Post by clockmaker on Jun 6, 2020 20:49:02 GMT
Hoping someone finds the following useful. The Quick Start Guide on the resources page is out of date and seems to be for a specific system. I sent the following to both sales@millright.com and support@millright.com. Neither could be bothered with responding. None of the following is original to me. All of it came from someone else. Unfortunately, I did not do a good job of referencing the sources. Apologies for that and the lack of formatting. This editor is limited.
MILLRIGHT CNC QUICKSTART GUIDE FOR RUNNING ASSEMBLED MACHINES Version RF
Important safety rules for operating your MillRight CNC:
• Never place your hands near a spinning end mill or bit.
• Unplug the router before changing cutting tools.
• Always wear eye and hearing protection while operating your machine.
• Always run dust collection or wear a mask while performing milling operations.
• Do not leave the machine unattended while running an operation.
• Do not operate your machine while under the influence of alcohol or drugs.
• Do not place your hands between the bed and frame while the machine is moving.
• Visually inspect wires prior to power up to prevent short circuits.
• Ensure work pieces are properly secured before running a milling operation.
• NEVER use the laser attachment on plastics without extensively researching suitability first. Many plastics can catch fire or emit very poisonous gas when lased.
This guide is intended to help you start running your assembled machine. CNC machining is a learning process that will take some time to master. The aim of this document is to get you familiar with the basic operation of the machine. Those with lasers may wish to review the laser setup instructions. That document describes hardware set up as well as the particulars of software settings for laser jobs. Additional machine operation support is provided via our forum at www.millrightcnc.proboards.com. MillRight CNC and fellow customers are there to help you.
Note that the control board is preloaded with GRBL, which is the firmware that will control the machine. Do not attempt the “reflash” the board using X-Loader or the Arduino IDE. It is ready to go, just as it was shipped to you.
1. Installing and using Universal G-code Sender (UGS) Platform
A. Make sure you have installed a recent version of Java (8+). You must have Java to run Universal G-code Sender (UGS). If you do not have Java, do a Google search for “Java download.”
B. If not already done, install Universal-G-Code-Sender (UGS) Universal Gcode Platform which can be download via the resources page at www.millrightcnc.com/resources. From here we will refer to it as UGS.
C. In UGS, change the setting for the maximum line length to 70. Go to Tools >> Settings >> UGS to access this option. Click the Edit button for Command Length Processor. Replace 50 with 70. DO NOT EDIT/REMOVE ANY OTHER TEXT. Click Yes >> OK.
D. Connect your computer to the machine using a USB cable.
E. Power up your machine’s control box. If you have the laser attachment, be careful not to plug the machine’s power supply into the laser’s female barrel plug receptacle. Doing so may destroy the laser.
F. On Windows 10 computers, the drivers for the control board should automatically load onto your computer. If you have another operating system or if they do not autoload, you might need to install the Arduino IDE linked here to get the drivers that you need. Then use device manager to point to the appropriate drivers.
G. You should now be able to establish a connection between UGS and the control board.
a. Select GRBL as the firmware.
b. Use the Port drop-down menu and select the port that you see available.
c. Select a baud rate of 115200.
d. Click the Connect / Disconnect icon or on the tool bar Machine >> Connect. The connection icon will turn from disconnected/black to connected/orange. The machine will tell you that it has been connected in the console window
.
H. Movement
a. Click on the commands tab at the top and type in $X then press enter.
This will unlock the machine to allow motion commands.
b. If you have homing switches, you can type $H then press enter. This will initiate a homing cycle. On a homing cycle, the Z axis will lift first. It will raise Z, hit the switch, back off, move very slowly into the switch again, and then pull off the switch a few millimeters. Afterwards, the X and Y motors will begin simultaneously moving the machine towards the switches (switches are in the positive direction) until those switches are engaged. It will do the same pull off, switch reengage, then slight pull off on each one of those axes. After a homing cycle, the machine is unlocked for additional motion commands. The advantage of homing is that the machine will obtain a known position which will allow you to utilize work position systems, which will be discussed later.
c. Go to the Console tab and type G21 into the command line and hit enter. This tells the machine you will be issuing movement commands where the units are in millimeters. Now you can jog the machine. Jogging means the machine is just being moved around to get it into position, such as to get it into place for a cutting operation.
d. Click on the Jog Control tab. You can use the axis control buttons to move the machine around. The X- button will move the router to the left; X+ will move the router to the right. Y+ will bring the table towards the front of the machine; Y- will move the table towards the back. Z+ will move the router up; Z- will move the router down. Be mindful of the step size. Since you set a G21, the step size figure is the millimeters that it will move when you press an axis button. It is possible to move the machine too far and crash it, so be careful. If you just homed the machine, you need to first move X-, Y-, and Z- because each axis is homed towards the positive side of travel. This is the conventional home direction for CNC routers.
2. Basic GCode Commands
a. In addition to using the axis control buttons, you can type in G code commands into the command line. Let us cover some basic G codes now.
b. G0 Rapid movement at the default feed rate (feed rate is how fast it moves) G0 movements are just for getting around. You do not cut anything with a G0.
c. G1 Linear movement at the specific cutting feed rate.
d. G2 Clockwise arc movement at the specific cutting feed rate.
e. G3 Counter-clockwise arc movement at the specific cutting feed rate.
