CNC BEGINNER GUIDE MUST READ.
Mar 23, 2017 15:44:08 GMT
mp4doggie, markwisniowski, and 12 more like this
Post by aforww on Mar 23, 2017 15:44:08 GMT
Well finally got it done, edited for the most part and ready for consumption. Thanks to Derek for helping out. I'll post the whole thing here and also I've attached a PDF that seems to want to show up at the bottom of the post for some reason.
The purpose of this thread is to address the most common questions and concerns that seem to come up in the forums from folks just starting out in the CNC world. This isn’t an attempt to cover everything as that would take pages upon pages to do. What it should do is lay a solid foundation for things you should know getting started and get you going in a direction to research further. You will see me reference things from Fusion 360 because that is what I use for my CAD and CAM.
For the purpose of this post:
“CUTTER” will refer to the end mill.
“SPINDLE” will refer to either the spindle kit or a router unless the need to differentiate presents itself.
The spindle kit operates at a much lower speed range and doesn’t have nearly the torque. They are very quiet in comparison. They also usually offer a more precise level of speed control and are more easily integrated into the milling process when it comes to having your software turn on and adjust spindle speed. Many people find that the spindle kits suit their needs when milling is mostly done in woods and plastics.
The next thing I want to cover is end mills. AKA “CUTTERS” or “BITS” and the correlation with your choice of spindle. In the hobbyist CNC world, you will have two basic sizes of cutters. 1/4 and 1/8 inch. This identifies the shank (part of the cutter that goes into the spindle) size. The portion of the spindle that holds the cutter is called the “COLLET” and the nut that tightens it all up is the “COLLET NUT”. If you are using a router, odds are you are going to have a 1/4 inch collet. If you are using the spindle kit you will have a 1/8 inch collet.
Now, just because you have either of these doesn’t mean you are locked into the corresponding size of cutter. There are both reducers/collets for routers that allow the use of a 1/8 inch tool and there are collets available for the spindle kit that allow the 1/4 tools. I won’t go into all the different styles as there are many. If you see “ER style, ER11, ER32” this is simply a style of the collet that works as a system. I recommend checking out www.elairecorp.com for router collets.
TOOL GEOMETRY
Often refers to the angle, length, diameter, and direction of the flutes. Of these, you really need to pay attention to cutter diameter. A cutter sold as 3mm, for example, may be 2.93mm. If tight tolerances and accuracy in cuts are in your game, you may want to buy a set of digital calipers and determine the ACTUAL diameter of all your cutters.
MATERIAL
The material the cutter is made from. The most common are HSS (High-Speed Steel) and carbide.
COATED
Some tools are coated for improved machining properties in certain materials.
CHIPS
The material removed by the cutter.
CHIP EVACUATION
The ability of the cutter to remove or evacuate the chips from the material.
CHIP LOAD
The amount of material a cutter will remove for each cutting edge. Too much and you are pushing the tool and the machine to the breaking point. Too little, and you end up just rubbing along the edge and creating TONS of heat. Heat is our enemy and you will see it mentioned often.
Keeping track of cutter types can seem complicated. Every material you cut will benefit from choosing the appropriate cutter. We’ll address them first by the cutter tip profile.
BALL (NOSE) MILL
These cutters will either resemble a ball or the cutter tip will be fully radiused. The cut profile will be a rounded bottom leading to vertical side walls.
FLAT / FISHTAIL
These cutters have a flat or fishtail tip. The cut profile will be flat bottomed with the sides intersecting at a 90-degree corner.
BULL/ROUND NOSE
The cutters have a flat end profile but unlike the flat cutters, the sides meet the tip with a small radius and not a sharp corner.
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).
Cutters can also be categorized by flute type:
Straight
The flutes run straight up and down. These types leave a decent finish on the top surface but are not efficient at evacuating chips from the material. This is an issue in deep cuts. The cutters are also less efficient at actually cutting since they are basically “chopping” at the material.
Up-Cut
These cutters have flutes that spiral in a direction that cut in an upward direction. They are extremely good at evacuating ships from the cut. Because they cut at an upward angle, the cutting is much more efficient as it “shears” away material. Compared to straight flutes, this allows for faster cutting and reduced heating of material and cutter. The downside is because the cutter cuts up, the surface of the material will often have to be torn upwards or you will have tiny pieces known as “fuzzies” or “tearout” on the top edge of the cut.
