Jump to content

Entry for May 2020's Guitar Of The Month is open - ENTER HERE!


Popular Content

Showing content with the highest reputation since 11/06/2011 in Articles

  1. 4 points
    So you’ve decided to launch yourself into the world of CNC machining. You’ve done some research and lurked around many online forums and resources looking for information regarding which model to choose and what features the unit needs. You’ve plonked down your hard earned cash and a big cardboard box has arrived in the mail containing a bright, shiny new CNC router. It’s been assembled and set up on your desk. Now what? Fundamentally, most basic CNCs will have a bed which workpieces are secured onto and a overhead gantry that travels the length of the table. Onto this gantry a secondary carriage travels over the width of table. The spindle itself is attached to this carriage and can move vertically. The spindle rotates a cutting tool at high speed to remove material from the workpiece. The three movement directions (side-to-side across the table, up and down the length of the table, vertically up and down perpendicular to the table) are the three axes of motion that the machine can operate in; X, Y and Z respectively. Each axis is independently controlled by specialised motors known as steppers, which are designed to rotate either direction by precisely known amounts. The rotation of these motors is translated into simple linear movement (backwards and forwards). Commonly, threaded rods ("lead screws") pulleys or toothed belts are used for this purpose. Larger machines can sometimes use these in combination (such as pulleys for X and Y, leadscrew for Z). Each have their respective advantages and disadvantages in accuracy, cost, speed, load capacity, etc. Lead screws are most common in small CNCs for all three axes. The precise rotation of the stepper motors is controlled through the application of electrical pulses. By co-ordinating the number, length and frequency of the electrical pulses, the CNC machine can be made to execute precise synchronous motions to move the cutting tool around the workpiece in complex paths. The generation of these control pulses is performed either by dedicated standalone control consoles or by software on a common computer. Non-production level CNC tends to utilise the second option; the steppers driven by a simple external interface unit that sits between the machine and PC which handles the translation of the software stepper signals into the heavier-duty control signals that drive the motors. Software generation requires that a motion control application be installed on the host computer. Two of the most popular motion control solutions at the moment are Mach3 or Mach4 (for Windows based computers) and LinuxCNC for (Linux-based operating systems). In this article we will use LinuxCNC to illustrate how to set up the desktop CNC router; fundamentally the operating principles are similar between the Mach-series software and LinuxCNC. Both options require the host computer to have a parallel port for communicating with the control interface. Laptops and USB-to-parallel adaptors are not recommended for software stepper pulse generation. The main advantage of favouring the "old" parallel port standard is that many signals can be sent simultaneously; despite being far faster, USB is purely serial and asynchronous; one piece of information at a time and "arrives when it arrives". Parallel is far closer to being a real-time interface, which USB to parallel adaptors do not reliably replicate. PCI parallel port cards on the other hand are a satisfactory option if your host computer doesn't feature a parallel port. Installation of a Linux operating system and the LinuxCNC application is beyond the scope of this article, however it is extremely simple; LinuxCNC is available as a LiveCD installation, whereby the user has the ability to boot a pre-compiled version of LinuxCNC from a CD, DVD or USB memory stick without installing the operating system onto the computer. This operating system image is available to be downloaded from the LinuxCNC website. A permanent installation of Linux and LinuxCNC can be performed from the LiveCD if the user so chooses at a later date. The first requirement in setting up the CNC machine is to create a configuration file. This contains the specifications of the CNC motors so that they are driven at the correct speed/rate, acceleration, direction, etc. From the menu bar Click ‘Applications’, navigate to ‘CNC’ and select ‘LinuxCNC StepConf Wizard’. If this is the first time that StepConf Wizard has been run a new configuration must be made. The user also has the option of opening an existing configuration to either adjust existing settings in their recently created configuration, or use another configuration as the basis for their new CNC router. In this case we will create a new configuration from scratch. Click ‘Forward’ to move to the next page in the StepConf Wizard. In the next screen the configuration can be given a meaningful name and basic setup parameters defined, such as units of operation (millimetres or inches), how many axes the machine operates with (in our case three axes – XYZ), parallel port addresses and driver signal timing. If your CNC machine comes with data or a user manual then use this to set the driver timing settings. If there is no data supplied you may have to search online to find some information regarding the suggested timing parameters, or experiment to find the best trade-off for reliable operation of the CNC router. Step Time and Step Space - the width of the electrical pulse applied to each stepper motor and the subsequent gap between each successive pulse, expressed in nanoseconds. Too small a step pulse or space and the motor will miss a step. Too long and the CNC axis movement can become unacceptably slow. Direction Hold and Direction Setup - In addition to the step pulses themselves, secondary signals are generated by the motion control software that change the order of the pulses being applied to the steppers. Changing the order of the pulses changes the rotation of the motors from clockwise to anti-clockwise. The "Direction Hold" and "Setup" parameters define the amount of time the direction signal applied to a stepper motor needs to remain activated after a step pulse has been issued, and the amount of time the direction signal needs to be applied to the stepper before issuing the next step pulse. Too small a direction hold or setup and the motor can miss a change in direction and overshoot its intended stop point. Too long and the CNC axis movement can become unacceptably slow. In most cases the values shown will work as-is and require no further adjusting. The last key item that requires attention on this page is the ‘Base Period Maximum Jitter’ setting. Instructions to the CNC (via the interface) are generated by software, so there is a potential that something occurring in the computer or operating system outside the control of the CNC machining application may interrupt the continuous supply of timely instructions (eg. graphics redrawing on the screen, hard drives being accessed, etc). Consequently we need to ensure that any interruptions that do occur do not interfere with the normal operation of the CNC machine. To find out what this minimum safety net should be the StepConf Wizard includes a ‘Jitter Base Period Test’ function. After running the test for a few minutes this returns a suitable ‘Base Period Maximum Jitter’ value. This states how much the system might be expected to be delayed during normal operation; the configuration then makes sufficient allowance to avoid interruptions in the generation of the stepper control signals. Click ‘Forward’ when all fields have been filled in. Leave the Advanced Configuration Options unchecked at this stage and click ‘Forward’ again. The Parallel Port Setup screen is where we define what each pin of the parallel port on the computer is expected to do when connected to the CNC machine. Again, consult any data or the manual supplied with the CNC router to determine how each pin is to be connected. As we are configuring a basic 3-axis machine the minimum required pins to be configured will be X Step, X Direction, Y Step, Y Direction, Z Step and Z Direction. The other important pin to configure is the Emergency Stop (or E-Stop) input from the machine. Nearly all CNC machines will be fitted with a large E-Stop switch that the user can hit in the event that the machine begins executing some unintended moves, and signals the motion control software to unconditionally stop moving the axes. The next three screens are used to configure the behaviour of each stepper motor; their speed, acceleration and limits of travel. Each axis is configured independently but the options presented are identical: Motor Steps Per Revolution – how many steps the motor needs to perform to complete one full rotation of the shaft. Manufacturers of stepper motors often express this value as degrees per step. If your stepper motor has this value specified as 1.8 degrees per step then Motor Steps Per Revolution is equal to 360 degrees divided by the degrees-per-step value, or 360/1.8 = 200. Driver Microstepping – the resolution of a stepper motor can often be increased by the action of microstepping. The basic degrees-per-step specification of the motor is enhanced by the driver forcing the motor to make an intermediate ‘soft’ step in between each 1.8 degree ‘hard’ step. In the same way that a picture with higher resolution can display more detail on a computer screen, a stepper motor with more resolution can perform finer movements. The trade-off is that the more microstepping you add the less torque that motor is able to generate. In practice a microstepping value of either 2 or 4 is a good compromise. Note that if you set microstepping to 2 it will require that Motor Steps Per Revolution be increased to 400 to maintain the relationship of the number of steps to complete one revolution of the motor shaft. Setting microstepping to 4 will require Motor Steps Per Revolution to be set to 800. Pulley Teeth – only required for CNC machines that use pulley systems to drive the axis. This is where you would specify the gearing ratio of the pulleys. We are using a lead screw in the desktop CNC machine so leave these two fields set to 1. Leadscrew Pitch – the pitch determines how far each axis will travel when the lead screw is rotated one full revolution, and its setting is critical to ensure that the axis travels the correct distance when commanded to do so. If the units of operation specified earlier were inches then the lead screw pitch is expressed as threads per inch. If millimetres were specified then this value is expressed as millimetres per revolution. Consult your CNC machine datasheet for information on the specifications of lead screw fitted. As an alternative most lead screw pitches can be measured reasonably accurately by using a ruler to count the number of thread ‘peaks’ within one inch, or the distance in millimetres between two successive thread peaks. Maximum Velocity and Maximum Acceleration – sets the maximum speed and acceleration