Search the Community

Hot off the press from G&W in Portugal is this compact solution to rough-radiusing fingerboards quickly using your router. Machined from CNC-cut aluminium with a black anodised finish, this jig is designed to be tough and precise like a good shop tool should be. The jig consists of two parts; the sliding router base and a lower sled. The base rides over the top of the sled, indexed off the radiused guides whilst the sled is designed to move back and forth over the fingerboard. The complete jig is available in the most common radii (7.25", 9.5", 10", 12" and 16") with additional radius side plates as an option. Bases are compatible with the Makita RT070xC, DeWalt D26200 and Bosch GKF600/Colt, however any other compact router should be easy to fit with a little modification. The jig can accommodate a 71mm wide fingerboard, allowing the radiusing of 7-string and bass fingerboards in addition to standard guitar sizes. Everything arrived neatly packaged as always. The torn foam was my fault! All parts individually wrapped Beautifully finished. Two minutes, easy to assemble. All of the screws and tools required were included. The fixed base of my Makita RT0701C fits perfectly. Price as of writing is €129,90 from Guitars and Woods. Keep your eyes peeled for our in-depth review of the jig in use.

As regular readers here at ProjectGuitar.com you will have followed the first two parts of this series of write-ups regarding the machining of fret slots on a compact CNC machine; the kind of machine typically available for less than $1000 on various online vendors. Part 1 dealt with the construction of a special jig that allows the accurate positioning of the fret board blank such that precise alignment between the two milled halves can be achieved. Part 2 covered the necessary formatting of the CAD design of a fretboard created with the FretFind2D web application, such that the milling process was safely executed without damage to the fragile endmills. In this, the third and final article we will finally use the jigs and CAD/CAM files and complete the milling of a fretboard on the CNC machine. Endmill Choice Throughout this article I will be using a 0.6mm (or 0.023") diameter endmill to cut the fret slots. The width of this cutter determines the width of the slot being cut and should match the width of the tang of the fretwire being used. In practice a 0.6mm endmill will cut a slightly wider slot by perhaps a few hundredths of a millimetre, due to eccentricity and runout in the spindle. This is advantageous to us; if the 0.6mm cutter could possibly cut a slot exactly the same width as the fret wire tang it would be very difficult to seat the frets. A little bit of leeway will actually help the frets go in easily. You will recall from Part 2 that we limited the final depth of cut to only 1.5mm. It is probably quite obvious that if the fret slot is only this shallow, after radiusing the fretboard this will not leave much depth at the sides to fit the fret wire tang. There are two reasons for limiting the depth of cut on the CNC: The process of slotting the fretboard on the CNC machine is quite slow and wear on the tiny endmills is relatively high. Effectively we are only using the CNC machine to accurately start the fret slot, While it is possible to machine the whole board to the correct depth, it is recommended that cutting the final depth of the fret slot be performed using a hand fret saw with a depth stop. The final accuracy of the slotted board should not suffer from finalising the slots with a handsaw. The low-cost CNC machines may have poor eccentricity specs for the spindle. If this becomes too severe and the fret slot being milled widens too much at the full depth the risk increases of the fret wire not being securely held in place. As ironic as it may sound, it is better that we rely on the CNC as little as possible to maximise our success in this area . Finally, it is highly recommended that you purchase decent quality cutters for this work. Cheap cutters increase the risk of breaking partway through the milling process. They will also likely dull more quickly, and leave behind slots that gradually deteriorate in quality as the work progresses. The endmills I am using are 2-flute cutters made by Kyocera, and are available in bulk packs of 5 or more from several online outlets. Higher-quality endmills with three flutes are also available for a corresponding increase in price - $25 or more for each piece. Right. Enough talking. Lets get machining. Milling the Board Assuming you have a suitable fret board blank at your disposal, use some double-sided tape to secure it to the MDF jig. Position it such that it is centred on the plate as closely as possible. Good planning will dictate that your blank will be cut oversize to allow the excess to be cut off afterwards (it is cut oversize, right?). In this example I am using a piece of Tasmanian Oak. Fit the base plate to the CNC table and tighten it securely. Install the jig with the attached fretboard such that the two holes nearest where the highest fret will be cut are located on the forward holes on the plate. Install some 1/8" pins or spare 1/8" shank cutters in all four corners so that the jig is held securely on