DOWN-CUT
These cutters work exactly like Up-cut cutters just in the opposite direction. These cutters cut down and thus push chips down into the cut. It is extremely helpful if you have a compressed air system in place to blow chips from the slot. These cutters will leave the best finish at the top edge of the cut but will tend to have the same effects of the up-cut at the bottom of the cut.
COMBINATION CUTTERS (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’s helpful to have compressed air to evacuate chips from the cut when it starts getting deep. These cutters are not common and can be expensive. I don’t think they have a practical use with the M3. To get the desired effect with a compression, you need to essentially be making full depth cuts.
Now that you are familiar with the profile, and flute type, we will cover the number of flutes a cutter has. This is a topic that tends to end up very subjective. The number of flutes your cutter has will affect your milling speed, and surface finish of the cut. The most common you will find will be single flute through four flutes. You can find cutters up to ten flutes. The thing to understand is that more flutes do not always equal better milling. We will cover it more in “feeds and speeds” but the bottom line is, the more flutes you have, the less area there is for the chips to go to be evacuated from the material. It also means that there are more surfaces in contact with the material in a given time. This translates into more heat being built up. However, when your spindle speed is limited to a low range of speed, more flutes will increase the speed at which you can mill. I can only suggest, for doing things that are sensitive to heat like plastics and aluminum, use a single flute cutter or a two flute for aluminum if you are using a router. This is especially true if you are doing plunge cuts or cuts where the cutter will be cutting through material opposed to cutting along an edge. It is a tad slower but it produces less heat and evacuates chips aggressively. If you are milling along the edge of stock you can get away with having more flutes and worry less about chip evacuation as the cutter is only working on one side. Again, we’ll cover this more in Feeds and speeds. For the vast majority of your milling needs, you will only need single and two flute cutters.
SPEEDS
The speed in which your spindle is turning. RPM. This affects surface speed.
FEED
The speed at which you are milling. Inches/millimeters per minute.
SURFACE SPEED
This is the speed at which the tool is moving across the material. Feet/meters per minute. This is not the same thing as feed. This is usually a manufacturer recommendation specific to the tool.
CHIP LOAD
We defined this earlier. Manufacturers will generally give a suggested chip load for individual cutters for different material types. Chip load is basically the target factor in setting up your feeds and speeds. This is generally indicated in hundredths or thousandths of an inch. So, .01 or .001 per flute for example.
Chipload in inches = Feedrate in Inches Per Minute / (Cutting RPM x Number of Flutes)
NUMBER OF FLUTES
As I mentioned earlier, the number of flutes directly influences your speeds and feeds. As all things come down to chip load per flute.
DEPTH OF CUT (DOC)
Also known as “STEP DOWN”. The depth the cutter cuts into the material with each pass. I generally try to keep my maximum step down less than the diameter of the cutter I am using.
STEP OVER
The distance the bit will travel to make a cut wider. Imagine you are cutting a slot that is 4mm wide using a tool that is 1mm in diameter. Obviously, that cutter is going to have to advance in/out with each pass. The distance moved is step over. The step over will never be larger than the diameter of the tool itself. I recommend keeping your step over to around 40% of the bit diameter. The larger the step over, the faster the operation but the crappier the finish at the bottom of the cut and the more pressure you introduce into the tool. Less step over is slower but leaves a better finish on the bottom. The smaller the step over, the more time it takes however, there will be less “waviness” to the surface. This really is only important to operations that don’t cut all the way through the material. Step over also comes into play when you do a finishing pass on a profile cut as you can define a small step over at full depth with a faster feed rate to smooth the edge surface. The length of the tool also comes into play as the longer it gets, the more it wants to deflect during big step overs.
There is an art to speeds and feeds. What works on one milling machine may not work on another to rigidity, type of drives (belt vs lead screws), and milling conditions. Proper feeds and speeds have two goals. Cut at the tools optimal rate, and keep heat in the chips and not in the workpiece.
I won’t get deep into the math here as it tends to get complicated and there are a plethora of “Speeds and Feeds” calculators available. But RPM is dependent on recommended surface speed, chip load, and depth of cut. RPM = (3.82 x Surface Feet per Minute) / tool diameter
Once you have your necessary RPM, you will figure your feed rate. This is accomplished by using
Feed Rate = RPM x Number of Flutes x Desired Chip Load.
Your best bet, use resources to do all this for you. There are plenty of free ones. For my desired chip load, I usually refer to this site: www.harveytool.com/cms/GeneralMachiningGuidelines_17.aspx This is where I start and may or may not adjust from here. I recommend you browse their site, find tools that are similar in geometry to the tools you are using and use the chip load charts for that tool. If you are buying upper end tools from companies like Dayton, Kyocera, Destiny, then use their recommended parameters.