of the axis before the CNC machine starts missing steps or losing accuracy when changing directions. As no real life object can accelerate from a standstill to full speed instantaneously, we need to specify a value in the ‘Max Acceleration’ field to limit how quickly the CNC motion control software tries to make the machine change its speed when either accelerating from zero, coming to a stop at the end of a manoeuvre, or changing directions suddenly when transitioning between two trajectories. In general this is set by experimentation with your particular machine, but the values presented here should work with the smaller desktop CNC routers as a starting point. Home Location – the default location the axis will set itself to when the machine is told to ‘return home’. The home location can actually be anywhere you like within the axis limits of travel, but is typically set at 0 (which would equate to the lower-left corner of the table with the Z axis at maximum height). Every time the software is started up the physical location of the CNC machine is undefined. Until the CNC machine is homed it cannot know where its limits of travel are (below) and therefore cannot commence a machining job. Table Travel – specifies the ‘soft’ limits of motion that the axis can move within, and is expressed as either millimetres or inches depending on how the units of operation were set earlier. For each axis this is typically set to the maximum travel that the axis can move to before reaching the end stops. When the motion control software detects that the axis has reached its soft limit it will not attempt to drive the CNC router beyond this value. Note that when setting the Z axis the Table Travel fields are normally set as a negative number to zero, rather than as zero to a positive number. The convention here is that the Z axis moves negatively with respect to the surface it is bearing down upon. The last option for each axis is the ‘Test this Axis’ function. Clicking on this will bring up a window that allows the user to see if the configuration created thus far is appropriate for their machine. With the CNC router connected to the computer and powered up the axis under test can be manually moved using the two ‘Jog’ arrow buttons, or the axis can be set to automatically swing back and forth by a set amount according to the ‘Test Area’ fields. This is useful for determining if the axis is moving by the correct amount based on the ‘Motor Steps Per Revolution’ and ‘Lead screw Pitch’ settings, and also if the ‘Max Velocity’ or ‘Acceleration’ settings are going to result in missed motor steps. Assuming that step direction was set up correctly earlier under the ‘Parallel Port Setup’ window for each axis, clicking the right ‘Jog’ arrow should make the X axis move towards the right of the table, the Y axis move away from the front of the table and the Z axis move vertically upwards. Clicking ‘Forward’ after configuring the last axis and then ‘Apply’ will create an icon on the desktop allowing the user to launch the motion control software using the created configuration file. And that’s it! If you’ve made it this far you’ve successfully created a configuration file to suit your CNC router. By double-clicking the 'launch CNC-router' icon on the desktop, the configuration file will pre-load all the necessary parameters for the CNC machine and start up the motion control software. ---------- In the next article we will begin creating a basic G-Code file to run the CNC router with. In doing so we will also verify that the machine operates correctly, and the axis motion is correctly scaled to create 1:1 cuts in preparation for applying the CNC machine's abilities to creating luthiery-related components.
  2. 3 points
    Fundamentally, two types of guitar neck construction exist; single and two-piece. In a single-piece neck the headstock is cut into the same piece of timber as that of the rest of the neck. In a two-piece neck, a separate headstock part is joined onto the longer part comprising the greater length of the neck using a scarfed joint. Origins Of The Term The term "scarfed joint" reaches back to traditional timber building and ship construction to denote a type of joint used to produce a long piece of timber where one single piece would not otherwise be possible. The joints themselves were often complex and varied, not glued and instead used a combination of friction, mechanical locking using wedges/pins, fasteners, gravity, etc. The development of strong adhesives beyond simple protein glues changed joinery and produced a whole new book to describe them. The term "scarfed joint" was appropriated and used to denote both the a lengthening strategy for joints glued at an acute angle for increasing mating surface area for glueing and as a method for improving the cosmetics of joints that would otherwise require weak and aesthetically poor butt joints, such as veneer wrapped around a cylinder. The term has again evolved in usage to describe how a two-piece neck is constructed for a guitar, derived solely from the increased mating surface areas they produce for glueing. In some ways it has become simplified over its original base meaning. So much so, the more descriptive and correct term "scarfed joint" has devolved into "scarf joint". Both are correct in the context of guitar neck construction through adoption (language and meaning evolves) however we'll stick to the more specific term "scarfed" for this article....we'll see why this is meaningful later.... Headstock Angles Most people will be familiar with the difference in headstock angle of a Gibson Les Paul versus that of a Fender Stratocaster. Whilst Fender-style designs have a headstock that lays in the same flat plane as the rest of the neck (zero headstock angle), headstocks of Les Paul-style headstocks typically fall away at an angle anything from a few degrees up to 20°. A few terms exist such as "angled headstock", "tiltback headstock" however they all represent the exact same thing; that the plane of the headstock is at an angle with respect to the rest of the neck. Angled headstocks offer benefits over flat headstocks, such as greater string pressure over the nut and the elimination of string trees. A side benefit is that they can also allow for easier access to the truss rod for adjustment. Why Use A Scarfed Joint? The main two reasons that scarfed joints are used is for the strength that they add to the finished workpiece and also one of economy. Many builders also incorporate aesthetic values to their scarfed joints as a secondary aspect, which in many ways also distracts from the true purpose of the joint being there in the first place. Wood Strengths/Weaknesses Wood is not an isotropic material; it is weaker parallel to the grain direction and splits along this easily. For necks whose length is more or less in line with the grain, (flat zero angle necks or very shallow angles) this is rarely a problem. The grain travels uninterrupted along the entire length from one end to the other. Headstocks angled against the direction of the grain build in an inherent weakness called short grain. This is simply the path of least resistance through the grain into and out of the wood, in this instance from the rear of the headstock a short distance through to the front. The greater the angle of the headstock, the shorter the grain distance and the weaker the headstock. Areas of short grain (red) in a single-piece angled headstock against normal grain direction (green) Short grain is one of the main reasons that Gibson guitars and basses are so prone to headstock breakage. Decades of adherence to their traditional building style maintains this weakness in spite of a simple solution having been around for far longer. The scarfed headstock joint. By glueing a second angled piece of wood to the first to produce a scarfed joint, short grain is virtually eliminated Economy It should be fairly apparent that a headstock angled against the plane of the timber increases the minimum dimensions that the timber is required to have for a single-piece neck, increasing the waste factor. Several strategies are possible for turning this into a more economical venture by employing a simple scarfed joint. The following diagram shows how shorter material can be used economically by recovering material wastage underneath the neck and using it as a scarfed headstock: Volutes In guitar terminology, a volute often refers to a strengthened area behind the union of the neck shaft and the headstock. These are useful for a number of reasons, not all of them related to scarfed joints. In this context however, they can be useful to lengthen grain when scarfing on a thicker headstock component that would otherwise invite short grain under the first two frets. Volutes also offer cosmetic options for hiding the join line; same as how a headplate can be added to the top of the headstock, a bent "backstrap" can be added to the rear face. A thicker scarfed headstock can add short grain from under the headstock The addition of a volute lengthens the area of short grain, adding vital strength Types Of Scarfed Joint As touched on earlier, the term "scarf joint" is less meaningful than "scarfed" since we're really discussing the idea of two-piece construction over single piece rather than any specific type of joint. There's no language police here, and both terms are just as correct through widespread usage and basic adoption. It is however useful to consider that there's lots of ways to achieve this end. The most common type of scarfed joint is that shown above; an acute face milled into the end of the neck, and a second flat piece of wood glued on. Several common methods exist to create a scarfed joint, however they all have two common aspects; they increase the mating surface areas of the two parts to ensure a strong glue bond whilst eliminating as much short grain as possible. The two most common types of scarfed neck joint; over and under the neck Notable exceptions to the common approaches on scarfing a headstock joint are the V-joint employed by Martin and many classical guitar makers, however this is seldom found on electric guitars or steel-strung acoustics. Cosmetically, this style of joint can be accentuated into a "dart" or even a diamond-shaped volute. Making a V-joint - https://www.youtube.com/watch?v=KocJHchKVZQ ....or the far more weird finger joint as employed by industrious inventor Bob Taylor: It might look strange, however as well-engineered as joints go this is near perfect in all but cosmetics In Closing Scarfed joints are an important building technique to increase the reliability and durability of guitar necks with angled headstocks, plus afford us opportunity to use raw materials more responsibly. However the joinery is approached, a well-planned and executed scarfed headstock produce an end product that can be both beautiful and superior to those made from a single piece of timber. They simply need to be applied to the problems that they are intended to be solving. Over in the tutorials section, we'll look at the different techniques used to produce basic scarfed joints plus jigs to simplify the various processes....