• G2 and G3 movements are accompanied by X, Y, or Z, and I, J, or K “words” to tell the machine how exactly to arc. You do not need to understand any of that right now because the CAM software (the program that makes your g code for cutting stuff out) will do all of that for you.
f. G20 Sets units to inches
g. G21 Sets units to millimeters
• Since these commands are “modal”, it remembers that you set it (while the controller is on!) and will not be changed until you issue the opposite command. If your CAM software generated G code in millimeters, you need to set a G21, and vice versa.
h. G90 Specifies absolute positioning
i. G91 Specifies incremental positioning
• G90 and G91 are modal commands as well. This is best understood by way of example. Let us say you were at X50 and then issued the command G0 X60. Where would it move? It depends. If you had a G90 set for absolute positioning, it would move 10 to the right. If you had a G91 set for incremental positioning, it would move 60 to the right. See the difference? Now let us say you were at X50 and issued the command G0 X0. Where would it move? If you had G90 set, it would move 50 to the left to take the machine to the position of X0. If you had a G91 set, it would not move it all. G91 is incremental, so 0 from where you are at is… well, where you are at. Be advised that using the axis control buttons under the Machine Control tab in UGS will set a G91. It does this every time you click one of the axis control buttons.
j. G92 Used to create a temporary work coordinate system. This is most often used to zero out each axis so you can declare the origin of your work. For instance, you might jog the machine to where you want to start the work, setting the cutting tool to the point you want to start the cutting file. For instance, G92 X0 Y0 Z0 will set the “work coordinate system” to zero for each axis. Many cutting files use X0 Y0 Z0 as the origin, so this is the position you will most often want to set before starting a file.
k. F Specifies the feed rate for G01, G02, and G03 moves. The F command must be used with a number. F 1000 or F200.0 for example.
l. S Specifies the spindle speed or laser intensity. The S command must be used with a number. S6000 or S 120000.0 for example. On machines shipped assembled with a laser installed, S12000 is the maximum value, with S3500 being about the minimum value that will come on after an M3 command.
m. M3 Turns on the spindle or laser (only if a spindle is configured for control by enable pin). An S command alone will not turn on the laser or spindle. An M3 will allow it to turn on.
n. M5 Turns off the spindle or laser (only if a spindle is configured for control by enable pin).
3. BITS/CUTTERS/MILLS
a. Bits are also referred to as a CUTTER or a MILL. Note that you will see cutter in CNC software and when you look at a list of cutters to choose from, they all end in MILL. When searching Amazon for home shop systems, ‘CNC bits’ will surface more relevant results for home shop systems than ‘CNC cutters’ or ‘CNC mills’.
b. In the home shop, CNC bits are often interchangeable with router bits. Smaller home shop systems are limited to 1/8 inch and 1/4-inch shank bits. Some higher end home shop systems can accommodate 1/2-inch shank bits.
c. Non-standard shank sizes can be accommodated if your router or spindle has an ER collet. ER collets have a wide clamping range and high accuracy. With a full set of ER collets you can hold any diameter that is in the clamping range of the set.
d. Terminology
• HOLDER: The collet is the ‘holder’. Holder is the term used by commercial systems and is found in CNC related software. Holder dimensions are needed to avoid collisions.
• ROTATION DIRECTION: Clockwise (CW) direction is what you find for most tools such as drills, routers, lathes, etc.
• FLUTE: The cutting edge and corresponding “trough”. Most home shop systems will use bits with between one and four flutes. More flutes are not necessarily better. More on this later.
• MATERIAL: Bits are usually made with High Strength Steel (HSS) or Carbide. If the cutting edge is carbide, then enter carbide in the software.
• GEOMETRY: The bit’s dimensions. If you can, measure your bits with digital calipers. Geometry terms software dependent, but most use shaft diameter, cutter diameter, cutter shape, overall length, cutter length, stick-out length, etc.
• COATING: Some software will ask about coatings used to reduce friction.
• CHIPS: The material removed by the bit.
• CHIP EVACUATION: The process of removing or evacuating the chips from the cut.
• CHIP LOAD: The amount of material removed by each cutting edge. Feed speed, cut depth, number of flutes and RPM determine the chip load. Other factors include the use of compressed air to clear the cut, cutting fluids, up-spiral, down-spiral, and straight flutes. Too much chip load results in chatter, rough finishes and broken bits. Too little results in heat which can burn the material and weaken the bit.
• DEFLECTION: Bit bending due to load. Deflection is bad for both the bit and the cut quality. A shorter stick-out length will reduce deflection.
e. Common Profiles (types)
• BALL END: The tip is fully radiused leading to vertical sides.
• BULL NOSED: The tip is partially radiused leading to vertical sides.
• CHAMPHER: Angled cutters for removing the edge from a corner.
• DOVETAIL: Flat bottomed cutters with inward angles side cutters.
• FACE: Flat bottomed cutters with relatively short 90-degree side cutters.
• FLAT END: Flat bottom with vertical sides.
• FORM: Used for side profiles with any shape possible.
• LOLLIPOP: Spherical end mill used to make undercuts and access hard-to-reach places. They are used in a variety of applications, including plunge, face, profile and tracer milling.
• TAPPERED: As the name implies, the sides are tapered. The tip can be pointed, radiused or flat. Also referred to a V-bit when the tip is pointed.
• THREADED: Used for cutting threads.
• Both ball and bull nose cutters are often used for 3D operations during finishing passes. Flat cutters are your most common cutters and will be used for everything from 2D to 3D (during roughing operations).
f. Flutes
• Most CNC bits have helical flutes. A helical flute allows the edge to gradually ramp up its engagement on the material unlike a straight flute where the edge engages all at once. Straight flutes are generally less expensive and are perfectly fine for wood and plastics as evidenced by the extensive use with wood routers. Do not try a straight fluted cutter on metals unless you know exactly what you are doing. If production is a concern, note that a spiral fluted cutter can cut about three times faster and will leave a better finish.
• There are four basic flute types.
1. STRAIGHT: The flutes run straight up and down.
2. UP-CUT: The flutes spiral in a direction that pull the chips towards the holder, same as a drill. UP-CUT flutes are good at evacuating chips from the cut. Because the cutters pull up towards the surface of the material, there will often be tear out on the top edge of the cut. UP-CUT flutes also pull the material up from the table which can be a problem for thin or flexible materials.