the baseplate. Remove the lower-left pin and set it aside for a moment. Turn on the CNC machine and start up the motion control software. Fit a 0.6mm diameter endmill to the collet and home the axes to the extreme minimum limits of their motion, ie X and Y at lowest-left corner of the table and Z at maximum height. Jog the cutter head to just above the centre of the lower-left hole. The and X and Y co-ordinates at this location will form the reference point for the whole milling operation. With the cutter head positioned here touch off the X and Y axes only - do not touch of Z axis yet. Retract the cutter head back from the table and reposition it such that the tip of the endmill just touches the surface of the fret board blank. Do this carefully as you do not want to snap the endmill by accidentally driving it down into the workpiece. Only touch off the Z axis to this position, Re-install the lower-left pin in the jig and load up the first half of the G-code for the fret board job. As we have the fret board blank positioned at the lower end of the table we will be cutting frets 24 to 9 first. If you analyse the toolpath for each of the fret slots on the screen you will notice that each slotting operation is represented as a series of shallow zig-zag patterns gradually increasing in depth until the final depth of cut is achieved. These are the G-code slotting subroutines we created in Part 2. If all appears OK on the motion control software, start the spindle and begin the cutting program. Watch the axis motion and spindle behaviour carefully to see if anything untoward is happening such as excessive vibration or slipping of the fret board on the jig, and be ready to hit the emergency stop button on the mill. Assuming the feed rate is set to around 300mm per minute the first 16 fret slots will take around half an hour to complete. It is a good idea to keep a vacuum cleaner handy while the cutting progresses, as a fair amount of dust and miniature chips will be generated during cutting. Keeping the fret slots clear of chips will also help with minimising wear on the endmill. When the final slot has completed you should have something similar to below. Switch off the spindle, but do not close the motion control software or turn off the power to the CNC machine. We need the machine and software to retain its home and touch-off co-ordinates. Remove all four pins from the jig and slide the plate down such that the first 16 fret slots are overhanging the front of the table. Re-insert the pins in the four holes to re-secure the jig to the bedplate. In the motion control software load up the second half of the fret slotting job. This file should contain the slots for frets 8 to 1, plus the nut position. With this file loaded, turn the spindle on and run the code. The cutter head should advance to the beginning of the 8th fret slot and begin cutting. Again, keep a close eye on proceedings and be ready to hit the E-stop button if things appear to be going amiss. As the number of frets being cut has reduced by half the job should take around a quarter of an hour to complete. With the nut slot cut and the cutter retracted to a safe distance from the workpiece, switch off the spindle and remove the four pins. The final product is shown below: All that remains now is to gently prise off the board from the jig with a paint scraper or similar, and cut the sides to match the taper of the neck you are building. Further thoughts While we have only machined the slots into the fret board lank, there's no reason why you couldn't perform further machining tasks while the fret board is attached to the jig. All that is required is to create the associated toolpaths from the original CAD drawing, split the toolpaths at the same point that the fret slots were split and run the extra stages as further two-part tiles: Using a larger cutter (say 1/8" diameter) the perimeter of the fret board could be machined to give you the correct taper, and also cut off the extremities behind the nut and beyond the 24th fret. If the truss rod you are installing in the neck is the spoke wheel type (with the adjuster at the heel) the notch at the end of the fret board that is normally cut to provide access to the adjuster head can be easily included in the fret board outline. A nut ledge or nut slot could be cut in place of the zero fret slot that we cut in the above example. If your build included a zero fret and nut this could also be incorporated. Multi-scale fret boards can also be machined using the same technique as outlined in these articles. The fret slots are still defined as straight lines, and the slotting subroutines described in Part 2 will work without any modification. Pockets for fret board inlays can be milled in the same fashion. With a little manipulation in CAD/CAM it is also possible to machine precisely sized inlays from contrasting timber, plastics or non-ferrous metals to match these pockets. The fret board radius can be roughed in on the CNC machine, either by progressively running the cutter head in an arc around the Y-axis up the length of the fret board, or by running the cutter head in straight lines parallel to the centre of the fret board in a "staircase" pattern that approximates the radius.

