CNC Router

Overview

"What is the CNC Router good for?"

A Computer Numerically Controlled Router can cut wood with higher precision than conventional methods (jigsaw, table saw, miter saw). It takes files that you draw in CAD or render to a vector format and cuts along those vectors. When used properly it produces a clean and consistent cut along the cut surface. It is one of the coolest tools the node has to offer.

Technical Details

The work surface is approximately 65” x 145”. 2 Stepper Motors control the gantry movement. These are powered by the ShopBot motor controller. This is a beige computer tower with a red switch. It is not actually a computer and you need to remember to turn it off before you leave. The spindle motor is a xxxx W AC motor controlled through Variable Frequency Drive. It can operate between xxx and xxxx RPM. The controller is the blue box on the wall and power to the controller is applied through the wall switch below the blue box. Acceptable CAD formats are: .dxf, .svg, .dwg, .eps, .ai, or .skp.

Terms

End Mill - this is a special type of bit for the router designed to cut in all directions.

Flute - is the spiral cutting feature on the end mill. More flutes means smaller chips.

Gantry - is the frame that the X and Y stepper motors move across to position the end mill.

Stepper Motor - A high precision motor which can move in very fine increments. Stepper motors have current applied to their windings, even at rest. This is called holding current and can damage the motor if left on too long. Make sure to turn off power to the gantry motors once you are done using the CNC Router. The power switch for these is on the beige computer tower beneath the desk.

Feed Rate - This is the rate at which the end mill moves through the cut, not the speed of the end mill itself.

Chip Load - This is a number that represents the size of the chips produced by the end mill and is critical to the quality of the cut.

Step-over - This is the amount of overlap that the end mill makes when going into uncut material. You can think of it this way, when mowing your lawn, you leave part of the lawnmower over grass that you have already cut. The amount of the lawnmower that overlaps uncut grass is the step over (Todd's Analogy). Stepover should be between 1/3 and 1/10 of the tool diameter. Use a larger stepover for softer materials and a shallower step over for hard materials.

Tool Path - This is the path that the end mill will go through during the cut. You can make any vector or grouping of vectors into a tool path and each tool path can have it’s own cut depth and assorted settings.

Conventional Cut - the flutes cut counter to the XY direction of travel

Climb Cut - is when the flutes cut into the piece in the same direction as the direction of travel. This can be dangerous as the forces generated pull at the piece more than a conventional cut and it carries a higher risk of sending your piece flying. Don’t use this setting.

Tear Out - is when the material is ripped out of an area where it shouldn’t be. This generally refers to stripping the veneer off of plywood and can happen during the cut or also during tab removal after you are done cutting.

CAD

The first step is to create CAD files of what you want to cut. The files need to be in a suitable format such as .dxf, .svg, .dwg, .eps, .ai, or .skp. LibreCAD is a free and open source 2D CAD program for Windows, OSX, and *nix systems that can output .dxf’s. Inkscape is another program that can produce .svg outputs. Additionally, you can import certain 3D files to do 3D carving however that is not currently covered in this guide.

Selecting an End Mill

There are different types of end mills of different sizes, flute types and counts. A thinner end mill can do a better job at detail but may need to run at a lower feed rate to keep the chip load in a good spot. There are a few end mills to choose from on a shelf above the spindle motor controller. If you don’t see the one you want to use, feel free to purchase one and donate it to the node.

Flute Types

Straight Flute - great all around end mill, decent chip removal [1]

Up Spiral - great chip removal, can tear-out the top of thin veneer such as finish grade plywood [2]

Down Spiral – poor chip removal, no tear out, slower feed rate [3]

Compression – combination of up and down spiral, great all around end mill, great for plywood or laminated sheet goods. [4]

You may also use certain conventional router bits provided they are capable of cutting in all directions

Changing out an End Mill

1. First ensure power is off to the spindle and gantry motors.
2. Remove the dust-collector hood. It is held on with magnets.
3. Use the two wrenches by the desk (picture) to turn the bottom nut (counter-clockwise/clockwise -need to check).
4. Remove the end mill and place it with the other end mills on the shelf above the spindle motor controller.
5. Insert your end mill and tighten down the nuts. Ensure that the nuts have tightened down the end mill and have not just tightened to each other.
6. Put dust collector hood back on.