  3. 2 points
    Laser cutting takes what we engineer at the desktop and brings it out into the real world. For a luthier, this enables creating our most common working tools - router templates - to be made simply yet precisely. A real game changer! Translating creative or technical design work into router templates opens up a world of design options. Anything from an accurate outline of your body/headstock, pickup and electronics cavities, through to complete modular templating systems for recessed tremolos, etc. Powerful desktop design tools and laser cutting takes your building to the next creative and technical level. "Having it laser cut" sounds like a magic bullet of sorts; draw something up and having it drop out of the other side with little to no real effort. That's not actually too far from the truth; the technology is definitely more usable and accessible than it ever had been. The key to winning lies in mastering a number of simple fundamentals and managing a few basic expectations. Once you've moved beyond these, laser cutting becomes a very workable part of your armoury and one that you'll always find new ideas and challenges for....and like any tool, it is only as good as what you make of it! ----==---- ARTICLE SCOPE - The focus of this article will be on how to locate and choose the right laser-cutting service, illustrate the desktop work necessary to produce drawing files that are pretty much good to cut and finally show a couple of real-world working examples. We are making a few assumptions here. First is that you know basic vector work (AutoCAD or other CAD packages, Illustrator, Inkscape, CorelDRAW, etc). Secondly, that you are more or less familiar with manipulating vectors, managing object types, inspecting and changing their attributes, etc. with your chosen vector drawing package. Beyond this, laser cutting is a pushover! ----==---- CONTENTS - 1. Finding Your Laser 2. Starting Out - Communication Is Key 3. Design-Time Considerations 4. File Exchange - Break It Down To Basics 5. Example 1 - Simple Bench Hold-Down Templates 6. Example 2 - Electronics Cavity Routing Template Set ----==---- 1. Finding Your Laser Okay, well we have two options for getting our templates made. First - getting your hands dirty at a Makerspace, Hacklab, community college/educational facility or wherever else offers public/membership access to a suitable laser cutter. By far, this is the best way of extending your skill set; your time can be spent fine-tuning (or replacing!) your templates hands-on. You have end to end control. This might be a bit more costly in the short term; mandatory safe usage courses and basic fees are a necessary price to pay. You'll probably burn through a lot of material (joke not intended, but apt) in your first attempts too. It's definitely a swift and easy complete control solution once you've ticked those boxes, and the cheapest route for the habitual user. The scope of this article is not intended to take any precedence over the advice you're given during laser cutter induction. Every location will have its own set of house rules, so rely on their expertise and recommendations. Every laser is different, every facility is different. The tutors who do this are your gurus, so drop preconceptions and let them guide you. The other option is reliance on third-party services. These can vary from brick-and-mortar shop/bureaus like Mostly Out Of Cardboard, turnkey online services such as Ponoko or specialist guitar supply companies with in-house custom laser cutting such as Guitars and Woods. Third party services are not necessarily an inferior choice or even an expensive one, however you do need to shop around for a service which understands your requirements and preferably does this work all of the time. Your local trophy maker "who happens to have a laser" might charge you well over the odds for the inconvenience of reconfiguring their machine for a one-off sheet job, however simple. It might simply not pay as much money on the hour as their normal line of work, or be an alien process to them. Even a shop signage maker who cuts sheet day-in day-out might not offer an attractive price on small one-off jobs. Third-party services have the advantage of experienced operators, and you should use that. Ask if they've cut templates for luthiers or woodworkers before. Familiarity - or at least an understanding - of what you're wanting to achieve is 90% of the battle won. If they've done anything similar before, they might be able to suggest improvements on your basic design for future work or simply snag any errors in your work submissions. If they haven't, gauge whether they're open to the idea of what you're wanting and understand its purpose. Companies that are genuinely interested in your product and having you as a satisfied customer are worth fostering a relationship with....as long as that isn't simply a way of sleazing deeper into your wallet! A lot of creative and inspirational people work in laser cutting services, Makerspaces and community colleges. Often the opportunity to collaborate on something new and exciting (as exciting as router templates get?) is more important to them than a bit of time or turning a quick buck. Some operators are genuinely excited just to see new things come off the laser and might be happy just for the cost of materials. "Head towards the people that have that creative spark and not the jaded old farts who might just see you as an inconvenient interruption to their non-stop conveyor belt of boring paint-by-numbers imported Chinese component school sport's day trophies given out just for participating rather than representing real achievement." - Benjamin Franklin ----==---- 2. Starting Out - Communication Is Key The people you need to be on friendly speaking terms with from day one are the keyturners or regular users, whether they're engineers on the other end of the phone, colleagues, Makerspace tutors or fellow denizens; whoever. Laser cutting is a fairly simple process with a few hidden tricks and obstacles you need know before you encounter them. Communicating your needs and existing knowledge will produce a smoother process from your desktop to the finished item. Design Protocols There are basic conventions within drawings which denote how the laser driver will interpret the job. We'll look at these later, however you should ask your service what their own in-house conventions are, or check with the other people in your Makerspace, etc. how to set up the drawing appropriately to work with the default laser configuration (this should be covered during safe usage courses). Firstly this saves time fixing things in the mix, or worse, trashing good material. Most importantly it may ease third-party setup charges if your drawing is good to go straight to the laser. It definitely gives you room to negotiate that cost. It has to be borne in mind that services will likely operate an hour rate on setup. These charges are superfluous when a drawing is poorly designed or doesn't conform to house protocols and needs the attention of an engineer or operator! We have a dedicated thread on laser cutting over on the Forums. If you're wanting to send jobs out to cut, but are unsure on whether your design is completely appropriate for that purpose, join the conversation and we can fix most things up! Material Selection Not all Makerspaces or third-party services have a full selection of materials on-hand. Prices may also vary due to wastage, availability and basic markup. Plywood designed specifically for laser work tends to be more expensive as it has to be free of knots and voids, plus needs to use glues safe for laser cutting. Acrylic will be (well, should be) tempered cell cast due to problems with cracking and poor finish quality with the extruded variety. The right materials cost a little more, but produce infinitely better and more durable results. Thicker materials can come with unexpected side effects, such as larger kerf (width of cut left by the laser) sizes or cut edges which are not perpendicular to the face. Thinner stock is a more accurate choice for closer-fitting parts. This is a good subject to discuss with the users/owners of the laser; if theirs has the right optics and power to cut 1/2" acrylic perfectly then go for it! Ask for advice on choice and comparative costings with stock materials; you might even get a great deal on a job if something can be pulled from the offcut bin. Asking the question costs nothing and can save you a significant amount of money. Exchange File Format More than likely you'll do your design work away from the site where the laser is located, and probably using different software also. Modern laser cutter drivers are far more forgiving of input formats than they were a few years ago, however that isn't to say that every bug has been rattled out. Choosing the most appropriate format for file exchange from your machine to that of the laser is vital. If you're going third-party, as what their preferred file format is and perhaps what software they are using; if you both happen to be using CorelDRAW you can cut out unnecessary conversion steps and swap native file formats directly. I prefer DXF (Wikipedia) simply because it is the most common and interoperable file format for vector information. The same rationale applies to