- Observe the line # your program halted at, or the operation you had in progress ( although G code looks complex, the general gist of what is happening can be identified with basic deduction).
- Launch the ACTIONS button and select VIEW G Code.
- Using the line number from step 1, scroll through the G code to find it.
- Once you have found the line you ended on, go backwards from there until you see a traversal height Z axis move ( usually looks like XX G0 Z0.6)
- Make sure the Z axis move is in a positive direction (for example, don’t use one with a G0 Z-0.6 as that is a plunge operation [its all about that - ]).
- Close the G code screen and press the GOTO button, enter the number of the line with your Z axis move.
- Ensure your machine is safe for a move, as the exact next instruction it gets after the Z axis move is usually a rapid move to an X.Y coordinate some distance from its current location (remember you can’t start exactly where you ended, but you can restart where the machine started with a plunge on the Z axis).
- Once ready for a move (remember to set the Z axis using the controls at the top right BEFORE you execute the GOTO command) Hit the PLAY button and away she goes. Some supervision will be required, I usually don’t turn on the Router until its about to start the plunge operation.
- Congratulations! you can now start off where you left off (mostly).
1 (1001) //program name
2 (T1 D=0.25 CR=0 - ZMIN=-0.875 - FLAT END MILL) //tool specs for program
3 G0 G40 G90 G17 //rapid move,//tool radius compensation off,//roughing for z axis,//xy plane selection
4 G20 //specify programmed in inches
6 (2D CONTOUR2)
7 T1 M6 //tool 1 T1 for turret 1, M6 for misc. 6, in this case 1/4" endmill
8 M3 S24000 //spindle speed (in this case its your router rpm)
9 G0 X34.2 Y8.775 //G0 is a rapid move, in this case, to the home point for the start of the toolpath
10 G0 Z0.6 //rapid move on z axis to traversal distance (THIS IS WHAT YOU ARE LOOKING FOR)
11 G0 Z0.2894 // rapid move z axis to safe distance (specified when creating toolpaths in CAM software)
12 G1 Z-0.225 F16. // interpolated plunge of z axis (note the negative number)
13 G1 X34.1997 Z-0.2289 //interpolate move, linear
14 G1 X34.1988 Z-0.2327 //" note
15 G1 X34.1973 Z-0.2363 //" that
16 G1 X34.1952 Z-0.2397 //" the
17 G1 X34.1927 Z-0.2427 //" z axis
18 G1 X34.1897 Z-0.2452 //" is slowly
19 G1 X34.1863 Z-0.2473 //" getting
20 G1 X34.1827 Z-0.2488 //" deeper
21 G1 X34.1789 Z-0.2497 //" in this
22 G1 X34.175 Z-0.25 //"part
23 G1 X34.15 F48. //feed rate 48 ipm
24 G3 X34.125 Y8.75 I0 J-0.025 // circular interpolation counter clockwise
In the example code above, line number 10 would be the ideal GOTO line, however lines 11 and 12 would also work, you would need to babysit the sled until it reaches your intended start point so the tool doesn’t gouge the workpiece though #unsafe.
If you have gone through a power cycle with the Maslow hardware, as long as the Workpiece hasn’t moved and you calibrate, you can usually start off again without too much distortion on the finished parts ( my last go at this had it maybe 1/32 in. from its original paths before the rogue Hibernation kicked in again. I had my laptop shut off on me three times in a row. how embarrassing. Cheers!