Once I know my desired chip load for the material I’m working with, I will use the calculator located here: www.daycounter.com/Calculators/GCode/Feed-Rate-Calculator.phtml I will use this calculator and adjust parameters as I need to, to match the speed in which my spindle will operate, and to adjust for how long a job will take.
There is also a very good and comprehensive program called G-wizard which will cost you some money but is very good at figuring out just about every aspect of this whole process.
Now that we have an idea of how we find our feeds and speeds, let’s talk about how we actually cut stuff. The last thing you want to do is take a cutter and plow it into material trying to cut out a 1/2 inch of material in one shot. You will also see that I recommend having compressed air to evacuate chips on more than one occasion. Sometimes it’s necessary, sometimes it’s just beneficial. Personally, I rely on it for most things. My reasonings are:
1. It keeps the tool cooler. This extends tool life.
2. It keeps chips from being recut. This extends tool life and keeps things from gumming up in plastics and aluminum.
3. It keeps chips from being rubbed against your cut surface which will degrade it’s finish effectively “burnishing” the edges.
This all really only comes into play when you are cutting deep grooves/pockets where the chips can not effectively be managed by the cutter and spindle alone. Use your judgment on this and pay attention to what your machine is telling you and you should be just fine either way.
PLUNGE
This type of entry is exactly as it sounds. The cutter will plunge into the material to a depth you set (usually referred to as a maximum step down) and then proceed along the path. Once it completes the path, it will plunge down that depth again for another pass. This works well when you are doing things where you want to keep a constant load on the cutter.
RAMP
Ramping does exactly as it sounds. It begins above the material following the cutting path and gradually ramping down as it makes its passes. This is usually the best method for harder materials and definitely a good method to use as you learn because there is less risk of catastrophe.
Keep in mind, not all CAD/CAM programs will allow for this. Easel, for example, does not allow ramping operations. It will only allow you to plunge.
So, how does material play into all of this? Well, certain materials like plastics and aluminum have characteristics that will cause you a ton of heartache. As we have mentioned previously, heat is our enemy. It causes wear on the cutters and can create some sticky situations in plastics. Getting rid of heat in the material and tool is a major goal. Plastics will gum up and stick to the cutter real quick if you aren’t moving material fast enough. The same with aluminum. It also causes work hardening of some metals like copper. Wood is pretty forgiving when it comes to feeds and speeds, plastics are not. IF you are using a spindle kit with lower RPM then you are going to have slower feed rates. Try those same feed rates with a router spinning at 15k and you are going to melt the plastic quicker than it can cut it. We want to err on the side of caution and mill slowly but that can be a quick end to your project.
I covered chip load previously. However, I want to cover it again. Chip load is critical. The heat that is building between the tool and the material is removed in the chips. You want to get rid of as much material as efficiently as you can. If your chip load is too small, you will not be removing enough material to get rid of heat. If it’s too much you will be asking a great deal from your machine mechanically. The more rigid the machine, the more you can take off at once. The shorter and thicker the cutter, the more you can take off at once. Use the resources I provided as a starting point.
Lastly, most CAM programs can calculate these things for you. Fusion360, for example, has literally everything I’ve mentioned in the options when you are picking the cutter for your operation. Pay attention to the numbers that are in there and how they change when you input your variables. As a side note for Fusion users, Measure and add your tools to the tool library instead of using the preloaded library. It requires some learning but in the end, you will thank me. Easel uses what inventables thinks you should use based on THEIR tools. If you are using something other than their tools, your results are not going to be optimal.
Speeds and feeds is a tricky thing to figure out. And this isn’t even getting into things like adaptive clearing and parallel tool paths! With the information I’ve given you, you should be able to get on the right track, though. Do not feel overwhelmed by it all. It’s taken me the better part of a year to wrap my brain around all of this in a way that I know exactly how I want to approach certain operations in certain materials. It’s a ton of information to take in. I recommend printing out the charts I mentioned earlier so that you have them readily available when it comes time. This I also why I recommend Fusion 360 so much. It’s a pain to learn because there’s so much to it. However, it’s calculations for speeds and feeds is dead on to every calculator I’ve tried.
G0 Rapid movement at the default feed rate (feed rate is how fast it moves)
G0 movements are just for getting around. You don’t cut anything with a G0.
G1 Linear movement at the specific cutting feed rate.
