Setting up to Cut Something

by

Setting up the Machine

There are several steps you need to do each time you start a job on your machine:

  1. Place your workpiece on the router table and fasten it down.
  2. Set your machine Zero point so it coincides with the G-Code origin point and your work
  3. Load the G-Code and do a trial run of your code with the Z axis lifted up to make sure it’s doing what you wanted
  4. Set the Z axis Zero and Check Gantry square
  5. Start the Job

We will go over each of these steps in detail.

Placing and Fastening Your Work

This simply involves placing your workpiece on the table and ensuring it is securely held so it won’t move during routing.  There are several ways to accomplish this:

  • Screw the workpiece to your spoil board using wood screws. This method is very strong, but you have to keep a couple of things in mind:
    • This will put holes in your table. This is going to eventually ruin your spoil board and it will need replacement.
    • Screws into MDF tend to make a little hump around the screw as it bites into the wood. This hump may cause problems down the road by making your spoil board surface uneven.
    • You have to pay attention the router will not hit the screw heads during any operations. This will surely break or dull the bit and render it useless
  • Use Double Sided Tape. This is probably the easiest and most expedient method of holding down the work.  It does no damage to the work or the bed, and if the correct type and amount of tape is used, makes a very strong bond.  Use a good quality wide carpet tape.  Work must be perfectly flat for this to work right.
  • Use Brad Nails.  Similar to using screws, but much lower impact.
  • Put Tee Nuts in your table. Tee Nuts are small circular T shaped nuts which are installed from below the table through a drilled hole.  They have a flange on the bottom which prevents them from pulling through, and are hollow with a threaded hole.  This allows you to put bolts through from the top to either hold your work directly, or use some kind of hold down clamp.  Again, caution is needed to prevent your router or bit from hitting them.
  • Put some kind of positioning fixture on the table. This could be a couple of wood battens, a framing square, or a couple of Tee Tracks.  These are used to locate your work so it is always in the same position.  This type of thing is often used where you have to make several pieces exactly the same, and it makes it easy to register the work in exactly the same location each time.  Some form of clamping arrangement is generally used with this method.

Note that the work should be fixed so it is square to the bed of the machine.  Use a small square to align the work so its square to the bed before fixing it down.

Setting your Work Zero

There are many ways to set up your workspace on your router.   Most CNC’ers, use the front left corner of the machine as the home point.   This is X and Y axes to their full negative value, and the Z axis to its full positive value.  Thus, all work will be in a positive direction for both the X and Y axes.  Most CAM programs for gantry type CNC’s work this way.

Some CNC users set their homing point at the right rear of the machine, and all work is in the negative X and Y planes.  This is less common, but it’s out there.  You can find any number of arguments on the forums about which is best.  Users of large CNC milling machines typically also use a different format.  Ultimately it depends on your CAM program and how it lays out the work space.  I typically use SketchUp and Sketch-U-Cam, which defaults to the lower left corner as zero.  Of course, when you do you toolpath generations, typically the CAM program will let you put Zero anywhere you want.

With the machine powered up, make sure all your axes are working and going in the right direction using the jog buttons:

  • Y + is to the rear, Y- is to the front (this will be opposite for a moving table machine)
  • X + is to the right, X – is to the left
  • Z + is up, Z – is down

If all this checks out, you can move the machine to your work zero point.

  • Use the jog buttons to raise the Z axis well up out of the way so the bit won’t hit any part of your setup.
  • Use the jog buttons again to move the X and Y axis so the bit is directly over your work zero point. The work zero point is defined in your CAM program when you generate the G-code.  Also known as the Origin.  You may want to bring Z down to just above the work to make this easier.
  • If you are going to trim up the workpiece after it’s milled, you don’t have to be really precise about this step. Just compare your workpiece size to the size of the g-code image, to make sure the machine won’t run off the edge of the work
  • If you are trying to position your cuts in some pre-existing piece, say, a cabinet door, you have to be precise with your positioning. It’s sometimes better in this case to put your G-code zero point in the center of the image; it will be much easier to accurately position this way.
  • Make sure the Z axis is high enough that the bit will clear all obstructions on the table. We will set its position later.
  • Now press the “Disconnect” button just to the right of the position display. Now press it again (it’s now called “Connect”).  This resets all the axis position indicators to zero.  This is for GRBL Panel, your program may have a different way to set zero.
  • Now you should have all zeros in your position display. This is good; your machine is now fully zeroed.