other packages (Inkscape, Illustrator, etc) where exporting to a widely-supported basic file type removes most common errors from translating across formats. "What-You-Get" If you're using a third-party service, ensure they are aware which cut pieces you're actually needing from the job. A negative space router template (such as a pickup cavity) may not be immediately obvious, leading to problems where you receive a "Tele pickup shaped piece of Masonite" in the mail instead of the surrounding template for cutting the cavity! Explicitly stating, "This is for a 200mm x 150mm rectangle of Masonite with that shape cut out" makes all the difference. For more complex jobs where you are needing both the negative and positive components from the cut, again, state this from the outset. It saves a lot of time and hassle. Not all laser services will know what a router template is or its end use. Obviously this is less of a problem when you're cutting work under your own steam. One issue that might crop up is when cutting out fine components. Air assist which prevents flareups will happily blow your valuable but newly-loose parts around the bed, or worse, into an exhaust port! A little double-sided tape under the material in the right places and the use of a spoil board underneath helps. Whilst this isn't a communication issue, double-checking with a third-party service that they use the same kind of approach is. ----==---- 3. Design-Time Considerations Keeping a design as simple and to the point as possible wins the day. Only add as much information as the templates really need. The true test of a template is in the quality of the workpiece it produces; not how tricked out the template is with text, logos and irrelevant detail. This is especially important if the service charges by time or in the case of Ponoko, a function of total laser work movement length! Going through your design from top to bottom pays off. Common problems that are not immediately apparent can be revealed by developing your own methodical approach to validating your designs. Alignment Marks - Transparent Materials Acrylic offers us a great opportunity to add engraved markings that can be seen through the template itself. The problem is that lasers cut from the top down. This just requires that the finalised design is mirrored prior to sending out for cut so engraved text will appear correctly when viewed through the template, plus alignment marks lay directly next to the workpiece. click to enlarge Alignment Marks - Opaque Materials Opaque materials such as Masonite or MDF may be difficult to reconcile with alignment marks such as a centreline; after all, engraved marks will be placed onto the top surface of the template and we can't see through the material like we can with transparent acrylic. For most cases, this is not too problematic; we can add additional auxiliary cutouts within a template to assist with alignment where it might not otherwise be possible. In the example above, diamond-shaped auxiliary alignment cutouts allow the template to be placed accurately on a marked centreline using internal corners rather than approximating from a top-engraved marking at an oblique angle to the edge. This is also invaluable for alignment on angled headstocks, where the centreline falls away past the nut area. Work Layers Use of separable layers improves workflow. Placing all engraving work onto a separate layer to cutting makes it a simple task to confirm that paths are not duplicated, incorrectly set and properly aligned, etc. Colour within the drawing is used as the primary guide for different laser settings. Most laser driver software can be configured so that many different colours to represent various combinations of speeds, powers and duty cycle frequencies. The accepted basic standard is that red (RGB 255,0,0 - #FF0000) represents a cut and blue (RGB 0,0,255 - #0000FF) represents an engraved line. If using a third party, confirm their house rules and conventions on colours and whether line weight is a consideration. My personal arrangement is to use black (RGB 0,0,0 - #00000) to denote the rectangular working outline for larger negative templates. Some houses may interpret this as an engraved mark unless it is explicitly stated that black represents a cut. Ensure that your drawing objects are explicitly set to the correct colours, not simply "By Layer". If your software has the ability to "select all items by colour", this helps with confirmation. Another check is altering layer colours to something unused, such as bright green.....if any objects are set to follow colour by layer, they'll stand out clearly. Kerfs Laser cutting produces small but still significant kerfs, or the "width of cut". Several factors such as material type and thickness affects the final size of kerf, however it is usually in the region of 0,15mm for thinner materials. Confirm with the laser operators what the expected kerf size of the material you are working with is, or make test cuts and physically measure it yourself. A typical kerf is in the region of 0,2mm and equates to an offset of around 0,1mm from the expected drawn outline. Kerfs are hardly worth concerning yourself with for headstock and body templates, and in fact it works in your favour for bolt-on neck/heels. Other precision joinery Items that require a tight conforming fit - such as set neck joint templates - will need test cuts to be made and the templates proofed for suitability. Offsetting the mortise half the kerf size smaller and the tenon half larger is a good start, however the proof is in how well the joints routed using the templates mate together. Adding in a larger offset than is necessary is also an option. It's better to fine tune the wood with some sandpaper than it is to have it loose straight off the router! ----==---- 5. File Exchange - Break It Down To Basics Many of the design tools in various CAD packages produce complex objects that are often handled in a manner specific to that package. For example, different types of curves, mathematically-generated contours or even text objects. Unless you are working in the exact same software that outputs jobs to the laser, the two different packages can have radically-different opinions on what how your work is supposed to render, resulting in incomplete or incorrect cuts by the laser. We can work through this by taking complex items and devolving them down into basic objects (called Primitives) that are unambiguous and are rendered equally by all software packages. A common error is font usage. They'll happily render within the package they were created within, however there is no guarantee that this will translate through to the finished product. Take the following example in TurboCAD: click to enlarge It might not seem immediately obvious that any kind of problem might exist here other than the font being solid rather than an outline. Times New Roman is a vector font, which might seem pretty universal to most systems. However, once this work is saved out to the common DXF format and re-opened in the software used for the laser (in this instance CorelDRAW for an Epilog platform) we see that the font has been substituted to a completely different one, and is no longer mirrored as in TurboCAD. How to we prevent file format exchange errors such as these? click to enlarge Complex to Simple (or "Simple > Complex") CAD packages have all kind of tools for producing high-level objects. Underneath it all, these objects are still built from a basic set of Primitives, such as lines and circles. Instructing your software to take each high-level object and strip away the complexity varies from package to package, however is usually called Explode. In the example above, taking the text object in TurboCAD and Exploding it down into Primitives should allow any other package to interpret it correctly. Often this will need to be performed more than once depending on the object being Exploded. For TurboCAD, this needs to be carried out twice in order to devolve the Text object to a single Group of objects, then down to individual Primitives (normally Polylines). However your own software works, inspect the objects to figure out whether they need Exploding further. Some objects such as characters within Text may Explode down into two individual parts; the fill and the outline. Deleting any fill prevents duplication of the same object, since we only need text character outlines. click to enlarge - a letter "O" Exploded down into internal and external polyline shapes. It is also worthwhile considering Exploding curves; whilst simple curves normally render correctly between different software packages, they usually cause the laser head to move slower than with sets of lines as the driver interprets the curve mathematically. Exploding a curve down into discrete Polyline objects is recommended to reduce job complexity and increase speed. Before committing, compare how granular a Polyline is in comparison to the original curve. Most software allows you to define how finely a curve is broken down into a Polyline. For most jobs, a cut made using Polylines is indistinguishable from one made with curves. Once you have a better understanding of which objects translate well via your chosen file exchange format, you can Explode only the ones that don't. Ultimately, if the end