3. DOWN-CUT: The cutters spiral in the opposite direction of UP-CUT flutes. Not generally used for CNC milling since they push the chips in to the cut unless the top finished edge is a concern. It is best to use compressed air system or fluids to remove chips. As noted above, UP-CUT flutes can pull flexible materials up from the table. DOWN-CUT flutes work well with thin, flexible materials where chip evacuation is less of a problem. Also good for inlays and shallow pockets. While these DOWN-CUT flutes will leave the best finish at the top edge of the cut, they will cause tear out at the bottom of the cut (less if the bottom of material is in contact with a spoil board).
4. COMPRESSION: These are a combination of up-cut and down-cut cutters. This will leave the best surface finish on both sides of the piece. The top half of the cutter is a down-cut while the bottom half is an up-cut. Again, it is helpful to have compressed air or fluid to evacuate chips from the cut when it starts getting deep. These cutters are generally only used for edge contours where material thickness is within the limits of a single pass.
• Flute count.
1. For home shop systems, available bits will likely have between one and four flutes. Less flutes equals bigger gullets which results in better chip clearing. Bits with more flutes will have shallower gullets, which results in a thicker core and a stronger bit. More flutes will produce a smoother finish but will generate more heat. More flutes will also allow higher feed rates, assuming chip evacuation is sufficient. The result is that spindles, because they operate a lower RPMs, can benefit from more flutes, while routers, because they operate at higher RPMs, generally work better with fewer.
2. The cutting operation type will also play a roll. Slotting and plunging cuts do not leave much room for chip evacuation, while side cuts and pocket clearing, three-dimensional paths are more forgiving.
g. Calculating RPM and Feed Rate
• The goal is to optimize the CHIP LOAD. The formula for Chip Load is:
Feed Rate / (RPM x Flute Count), where Feed Rate is inches per minute
• The typical Chip Load is typically hundredths or thousandths of an inch. You can find many cutter manufacturers sites that will provide Chip Load for their bits. You may be able to find one that is similar to the bit you are using. One such site is www.harveytool.com/cms/GeneralMachiningGuidelines_17.aspx
• There are free feed rate calculators available and Fusion 360 has built-in feeds and speeds for various cutters. Those are generally going to be conservative and might be good enough. If you want to optimize your feeds and speeds, you should consider spending a few dollars on G-Wizard. If your system is under three horsepower, which if you are reading this it almost certainly is, then the cost is under $100 for a lifetime license. It will likely pay for itself in bits very quickly. It is available here: www.cnccookbook.com/g-wizard-cnc-speeds-and-feeds-calculator/
• When performing multiple milling operations on a part, for each bit use the most difficult path for calculations. This will likely be a slotting or deep pocket clearing operation.
• The depth of cut should not exceed the bit’s diameter and the overlap between passes, called STEP OVER, generally should not exceed 40% of the bit’s diameter. Too little and there is a risk of burning the material and overheating the bit, too much and the bit may not be able to evacuate the chips and the bit may fail. Smaller step over passes will result in a smoother finish. Longer bits should have smaller step overs to avoid deflection.
• Other considerations include the rigidity of the system, i.e., belts vs lead screws, the material, MDF vs Aluminum, spindle vs router, etc.
h. Operations
• There are a few basic milling operations: Hole, Pocket, 2D Profile, 3D Surface and Facing. In all cases, tool entry is especially important. There are three options: Plunge, Predrill and Helix Ramp. Plunge should almost never be used unless there is no other way as it is hard on the bit. Instead use Predrill, but this will require a bit change. Helix ramp is usually the best option. Ramp feed speed can be slower but be careful not to make it too slow. RPM can also be adjusted if using a speed-controlled spindle.
4. Work Coordinate Systems
Note that this part is a bit advanced. Most will not understand this until they have some experience. You can keep running things using the G92 method described above until you get ready for this. Programmed work coordinate systems can only be used if you have homing switches. This allows you to move the machined to predetermined starting positions even after powering off the machine. This is especially useful if you have a clamping fixture and wish to run the same operation over and over, or if you wish to machine a part with two or more different tools.
a. Work coordinate systems are designated with G10 commands and accessed using the G54 through G59 commands. Let us cover the basics of the commands:
G10 L20 P1 X0 Y0 Z0 Sets the current position of the machine as the origin (0,0,0) point of the G54 coordinate system.
G10 L20 P2 X0 Y0 Z0 Sets the current position of the machine as the origin (0,0,0) point of the G55 coordinate system.
G10 L20 P3 X0 Y0 Z0 Sets the current position of the machine as the origin (0,0,0) point of the G56 coordinate system.
Do you see the pattern? P4 is for G57, P5 for G58, and P6 for G59.
There is another way to set work positions, but this is perhaps the most easily understood.
G54 Modal Interpret all further absolute positioning commands (those commands issued when a G90 is set) as places to go in the G54 system.
G55 Modal Interpret all further absolute positioning commands (those commands issued when a G90 is set) as places to go in the G55 system.
G56, G57, G58, and G59 are set the same way. You can tell where the origins of these work coordinate systems are relative to the origins of the machine coordinate system by typing $# into the command line.
G53 G53 Specifies the machine coordinate system for the motion command that follows on the same line. This is a “non-modal” command, so any further commands issued without a G53 on the same line will be interpreted within the context of the work coordinate system.
