Using the 4x4' CNC Router at Twin Cities Maker Hackerspace

In the Instructable we'll run through the basics of operating the hand-made 4x4' CNC machine at the Minneapolis-based Twin Cities Maker hackerspace (also known as the Hack Factory), affectionately named "Chico".

If you don't know much about CNC workflows in general, or just want some tips about specific steps in the process, we'll also cover a variety of fundamental topics, including:

• CAD
• CAM
• End mill identification, sourcing, and mounting
• Speeds and feeds
• Workholding

If there is anything that is missing or incorrect in this Instructable, please leave a comment!

Step 1: Machine Specifications

The machine itself is very much DIY, comprised mostly of aluminum extrusions and MDF (all parts painted blue are MDF). It is unbranded and therefore comes with no support or standardized parts. Therefore it is important for all users to learn the limitations of the machine and be careful not to exceed, or even come close, to them so that we can all continue using the machine for years to come.

Here are the key specifications at a glance:

• Bed size = roughly 48x48"
• Z height = roughly 3", less your workpiece thickness and end mill flute length
• Host machine software = LinuxCNC 2.7.8
• Controller electronics = MESA 5i25 + 7i76 with HobbyCNC Chopper Driver board
• Spindle = unbranded, water-cooled Chinese spindle with 2.2kW of power, capable of up to 24,000RPM (recommend 20,000RPM or lower in practice). Uses ER20 collets.
• Maximum cutting speed = about 120 IPM. Recommend between 60-100 IPM for most operations.

Step 2: Official Github Repository

All of the information in this Instructable is derived from resources and information I've compiled over on a Github repository that I created during the recent restoration cycle of the machine.

This Github repo was (and still is) used to track outstanding functional and maintenance issues, store all manuals, datasheets, guides, and other documentation, and serve as a comprehensive reference resource for members who want to deep dive into the technical aspects of the machine (for maintenance or educational purposes).

If there is any particular topic that is not covered clearly or completely enough in this Instructable, check out the Github repo's wiki. If you still don't find the info you need, please feel free to reach out to myself, or whoever else is taking charge in the CNC area.

Step 3: CAD Overview and Tips

Before you can get the machine to do anything, you first have to have a digital design that represents what you want your final product to look like. To do that you need to use something that we refer to generally as CAD.

Computer-aided design (CAD) is a piece of software that allows you to create 2D designs or 3D models that accurately represent the thing you want to create. Different programs are appropriate for different types of objects, so don't be afraid to try out more than one and see what works for you!

.

General tips

1. Make sure your design is no larger than the X/Y/Z work envelope of the machine.
2. Think ahead to how you plan to secure your workpiece to the spoilboard, and make sure you have enough extra room in your design for clamps, plastic nails, or whatever fixturing method you want to use.
3. Be aware of the constraints of the machine, and avoid using features that are impossible to reach or would require risky tool changes. For example, overhangs cannot be easily achieved because the spindle is rigidly mounted perpendicularly to the spoilboard.
4. Always consider the size of the end mill(s) / router bit(s) you plan to use to fabricate your part while you are designing. Is there enough space for it to get in there and move around?
5. Be aware of the inside corner problem, and be sure to add dogbone or T-bone fillets to your design as needed.
6. If you want to use a piece of CAD software that you haven't seen many people use for CNC work, test it out with your CAM program before you invest too much effort in it.

.

2D software options

Just about any vector art program that can output in the vanilla SVG or DXF format can work for CNC. However, some low-end design software (like Inkscape) can sometimes do a bad job of exporting with the right flavor of SVG/DXF that is expected by your CAM software, so be sure to try a test design before doing too much real work.

1. Fusion 360
2. Adobe Illustrator ($$$)
3. Vectric Cut2D or VCarve Pro ($$$)
4. Inkscape

.

3D software options

Whichever program you choose to use for 3D modeling should be capable outputting manifold (watertight), well-formed STL or OBJ models.

1. Fusion 360 - (recommended)
2. Rhinoceros ($$$) - add Grasshopper for extra awesomeness!
3. Tinkercad (web-based)
4. Onshape (web-based)
5. OpenSCAD
6. Blender - tricky to get units and file format correct, but very powerful for organic modelling!
7. Meshmixer
8. Sketchup is NOT recommended, as it does not do a good job of exporting 3D models for use elsewhere.

.

Fusion 360 resources

Fusion 360 has quickly become my personal favorite for all CNC design work due to its ease of use, integrated CAM workflow, wealth of learning materials, strength of user community, and rate of on-going updates. However, like most CAD software, it is complex, so first figure out a project you want to build, then incrementally learn specific topics that help you make your project.