product cuts quickly and efficiently, breaking your drawing down to its absolute basics prevents unexpected bugs from creeping into your designs. ----==---- 6. Example 1 - Simple Bench Hold-Down Templates A few months ago, I sent out a quick turnaround job to Henri at Mostly Out Of Cardboard (MOoCB) for some acrylic pin routing templates. The files were supplied as individual DXFs. Each holddown consists of an outline plus several holes used for aligning and stacking pieces together. Henri simply imported the DXF files into CorelDRAW, set each outline for the appropriate cutting settings in the laser job driver. Being extremely simple, Henri was happy to accept the DXF files as-is straight from my CAD package and set colours for cutting, etc. at his end. ----==---- DEMO FILES - 125mm offset holddown.DXF - 175mm offset holddown.DXF - 200mm offset holddown.DXF preview of 125mm offset holddown.DXF ----==---- On my doorstep the next day I had these (love the packaging): This was an extremely simple job, which required very little back-and-forth communication. Henri is experienced at cutting a great number of different materials, so three small acrylic components was a walk in the park. In fact, I asked for "whatever light acrylic stock" they have on hand which resulted in these 4mm. A job such as this is mostly material cost with minimal setup time; even the packaging is only a minute job on top of the parts themselves. Like any job, there will be a degree of setup on some level, whether it be a complete treatment and check of the vector file sent (some bureaus insist on this, and make the charge mandatory...) copy grouping parts for efficient batch cutting or laser configuration (origin locating, focusing, etc) prior to running the job. The templates worked fantastically. 8mm-thick Oak blanks were pre-drilled and bolted down to the sled and shaped using an overhead pin router. The templates seat underneath and the pin rides against them. A very simple and neat use of laser-cut templates! ----==---- 7. Example 2 - Electronics Cavity Routing Template Set Anybody that knows me enough will be aware that I think far too much about the classic basses that came out of the Matsumoku factory in Japan from the late 70s to the late 80s. The most known of those is the Aria Pro II SB-1000 with its tank-like dual-mode 18v electronics and recognisable signature sound. A slow-burning project of mine has been to make a more or less authentic replica of the SB-1000, but with altered specifications....and a fifth string. The electronics cavity is something I'd like to replicate rather than make "similar to", so I recorded the measurements from a real SB-1000 and drew the cavity up in CAD with a few basic improvements and some cleanup. An original SB-1000 electronics cavity, bereft of life. Whilst not the most elegant or precise of electronics cavities, the space for the preamp module and batteries, plus the recesses produce a nicely-organised electronics cavity that isn't thin and weak like most "swimming pool" cavities. I figured that a set of four templates would be perfect. The first being the main outline of the cavity cover recess and cover plates (the plate is split into two pieces), a template for the main "body" of the rout down from the outer cover plus the narrower part of the battery/preamp niche, an auxiliary template to produce the wider ledge either side plus a template for the recesses. Since these templates are all related to each other, I decided that it would be useful to have engraved alignment markings on the lower face along with some basic information to remind me what to do (or not to do). As mentioned previously, lasers only cut from the top down, so engraving on the lower face means these will all need to be cut in mirror image. A vector line font was used for the text for both clarity and simplicity. Screwhole locations were marked with 2,5mm diameter circles with Point objects (crosses) engraved in their centre. The Points were Exploded down into Line pairs. A potential issue would be duplicating the cavity cover split Line. Since I drew the whole outline and added the split later, this was no problem. A look at the layer manager ("design director") shows that I defined several layers for this project. Each one contains references and guidelines, text labels or the work for the laser. This helped me create a template set from one master drawing, with the organisation allowing me to work on all of the templates as a group or individually. Turning on all of the layers shows how everything was designed. A bit of a nightmare when you look at it like this, but it works! Diary of a CADman (ergh.....) TurboCAD allows me to electively export specific objects to DXF files, so I selected the objects relevant to each template and sent them out to four individual DXF files. As you would expect, all Text, Arc, Point, etc. objects were Exploded to Lines and Polylines. I contacted Guitars and Woods to produce my template set in 5mm acrylic along with a few different designs. G&W sell templates for many common guitar designs (Strat, Tele, Flying V, etc.) and do all of their cutting in-house. Since they know the product and a luthier's needs, it seemed perfect to use them for these templates. After an email exchange with G&W on their convention on cutting and engraving colours, material availability, pricing, that DXF was an appropriate exchange format, that the outline was denoted by the outer black rectangle, etc. I sent the four DXFs to cut. Just over a week down the line we received this tidy little package.... click to enlarge So here's that first template described earlier. The alignment crosses and text appear the right way around and are engraved on the underside. Each screw/threaded insert location has the small hole for punching and the alignment marks. I used the kerf of the laser (~0,15mm) to my advantage; the cavity cover plates will drop in perfectly. click to enlarge The cavity cover recess will of course require a thicker (and wider) template to be made up since it is only meant for a 2mm cut depth. I don't think router cutters are even available that shallow! Nonetheless, marking out the location internally is important and a transparent template is excellent for alignment purposes.... click to enlarge ....due to how the other templates were designed. The outline of the cavity cover recess is replicated here as an engraved reference on the underside. By aligning this with an outline drawn using the first template (or marking off the outline since the templates are all cut from 250mm x 120mm pieces!) we have an accurate placement for each subsequent template. click to enlarge The auxiliary template is shaped similarly, but is only used for the battery ledge. click to enlarge Finally, the control recesses. click to enlarge I labelled the templates 1 through 4 and added pertinent routing information to each one. In most instances, these templates would be retained as "master templates" and copied across to a thicker sacrificial material such as Masonite, plywood or MDF. ----==---- In Closing Access to and use of laser cutting services is far easier than you might expect. Maker culture has gone a long way towards normalising this sort of technology almost into everyday life; taking advantage of that as a luthier is a simple and economical step in taking your work forward in huge bounds. Over on the ProjectGuitar.com forums we've opened up a Laser Cutting Discussion And Advice Thread. We hope this article has inspired you with new ideas and methods of producing your instruments; ask anything you want about laser cutters, designing templates or components, CAD-related issues or even service recommendations. http://www.projectguitar.com/forums/topic/48625-laser-cutting-discussion-and-advice-thread/ ----==---- www.patreon.com/ProjectGuitar This article was made possible by the generous donation our our Patreon supporters, plus invaluable input and assistance from Henri at Mostly Of Of Cardboard and Carlos of the Guitars and Woods web store. Cheers guys! If you enjoyed and benefitted from this article. become a Patron of ProjectGuitar.com and help us bring you even more articles, tutorials and product reviews like this, week-in week-out! Thanks to ProjectGuitar.com's Patrons sirspens a2k Chris G KnightroExpress Stavromulabeta Andyjr1515 sdshirtman djobson101 ScottR Buter curtisa Prostheta 10pizza verhoevenc VanKirk rhoads56 Chip
  4. 2 points
    Two bearings are better than one - if the length of your bit shaft and router collet safely allow it.....add another. This 19mm/8mm shaft Luna Tools bearing-guided template bit from neteberg.eu is a prime candidate for an additional bearing. The code for a 19mm OD, 8mm ID shielded bearing is 698ZZ. A few of these cost a couple of Euros. A bargain considering that one "official" bearing costs €6! The collar was loosened with an Allen key and removed. Now's a good time to clean up your cutter and existing bearing. Wipe off any excess packaging machine oil from the new bearing with an alcohol-soaked cloth, drop it on with the original and you're good to go. Safety note: router collets require a certain length of shaft inserted to ensure a secure safe fit. If you're not 100% sure what this is then think twice about reducing the available shaft length by adding more bearings!