Let us look at a real-world example. Imagine that you wish to do a 3D carving that will first be roughed (material removed in bulk close to the finished contour) with an end mill and then finished with a ball nose mill. After you lay your board on the machine table and clamp it, you might have a particular point on the board that you wish to begin your work (possibly at the bottom left corner). You could jog the machine to that location then establish that point as the G56 work coordinate origin by typing G10 L20 P3 X0 Y0 Z0. You would type G56 and then run the roughing operation and change the cutting tool to a ball nose end mill. You would then home the machine again and type in G56 X0 Y0. Notice that you did not issue a Z0. The ball nose tool you installed will almost certainly be sticking out more or less than the end mill you used, so you will not want to command the machine to Z0 before resetting it. Jog the Z down to the stock top. You can either issue a G92 Z0 or reset the Z origin for this coordinate system using G10 L20 P3 Z0. Keep in mind, we are using “P3” because in this example we are setting the G56 coordination system.
5. Touch-plate Set Up
a. There are two kinds of touch plates, the first is just to set the Z axis height. The other locates the work piece edges in all three dimensions and can also be used for just Z axis height. The cost is about the same, so go with the edge finder.
b. UGS Platform has a probe module available as a plug-in. The process is straight forward. This YouTube shows how to set it up: www.youtube.com/watch?v=kpz-6x_synE
• Install and open the Probe Module.
• Measure your edge finder and enter the dimensions into the module. A digital caliper works best.
• Place the edge finder on the material to be machined in the same corner used to orientate the tool paths.
• Select a bit, measure the diameter and enter the diameter into the Settings section of the Probe Module.
• Connect the edge finder to the control box and to the bit. When the bit touches the edge finder it will complete the circuit to let the control box know that the bit has reached the edge.
• Jog the machine so the bit is about a 1/4-inch above and over the edge finder about 1/4-inch from the outside edges.
• In UGS, reset the X, Y and Z axis locations to zero.
• In the Probe Module select the XYZ option.
• Set the X and Y probe distances to 15 and the Probe Distance / Direction to -10.
• Click the Measure Outside Corner button.
• Remove the edge finder.
• Zero the location coordinates by entering g0x0y0z0 in the console.
• The bit should now be just about touching the corner of the work piece.
6. Running Your First Job:
a. You might be interested in running a cutting file now. You can run a very basic engraving file using this GCode file that you can download from the link in the original Quick Start Guide. This will require a piece of wood about 8 x 8 and between 1/2” inches, and 3/4” inches thick (200mm x 200mm and 13mm to 19mm thick). A larger piece is okay. Recommend using something soft like MDF or Pine.
b. Put the cutting tool in the router. This file was designed for a 1/4” (6mm) core box router bit, but an end mill, ball nose, or V bit in a size 1/4” or under will work as well.
c. Place the board on the table and clamp it down. Keep the clamps towards the edges so the cutting tool will not collide with them.
d. We will now set a G92 X0 Y0 Z0. To do this, jog the machine towards the lower left side of the board (X and Y position). After jogging to the desired X and Y position, start lowering the cutting tool towards the board. Be mindful of your step size here. Once the tool gets close to the board, change the step size to 0.1mm and keep dropping it. Place a sheet of notebook paper underneath the cutting tool and on top of the board. Slide the paper back and forth to see if it catches on the cutting tool. Keep lowering the Z axis until it just barely drags on the paper. At this point, issue the G92 X0 Y0 Z0 command.
e. Change the step size back to millimeters. Now, issue a G90 G0 Z5 command to lift the Z axis above the stock. Assuming you had a G21 (millimeters) set, this will raise the Z axis 5 mm. This is because it is best to turn the router on when it is not engaged with the stock.
f. The program will move the machine about 6.5 inches (165mm) in the Y+ directions and 7.5 inches (190mm) in the X+ direction. Watch to make sure the bit does not collide with your clamps.
g. Now load the GCode file you just downloaded by clicking on the File >> Open GCode File… then browse and select the file. You should see the milling path displayed in the Visualizer.
h. You are now ready for a simulation run.
• Remove the board but leave the clamps in place.
• Click Machine >> Send in the menu bar or click the Play icon in the tool bar.
• Stay clear and do not reach into the cutting area under any circumstances. Be prepared to click the Stop icon or cut the power in case something goes wrong.
• The machine should move the router around for about 4 and half minutes.
i. Assuming everything performed as expected, you are now ready for your first machining operation. If the bit hit your clamps or the router went to areas not where your board would be. then go back and check the system and settings.
• Turn on the router and click Machine >> Send in the menu bar or click the Play icon in the tool bar.
• Stay clear and do not reach into the cutting area under any circumstances. Be prepared to click the Stop icon or cut the power in case something goes wrong.
• After about 4 and half minutes you will end up with a board with Mill Right CNC inscribed on the surface.
7. Designing your own parts
You will need to use some other software to design your own parts and make g code for them. MillRight does not officially support software, but basic tutorials for Autodesk Fusion 360 and Inscape are on the MillRight CNC Resources Page. These software packages are free. You will need to get a hobby or free small business license from Autodesk for Fusion 360, as appropriate. Do a google search to download these programs.
8. Troubleshooting
P: Universal G Code Sender gives an error when trying to open a connection, or the machine has stopped responding.
S: Close UGS, remove USB cable from USB port, wait five seconds, plug back in, open UGS, and attempt to open a connection.
P: The motors make a noise that sounds like radio static.
S: This is normal when the machine is first booted up and no motion commands have been issued.
P: The machine is not moving to the commanded position.
S: Most often this happens when incremental positioning is set (G91) but the user thinks the machine is in absolute positioning (G90). Set the appropriate mode.
P: The machine appears to be missing steps or not moving the full distance commanded on one axis.
S: The set screws should be checked on the motor pulley and tightened if loose. If this is not an issue, the belt may need to be tightened. Also, the voltage should be checked on the stepper motor driver to ensure that it is around 0.60 volts.
P: Files are running erratically, or commands are being skipped with a warning that the command length is too long. Confirm that the line length maximum is set to 70 in UGS. Also confirm that S: your CAM software is not using more than four decimal places for a position command.
