Liutaio Mottola Stringed Instrument Design

Woodworkers' Popup Units Conversion Tool / Calculator

Calculator converts to/from decimal inches, fractional inches, millimeters. Popups must be enabled for this site. From the Liutaio Mottola lutherie information website.

Did you know ....

.... you can click on most of the assembly photos on this site to enlarge them for a close look? Also, hovering the cursor over most linear dimension values will convert the values to decimal inches, fractional inches, and SI units.

Generating Pocket and Boss Tool Paths Manually

I use a small shop-built desktop CNC Router in my lutherie work but, as I do no production work, it gets very little use. So little in fact that it is not practical for me to invest a lot of money in the machine nor in the software that supports it. Of all the software needed to make use of a CNC machine the most expensive is the CAM software that converts CAD drawings and models into the G code instructions that run the CNC machine. For the longest time I didn't have any CAM software as I couldn't justify the cost in my work. Prices are coming down considerably for this class of software but are still pretty high. So this means I had to use a combination of free software and some manual work to generate the tool paths needed for machining and then convert these into machine instructions. With this software and the CAD technique mentioned here, it is possible to do all the 2.5D work you'll need to do - cutting out parts in sheet stock, drilling, and cutting pockets and bosses. What is described here will not necessarily yield an optimum tool path but it will get the job done.

Last updated: Saturday, August 15, 2015

There are two pieces of free downloadable software which are invaluable in doing the work of converting 2.5D CAD drawings and models to machine instructions. The first is DeskEngrave, a program from Deskam which will convert text in TrueType fonts into either AutoCAD r12 .dxf format or directly into g code instructions. This converts the outline of each letter into CAD lines (or a toolpath) and so is directly useful for use with engraving bits. But if you want to use it to pocket out large letters a little more work is needed after this program is run, to generate the tool paths for the pockets. I don't do much text work like this in my lutherie work so this program doesn't see much use here.

The other program that is available for free download is Ace Converter from DAK Engineering. This one will convert the lines of an AutoCAD .dxf file to a gcode toolpath. It has some nice optimizations when it does this, including the ability to generate deep cuts in multiple passes, and the ability to move directly from the end of one line segment to the next one without an extract/move/plunge cycle if the ends of the lines are within a user specified distance from each other.

From these short descriptions it should be obvious that these two programs can be used to generate the kinds of tool paths needed to engrave, cut out parts from sheet goods, or perform drilling operations. About the only thing that you will have to do to the generated gcode files for these operations is add feed and speed data manually. And you may not even have to do this, as the program you use to run your CNC machine may provide for default values to be set for these. I use Mach 3 from Art of CNC and it provides nice default configuration for feed rate and spindle speed.

The most complicated of the 2.5D operations is contouring of straight sided packets and bosses, and neither of the free programs mentioned above will do this directly. To perform these operations you first have to generate a toolpath from your pocket/boss outline drawing. Again this is an operation that is usually done by CAM software but lacking that the tool paths will have to be constructed manually. Here is how I do this for the pockets and bosses needed for stringed instruments made of wood.

The first step is to start with the outline drawing of the pocket and/or boss you will be cutting. This should be drawn as a closed polyline if possible, but in any case should contain only straight line segments and circular arcs. Drawing the outline as a closed polyline will make subsequent steps much quicker.

Next, make a separate layer for the toolpath, and on that layer create a parallel polyline at half the width of the tool you will be using to cut the pocket/boss. This polyline goes inside the outline for pockets and outside the outline for bosses. In the example I have both.

Note that if this toolpath crosses itself (as it does in the upper right hand corner of the example) or if the toolpath for one of the bosses crosses that of the pocket then the diameter of the tool is too large to accurately machine the feature. In either of these cases you'll either have to use a smaller tool, or modify the toolpath for use with the selected tool, understanding of course that the feature will be end up distorted. In the example I'm just going to trim the overlapping toolpath and consider that to be good enough for my purposes.

Now, you can repeat this process if you like to make a toolpath, making another parallel polyline inside this one and then another inside that etc., each time trimming any place the polyline crosses over itself or another line. But this is kind of tedious work, especially if you have to make a lot of lines. So generally I do the following instead.

The next step is to fill the areas to be hogged out with toolpath lines. In AutoCAD you can simply use a user defined hatch pattern of lines that are a little closer together than the diameter of the tool you will be using. After the hatch is made it is exploded into separate lines. The line spacing (the stepover value) is also chosen to determine how smooth the bottom of the pocket will end up. If your CAD program doesn't do hatches or can't convert these to plain lines, then the lines will have to be drawn manually. This is no big deal. Draw a straight line so it falls just below the highest point of the toolpath outline ...

... then make parallel copies of that line at the stepover distance.

Trim these lines to the original outline polylines ...

And you're done. Again, there are plenty of optimizations possible. For example, shortening each of the horizontal lines on both ends by the stepover value will shorten run time, possibly by a considerable amount if there are a lot of lines. Save the drawing as an r12 .dxf file and then run Ace Converter on it. In Ace Converter you'll want to ignore (turn off) the layer with the original outline of the pocket. Here you get to specify how deep you want the pocket to be and how deep to cut at each pass. You also get to specify how close two end points have to be for the converter to optimize motion by not generating a retract/move/plunge cycle to get from one point to the next. Set this to the stepover value. This way the tool path will be generated so that, when one of the parallel lines is done the cutter will move directly to the start of the next one.