belt , etc )
(*2) ( R means rapid )
(*3) ( when this line is executed, only Z axis is moved; it's target position is a compensation position for the toolpath that follows in XY plane )

if you can not read tool_radius inside the program, than maybe you may use imaginary vectors; next code may need a bit of customization, because compensation starts at Z safe, while machining is done at a lower Z; requires knowing how the control behaves on such codes

    intro codes
    R                         Zsafe
    R                X-2.5 YA           imaginary vectors
    R                         ZA    G41
    linear   feed to XB    YB
    circular feed to XC    YC
    linear   feed to X-2.5 YD           imaginary vectors
    R                         Zsafe G40

if possible, is good to eliminate unnecesary movements :
... corresponding to lead-in and end-out comps among a toolpath
... keep constant clearance, regardless of tool diameter
...... some 10s of a second can be spared ; if you have read this post, then you have allready lost them / kindly

[cogsman1]

Check your Plane select to be sure the radius you are cutting is using the proper axis'

MY MACHINE USES;
G17- Plane select X-Y
G18- Plane select X-Z
G19- Plane select Y-Z