In the previous article on fret slotting using a compact CNC machine we explored a sectionalised approach to milling a big object in multiple stages, also known as tiling. We also went through the process of constructing a jig that allowed us to accurately position the workpiece such that the end of the first stage of the milling process would align successfully with the next. In this week's write-up we will go through the process of generating a custom template using the online FretFind2D fret board designing tool and formatting the drawing and G-code ready for the milling process, Let's assume that we're in the process of making a guitar and, for whatever reason - be it ergonomic, tonal, a request from a client or sheer curiosity - the design has called for a slightly unusual scale length of 24.6" with 24 frets, made from some eastern-Martian Grumblebum wood we have laying around. No ready-made pre-slotted fret board can be found with this scale length in the timber that we want to use, so we're stuck with having to make our own. Designing a fret board with a particular scale length in itself presents no real challenges; there are several online calculators that will automatically spit out the a table of fret spacings based on an input of scale length It's just a matter for us to transfer this table of measurements onto a blank piece of timber and start sawing away. But in our case we want more precision than simply eyeballing the cut. FretFind2D is an excellent online tool to assist with laying out a graphical representation of a fret board based on some input parameters. It also includes a DXF export function that will generate a CAD drawing file that can be (almost) directly used to generate the G-code in order to drive the CNC mill. Based on our design requirements lets enter the appropriate values into FretFind2D and make up our fret board layout: Units = Inches Scale length = 24.6" String width at Nut = 1.375" String width at bridge = 2.125" Fret board Overhang = 0.125" Calculation method = 12th root of 2 Number of strings = 6 After entering the above data click on the 'DXF - Save to Disk' button and choose a convenient name and location to save this file as. Upon opening this DXF file in a CAD application it is clear that a little formatting work will need to be done before we can start milling; Along with modelling each fret position, FretFind2D also includes the generation of the strings and bridge location, which we won't need when milling the fret slots. Spend some time deleting the unnecessary components - the strings, fret board edges and bridge position lines are not required for our work. I also like to orient the drawing such that the nut is at the top of the screen rather than at the bottom (as FretFind2D positions it in the export), If you normally work in metric units of measurement, scale the drawing up by a factor of 25.4 or allows your software to convert it. You should end up with something that looks similar to this: You will recall in the previous instalment of this series we created a CAD drawing of the fret board holding plate, including the drill hole locations for the tiling jig. We need to now open this drawing and copy it into the fret board layout. When doing so ensure that the lower-left drill hole position gets inserted at X0, Y0. When this is complete re-position the fret slots such that they roughly sit in the middle of the fret board holding plate. Absolute accuracy isn't critical, just make sure you have roughly-equal space around the fret slots: Note the position of the middle drill holes on the tiling jig relative to the fret slots. When moving the fret slots onto the tiling jig, position them vertically such that an imaginary horizontal line drawn between these two holes would fall within the gap between two frets. One limitation of the drawing generated by FretFind2D is that it models each intersection of a fret with a string as a short 'fretlet', each one overlapping the next to give the impression of a continuous line. What we really want is each fret to be a single line. Depending on the CAD package used it may be possible to select each group of 'fretlets' and perform a union operation on them. Failing this we will need to manually rebuild the fret lines. Fortunately this is a simple task of using the existing outer end points of the 'fretlets' to draw straight lines utilising object oriented snapping. It is also a good idea to place the new one-piece fret lines on a new layer to assist with being able to delete or turn off the original 'fretlets' that FretFind2D generated. In the example below I have created two new layers - one for the redrawn frets below the midpoint of the jig (green) and one for the frets above the midpoint (yellow). Now we have our fret board formatted it is time to split it into the two tiles for our jig. Select the upper 8 frets and move them down using a middle drill hole as a start point and a