P: The motor stalls or the machine jumps off the planned path when cutting. Solution: Slow down the feed rate and/or shallow up the cut.
S: The machine stops during homing before it hits the homing switch. Separate motor wires from switch wires to reduce electromagnetic noise creating a false trigger.
MILLRIGHT CNC QUICKSTART GUIDE FOR RUNNING ASSEMBLED MACHINES Version RF
Important safety rules for operating your MillRight CNC:
• Never place your hands near a spinning end mill or bit.
• Unplug the router before changing cutting tools.
• Always wear eye and hearing protection while operating your machine.
• Always run dust collection or wear a mask while performing milling operations.
• Do not leave the machine unattended while running an operation.
• Do not operate your machine while under the influence of alcohol or drugs.
• Do not place your hands between the bed and frame while the machine is moving.
• Visually inspect wires prior to power up to prevent short circuits.
• Ensure work pieces are properly secured before running a milling operation.
• NEVER use the laser attachment on plastics without extensively researching suitability first. Many plastics can catch fire or emit very poisonous gas when lased.
This guide is intended to help you start running your assembled machine. CNC machining is a learning process that will take some time to master. The aim of this document is to get you familiar with the basic operation of the machine. Those with lasers may wish to review the laser setup instructions. That document describes hardware set up as well as the particulars of software settings for laser jobs. Additional machine operation support is provided via our forum at www.millrightcnc.proboards.com. MillRight CNC and fellow customers are there to help you.
Note that the control board is preloaded with GRBL, which is the firmware that will control the machine. Do not attempt the “reflash” the board using X-Loader or the Arduino IDE. It is ready to go, just as it was shipped to you.
1. Installing and using Universal G-code Sender (UGS) Platform
A. Make sure you have installed a recent version of Java (8+). You must have Java to run Universal G-code Sender (UGS). If you do not have Java, do a Google search for “Java download.”
B. If not already done, install Universal-G-Code-Sender (UGS) Universal Gcode Platform which can be download via the resources page at www.millrightcnc.com/resources. From here we will refer to it as UGS.
C. In UGS, change the setting for the maximum line length to 70. Go to Tools >> Settings >> UGS to access this option. Click the Edit button for Command Length Processor. Replace 50 with 70. DO NOT EDIT/REMOVE ANY OTHER TEXT. Click Yes >> OK.
D. Connect your computer to the machine using a USB cable.
E. Power up your machine’s control box. If you have the laser attachment, be careful not to plug the machine’s power supply into the laser’s female barrel plug receptacle. Doing so may destroy the laser.
F. On Windows 10 computers, the drivers for the control board should automatically load onto your computer. If you have another operating system or if they do not autoload, you might need to install the Arduino IDE linked here to get the drivers that you need. Then use device manager to point to the appropriate drivers.
G. You should now be able to establish a connection between UGS and the control board.
a. Select GRBL as the firmware.
b. Use the Port drop-down menu and select the port that you see available.
c. Select a baud rate of 115200.
d. Click the Connect / Disconnect icon or on the tool bar Machine >> Connect. The connection icon will turn from disconnected/black to connected/orange. The machine will tell you that it has been connected in the console window
.
H. Movement
a. Click on the commands tab at the top and type in $X then press enter.
This will unlock the machine to allow motion commands.
b. If you have homing switches, you can type $H then press enter. This will initiate a homing cycle. On a homing cycle, the Z axis will lift first. It will raise Z, hit the switch, back off, move very slowly into the switch again, and then pull off the switch a few millimeters. Afterwards, the X and Y motors will begin simultaneously moving the machine towards the switches (switches are in the positive direction) until those switches are engaged. It will do the same pull off, switch reengage, then slight pull off on each one of those axes. After a homing cycle, the machine is unlocked for additional motion commands. The advantage of homing is that the machine will obtain a known position which will allow you to utilize work position systems, which will be discussed later.
c. Go to the Console tab and type G21 into the command line and hit enter. This tells the machine you will be issuing movement commands where the units are in millimeters. Now you can jog the machine. Jogging means the machine is just being moved around to get it into position, such as to get it into place for a cutting operation.
d. Click on the Jog Control tab. You can use the axis control buttons to move the machine around. The X- button will move the router to the left; X+ will move the router to the right. Y+ will bring the table towards the front of the machine; Y- will move the table towards the back. Z+ will move the router up; Z- will move the router down. Be mindful of the step size. Since you set a G21, the step size figure is the millimeters that it will move when you press an axis button. It is possible to move the machine too far and crash it, so be careful. If you just homed the machine, you need to first move X-, Y-, and Z- because each axis is homed towards the positive side of travel. This is the conventional home direction for CNC routers.
2. Basic GCode Commands
a. In addition to using the axis control buttons, you can type in G code commands into the command line. Let us cover some basic G codes now.
b. G0 Rapid movement at the default feed rate (feed rate is how fast it moves) G0 movements are just for getting around. You do not cut anything with a G0.
c. G1 Linear movement at the specific cutting feed rate.
d. G2 Clockwise arc movement at the specific cutting feed rate.
e. G3 Counter-clockwise arc movement at the specific cutting feed rate.