• Learn Fusion 360 in 60 Minutes

Step 4: CAM Overview and Tips

After creating your digital design in CAD, you need to create toolpaths for the machine to follow in order to carve your design out of your material. These toolpaths are generated using something called CAM.

Computer-aided manufacturing (CAM) is a piece of software that takes as input either a 2D or 3D design file (made in a CAD program) and creates commands (G-code) for the machine to follow in order to carve that design into or out of a piece of material (called "stock").

In production environments CAM is taken very seriously, can cost many thousands of dollars and take a very long time to learn how to do well. The more efficient the toolpaths, the more parts you can produce per hour, which means more profit.

However TC Maker is not a production environment, so we don't need to as obsessed with efficiency. This means that we have a lot more (and cheaper) software options available. Though this is a bit of a double-edged sword - for every free, easy-to-use CAM package there are likely dozens that are pretty unpleasant to use and require a huge amount of overly-specific knowledge.

.

General tips

1. Tabs are your friend! Use them whenever you can to prevent loose parts from getting sucked up into the dust collector or worse, shifting around and jamming up the machine.
2. In general, use a feedrate of 80 IPM and a spindle speed of 20,000 RPM. These speeds can be adjusted while running the job, and these values provide a good starting point.
3. Keep the step down, or depth of each pass, no larger than 1/2 the diameter of the end mill. For example, when using a 1/4" diameter end mill, make each pass 1/8" deep or less. Smaller step down means less material to cut per pass, so you can push the feedrate up, possibly reducing overall cutting time.
4. Ramping into cuts can significantly reduce stress on the tool and prolong it's life.
5. Take note of where the origin is being placed. This is where you will move the spindle to when its time to run your job.
6. Accurately measure the real thickness of your workpiece (stock) using calipers at multiple places. Help preserve our spoilboard!

.

Enabling dust collection

Our dust collector is currently wired up in a bit of a strange way, and must be turned on by the G-code created in your CAM software. Make sure to enable coolant either in your tool properties or general CAM settings to get the dust collector to start up when you run your job!

.

2D-only tools

1. gcodetools for Inkscape

.

2D and 3D tools

1. Fusion 360 - (recommended)
2. Vectric Cut2D or VCarve Pro ($$$)
3. MeshCAM ($$$)
4. CamBam ($$$)

.

Fusion 360 resources

Autodesk and the Fusion 360 community provide a wealth of great tutorials and videos that you should check out. For me, watching video tutorials about flat-pack furniture design and fabrication got me 90% of the way towards using the machine for my own projects!

• CNC Router with Fusion 360, Bookshelf Tutorial by Patrick Rainsberry [video]
• Overview of Fusion 360 for CNC Routers (Chair Design) by Patrick Rainsberry [video]
• CAM for CNC Router: Fusion 360 Beginner Tutorial by Design The Everything [video]
• Getting Started: Introduction to CAM and Toolpaths by Autodesk [article]
• CAM basics from Autodesk by Autodesk [videos]

Step 5: Post-processing Tips

When you are ready to export the toolpaths created inside of your CAM software you will find that you often need to tweak the resulting G-code to match the particular "flavor" that is expected by the machine you want to use.

A post processor is a piece of software that alters the initial raw G-code created by the CAM software by adding any proprietary codes or formatting that your particular CNC machine expects. Most of the time this functionality is built into whatever CAM program you are using, but its good to be aware of this step.

Regardless of the CAM package you choose, try to make sure that the G-code you end up with is in the LinuxCNC or EMC2 format. If you don't know, that's OK - you can simulate the G-code on the CNC machine's computer before trying to run it!

.

Fusion 360 notes

Set the allowHelicalMoves property to No to disable the use of very small arcs used by some operations. LinuxCNC does not like the way these arcs are created and will reject any file that contains them.

The default LinuxCNC post-processor will also add a couple of movement commands that can seriously mess up the machine or your workpiece. Remove the following lines from all G-code files you create:

1. Near the beginning of the file is G53 G0 Z0. This would plunge the end mill down onto or into your workpiece before moving to the first cutting coordinate, often marring the material or breaking the end mill. Removing this line will make the machine move to the first coordinate from wherever you positioned the spindle before the job.
2. At the very end of the file are two movement commands that plunge the end mill into the material directly after the final move - G0 Z0.6 and G53 Z0.. Remove these lines to make the spindle just spin down after the last command without moving anywhere. You could also change the coordinate to a negative number to move the spindle above the workpiece.