lower drill hole as the end point. The result should look like this: While this looks messy at the moment, each layer can be independently turned on and off to display each half of the fret board. This forms the basis of the phyical alignment of the two tiles that need to be cut on the machine to complete the full fret board. In the above image, the green slots would be milled on the fret board blank in the position as shown. At the end of this milling operation the workpiece gets shifted down and the yellow slots are then milled at the positions shown. But because the fret board blank has been moved to a new position the remaining yellow slots get milled above the relative position of the green slots, thus completing the full fret board. Turn off any remaining layers and leave the (green) layer containing the lower 16 frets visible. Perform a CAM export of this drawing with a feedrate of 300mm/min and a Z depth of -0.3mm (or 12 inches/min, Z-0.0118" if you work in imperial units). Switch off the lower-16 layer and switch on the upper-8 layer. Perform a CAM export of this display with the same values as before. You should now have two G-code files describing the geometry of each half of the fret board. It is tempting to now simply run these two G-codes and complete the fret slotting operation, and indeed you could conceivably run these G-code listings and have the slots scribed onto a timber blank right now. The limitation is that we currently are only cutting the slots to a fixed depth of 0,3mm. We want the fret slots to be deep enough to accept the tangs of our fret wire, which could be a couple of mm tall. So maybe we could increase the depth of cut when we export the G-code from CAD? The problem here is that the cutters used to mill a fret slot are only 0.6mm in diameter and extremely brittle. Attempting to move such a tiny endmill through a hard material like ebony or rosewood at the full depth is likely to immediately destroy the endmill. So perhaps we could run the entire program multiple times and bit-by-bit increase the depth of cut on each successive pass? That is an option, provided your step change in cutting depth is quite small. The risk here is that even if the cutter is plunged in only a small amount the sudden lateral jerk as the endmill begins its traverse slotting operation can again stress the cutter too much and break it. The process of copying and pasting the entire run of code many times over is also very wasteful and hard to follow if something needs debugging. What we can do is gently ramp the endmill into each cut and zig-zag our way to the bottom of the slot. That way we can break up a deep slot into smaller steps that won't overly stress the endmill, and avoid the shock of suddenly forcing the cutter to remove too much material as soon as we move sideways after plunging: Anyone who spent time at school in the computer lab may recall programming FOR-TO loops or IF-THEN-ELSE evaluations using BASIC language. G-code features similar abilities to run repetitive milling operations and allow milling parameters to change based on variables. We can use this feature to implement our zig-zag slotting operation and make the code run more efficiently. Below is the first few lines of one of the raw fret slot G-code listings for our fret board. The code dealing with the first slot has been highlighted: Each fret slot is nothing more than a horizontal line between two points - X18.297 Y50.087 and X73.22 (the second instance of Y50.087 is not required as it only needs to be defined once when describing a straight horizontal line). Initially what we want is for the endmill to run repeatedly left and right between the two points . Using pseudo-BASIC code this could look something like the following (NB, there is no literal G-Code equivalent to a GOTO loop, this is just for illustrative purposes): Each subroutine must have a unique 'O' number. When the subroutine starts the cutter moves to X18.297, Y50.087. The next line plunges the cutter into the workpiece by 0.3mm. The slot is then cut with the endmill moving to X73.22 with Y unchanged. The endmill then moves back to its starting position of X18.297. (NB, the return X co-ordinate is simply copied from the original start point of the fret slot, three lines above it). The 'GOTO LOOP' command at the end of the subroutine returns us to the start and the process is repeated. Shuttle right. Shuttle left. Repeat. But we're still not moving the Z axis any deeper than 0.3mm, so no change in slot depth is being achieved. The other bug in this program is that because the 'G0 Z2' line falls outside the O100 LOOP it never gets executed, and the cutter remains stuck at a depth of Z-0.3mm. The next trick we need the cutter to do is gradually ramp the Z-axis down on each left-to-right run to increase the depth of cut. G-code allows the use of variables to substitue for direct co-ordinates. If we assign an automatically-changing