Learn CAD/CAM or Gcode

The first thing I see is you set incremental mode in your preamble. This may be a source of confusion for you. Another thing is G1 is a modal command in group 1 so it will stay in effect until you issue another G code from modal group 1.

gnipsel.com/linuxcnc/reference/page2.html

I would use G81 to drill identical holes in different locations.

The "go to home" move at the end went to the G91 X0 Y0, either change back to G90 or put a G53 G0 X0 Y0 to go to machine zero.

I use G92 on my plasma where I jog to a start point and want that to be X0 Y0 then all the coordinates make more sense as you use the actual X Y coordinates. Then at the end you use G92.1 to clear the offset.

John

Can you be more specific about #1?

#3 your probably drilling much too slow for 26k in wood. You might try the peck drill cycle G83 or a pause between each hole for the bit to cool down a bit. What size hole are you drilling?

John

At 27k rpm with a 1/8" drill bit that is 850 SFM (Surface Feet per Minute) which is really fast. If you tried to take 0.001" per revolution you would have to feed at 52 IPM (Inches Per Minute). I don't think you can feed too fast while you drill unless you stall the spindle. Using G81 will rapid out of the hole which will help reduce the friction on the bit and keep it cooler.

The G81 line goes at the start of the drill sequence not in the preamble. The preamble is for setting up the machine and contains things like units, turn off compensation, turn off any cycles, set your path control mode, the active plane etc. The preamble is to put the machine into a known state so G codes that follow are interpreted correctly.

The G81 followed by the location of the first hole in your X and Y corrdinates then the Z depth to drill and finally the R retract position. There are a few more options but the basic is G81 X Y Z R. The reason for the R is to specify the retract height after first hole. You can be higher when you start the G81 cycle but the retract height is where it ends up.

Normally you touch off the tools to the top and set that as Z0. In this example I assume that. I assume you jogged to the starting point and the G code assumes that to be X0 Y0.

If you didn't specify the path control mode then you get G64 which is move as fast as you can no matter what corners you cut... Also the GUI back plot is not in real time so the path it shows may not be the exact path the tool takes.

John

One thing that helps me is to put a comment for G codes I'm not familiar with.

So this:
Would be changed to this:

The G17 XY plane is generally for mills and mill like devices and the G18 XZ plane is for lathes. This defines how some cycles work and how arcs are interpreted. The G17 plane is a flat plane drawn through the X and Y axis so this makes the Z axis perpendicular to the plane. On a lathe the G18 XZ plane is drawn through the X and Z planes and the imaginary Y axis is perpendicular to the plane.

www.linuxcnc.org/docs/html/gcode/gcode.html#sec:G17-G18-G19

This is a short heads up on using the trajectory planner.
www.linuxcnc.org/docs/html/common/User_C...trajectory_control_a

Don't feel bad I still don't know what the naive cam detector is... I only know what it does.

John