.

Don't forget about dust collection!

Don't forget to enable coolant in order to get the dust collector to turn on! I know, its strange, but it works!

Step 6: Overview of End Mills and Usage

For a more comprehensive guide and specific recommendations for different materials, see the End mills overview and usage page on the Github wiki.

.

End mill characteristics

• Flutes = single, 2, 3 and more
• Flute type = straight, spiral and O
• Nose profile = flat, ball, bull, tapered/conical, and V
• Cutting length = the usable length of the tool, excluding shank.
• Mill diameter = 1/8" to 1/2" is common for this size of machine, but can be much smaller or a little bit larger.
• Shank diameter = our spindle has an ER20 collet, with a maximum shank diameter of 1/2". We have a variety of collets on-hand for common sizes, including 1/8", 1/4", 1/2" and more.
• Cut direction = up, down, and compression cut
• Composition = HSS, carbide, and exotic coatings

.

For 2D routing

In general, stick with flat nose end mills in order to cut all the way through material with minimal spoilboard penetration.

For cleaner, slower cuts, try a 1/2" or 1/4", flat nose, 2-flute (spiral).

For rougher, faster cuts, try a 1/2" or 1/4", flat nose, single or 2-flute, straight flute. Otherwise known as conventional router bits.

When surface finish matters (with plywoods, for example), look for end mills with different cut directions:

• Up-cut cuts from the bottom up, which can cause tearout on the top surface
• Down-cut cuts from the top down, which can cause tearout on the bottom surface
• Compression-cut cuts from both directions at the same time (!), leaving both the top and bottom surfaces looking good. Can be more expensive though.

For plastics, try a 1 or 2 flute, up-cut, "O" flute end mill to scoop out long curls of material and immediately eject them up and away from the cutter to minimize melting and re-attachment from heat.

.

For 3D milling

In general, stick with ball nose end mills. A 1/8" ball nose, 2-flute end mill is a great all-around choice.

A tapered end mill can also be used for the same effect, with the added bonus of having a much larger shank compared to the tip diameter. This helps prevent breakage and may even allow for faster cutting.

.

For detailing and engraving

• V bits are popular for classical signage, but also impose a strict (though sometimes desirable) aesthetic.
• The smaller the diameter, the finer the features.
• Look into PCB isolation / micromachining bits
• Flat nose preferable to ball nose.

.

Where to buy

• McMaster-Carr = moderate selection of high quality, moderately priced end mills
• ToolsToday = large selection of good quality, reasonably priced end mills
• Discount-Tools = large selection of varying quality, low-priced end mills. Good deals, but can be hard to locate appropriate end mills across multiple sections.
• MSC Direct
• Carbide3D = small selection of high quality, low and high-priced end mills. Focused on delivering fewer, but well-researched options for amateur/DIY users.
• Inventables = same idea as Carbide3D.
• Amazon = large selection of pretty much every level of quality and price. Can be hard to find what you need, but good deals are out there. Looks for end mills with lots of ratings/reviews!
• Menards and Home Depot both sell some low-cost, moderate quality straight router bits

Step 7: Understanding Speeds and Feeds

Credit for the above image goes to CNC Cookbook, who have published this great article on speeds and feeds.

The topic of speeds and feeds is one that makes CNC work more difficult to jump into than other digital fabrication technologies like 3D printing or laser cutting. Nonetheless, understanding the fundamental principles at work is essential to your success in using the machine with a minimal amount of frustration. Firstly, some definitions:

• Feedrate is the linear movement speed of the machine, measured in inches per minute (IPM)
• Speed is the rotational speed of the spindle, measured in rotations per minute (RPM)

When the feedrate and speed aren't balanced correctly, all sorts of unpleasant (and costly) things can happen, including:

• End mills breaking (too much feedrate, too little speed).
• End mills softening due to excess heat, causing dulling and breaking (too much speed, too slow feedrate).
• Materials burning, melting, or even catching fire due to friction (too much speed, and/or too slow feedrate).

What makes this topic so hard to teach is that every machine is different, with it's own combination of end mills, spindle, linear motion system and more. The best we can do is mindfully experiment with scrap material, then record and share what works for us on this particular machine.

.

General tips

For most tasks, try starting with a feedrate of 80 IPM and a spindle speed of 20,000 RPM, then adjust these values during the job using LinuxCNC's override sliders. Once you've dialed in a good balance of speed and feed, use that as your starting point for future toolpaths.