variable to the Z-axis we could increase the depth of cut gradually to perform the ramping operation: Breaking this down line by line: A variable called #1 is assigned a value of 0 and a second variable #2 is created with a value of 0.3. On the first run of the subroutine the cutter will move to X18.297, Y50.087. The cutter then gets plunged to Z=0 (the value assigned to #1 gets substituted in place of the literal Z co-ordinate). The value currently stored in variable #2 (ie, 0.3) then gets subtracted from variable #1 (ie, 0) and the result stored back into variable #1, so now variable #1 has been updated to -0.3. The cutter then moves right to X73.22, and Z uses the new value of variable #1 as its destination. This creates the downwardly-ramping cut that we're after, starting from a depth of Z0 and finishing with a depth of Z-0.3. The cutter then moves back to its starting point of X18.297, but because Z is not listed it simply moves back at the last recorded depth of Z-0.3, flattening off the top of the initial ramping cut. The routine then returns to the top and runs again. Variable #2 once more gets subtracted from variable #1 and the result stored back into #1. But because #1 was set to -0.3 from the last run of the subroutine the new result of #1 - #2 (-0.3 - 0.3) is now -0.6. So when #1 gets used for the next Z co-ordinate it will ramp from -0.3 down to -0.6. With a bit of mental gymnastics it can be seen that on each successive pass of the subroutine Z will continually ramp down in increments of 0.3mm. But we still need some way of determining when we've cut the slot deep enough. At the moment there's nothing to stop the loop running for ever and giving us infinitely-deep slots. By changing our pseudo-GOTO loop to a WHILE/ENDWHILE statement we can place a limit on how many times the subroutine runs before it stops. Here's what the new version looks like: The WHILE/ENDWHILE loop will run until the expression evaluated by the WHILE statement is determined to be false. In our case we have specified that the G-code commands contained between the WHILE/ENDWHILE statements will run until the value stored in #1 is no longer greater than -1.5 ('GT' in the WHILE statement is short for 'Greater Than'). As variable #1 is being used to control the depth of cut within the subroutine and gets 0.3 subtracted from it on every cycle, when #1 eventually becomes less than -1.5 this will trigger the subroutine to finish and jump to 'G0 Z2' which retracts the endmill out of the bottom of the cut, ready to move to the next fret slot. Further refinement of this subroutine can be performed by removing or repositioning unnecessary or duplicated steps within the WHILE/ENDWHILE loop, giving: So now the only thing left to do is step through the remainder of the G-code listing, identify the start and end points of each fret slot and apply the same subroutines to them. Remember to use a unique O-number for each new subroutine. If you get stuck performing this manual G-code manipulation, both the raw and formatted versions are available to download at the end of this article to reference against, along with the DXF files used to generate the fret board geometry used in this article. ---------- In the next and final instalment we will get down to the nitty-gritty of using the fret slotting G-code and finally machine ourselves a fret board. We will also discuss some further ideas and applications of tiling on the CNC machine relevant to guitar building. Fretboard 24_6.zip

If you're a regular visitor here at ProjectGuitar.com you may have caught our four-part series on using a compact desktop CNC milling machine and its application in lutherie. In the first instalment it was mentioned that a CNC is ideal for applications where precision and flexibility is required. One of which was milling fret slots in a fretboard blank, where positioning of the fret slots is crucial to the accuracy at which the resulting instrument can intonate, particularly in the higher registers where a small error in fret placement can result in a a major error in fretted pitch, The trade-off to owning a small CNC machine (or indeed any CNC machine) is that it has a practical limit to how big a piece of material it can fit within the confines of the milling area - the X, Y and Z axes can only move so far before they eventually run into the endstops, and no further reach of the cutter head is possible. If you take a guitar fretboard for example it will comfortably fit within the limits of one axis of even the smallest CNC machines - unless you are building some kind of 17 string monster most fretboards will not exceed more than about 70mm in width. The problem is that the fretboard length is usually in the vicinity of 500mm or more. To machine such a long object on your CNC machine in one hit obviously requires an axis with a reach of at least this length. There is, however, a way of expanding the reach of an axis