  5. 2 points
    No two workbenches are created equally, and a surprising number of details fundamentally alter their suitability despite (what might at first seem) superficial differences. Of course, a humble Black & Decker Workmate might not easily be comparable to a 16ft French-style Oak bench or even the dining table, however they can all be examined using the same criteria of, "what is useful to us as luthiers?". I think we can agree that this is far from ideal for working during winter on the patio (Source: Black n Decker) Go and do a quick Google Image Search for "luthier workbench" and briefly browse the thumbnails. Absorb a bit about what you see; we'll come back to that again later. The reason I recommend this is that I have noticed numerous shortcomings in most people's workbenches, even those of established luthiers. It might not seem immediately apparent at this stage what the problems are, but we'll gradually illustrate that.... Primarily, most luthiers have learnt to "make do" with existing solutions that originally evolved to solve other woodworkers' problems. Sometimes this is out of necessity (any workbench is better than none!) but often we just don't recognise that traditional workbench styles are inadequate for the needs of a luthier. Smart luthiers spend much of their time adapting ideas to better suit their own work, or creating entire new ones. A luthier's work is uniquely demanding in comparison to that of a furniture woodworker, kitchen fitter or patternmaker. Not recognising these demands and reacting on them by tailoring the functionality, ergonomics, efficiency, safety, etc. of the work area sets up larger problems waiting to happen. The work area has to be made to work in your favour; not left with the default settings and allowed to cause you more problems than it solves. At the low end of the scale a poor work area causes beard-stroking and time-wastage. At the catastrophic end, errors are made, general work quality suffers, risks taken and money is lost. Dedicating thought into improving your work space impresses itself on the quality of your output and on your sanity. Fundamentally, we just need to break down why benches are configured the way they are, the uses this configuration serves and then re-engineer ideas from the ground upwards. No one "real" luthier's workbench configuration exists since we gradually mould our working habitat around the needs of the work itself. No two luthiers have the same working processes, preferences or range of experience so it is impossible to hope that "one-size-fits-all". Regardless, the process of detailing a generalised design driven by general luthiery tasks should illustrate how simple it is for any individual luthier to evaluate their needs and craft their own solution. After we've broken down the purposes of workbenches a little bit, we'll go back to that Google Image Search with new eyes. Hopefully you'll be able to spot which benches are less than ideal, and which ones are truly inspired. ------ Dining room warriors About all luthiers, modifiers, tinkerers, etc. have worked off the dining room table at some point in their careers, and most people reading this might still be doing that. When did you last change strings or carry out a setup on the dining table? There's absolutely nothing wrong with making do with what is available, especially when options are at a premium because of money, space, etc. Working off a simple flat surface is vital to luthiers of all levels whether it's the dining table or a carpeted 2x4 frame bench. Using a table in the home may not offer reasonable access to tool storage, ideal lighting conditions, workholding options or a sacrificial surface but it shares many points in common with a work area that a luthier would benefit from. Dining tables tend to be free of clutter, they sit at a height which is idea for seated close-up work, there is freedom to move around it, etc. Many excellent guitars wouldn't exist if it weren't for delicate negotiation with one's spouse to utilise them. This is not me advocating that you move out of the workshop and migrate back into the home however. Simply, it emphasises that we need good clear and clean space. A poorly-organised workbench that encourages disorder and sloppiness is a magnet for Bad Times. Traditional bruisers At the other end of the scale are the workbenches that populate many "fine" woodworkers' workshops, schools and old-school shops. My first explorations in workbench design started in this very same territory. Christopher Schwarz' excellent, "The Workbench Design Book" inspired me to build my own French-style workbench from solid Birch. Despite a traditional woodworker's bench being very useful for the non-guitar work I was doing at the time, it reinforced how well-suited it is at doing the tasks it originally evolved for; hand tool working the faces, ends and edges of large rectangular things! Applying luthiery tasks to this workbench just highlighted its lack of finesse, unless I really wanted a flat rectangular instrument. Most of the time it only provided me with a useful flat area to work on....which isn't that much of a step up from the dining table example is it? Big bruisers like my several-hundred kilo Roubo excel at providing an unmoving structure which won't rock, slide or react to having a hundred-kilo gorilla driving wide jointing planes down workpieces secured to it. We rarely need to exert that much force on anything we do making or repairing guitars! Even planing the sides of neck-through blanks or facing lumber by hand. More than likely when I set up a new working space, the Roubo will become a base for securely holding larger jigs such as the router thicknesser bed or even the Myka neck jig. Fundamentally, its uses are just too coarse for guitar work and it's the wrong height for eating dinner. Typical French "Roubo"-style workbench for working the face, edges and ends of boards (Source: 3D Warehouse) Workbench styles evolve from the pressures of the work expected of them. A Black Forest cuckoo clock maker's bench is radically-different from that of wooden gate maker. Shoehorning a bench whose DNA is fundamentally different to the task at hand means that everything becomes a series of compromises and workarounds to get even the simplest job done efficiently and correctly. A hammer isn't really the best tool for driving a screw. Fundamentally, the Roubo grew to satisfy the requirements of pre-industrial hand tool users working on large heavy (generally flat and/or long) boards. The same rough arrangement exists today in commercial woodworking benches, such as those in the core range from Sjöbergs: Sjöbergs Elite 1500 model bench. A more practical size, but not the workholding we need. (Source: Sjöbergs) Whilst being a little more universal than the Roubo, the underlying configuration of Sjöbergs' standard benches is more or less identical; designed to work on face, edges and ends by hand. The front vise might seem useful at first glance, however it will likely spend more time as an obstacle than being in use, and ultimately is designed for holding non-guitar shaped things. The wide tail vise in combination with the dual bench dog rows is more useful for routing operations on flat pieces, however simpler workholding arrangements exist and the ergonomics may not be ideal. As a turnkey bench, these would get you in the ballpark however I would have a difficult time rationalising the hacking and deconstructing necessary to my thousand-plus workbench to make it do what I wanted it to. Ergonomics How do you decide on the height of your workbench? Do you spend more time sat or stood around it? Traditional benches are surprisingly low; mostly due to their expected tasks requiring a wide and powerful stance. Physical tasks such as hand planing (especially with old tall wooden planes) benefit from a lower bench than relatively static standing jobs such as hand routing. Pleasantly, the Sjöbergs bench weighs in at an ideal height of around 36" which is also somewhat odd given that this makes it almost too tall for a good planing stance. It is however about the correct height for seated work such as soldering and other fine work. Unlike many other bench aspects, raising the height is not usually too onerous, especially given how transformative 2" can be to a bench you spend any length of time hunched over. Designs with foot stretchers such as the Sjöbergs are difficult to lower however. Workholding Workholding is an enormous topic which we'll partially cover in part two of this series, whilst introducing design aspects for a more usable luthier's bench. For the moment it is sufficient to say that guitars are rarely (if at all) comfortable being secured using the vises and clamping methods designed for handling rough semi-finished wood that is more or less of square dimensions. We are needing to fit our delicate guitar-shaped pegs into somewhat rectangular shaped holes, however the vast majority of workbench designs - both commercial and traditional - do not entirely satisfy our needs. We need better ways of stopping our work dancing around the table. A more universal productive luthier's bench should be capable of holding necks and bodies in all states of the process firmly yet safely whilst offering free workpiece access from any angle we choose....all without devices and whatnot cluttering up the valuable flat real-estate around our bench. In part two, we'll look at how we can move beyond this by making our benches smarter. ------ Post photos of your own workbench in the comments below! We'd love to hear exactly how everybody arrived at their own bench designs, the troubles you experience with it or the problems you solved!