Most of the time you'll want to adjust the feedrate down and leave the spindle speed alone.

IMPORTANT: Do not push the spindle speed close to or above 24,000 RPM! That is it's maximum rating, and bad things can happen at those speeds.

Step 8: Inspect and Lightly Clean the Machine

Before running your job, or even securing your workpiece to the spoilboard, let's first make sure that the machine is in good condition and that all the electronics are still working as intended.

This machine is very hacky and temperamental, so you can never really be sure that everything is OK without taking a look yourself. You wouldn't want to have your job fail halfway through due to something you didn't take a minute to look at!

In order to keep the machine running for the community as long as possible, please run this checklist before running any job on the machine. Since we don't have a dedicated maintenance tech we all need to do our part to identify and prevent problems from getting out of hand.

1. Clear any debris away from the aluminum extrusions and angle iron ways using your hands or a soft brush.
   • You don't want those v-wheels getting stuck on anything!
2. Clear any excess debris from the leadscrews, especially around the drive nuts.
   • These suckers are robust as heck, but keeping them clean will decrease the chance of your job failing.
3. Check the condition of and clear any debris around all of the v-wheels throughout the machine.
   • If any look to be unusually worn down, visibly broken or spinning freely, contact the CNC or Wood Shop manager and let them know. It may not necessitate stopping your job completely, but do make sure to test the movement of the machine by jogging.

Step 9: Inspect and Turn on All Controller Electronics

1. Check that all stepper motors cables are firmly plugged in to the appropriate connectors on the interconnect panel.
2. Check that all endstops cables are fully plugged in to the appropriate connectors on interconnect panel.
3. Check that the spindle cable is fully connected to the white cable coming through the hole in the side of the box.
4. Plug the dust collector power cord into the AC outlet labelled "DC", if it is not already.
5. Plug in the 110V power cord that hangs out of the hole in the box.
   • The outlet fans should immediately light up blue when power is supplied.
6. Turn on the host machine PC if it is not already on.
7. Check that the stepper driver board is ON, indicated by the green light on the interconnect panel.
   • If the green light is not lit, flip the switch labelled "Step Drive".
   • If the light still does not come on, check that the power cord is plugged in to a working socket. Also check that the power strip inside the control box has not had its fuse tripped.
8. Plug in the 220V power cord hanging out of the box to the nearby 240V twist-lock outlet.
9. Turn on the coolant pump and VFD using the toggle switch on the interconnect panel labelled "Spindle".
   • You should see the blue coolant begin to flow through the tubing and into the spindle.
   • Check for any coolant leaks coming from the mobile control station, the interconnect panel connectors, or the connectors on the spindle itself.

Step 10: Secure Your Workpiece to the Spoilboard

With a big, heavy gantry moving around and an end mill ripping through material at 20,000 RPM, you're going to need a way to securely and safely hold your workpiece in place!

Built into our current spoilboard are 5 rows of aluminum T-track channel that allow us to slide the heads of long 1/4" hex bolts up and down the length of the bed. We can then use some neat hold down clamps and knobs to clamp the workpiece down at strategic locations.

We currently have about 4 functioning clamps floating around for anyone to use. You can usually find them either on the machine bed or keyboard shelf, or on the shelving nearby.

When placing your clamps try to make sure that the knobs and screws will be clear of the spindle and end mill throughout the entire cutting of your design. We will check for this more thoroughly in a bit, but just try to get them in the ballpark for now.

Be aware that as of August 2017 the spoilboard is in pretty rough shape and needs to be rebuilt. This will make workholding a bit trickier for now as workpieces will tend to settle in unusual positions.

Step 11: Mount Your End Mill in the Spindle

To prevent your tool from getting pulled out during the cut, it is very important to mount your end mill correctly! Track down an expert and have them show you in person sometime just to make sure you really get it!

Mounting an end mill is a pretty simple process, but it can be tricky to get right without knowing the proper steps. If you aren't 100% sure about these instructions, ask!

1. Find a collet that matches the diameter of your end mill's shank.
   
   • In the main accessories tub there are 1/2", 1/4" and 1/8" collets, but about a dozen other sizes (including metric) are floating around in the shelving or storage nearby.
2. Insert the collet into the collet nut. Press it in slightly and it should "click" into place as the indented ring on the collet snaps into the guide on the inside of the collet nut.
3. Insert your end mill into the collet until the end of the shank is flush with the end of the collet. Be careful not to pop the collet out of place!
4. Loosely screw the collet nut onto the threaded column of the spindle. Just finger tight is good.
5. Use the blue wrenches to tighten the collet nut, without overtightening it.
   • The blue wrenches both fit ER20-sized things on one end, and have another size on the other. Look for the white markings.
   • Slip the ring-shaped wrench around the collet nut.
   • Slide the open-ended wrench onto the flattened notches on the spindle body just above the collet nut.
   • Turn the wrenches so that your hands move away from each other to tighten the collet nut. Don't overtighten - just a quarter turn or so should work!