so that you can machine objects bigger than the physical limits of your CNC machine. By milling the object in two (or even several) stages, moving and accurately repositioning the material midway through the process, it is possible to complete a complex milling operation on an object larger than the CNC router. This operation is known as tiling, and while it presents its own set of challenges and hurdles it is not unheard of to operators of CNC machines; tiling can be often be required no matter how big your CNC machine is - if the client requests an object bigger than your machine, if you simply don't have access to a larger CNC router you'll likely resort to tiling to complete the job. Successful tiling requires that the job be accurately repositioned partway through the milling process, such that the end of the first stage of milling aligns perfectly with the beginning of the next stage. This can be achieved through the use an indexing plate affixed to the CNC bed and a series of locating holes in the workpiece that align with matching holes in the indexing plate. Conveniently for us, we can use the CNC itself to create the indexing plate and holes to minimise any milling inaccuracies that may occur when changing positions. Creating the Jig Materials List: V-cutting engraving tool 1/8" diameter stubby rivet drill 6mm MDF sheet, approx. 600 x 450 12mm MDF sheet, large enough to cover table of CNC machine M6 or 1/4" nuts and bolts (20mm length) Four spare 1/8" drill bits, cutters or other solid rod material (to use as indexing pins) Glue, clamps, pencil, straightedge Patience Most CNC machine beds are made from slotted aluminium extrusions to allow the user to freely affix the workpiece to the bed using nuts and bolts. Our indexing plate will be rigidly secured to the bed and is made from a flat, smooth, easily-machined material - MDF suits our needs admirably. Cut a piece of 12mm-thick MDF large enough to cover the entire bed of the CNC. Neatness and squareness of this piece is not super-critical at this stage. With the MDF laid on the table carefully mark the locations of two outermost channels on the bed to allow us to drill some securing holes for the indexing plate. Drill a hole in each corner that aligns with the mounting channels used on the CNC bed. Use countersunk screws or otherwise recess the heads of whatever bolts you use to secure the plate to the bed. Once the plate has been drilled to accept the mounting hardware, return to the CNC machine and fit the plate to the bed. The slots on this machine will accept an M6 nut, the channels being narrow enough to prevent the nut from turning once the bolt is tightened. Mark a starting point about 50mm in from the left edge of the CNC bed. This will form the origin of a vertical line that will be engraved parallel to the long edge of the table. By using the CNC to scribe this line we ensure that the line engraved is square to the CNC machine's motion, rather than square to the table or MDF edges. This is essential for ensuring accuracy of the jig. Fit an engraver cutter to the collet. Home and touch-off the CNC to the indexing plate at the mark that was created. Most motion control applications include a manual G-code entry mode. This is useful if you want to perform some basic milling operations where generating a comparable G-code would be unnecessary or wasteful. If using LinuxCNC for example, click the 'MDI' tab in Axis (or press F5) to display the manual entry window. By typing G-commands one line at a time we can instruct the CNC machine to perform movements on a step-by-step basis. With the CNC machine homed and touched off to the MDF sheet, switch on the spindle and type the following lines into the MDI tab, pressing <enter> after each. Alternatively copy the below text into a blank G-code file, save and run it within your motion control software: G1 Z-0.5 F300 G1 Y280 G1 Z10 The above listing will lower the cutter to a depth of 0.5mm into the surface of the MDF, engrave a 280mm straight line up the Y axis and then retract the cutter out of the MDF to a height of 10mm, where the spindle can safely be switched off again. The line engraved on the MDF will form the reference to assist with assembling the next part of the jig. Using a piece of 6mm MDF cut a piece about 25mm wide and the same length as the CNC bed. Take care to ensure that one of the longest edges is as straight and square as possible (hint: the factory cut edge from a sheet of MDF is often very squarely machined - use this as the reference edge). This thin strip of MDF will form a fence for the indexing plate. Glue and/or screw the fence to the MDF indexing plate, lining up the square edge of the 6mm MDF to the engraved reference line as closely as possible. Be careful to ensure that the fence doesn't accidentally slip or move while the glue is drying. Using some more 6mm MDF, cut a baseplate large enough to comfortably hold a fret board blank