• G2 and G3 movements are accompanied by X, Y, or Z, and I, J, or K “words” to tell the machine how exactly to arc. You do not need to understand any of that right now because the CAM software (the program that makes your g code for cutting stuff out) will do all of that for you.
f. G20 Sets units to inches
g. G21 Sets units to millimeters
• Since these commands are “modal”, it remembers that you set it (while the controller is on!) and will not be changed until you issue the opposite command. If your CAM software generated G code in millimeters, you need to set a G21, and vice versa.
h. G90 Specifies absolute positioning
i. G91 Specifies incremental positioning
• G90 and G91 are modal commands as well. This is best understood by way of example. Let us say you were at X50 and then issued the command G0 X60. Where would it move? It depends. If you had a G90 set for absolute positioning, it would move 10 to the right. If you had a G91 set for incremental positioning, it would move 60 to the right. See the difference? Now let us say you were at X50 and issued the command G0 X0. Where would it move? If you had G90 set, it would move 50 to the left to take the machine to the position of X0. If you had a G91 set, it would not move it all. G91 is incremental, so 0 from where you are at is… well, where you are at. Be advised that using the axis control buttons under the Machine Control tab in UGS will set a G91. It does this every time you click one of the axis control buttons.
j. G92 Used to create a temporary work coordinate system. This is most often used to zero out each axis so you can declare the origin of your work. For instance, you might jog the machine to where you want to start the work, setting the cutting tool to the point you want to start the cutting file. For instance, G92 X0 Y0 Z0 will set the “work coordinate system” to zero for each axis. Many cutting files use X0 Y0 Z0 as the origin, so this is the position you will most often want to set before starting a file.
k. F Specifies the feed rate for G01, G02, and G03 moves. The F command must be used with a number. F 1000 or F200.0 for example.
l. S Specifies the spindle speed or laser intensity. The S command must be used with a number. S6000 or S 120000.0 for example. On machines shipped assembled with a laser installed, S12000 is the maximum value, with S3500 being about the minimum value that will come on after an M3 command.
m. M3 Turns on the spindle or laser (only if a spindle is configured for control by enable pin). An S command alone will not turn on the laser or spindle. An M3 will allow it to turn on.
n. M5 Turns off the spindle or laser (only if a spindle is configured for control by enable pin).
3. BITS/CUTTERS/MILLS
a. Bits are also referred to as a CUTTER or a MILL. Note that you will see cutter in CNC software and when you look at a list of cutters to choose from, they all end in MILL. When searching Amazon for home shop systems, ‘CNC bits’ will surface more relevant results for home shop systems than ‘CNC cutters’ or ‘CNC mills’.
b. In the home shop, CNC bits are often interchangeable with router bits. Smaller home shop systems are limited to 1/8 inch and 1/4-inch shank bits. Some higher end home shop systems can accommodate 1/2-inch shank bits.
c. Non-standard shank sizes can be accommodated if your router or spindle has an ER collet. ER collets have a wide clamping range and high accuracy. With a full set of ER collets you can hold any diameter that is in the clamping range of the set.
d. Terminology
• HOLDER: The collet is the ‘holder’. Holder is the term used by commercial systems and is found in CNC related software. Holder dimensions are needed to avoid collisions.
• ROTATION DIRECTION: Clockwise (CW) direction is what you find for most tools such as drills, routers, lathes, etc.
• FLUTE: The cutting edge and corresponding “trough”. Most home shop systems will use bits with between one and four flutes. More flutes are not necessarily better. More on this later.
• MATERIAL: Bits are usually made with High Strength Steel (HSS) or Carbide. If the cutting edge is carbide, then enter carbide in the software.
• GEOMETRY: The bit’s dimensions. If you can, measure your bits with digital calipers. Geometry terms software dependent, but most use shaft diameter, cutter diameter, cutter shape, overall length, cutter length, stick-out length, etc.
• COATING: Some software will ask about coatings used to reduce friction.
• CHIPS: The material removed by the bit.
• CHIP EVACUATION: The process of removing or evacuating the chips from the cut.
• CHIP LOAD: The amount of material removed by each cutting edge. Feed speed, cut depth, number of flutes and RPM determine the chip load. Other factors include the use of compressed air to clear the cut, cutting fluids, up-spiral, down-spiral, and straight flutes. Too much chip load results in chatter, rough finishes and broken bits. Too little results in heat which can burn the material and weaken the bit.
• DEFLECTION: Bit bending due to load. Deflection is bad for both the bit and the cut quality. A shorter stick-out length will reduce deflection.
e. Common Profiles (types)
• BALL END: The tip is fully radiused leading to vertical sides.
• BULL NOSED: The tip is partially radiused leading to vertical sides.
• CHAMPHER: Angled cutters for removing the edge from a corner.
• DOVETAIL: Flat bottomed cutters with inward angles side cutters.
• FACE: Flat bottomed cutters with relatively short 90-degree side cutters.
• FLAT END: Flat bottom with vertical sides.
• FORM: Used for side profiles with any shape possible.
• LOLLIPOP: Spherical end mill used to make undercuts and access hard-to-reach places. They are used in a variety of applications, including plunge, face, profile and tracer milling.
• TAPPERED: As the name implies, the sides are tapered. The tip can be pointed, radiused or flat. Also referred to a V-bit when the tip is pointed.
• THREADED: Used for cutting threads.
• Both ball and bull nose cutters are often used for 3D operations during finishing passes. Flat cutters are your most common cutters and will be used for everything from 2D to 3D (during roughing operations).
f. Flutes
• Most CNC bits have helical flutes. A helical flute allows the edge to gradually ramp up its engagement on the material unlike a straight flute where the edge engages all at once. Straight flutes are generally less expensive and are perfectly fine for wood and plastics as evidenced by the extensive use with wood routers. Do not try a straight fluted cutter on metals unless you know exactly what you are doing. If production is a concern, note that a spiral fluted cutter can cut about three times faster and will leave a better finish.
• There are four basic flute types.
1. STRAIGHT: The flutes run straight up and down.
2. UP-CUT: The flutes spiral in a direction that pull the chips towards the holder, same as a drill. UP-CUT flutes are good at evacuating chips from the cut. Because the cutters pull up towards the surface of the material, there will often be tear out on the top edge of the cut. UP-CUT flutes also pull the material up from the table which can be a problem for thin or flexible materials.
