Cnc table top surface skimming

[oakmeadows]

Hello i have recently made a cnc router and would like to skim a tad off the table just to level it to its best does anyone have any idea the best way to go around this or where i can find some gcode to do it thanks to anyone that helps

[OCNC]

What is the size of the working surface that you want to skim?  What size (diameter) is the bit you would use?  What feed rates does your machine work with?

Chris

[oakmeadows]

Hello and many thanks for you reply
my table size is only 400mm x 300 mm and i was going to use a Dovetail bit (as i have one handy)
tip dia is 19.1mm as my feedrates well im not too sure as i made this cnc myself but my other feedrates seem to
be around 30/40 mm/sec

[Ya-Nvr-No]

   here is a program I created to face stock,  you can adapt it to your needs to surface your table top.
You can make multiple light passes till it cleans up. Play/learn with it, till you understand what it can do for you.

    (CUTS Top Face of stock)
    (STARTED AT Z0 TOP OF rough PART)

    M03 (start spindle)
    G1G90X0Y0Z0.25F60. (Go to lower left corner of stock)
    Z0 ( Feed to face of rough stock)

    (load variables)
    #1000=[2] (Length in X in this case inches)
    #1001=[2] (Width in Y)
    #1002=[-0.1] (depth each of cut pass)

    #1004=0 (Top of part)
    #1005=0.65 (offset cut distance smaller than .75 cutter diameter)
    #1006=[#1005*2] (Compute step over)
    #1007=[#1001/#1006] (Compute passes)

    M98 P5 L8 (call subroutine CUT DOWN IN Z in this case 0.1 * 8 = .8")
    M05 (stop spindle)
    G0G90Z.25 (move back up)
    X0Y0 (go home)
    M30 (All done)

    O5
    M98 P10 L1 (call sub to feed down)
    M98 P20 L1 (call sub to face part)
    G0G90Z0 (Move out of the way)
    X0Y0 (Go Home)
    M99

    O10
    #1004=[#1004+#1002] (Calculate New cut depth)
    G1Z[#1004] (MOVE TO CUT DEPTH)
    M99

    O20
    M98 P30 L[#1007] (call sub to cut reps ACROSS)
    M99

    O30
    (THIS IS THE SUB TO CUT FACE)
    G1 G91Y[#1005] (Increment over in Y)
    G90X[#1000]F80. (Cut across part)
    G91Y[#1005] (again increment over)
    G90X0 (Cut back across part)
    M99

[oakmeadows]

Mant thanks for this i will have a play with it and let yuo know how i got on

[OCNC]

This was my take on it.  It assumes that you were going to use the 19mm bit and that you're cutting a wooden table surface.  The skim cut is set to 1mm.  You can change any of the values in a text editor.
Try it in air before you actually cut something.  The hardest part to guess is what your feed speeds might be.  3000mm per min was conservative for my machine...adjust to suit yours.

Chris

(SET Z=0 IN ABSOLUTE COORDS. TO TOP OF SURFACE TO BE SKIMMED)
G21(SET METRIC UNITS)
G01 Z-1.0 F3000 (CHANGE Z VALUE TO SKIM MORE OR LESS MATERIAL;CHANGE F VALUE TO ADJUST FEED IN Z)
M98 P1 L10 (RUN XY MOTION FOR SKIMMING SURFACE; Y DISTANCE EQUALS CYCLE COUNT TIMES 30mm)
G90 Z5.0 (SET ABSOLUTE COORDS.;MOVE OFF WORK SURFACE)
M30
%

O1 (XY MOTION SUB-PROGRAM)
G91 X400 F3000 (CHANGE X VALUE TO SET X CUT DISTANCE; CHANGE F VALUE TO ADJUST FEED IN X & Y)
Y15 (CUT WIDTH PER PASS BASED ON 19mm CUTTER DIA.)
X-400 (THIS VALUE SHOULD BE THE NEGATIVE OF THE X VALUE SET ABOVE)
Y15 (CUT WIDTH PER PASS BASED ON 19mm CUTTER DIA.)
M99 (EXIT SUB-PROGRAM)