with about 15-20mm overhang on all sides. For example, if your fret boards are nominally 60mm x 550mm, make the MDF plate about 100mm x 600mm. On one of the longest sides sand/cut/file/plane a nice, clean square edge. This edge will ride along the fence on the indexing plate and needs to mate with minimal gaps and bumps. For the next step we will need to create CAD drawing and resultant G-code program to drill the locating holes. The reason we do this is that the CAD drawing of the holes is subsequently used to determine the 'split point' of the fret slotting job when milling in two halves, Without an accurate reference for the split the two halves will never align properly when machined, no matter how well the jig has been constructed. In your favourite CAD program draw a rectangle representing the fret board holding plate at a scale of 1:1 (ie, 100mm wide by 600mm long) with a lower-left corner origin at X-5, Y-5. Make sure the rectangle is drawn vertically aligned such that the longest edge is in the Y-direction. Next, draw four vertexes/points in the locations shown - two positioned 5mm in from the bottom corners and two 5mm in from each side at the exact midpoint of the rectangle (hint: use object oriented snaps and draw reference lines to accurately position these points, and delete afterwards). The critical point is that by virtue of creating a rectangle with origin X-5, Y-5 and then offsetting each edge inwards by 5mm, the lower-left drill hole is at exactly X0, Y0. In the below example the points have been added on a new layer in red. The four points now need to be exported as G-code. When doing so, set the feedrate fairly low (say 50mm/min) and set the Z depth to -10mm. The resulting G-code should look something similar to the following. Note that I have broken up the listing a little and included some comments to better illustrate the four drill hole steps. Now we get to cheat a bit with the CNC machine. The collets on the smaller units are usually designed to accept 1/8" shank bits. A 1/8" 'stubby' rivet drill, with its short cutting flutes can also comfortably fit into the collet of the CNC machine, and can be used to accurately drill the workpiece locating holes for the jig. Re-install the MDF indexing plate and lay the fret board MDF plate on top with the reference edge hard up against the fence. Position the leading edge of the fret board plate flush to the front of the indexing plate and secure in place with some temporary clamps. Fit a 1/8" stubby drill bit to the spindle and tighten securely. Open the drill hole G-code in your motion control software. Home and touch-off the tip of the drill bit such that X0, Y0 is 5mm from the bottom edge of the fret board plate and 5mm from the left edge - this is where we want to begin drilling the four holes. Turn on the spindle and run the G-code - four holes will will be drilled into the holding plate and through to the indexing plate. The final step of creating the jig also serves to illustrate how the tiling technique is performed. Remove the temporary clamps and slide the fret board holding plate down such that the top two holes are now positioned over the bottom two holes in the indexing plate. Insert two spare 1/8" shank cutters or drill bits into these two holes, locking the holding plate to the index plate, and temporarily clamp the top of the holding plate in place to prevent it shifting from side to side. Open up the G-code for the four locating holes and edit out the lower two drill hole entries (hint: enclose the relevant lines within brackets to convert them to non-executable comments). We obviously don't want to re-mill the first two holes, not the least because we now have two pins inserted into them, but we do want to mill the second pair of holes again for the top section of the fret board holding plate. Note that the X90 co-ordinate has now been added to Y295. As the previously defined X co-ordinate has now been disabled it needs to be moved to the new 'initial' drill hole position, which is now at the upper-right corner. Save this file and re-open within the motion control software, but do not re-home or re-touch off the machine. Run this G-code again and note that only the top pair of holes are drilled into the holding plate through into the pre-existing holes in the indexing plate. The jig is now complete and ready to be used. By using four 1/8" pins and securing the holding plate at the lower position the first half of the job can be machined. When this operation is complete the pins are removed, the plate shifted down, the four pins re-inserted and the second half of the job run with perfect alignment between the two halves. ----==---- In the next installment we will delve into formatting and splitting an over-sized job into the requisite halves such that the milling of a fret board can be achieved, and also learn a little about optimising our G-code to run a little more 'intelligently'.