Don’t move your machine yet!  I like to set G28, or Special Position 1 button to this zero point for later.  If something were to happen, I can always return to the zero position without having to do it manually.  To do this:

  • Go to the Settings Tab
  • About the center of the page, at the bottom, you will see Machine Locations G28 and G30.
  • Press the Set button beside the G28 values
  • You should see the current position in the G28 display
  • You have now set G28 to your Work Zero position

This is handy anytime you want to return the machine to its Zero position.  Just hit the “Special Position 1” button on the screen, the machine will return to the zero point.  G28 or “Special Position 1”  as well as G30, “Special Position 2” are user programmable position points that can be set to any table position.

Do a Trial Run

Now it’s time to load up the G-code file into your software.  Hit the load button, and locate the file.  It will normally have a .nc , .tap, or .ngc suffix.  The code should be displayed in the g-code window of the software.

Since your machine is still zeroed, you should be good for a trial run.  Make sure the router power switch is off, we don’t want the router running for this step.  Your Z axis should be well above the work.  It must be at least the maximum depth of your cuts above the work, an extra margin of 10mm or so above that is best.  You don’t want it so high that it may run into the upper stop for the Z axis, however.  Now you want to make sure the Z axis position window shows zeros at this point.  If it doesn’t, click the “0” button beside the Z axis position display.  All axis positions should now read “0”.

Ready to go.  Click the “Play” button on the G-code window.  Be ready on the E-stop in case something unexpected happens.  Watch carefully as the machine goes through it’s program.  Make sure the position looks right, and the program ends up where it should without coming close to any hold downs or mounting screws.  If the program is very long, you may not want to go through the whole thing, just hit the Stop button in the G-code Window.  (This Stop button stops sending G-code to the machine, but there is a buffer holding several instructions in advance in the machine itself.  It may take a few seconds for the machine to actually stop moving)

When you are satisfied that everything looks OK, it’s time to generate some sawdust.

Zeroing the Z Axis

Before each time you start your final G-Code run, you should zero your Z axis.  This can be done in a couple of ways.  If your machine is equipped with a Z Axis Probe function, you can use the Probe software in the GRBL program, and a Z axis zero pad connected to your Arduino to set the Z axis zero when you are above your work.

  • Make sure you have the bit you are going to use installed and the collet tightened down.
  • Connect the probe clip to the router bit, and place the sensor pad directly under the bit (make sure the pad is sitting on top of your work piece)
  • Move the Z axis down until the bit is less than 10mm above the pad
  • Enter the manual G-Code [G38.2 Z-10 F50] (without brackets). This will move the Z axis down up to 10mm, at a very low speed.  This can also be programmed in as a Macro with the new version of GRBL Panel.
  • When the bit contacts the pad, it will stop
  • Enter G92 ZXXX where XXX is the height of your pad in mm. (this command can also be part of your macro)
  • Your Z axis indicated height is now shown as XXXmm on your screen, and the Z axis is calibrated.

The Old School manual method of doing this is similar, but a bit of paper is used to determine when the Z axis is down:

  • Bring the bit very close to your work surface, a millimeter or two above it
  • Put a piece of paper on the work surface between the bit and the work
  • Set your Z axis jog distance to .1 or  .01 mm
  • Jog the Z axis down manually, while sliding the paper back and forth under the bit
  • When the bit traps the paper against the work, your bit is touching the surface
  • Set the Z axis to 0 at this point.  It may be prudent to use the Disconnect/Reconnect to ensure that everything is properly zeroed at this time.

Now you can raise the Z axis height up a few mm using the jog buttons.  This is just to ensure it starts out above the work and doesn’t hit anything at the beginning of the program.

Squaring the Gantry

Before running your program, it is a good idea to square up the gantry.  No gantry is flex-free; it is always possible for one of the motors to be a bit out of synch on a 2 motor Y axis drive system.

  • Using a small, accurate ruler, measure the distance from one gantry plate to a convenient point on the v-slot at the end of the axis.
  • Now measure the distance from exactly the same points on the other side of the gantry.  These distances should be exactly the same.  If so, your gantry is square and does not need adjustment.
  • If the measurements are not the same, simply move one side of the gantry by turning its motor pulley by hand (do not just reef on the gantry – it is too difficult to control the movement) until the measurements are the same.  On a lead screw type machine, rotate the motor coupling on the side with the shorter measurement until it equals the measurement from the other side.  On a belt drive machine, slowly rotate the pulley on the motor until the measurements match.  Power must be off to the machine to do this step.  The motors are locked in place when the power is on.

This should be all there is to it.  The gantries should stay square after setting, unless the machine hits something or one motor is blocked from moving for some reason.  It’s a good idea to check gantry squareness before every job just to be sure.