  6. 2 points
    Recently I made the decision to step into the world of CNC routing machines and augment my small workshop and tool collection with a modestly-sized unit. With the rise in quality of low-end Chinese-made machines in recent years it has become easier than ever to purchase a small CNC router for home use capable of high precision. A quick search on online auction sites will reveal a vast array of pre-assembled units for sale starting in price from less than $700, with cutting beds up to 600mm x 900mm in size. While I am still a novice at CNC, hopefully my experiences can help others decide if taking the plunge is for them too. So, why choose a small CNC router? There were several reasons why I personally decided to purchase a desktop machine with the intention of applying it to guitar work: I had a limited budget and a small area where I could set up such a machine. A CNC router capable of directly milling a guitar body from a timber blank is physically large, noisy and expensive; I was after a way to improve the appearance of my builds by including professional-looking headstock logos and markings, and had thus far been dissatisfied with many of the solutions that utilised decals or transfers; I wanted a quicker and safer way to create templates for routing smaller shapes and components used in guitar construction (eg, pickup cavities, headstock outlines, truss rod covers); Having decided to explore multi-scale instruments I needed a way to make accurate drilling templates for the individual bridge assemblies commonly used for these instruments; Despite wanting to automate some of the construction process, I still wanted to retain the hands-on nature of building an instrument rather than transfer the bulk of the cutting and shaping work directly to a machine; The increased accuracy afforded by the machine for particular tasks was attractive (eg, scribing fret slots directly onto a fretboard blank, creating perfectly-fitted control cavity covers). The CNC machine I eventually settled on was at the smaller end of the scale; a 3-axis desktop unit with a similar footprint to a mid-sized inkjet printer, having a cutting bed of 200mm by 300mm (X- and Y-axis respectively) and a vertical travel of 50mm (Z-axis). The spindle is rated at 200W, with a 1/8” collet which allows the changing of cutters using a wrench system similar to that used on many handheld routers. The build quality of the frame and gantry seems quite acceptable, although for the price paid I would expect some shortfalls in terms of frame flex and milling accuracy of the spindle due to runout and eccentricity. However if you don’t work the CNC router too hard any errors in the finished milling process will be minimal, and achieving sub-micron precision in a material such as timber is probably a moot point anyway. A separate controller interface unit is supplied featuring variable spindle speed via a dial on the front panel and PC connectivity through a parallel port on the back. It is worth noting that most of the models which utilise a parallel port to interface with the computer require a desktop PC rather than a laptop, as the battery power management features of the latter are not conducive to reliable operation of the CNC router. Commonly available USB-to-Parallel Port adaptor cables are also incompatible with these units. However, if your host computer does not have a built-in parallel port you can purchase and install an aftermarket PCI parallel port card, which is exactly the path I chose. The unit also came equipped with a selection of endmills, a set of rudimentary work piece holding clamps, a number of allen wrenches and spanners and an evaluation copy of the Mach3 CNC motion control software. While the supplied endmills are satisfactory for learning the ropes and experimenting with different cutting operations, you may wish to invest in a small collection of higher quality endmills, which afford a far superior finish and longer working life than the factory-supplied ones. The controller is connected to the CNC mill via several cables with locking collars to prevent them inadvertently working loose. An unexpected bonus feature of the particular model I chose was that the controller circuit board is fitted with several unpopulated connectors that allow the retro-fitting of axis limit switches. On more fully-featured units these limit switches are fitted to the moving components as a safety measure to prevent the software accidentally driving the CNC machine past its maximum limits of travel, or to allow automatic homing of the cutting head (more in this in future articles). On the subject of software, there are two main options for driving a parallel port-based CNC router; the above-mentioned Mach Series software which is for Windows-based machines and LinuxCNC (formerly known as EMC2) for Linux-based systems. As LinuxCNC is a well-supported open-source option for these machines I elected to take this option and install a Linux partition on my host computer. Conveniently, LinuxCNC offer several LiveCD versions of their software, which has the motion control software pre-installed on a Linux operating system. The operating system can be run directly from CDROM or DVD without having to be installed on the PC. If the user decides that they would like to continue using Linux, they can choose to install the operating system and motion control software directly from the LiveCD. As these machines are directly exported from China or imported via an agent, technical support tends to be quite limited. The units require some software configuration in order to move the axes in the correct direction at the correct rate. The machine itself is incapable of knowing where it is positioned relative to the cutting bed, or how many turns of the axis motors are required to move it an exact distance without some form of calibration data maintained by the host software. Fortunately there are several online resources to help users configure their CNC routers in order to achieve precise operation. Once configured to run from the motion control software, the user can load files into the application to direct the cutting head to manoeuvre around the work piece at pre-determined directions, speeds and depths in order to create the final object. The language used in these files is known as G-Code and consists of text entries directing the axis motors to move in a specific direction at a certain rate. Other specialised commands in G-Code are used to command the spindle motor to turn on and off, make the program pause at key steps in the routine, or cause the axes to move in predefined ways such as cutting an arc or drilling a hole. While it is possible to create a G-Code file from scratch by typing commands one at a time in a text editor, it is far easier and quicker to use a Computer Aided Drafting or Computer Aided Machining (CAD/CAM) application to draw the intended cutting paths and convert the subsequent drawing to its component G-Code commands. The user has the ability to quickly mock up an outline of, say a pickup routing template, export the resultant drawing as a G-Code file, open the file in the motion control package and cut out the routing template from a sheet of MDF with sub-millimetre accuracy in a few minutes. While some CAD and CAM applications are integrated into one common application, there are also many offered as separate software solutions. Some packages are open-source and free while others cost anywhere from a few tens of dollars to well in excess of $1000, all with varying levels of ease of use, feature sets and functional integration. Below are a few examples of what operations are possible using the small desktop CNC machine when applied to guitar building. This headstock logo was first engraved while being held in a simple jig to allow the workpiece to be accurately positioned without moving. The work was done in two passes, with the larger of the two pieces of text milled using a 0.8mm diameter endmill, and switching to a 0.7mm endmill for the smaller text. The resultant cavities were filled with black-tinted epoxy and sanded flush: Cavity covers can be directly cut on the CNC router from thin timber stock, including drilling the screw holes in one pass. To create a matching routing template for recessing the cover into a body it is a trivial matter to take the original cavity outline and scale it in CAD. The resultant file will create a perfectly fitting routing template for that cover. As I was unsure if the machine would struggle to mill such a thick piece of perspex, I milled a 'master' template from 6mm MDF and then used a handheld router fitted with a pattern-following bit to transfer the MDF template to the perspex sheet: If your router has a bushing guide or pattern-following plate attachment you can use it in combination with a small diameter bit to cut cavities with tighter radius corners than woud be possible using a typical 1/2" template bit with integrated bearing. The problem with using a bushing guide is that the template used must be created oversize by the radius of the bushing minus the radius of the cutter. Creating such a template in CAD and then milling it on the CNC router is simple. In the following example I have created a routing template to suit the bushing guide for my router. The cutter used was a 1/4" straight bit and the bushing guide is 16mm in diameter, so the template has been created with a consistent (8mm - 3.175mm) 4.825mm offset to achieve the intended cutting profile for a humbucking pickup cavity: Accurately positioning the independent saddles used on multi-scale instruments can be tricky, as the risk of misalignment is increased compared to a one-piece bridge. Determining the angle of the saddles for the differing scale lengths can be problematic, and if you are constructing instruments where the scale lengths used differ from build to build, making a drilling jig by hand is time consuming. This drilling template was milled and engraved into 1/8" perspex in about 15 minutes and includes the mounting holes for the saddles, the through-body holes at the rear of each saddle, a centreline to assist in positioning the template on the body and the intonation reference mark for the scale lengths used: The CNC machine can also be used to create simple tools for use in building and setting up instruments. The time taken to create this four-sided radius gauge was about half an hour, from mocking up the basic shape in CAD to removing the perspex sheet from the machine's cutting bed. If the tool was to get lost or damaged, creating a replacement should only take a few minutes: Pros: A ready-to-go solution out of the box with minimal assembly required Competitively priced with good accuracy and construction quality Excellent finish achievable on the object being machined Capable of machining a wide range of raw materials (MDF, plywood, timber, plastic, soft aluminium) Good support from open-sourced software solutions Small footprint for installations where space is at a premium Cons: Generally not suitable for direct cutting/shaping of the major components used in guitar construction (eg, cutting body outlines, neck profiles, cavity routing) or machining harder materials (eg, making custom metal components for bridges) Minimal after-sales technical support The control interfaces supplied with the smaller and cheaper units usually require a desktop PC fitted with an archaic parallel port. The software used can be challenging to get to grips with if you’re not familiar with Computer Aided Drafting principles and terminology. Hidden costs associated with using a CNC – purchasing good quality cutters and CAD/CAM software for example ---------- In future articles I will explore calibrating the desktop CNC router and covering some of the basic operations of the associated CAD, CAM and motion control software packages.
  7. 1 point
    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.