.

Unmounting your end mill

Do all these steps in reverse (including turning the wrenches towards each other) to loosen and remove the end mill.

To get the collet out of the collet nut, just gently tilt it and it should pop right out of the guide.

Step 12: Log on to the Host Machine (PC)

The host machine is password protected in order to prevent untrained members from hopping on and causing mayhem (unintentionally or not).

To get the current password for the machine please contact one of the CNC experts - either Pete McKenna or Jason Webb. If you can't reach either, try reaching out to the Wood Shop manager to find out who to talk to.

Step 13: Launch LinuxCNC With the Mesa 4x4 Configuration

Use the Mesa 4x4 desktop icon to launch LinuxCNC pre-configured with all the settings for our machine.

Step 14: Load and View Your G-code File

Load your G-code file using File > Open (Ctrl + O).

Once loaded, use the mouse to fly the camera around and orient the screen in a way that makes sense to you. You can also use the X/Y/Z view buttons to snap to standard views.

Note the cube marked by the red dotted lines. This indicates the work envelope of the machine, and no toolpaths or movements are allowed outside of this box (they will be stopped by "soft" limits).

Step 15: Unlock and Enable the Machine

The machine is locked by default until you manually enable it.

First click the Emergency Stop button (red X), which should enable other buttons on the toolbar.

One of these buttons is the Machine Power button directly next to the Emergency Stop button. Click it to enable the system and establish a connection to the machine itself.

You may notice the machine jump slightly and start to hum - that means its alive!

Step 16: Home All Axes

Before the machine can understand how to move where you want it to, it needs to first understand where it is. We do this with a process called homing, which involves slowly moving each axis until it hits it's respective minimum endstop, at which point the machine knows for sure that the axis is at the 0 position.

You can home each axis individually using the Homing > [Axis name] options under the Machine menu. It is recommended that you start with the Z axis to get the spindle out of the way of any clamps.

Alternatively you can home all axes using the Homing > Home all axes option, which will automatically home each axis individually starting with the Z axis.

To abort the homing process at any time, either turn off Machine Power, or activate the Emergency Stop button.

Step 17: Jog Machine to Desired Origin on Your Workpiece

Use the keyboard arrow keys to move the spindle to wherever you want the origin to be on your workpiece.

• Move the X axis with left/right arrow keys.
• Move the Y axis with up/down arrow keys.
• Leave the Z axis all the way up for now.

If the machine is running too fast or too slow for you, check that the movement increment in LinuxCNC is set to Continuous, and/or adjust the Jog Speed slider on the left side of the screen.

Step 18: Align Machine Coordinates to Your Workpiece

Although we've physically moved the spindle to where we want our job to start, right now LinuxCNC still thinks that the origin (0,0) is at the very bottom left of the spoilboard. This means that if you were to hit the "Play" button to run your G-code, the machine would run all the way back there to cut out your part!

To tell the machine that we want it to consider the current position to be the new origin we need to touch off each axis using the following process:

• In the Machine control (F3) tab on the left, make sure that the X axis is selected.
• Click the Touch off button.
• In the dialog box that pops up make sure that the value is "0", then click OK.
• The screen on the right should update and move your toolpaths to the current position of the spindle along the axis you selected.
• Repeat this process for the Y axis, but leave the Z axis alone for now.

Step 19: Jog Machine Around Your Job to Check Travel

With the Z axis still all the way up, use the keyboard arrow keys to carefully jog the machine all the way around your toolpath, checking to make sure that the movement is smooth and even and that there is no risk of the end mill, collet or dust shoe running into any clamps once they are lowered. Adjust the placement of any clamps that are in the way.

You can use the page up/down keyboard keys to move the Z axis up and down if you want to see where the various spindle parts at different stages of the job.

Step 20: Run Your Job in the Air to Check for Problems

With the Z axis still all the way up, let's go ahead and do a test run of your job in the air to make extra sure that no problems will happen when the Z axis is lowered.

