rcamhub
Sign in

Learn

Set your zero: where your machine starts counting

Every number in a G-code program is measured from a point called zero, and the machine has no idea where on your material that is until you show it. Get this wrong and the program is perfectly good and the cut lands in the wrong place, or too deep. RapidCAM asks you to say where your zero is, so what it writes matches what you do at the machine. This guide covers both halves.

Open RapidCAMNothing to install, no account.

  1. Pick a spot you can find with the machine

    Zero is a position in three directions, and you will have to put the cutter on it by hand, so choose one you can find. Across and along, that is a corner of the material or its centre. Up and down, it is the top surface of the material or the bed it sits on.

    RapidCAM’s default is the front-left corner, at the top of the stock: the corner nearest you, at the surface. A round or symmetrical part is easier from the centre. Choose Bed for the height if you would rather measure up from the table, for example from a spoilboard you have zeroed on.

  2. Tell RapidCAM where it is

    In New Project, the Origin (WCS - Work Coordinate System) section has three pickers: X (Left, Center, Right), Y (Front, Center, Back) and Z (Top of stock, Bed). The little block beside them shows where that puts the origin. WCS is the usual name for it: the physical 0, 0, 0 of your job.

    New Project: the Origin section, set to the default (left, front, top of stock).
    The New Project dialog with a 100 by 60 millimetre stock, 10 millimetres thick, and the Origin section set to Left, Front and Top of stock beside a small diagram of a block

    The red and green axes drawn on the stock are your zero, so you can see it before you export anything. Here it is on the stock’s front-left corner, with the 80 × 50 mm plate used in the rest of this guide drawn inside it.

    The axes sit on the stock's front-left corner: that is where RapidCAM thinks your zero is.
    A lighter 100 by 60 millimetre stock inside the larger sheet, with an 80 by 50 millimetre rectangle inside it and red and green axes at the stock's front-left corner

    Already have a project? Open the Toolpaths tab and press the › beside Project Settings. The same Origin (WCS) pickers are there, and the axes jump as you change them.

    Origin set to Center and Center: the axes move to the middle of the stock.
    Project Settings open on the Toolpaths tab with the Origin pickers set to Center and Center, and the axes moved to the middle of the stock

  3. See what it changes

    Here is one drawing, an 80 × 50 mm plate centred on a 100 × 60 × 10 mm blank, cut with an outside profile, exported three times with only the origin changed. The cutter runs 3 mm outside the plate, which is why the cuts start at X 7 and not X 10.

    Origin (X / Y / Z)Cutting XCutting YCutting Z
    Left / Front / Top of stock7 to 932 to 580 down to -10
    Center / Center / Top of stock-43 to 43-28 to 280 down to -10
    Left / Front / Bed7 to 932 to 5810 down to 0

    The part did not move. Only the numbers that describe it did. From the centre, the plate’s edges are at ±40 and ±25 and the cut runs 3 mm beyond them. With Bed, every height is measured up from the table, so the top of the material is at Z 10 and the cut finishes at Z 0. That is why the stock thickness has to be the real thickness: with Bed it sets where the surface is.

    The program records the choice in its own header, which is worth a glance before every job:

    ; WCS origin X: Left  Y: Front  Z: Top of stock
; Stock: 100 x 60 x 10mm

    With Bed it reads Z: Bed (top at Z=10mm).

  4. Set the same zero on the machine

    RapidCAM cannot see your machine, so this half is yours, and it must match step 2. In your sender (the program that streams G-code to the controller), jog the cutter to the spot you chose and set X and Y to zero there. Then set Z: bring the cutter down to the top of the material and zero Z, or, if you chose Bed, touch off on the bed instead. Senders usually have a zero button for each axis. On a GRBL controller you can also type G10 L20 P1 X0 Y0 Z0, which makes wherever the cutter is now the zero of work offset 1.

    One detail: RapidCAM’s program does not choose a work offset (it has no G54 line), so it runs in whichever one your controller has selected. On GRBL that is G54 unless you have changed it, so zero in that one.

    Before you run it: compare the header’s WCS origin line with what you just did at the machine. If they differ, stop. Then run the program once with the cutter well above the material, watch it trace the outline where you expect, and only then lower Z and cut. Wear eye protection and stay with the machine while it runs.

Open RapidCAMNext: from an SVG to G-code

Checked against RapidCAM on 2026-10-05. If something here no longer matches what you see, the app has changed and this guide is behind: please tell us.