Securing your work piece

The spindle motor is incredibly powerful and will send your piece flying if you do not properly secure it to the work surface. There are different methods of securing your work piece but in general screws work. You want to make sure these screws are outside of any tool paths. For larger pieces it may be difficult to reach the spot where you need to put a screw. You are free to carefully climb up onto the work surface to reach these locations. Ensure everything is powered off during this time and make sure you do not move the gantry.

!!!SAFETY NOTE!!!
Make sure your workpiece is securely fastened to the work surface. The CNC Router is incredibly powerful and can send pieces flying across the room.

!!!SAFETY NOTE!!!
Ensure that the fasteners are clear of any tool paths. An end mill hitting a screw is a dangerous situation.

!!!SAFETY NOTE!!!
Also make sure that you fasten down any relief pieces that may be secure before you cut but will become dislodged during the cut.

Aspire

1. Open up Aspire.
2. Start a new project (you can not directly “open” a vector file, you can only open Aspire project files so you must start a new project).
3. Specify material size. Measure your material in multiple places and go with the thickest value.
4. Import your file. File > Import > Import Vectors.
5. Delete any reference vectors or lines that you do not intend for cutting.
6. Make sure your vectors are contiguous. If they are not, you can join them by first selecting the vectors to join then Edit > Join Vectors. A pane will appear telling you how many vectors are open and which tolerance you should have on joining the vectors.
7. Click on tool paths on the right pane. You may need to click out of a pop-up pane.
8. For general cutting along a vector, select 2D Profile Tool path. Click on “Show advanced tool path options”.
9. You can set your start depth. 0 is the top of the work piece. Set your cut depth to be just slightly over the thickness of your piece, an extra .005” is a good max.
10. Next, select your end mill. Clicking Select will allow you to choose different styles of end mills and bits. Click on Edit to edit the tool options.
11. Enter your tool diameter. Don’t worry about pass depth, that will be set another way.
12. Enter your Spindle Speed, Feed Rate, and Plunge Rate. To determine these, see the section on Chip Load.
13. Click on Edit Passes to specify the number of passes and pass depths. When selecting the number of passes, you need to consider the end mill. Given a chip load of .01 inches per tooth, the pass depth should never exceed the diameter of the bit, and even then only briefly. You should ideally minimize the depth of the cut per pass to reduce wear on the bit and produce a cleaner cut. However, increasing the number of passes increases the time it takes to complete. For a ½” sheet of plywood, I’ve selected 5 passes at a depth of 0.114 inches. The pass depth is calculated off of your cutting depth value and not your material thickness value.
14. Next select the direction and orientation of the cut. You can cut inside your lines, outside of your lines or on the line. Stick with a conventional cut as opposed to a climb cut because it reduces the forces on the wood and reduces the risk of sending a piece flying.
15. Next, add tabs. Tabs are critical to safe CNC routing. Tabs are pieces of material skipped over by the router to hold your pieces together. For instance, if you are cutting a circle, when you are done the piece will be loose on the table top. Tabs ensure that the pieces stay put and resist the forces of the end mill that want to send the piece flying.
    

!!!SAFETY NOTE!!!
Tabs are important to make sure you do not turn your project into a dangerous projectile

1. Choose your tab dimensions. These should be substantial sized tabs to hold the piece. As mentioned above the forces at the end mill are very strong and without substantial support on your piece it will go flying. A good rule of thumb is they should be no thinner than 25% of thickness of your work piece and no shorter than .5” wide.

2. After selecting tab dimensions, click on Edit Tabs. You can auto place them or manually place them but either way you should re-arrange them to make sure there are enough of them for the piece being cut out. A good rule of thumb is 4 tabs minimum per piece but it doesn’t hurt to err on the side of caution and add more.
3. To interactively place them, select your vector, then hover over where you want the tab and left click.
4. After making your tabs, select Project tool path onto 3D model. Choose a name for your profile and click calculate. If you set it up right, you will get a warning that the tool will cut through the material. This is ok as you want the tool to cut all the way through.
5. Next preview your tool path by clicking play. You will probably need to slow down the speed all the way. You can change the orientation by left clicking and dragging, and you can move the piece by clicking and dragging the scroll wheel. Clicking and rolling the scroll wheel will zoom in and out. Take some time to review your preview. Make sure you are conscious of where your screws are holding down your pieces and where the end mill will go.
6. Close out of the Preview pane. Select the toolpaths you want to export click on save toolpath. Export the file to ShopBot (inch)(*.sbp).