  8. 1 point
    After going through the StepConf Wizard to set up our CNC router LinuxCNC will have created a shortcut on the desktop to allow us to run the CNC machine with our configuration. Double-clicking this icon will launch Axis, the default graphical user interface. Upon opening Axis the user is presented with a 3D representation of the physical machinable cutting area of our CNC machine. A default test cutting program is loaded on startup featuring the LinuxCNC logo and a small cone object in the preview window represents the position of the CNC cutting tool. The maximum bounds of movement of the CNC machine, as defined by StepConf Wizard in part 2 of this series, are represented as a rectangular cuboid object with dotted red edges. In our case the cube is 200mm wide, 300mm long and 50mm high, which aligns with the maximum limits of travel of our particular CNC router. Take a fresh piece of plywood, MDF or other flat material at least 150mm x 150mm and secure it to the table. Fit a small engraving cutter to the spindle and tighten the collet. Open a blank text document using whatever text editor you prefer to use on your system and enter the following G-Code. If your machine is set up for millimetres use the left column. If you’re running your machine in inches use the right column: Save this file as ‘100square’ with the file extension ‘.ngc’ to a convenient location on your computer. Using the metric version, let’s break the code down into its components: G21 – This command tells Axis that the units of measure contained in the following code is expressed in millimetres. If G20 is used then the units of measure are inches. G0 Z15 – the G0 command instructs the CNC machine to linearly move its axis or axes at maximum velocity. This is useful to speed up moving from one area to another in preparation for the next cut, but should not be used when actually cutting as the speeds and forces involved could damage the tool. Z is the axis that is to be moved and the number immediately following is the position the axis is required to move to. In effect this line is commanding the CNC router to raise the Z axis to 15mm above the surface of the workpiece at maximum speed. G0 X0 Y0 Z5 – The CNC machine is again required to execute a rapid move, but this time we have also included destinations for the X and Y axes (X0 and Y0). Z axis is also instructed to lower to 5mm (Z5). G1 X0 Y0 Z-0.5 F300 – G1 tells the machine to linearly move at a rate which is specified by F300, expressed in units per minute. Because the Z axis is required to move to a negative value (Z-0.5) we are now plunging the tool into the workpiece to begin cutting and a slower axis velocity is required. X and Y axes are set at 0, but because we already moved to X0/Y0 in the previous step there will be no change in these two axes. G1 X100 Y0 Z-0.5 F300 – G1 again instructs the machine to use the feed rate F300. The X axis is requested to move to 100 while maintaining Y at 0. This will result in the X axis moving to the right in a straight line to a distance of 100mm. The Z axis remains at the same value as previously commanded by the G1 instruction. G1 X100 Y100 Z-0.5 F300 – The machine will move Y up to 100 at low feed while keeping X at 100 and Z at -0.5. G1 X0 Y100 Z-0.5 F300 – The CNC router will move X axis back to 0 at low feed G1 X0 Y0 Z-0.5 F300 – The Y axis is reduced to 0 at low feed. G0 X0 Y0 Z15 – The Z axis is raised to 15mm above the surface at maximum rate. The cutter is withdrawn from the work piece. M2 – This command signifies the end of the program and the CNC can stop operation. Many G-Code commands and variables are ‘modal’ and remain in effect until another contradictory command is executed. As an example the above program could be re-written for maximum modality and provide the exact same output. The drawback is that it can become difficult to read to the user, as much of the detail is removed: You will note that the F300/F12 feed rate that originally appeared at the end of each G1 line now features at the top of the program. This is because each successive G1 command will utilise the last known feed rate, which is now defined at the beginning of the code. Returning to Axis it can be seen that on start-up the location of the cutting tool is exactly at the upper-left corner of the machine limits of travel (X=0 and Y=0) and the tip of the cone is positioned at maximum height (Z=0). This corresponds with the home position that was defined earlier while running the StepConf Wizard. In reality the cutting head could be physically located anywhere within the limits of travel, as is the case below: Before the CNC router can be operated it needs to be returned to its home position. On more advanced machines this procedure can be automatic, with the axes seeking their home positions when the user commands the machine to home itself. In our case we will home the machine manually. Click the File open button or press <O>, navigate to where you saved the G-Code program we created and load ‘100square.ngc’. You should be presented with the following in the preview window: Check the Emergency Stop pushbutton on the CNC router control interface has been reset, and press <F2> or click the ‘Toggle Machine Power’ orange button on the top menu bar. A number of greyed-out options under the ‘Manual Control’ tab become active. With the CNC machine connected to the PC and powered-up, use the four arrow keys on the computer keyboard to move the machine around the cutting bed in the X and Y directions. The <page up> and <page down> keys will also move the Z axis up and down. Manually moving the cutting head around the table is called jogging. As the cutting head moves around the display updates the position of the cone object and shows the path taken as a solid yellow line. In the below example the cutter has been jogged towards the front edge of the table by 31.739mm (Y axis), across to the left 21.547mm (X axis) and up 20.545mm (Z axis). These values appear in the upper-left corner of the display; the Digital Read-out or DRO: The CNC machine, having now executed the above moves is sitting with its cutting head physically home, but well away from the workpiece at a distance which does not yet correspond to the values shown in the preview window: Now that the CNC machine itself is at its home position Axis needs to be told that this is now the position that corresponds with the upper-left corner of the red dotted-edged cuboid object, ie the 'soft' home position. The ‘Home Axis’ button is then clicked for each of the X, Y and Z axes. As each axis is homed the DRO updates to indicate that the associated axis is at position ‘0’ and a symbol is added next to the readout. Note also that the position of the cutting head in the preview window returns to the upper-left corner of the work area box to reflect the fact that it has now had its home position reset. The second step to perform before we can run a job is to ‘touch off’ the cutter against the workpiece. This is the process of setting the position of the workpiece relative to the home position of the machine. With the CNC router homed the job can be run, but unless the tool is touched-off Axis does not know where the workpiece lies relative to the tip of the cutting tool. In the above example the square object looks as if it sits bang-up against the top of the limits of travel, when in actuality the workpiece is about 25mm below the tip of the cutter and a few inches inside the edges of the table. Without touching-off, at best the machine may run the job with the tool completely missing the workpiece. At worst the CNC may try to drive the cutting tool through the workpiece into the table, ruining the job, damaging the table and destroying the cutting tool. To touch off manually jog the cutting head to the point at which you require the origin of the job to be positioned on the material. In the below example the cutting head has been jogged right 34.071mm (X axis), jogged away from the front of the table 42.856mm (Y axis) and jogged vertically down by 22.156mm (Z axis) to place the tip of the cutter at exactly the spot where the job origin is required to be. In our case I have marked the workpiece with a cross to indicate where I want the square shape to begin: As each axis is moved into position click the ‘Touch Off’ button. A dialogue box opens to allow the user to manually specify an additional offset to the workpiece relative to the axis being touched off, but in most cases it is sufficient to use the default of 0. After touching off the axis the DRO updates to show the position of the cutter has now been reset to 0. Note also that the square object has now moved 'deeper' into the red cuboid object that defines the limits of machine movement. Click the ‘Clear Live Plot’ button or press <CTRL-K>. This clears the preview window of any paths that were created by the manual jogging of the cutting head. Manually jog the cutter away from the workpiece a few centimetres. With the machine homed and touched-off we are now ready to run the job. If the CNC machine has a manual spindle control turn it on and set the spindle speed appropriately. Click the blue ‘Play’ button or press <R>. The CNC machine and preview window will now begin stepping through the code and manoeuvring around the workpiece. Note that the movement of the cutting head in the preview window is indicated by pale red lines for slow cutting motions, and for rapid jogging motions between each cut the tool follows the cyan dotted lines without leaving a trail. After a few minutes the program completes and the cutter retreats away from the workpiece to a safe distance where the spindle can now be turned off. If all things have gone to plan you should now have the 100 x 100 square engraved on your workpiece. Take a good quality ruler or Vernier calipers and measure each of the four sides of the engraved square and confirm that they each measure 100mm. If the sides of the square do not equal 100mm then some tuning of the configuration file must be undertaken to correct this error. The most likely culprit is that the lead screw pitch has been incorrectly set. The correction factor to apply to bring the axis scale back to the correct value is: If the square is exactly out of scale by a factor of two the other possibility is that the 'Motor Steps Per Revolution' setting is out by a factor of two. Doubling the value of 'Motor Steps Per Revolution' will make the edge of the square twice as big, whereas halving this setting will reduce the length of the square’s edge by half. ---------- Now that we have the CNC router actually cutting something and each axis is scaled correctly, we can move on to creating something a little more exciting. In the next instalment in the CNC series we will create a truss rod cover from scratch using CAD and mill it on the CNC router.
  • Create New...