Similar to the X and Y axes, use the keyboard page up/down buttons to move the Z axis to where you want it, then use the Z axis "Touch off" button to set the new 0 coordinate. It is recommended that you place the tip of the end mill somewhere between the minimum endstop location and the top of your workpiece.

Hit the Play button to run your job, and get ready to hit the Stop button at any moment should anything go wrong.

Step 21: Touch Off Z Axis to Top of Your Workpiece

NOTE: In order to preserve the spoilboard and extend it's life as long as possible, this step is critical to get right! If you measured your workpiece thickness accurately enough during your CAM setup, the spindle should not even touch the spoilboard (or just make very, very shallow indentations in it) when cutting all the way through.

Consider using another piece of material between the spoilboard and your workpiece so that the machine's spoilboard does not take any damage at all.

If running your job in the air looked good, you can now align the Z axis to your workpiece by using the keyboard page up/down keys. Use a relatively large movement increment when you're far away from the workpiece, then use a much smaller increment (like 0.1in) when you are getting close.

If you need to get it really accurate, try putting a piece of paper on the workpiece and moving the Z axis downward until you can just barely move the paper between the end mill and spoilboard.

In the future we will have a more precise automatic Z height probe, but for now just get as close as you can!

Step 22: Put on Personal Protective Equipment (PPE)

The Wood Shop has a small collection of ear muffs and safety glasses for general use, which are all available on the clamp rack.

The CNC machine is LOUD, and tends to produce a constant, relatively high-pitched tone when cutting through material, which can fatigue the ears over long periods of work. Use ear protection and take breaks to give your ear drums some rest from time to time.

End mills can break and be thrown long distances at high speeds. The dust shoe should help contain these disasters, but its better to be safe than sorry - protect yourself with safety glasses!

Step 23: Install the Dust Shoe

The last thing you need to do before actually running your job is attach the dust shoe. The dust shoe does a great job of containing dust and chips while also focusing the suction of the dust collector. It also lightly brushes previous cuts when it moves over them, cleaning up the really rough cut edges a bit.

The dust shoe attaches to the mounting plate using strong magnets. Just get the orientation of the shoe correct and it should just snap together!

Note the positions of the magnets - two on the left and one on the right. This, along with the red sticker, can be helpful in getting the orientation right.

With an end mill installed it can be a little tricky to get the dust shoe installed, even with the Z axis all the way up. Just raise the Z axis a bit and tilt the dust shoe until you can slip one of the edges between the spoilboard and end mill.

Step 24: Run Your Job

Check one last time for the following:

1. Blue coolant should be flowing in and out of the spindle. If not, go back to the Machine setup step.
2. The X, Y and Z axes should all be "touched off" so that the machine knows where your workpiece is.

If things look good, hit the Play button and be ready to hit the Stop or "Emergency Stop" button at any moment. The spindle should spin up right away, then the machine will follow all of the toolpaths.

If you don't hear or see the dust collector turn on the moment you start your job, hit Stop and go back to your CAM software to enable coolant. See Step 3.

Step 25: Monitoring, Pausing and Stopping Your Job

Once the job has started running you have a number of options for stopping it depending on why you want to stop.

If you want to stop the machine to check it's progress or because you don't like the toolpath for some reason ...

• Use the Pause button to stop all axis movement and keep the spindle spinning, without forgetting our place in the G-code file. Use this when you just want to adjust a clamp or take a close look at something you just cut. Hit the Play button again to resume cutting.
• Use the Stop button to stop all axis and spindle movement, forgetting our place in the G-code file. Use this when the toolpath is definitely not what you want and you just want to start over completely.

If there is some sort of catastrophic and/or imminent failure, like the workpiece coming loose, axis movement jamming, workpiece catching fire, etc. ...

• Use the Machine Power or Emergency Stop button to completely turn off the machine and sever the connection with the computer. This will stop all axis and spindle movement, and may require the machine to be re-homed.

Step 26: Power Down and Reset the Machine

When you're done using the machine, please return it to the state you found it in (or nicer) to help the next person to use the machine get up and running quicker. This includes:

1. Remove your end mill
2. Remove and return any clamps you used to hold your workpiece.
3. Clean up any dust that is left on the spoilboard. Hint: turn on 'coolant' and jog the machine to vacuum it all up!
4. Place the dust shoe back on the mounting plate, or place it very near by.
5. Delete your files from the PC, especially if they are on the desktop.

Finally, and most importantly, power down the control electronics by flipping both of the light switches on the side of the box. You should hear the machine noise stop entirely, and the coolant stop flowing. You will also see the overhead light turn off.