3. DOWN-CUT: The cutters spiral in the opposite direction of UP-CUT flutes. Not generally used for CNC milling since they push the chips in to the cut unless the top finished edge is a concern. It is best to use compressed air system or fluids to remove chips. As noted above, UP-CUT flutes can pull flexible materials up from the table. DOWN-CUT flutes work well with thin, flexible materials where chip evacuation is less of a problem. Also good for inlays and shallow pockets. While these DOWN-CUT flutes will leave the best finish at the top edge of the cut, they will cause tear out at the bottom of the cut (less if the bottom of material is in contact with a spoil board).
4. COMPRESSION: These are a combination of up-cut and down-cut cutters. This will leave the best surface finish on both sides of the piece. The top half of the cutter is a down-cut while the bottom half is an up-cut. Again, it is helpful to have compressed air or fluid to evacuate chips from the cut when it starts getting deep. These cutters are generally only used for edge contours where material thickness is within the limits of a single pass.
• Flute count.
1. For home shop systems, available bits will likely have between one and four flutes. Less flutes equals bigger gullets which results in better chip clearing. Bits with more flutes will have shallower gullets, which results in a thicker core and a stronger bit. More flutes will produce a smoother finish but will generate more heat. More flutes will also allow higher feed rates, assuming chip evacuation is sufficient. The result is that spindles, because they operate a lower RPMs, can benefit from more flutes, while routers, because they operate at higher RPMs, generally work better with fewer.
2. The cutting operation type will also play a roll. Slotting and plunging cuts do not leave much room for chip evacuation, while side cuts and pocket clearing, three-dimensional paths are more forgiving.
g. Calculating RPM and Feed Rate
• The goal is to optimize the CHIP LOAD. The formula for Chip Load is:
Feed Rate / (RPM x Flute Count), where Feed Rate is inches per minute
• The typical Chip Load is typically hundredths or thousandths of an inch. You can find many cutter manufacturers sites that will provide Chip Load for their bits. You may be able to find one that is similar to the bit you are using. One such site is www.harveytool.com/cms/GeneralMachiningGuidelines_17.aspx
• There are free feed rate calculators available and Fusion 360 has built-in feeds and speeds for various cutters. Those are generally going to be conservative and might be good enough. If you want to optimize your feeds and speeds, you should consider spending a few dollars on G-Wizard. If your system is under three horsepower, which if you are reading this it almost certainly is, then the cost is under $100 for a lifetime license. It will likely pay for itself in bits very quickly. It is available here: www.cnccookbook.com/g-wizard-cnc-speeds-and-feeds-calculator/
• When performing multiple milling operations on a part, for each bit use the most difficult path for calculations. This will likely be a slotting or deep pocket clearing operation.
• The depth of cut should not exceed the bit’s diameter and the overlap between passes, called STEP OVER, generally should not exceed 40% of the bit’s diameter. Too little and there is a risk of burning the material and overheating the bit, too much and the bit may not be able to evacuate the chips and the bit may fail. Smaller step over passes will result in a smoother finish. Longer bits should have smaller step overs to avoid deflection.
• Other considerations include the rigidity of the system, i.e., belts vs lead screws, the material, MDF vs Aluminum, spindle vs router, etc.
h. Operations
• There are a few basic milling operations: Hole, Pocket, 2D Profile, 3D Surface and Facing. In all cases, tool entry is especially important. There are three options: Plunge, Predrill and Helix Ramp. Plunge should almost never be used unless there is no other way as it is hard on the bit. Instead use Predrill, but this will require a bit change. Helix ramp is usually the best option. Ramp feed speed can be slower but be careful not to make it too slow. RPM can also be adjusted if using a speed-controlled spindle.
4. Work Coordinate Systems
Note that this part is a bit advanced. Most will not understand this until they have some experience. You can keep running things using the G92 method described above until you get ready for this. Programmed work coordinate systems can only be used if you have homing switches. This allows you to move the machined to predetermined starting positions even after powering off the machine. This is especially useful if you have a clamping fixture and wish to run the same operation over and over, or if you wish to machine a part with two or more different tools.
a. Work coordinate systems are designated with G10 commands and accessed using the G54 through G59 commands. Let us cover the basics of the commands:
G10 L20 P1 X0 Y0 Z0 Sets the current position of the machine as the origin (0,0,0) point of the G54 coordinate system.
G10 L20 P2 X0 Y0 Z0 Sets the current position of the machine as the origin (0,0,0) point of the G55 coordinate system.
G10 L20 P3 X0 Y0 Z0 Sets the current position of the machine as the origin (0,0,0) point of the G56 coordinate system.
Do you see the pattern? P4 is for G57, P5 for G58, and P6 for G59.
There is another way to set work positions, but this is perhaps the most easily understood.
G54 Modal Interpret all further absolute positioning commands (those commands issued when a G90 is set) as places to go in the G54 system.
G55 Modal Interpret all further absolute positioning commands (those commands issued when a G90 is set) as places to go in the G55 system.
G56, G57, G58, and G59 are set the same way. You can tell where the origins of these work coordinate systems are relative to the origins of the machine coordinate system by typing $# into the command line.
G53 G53 Specifies the machine coordinate system for the motion command that follows on the same line. This is a “non-modal” command, so any further commands issued without a G53 on the same line will be interpreted within the context of the work coordinate system.
Let us look at a real-world example. Imagine that you wish to do a 3D carving that will first be roughed (material removed in bulk close to the finished contour) with an end mill and then finished with a ball nose mill. After you lay your board on the machine table and clamp it, you might have a particular point on the board that you wish to begin your work (possibly at the bottom left corner). You could jog the machine to that location then establish that point as the G56 work coordinate origin by typing G10 L20 P3 X0 Y0 Z0. You would type G56 and then run the roughing operation and change the cutting tool to a ball nose end mill. You would then home the machine again and type in G56 X0 Y0. Notice that you did not issue a Z0. The ball nose tool you installed will almost certainly be sticking out more or less than the end mill you used, so you will not want to command the machine to Z0 before resetting it. Jog the Z down to the stock top. You can either issue a G92 Z0 or reset the Z origin for this coordinate system using G10 L20 P3 Z0. Keep in mind, we are using “P3” because in this example we are setting the G56 coordination system.
5. Touch-plate Set Up
a. There are two kinds of touch plates, the first is just to set the Z axis height. The other locates the work piece edges in all three dimensions and can also be used for just Z axis height. The cost is about the same, so go with the edge finder.
b. UGS Platform has a probe module available as a plug-in. The process is straight forward. This YouTube shows how to set it up: www.youtube.com/watch?v=kpz-6x_synE
• Install and open the Probe Module.
• Measure your edge finder and enter the dimensions into the module. A digital caliper works best.
• Place the edge finder on the material to be machined in the same corner used to orientate the tool paths.
• Select a bit, measure the diameter and enter the diameter into the Settings section of the Probe Module.
• Connect the edge finder to the control box and to the bit. When the bit touches the edge finder it will complete the circuit to let the control box know that the bit has reached the edge.
• Jog the machine so the bit is about a 1/4-inch above and over the edge finder about 1/4-inch from the outside edges.
• In UGS, reset the X, Y and Z axis locations to zero.
• In the Probe Module select the XYZ option.
• Set the X and Y probe distances to 15 and the Probe Distance / Direction to -10.
• Click the Measure Outside Corner button.
• Remove the edge finder.
• Zero the location coordinates by entering g0x0y0z0 in the console.
• The bit should now be just about touching the corner of the work piece.
6. Running Your First Job:
a. You might be interested in running a cutting file now. You can run a very basic engraving file using this GCode file that you can download from the link in the original Quick Start Guide. This will require a piece of wood about 8 x 8 and between 1/2” inches, and 3/4” inches thick (200mm x 200mm and 13mm to 19mm thick). A larger piece is okay. Recommend using something soft like MDF or Pine.
b. Put the cutting tool in the router. This file was designed for a 1/4” (6mm) core box router bit, but an end mill, ball nose, or V bit in a size 1/4” or under will work as well.
c. Place the board on the table and clamp it down. Keep the clamps towards the edges so the cutting tool will not collide with them.
d. We will now set a G92 X0 Y0 Z0. To do this, jog the machine towards the lower left side of the board (X and Y position). After jogging to the desired X and Y position, start lowering the cutting tool towards the board. Be mindful of your step size here. Once the tool gets close to the board, change the step size to 0.1mm and keep dropping it. Place a sheet of notebook paper underneath the cutting tool and on top of the board. Slide the paper back and forth to see if it catches on the cutting tool. Keep lowering the Z axis until it just barely drags on the paper. At this point, issue the G92 X0 Y0 Z0 command.
e. Change the step size back to millimeters. Now, issue a G90 G0 Z5 command to lift the Z axis above the stock. Assuming you had a G21 (millimeters) set, this will raise the Z axis 5 mm. This is because it is best to turn the router on when it is not engaged with the stock.
f. The program will move the machine about 6.5 inches (165mm) in the Y+ directions and 7.5 inches (190mm) in the X+ direction. Watch to make sure the bit does not collide with your clamps.
g. Now load the GCode file you just downloaded by clicking on the File >> Open GCode File… then browse and select the file. You should see the milling path displayed in the Visualizer.
h. You are now ready for a simulation run.
• Remove the board but leave the clamps in place.
• Click Machine >> Send in the menu bar or click the Play icon in the tool bar.
• Stay clear and do not reach into the cutting area under any circumstances. Be prepared to click the Stop icon or cut the power in case something goes wrong.
• The machine should move the router around for about 4 and half minutes.
i. Assuming everything performed as expected, you are now ready for your first machining operation. If the bit hit your clamps or the router went to areas not where your board would be. then go back and check the system and settings.
• Turn on the router and click Machine >> Send in the menu bar or click the Play icon in the tool bar.
• Stay clear and do not reach into the cutting area under any circumstances. Be prepared to click the Stop icon or cut the power in case something goes wrong.
• After about 4 and half minutes you will end up with a board with Mill Right CNC inscribed on the surface.
7. Designing your own parts
You will need to use some other software to design your own parts and make g code for them. MillRight does not officially support software, but basic tutorials for Autodesk Fusion 360 and Inscape are on the MillRight CNC Resources Page. These software packages are free. You will need to get a hobby or free small business license from Autodesk for Fusion 360, as appropriate. Do a google search to download these programs.
8. Troubleshooting
P: Universal G Code Sender gives an error when trying to open a connection, or the machine has stopped responding.
S: Close UGS, remove USB cable from USB port, wait five seconds, plug back in, open UGS, and attempt to open a connection.
P: The motors make a noise that sounds like radio static.
S: This is normal when the machine is first booted up and no motion commands have been issued.
P: The machine is not moving to the commanded position.
S: Most often this happens when incremental positioning is set (G91) but the user thinks the machine is in absolute positioning (G90). Set the appropriate mode.
P: The machine appears to be missing steps or not moving the full distance commanded on one axis.
S: The set screws should be checked on the motor pulley and tightened if loose. If this is not an issue, the belt may need to be tightened. Also, the voltage should be checked on the stepper motor driver to ensure that it is around 0.60 volts.
P: Files are running erratically, or commands are being skipped with a warning that the command length is too long. Confirm that the line length maximum is set to 70 in UGS. Also confirm that S: your CAM software is not using more than four decimal places for a position command.
P: The motor stalls or the machine jumps off the planned path when cutting. Solution: Slow down the feed rate and/or shallow up the cut.
S: The machine stops during homing before it hits the homing switch. Separate motor wires from switch wires to reduce electromagnetic noise creating a false trigger.