G2 Clockwise arc movement at the specific cutting feed rate.
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.
G20 Sets units to inches
G21 Sets units to millimeters
Since these commands are “modal”, it remembers that you set it (while the controller is on!) and won’t 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.
G90 Specifies absolute positioning
G91 Specifies incremental positioning
G90 and G91 are modal commands as well. This is best understood by way of example. Let’s 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’s 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 wouldn’t 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.
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.
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.
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.
M3 Turns on the spindle or laser. (Only if a spindle is configured for control by enable pin) An S command alone won’t turn on the laser or spindle. An M3 will allow it to actually turn on.
M5 Turns off the spindle or laser. (Only if a spindle is configured for control by enable pin)
If you have a machine with homing switches and you fire it up and push the $H button in UGS, it will send the machine to the back right corner, and the Z axis up until it trips the limit switches. It then backs off from that point 4mm. This is your MACHINE ZERO. This is the known point all other coordinates will originate from. This is the machines known point of reference and is irrelevant in the design phase.
Now, when you slap your slab of material down, we’ll use a square for simplicity, you still have to tell the machine where to start your operation from. This is where your design comes in and will be referred to as WORK ZERO. When you are designing your part and begin to build your cut operations, you will generally have an option of where you want the machine to reference on your part. In Easel for example, if you look at the lower left corner of the grid, you will see a black dot. That is where the work zero is set to. That means if you are using square material then you should jog the machine to the lower left corner of the stock and zero to there. This tells the machine that “this is where the 0 point of my design is”. That being said, it’s imperative that your work zero point in your design is transferred to the workpiece whether it be one of the corners or the center. I tend to use the lower left corner for everything unless I am using irregular shaped material at which point I change the work zero location to the center in my design. This allows to me to set my work zero on the machine to the center of the material. So, machine zero is home. Work zero is the reference point for your design transferred to the material.
On a side note for Easel users. If you want to set your work zero to the center of your design, click on the “shape tab” of the floating box that is there when you are editing your design. You will see a series of five dots like on dice. Click the center dot and change the X and Y values to 0. You will see your design move and will appear both on and off the design area with that black dot on the grid in the center of your design. Don’t worry, it will still cut all the stuff outside of the grid.
Units. Do not design in inches, then send g-code to a machine that is in millimeters. Obviously, things are going to go awry. Make sure your machine, G-code, and design are all using the same unit of measure.
Here’s the nitty gritty detail on WCS. It seems confusing the first ten times you look at it, but if you don’t get to the point you understand the below then you are leaving a lot of capability on the table. 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.
Let’s cover the basics here. Work coordinate systems are designated with G10 commands and accessed using the G54 through G59 commands.
Let’s cover the basics of the commands:
G10 L20 P1 X0 Y0 Z0 This command would designate the current position of the machine as the origin (0,0,0) point of the G54 coordinate system.
G10 L20 P2 X0 Y0 Z0 This command would designate the current position of the machine as the origin (0,0,0) point of the G55 coordinate system.
G10 L20 P3 X0 Y0 Z0 This command would designate the current position of the machine as the origin (0,0,0) point of the G56 coordinate system.
See the pattern? P4 would be 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 command that tells the machine that it should interpret all further absolute positioning commands (those commands issued when a G90 is set) as places to go in the G54 system.
G55 Modal command that tells the machine that it should 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 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’s give 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 didn’t 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.
There’s no way I can address all the possible problems you are going to run into. I can, however, address the ones we see most often.
● The machine seems to cut things in the wrong direction or appear to be mirrored along one axis.
o Check your motor connections. Are they wired up correctly? When you push X+ in UGS does the spindle move left? If so, that's opposite of what it should be. When you push y+ does the table move towards the back? If so, that's also opposite of what it should be. The X plate should move to the RIGHT when you press X+ and the table should move to the front when you press Y+.
o Some steppers drivers have been found to have inverted direction logic. This means that even if you plugged it in according the the directions it might be traveling opposite what you expect. If that happens, power EVERYTHING down, including unplugging the board from the computer’s USB, waiting 10 seconds, and flip the plug the other way on the offending axis.
● Lines don’t appear to be straight or circles aren’t perfectly round.
o This is likely to be caused by three different issues. Either the table is not square to the X and Y axis, the spindle is not plumb, or there is slop in the movement somewhere. Check for square along both the X and Y axis. Check that all belts are tight. They should sound like a stretched rubber band does when you pluck it. Make sure that there is no side to side motion in the table. If there is, adjust the eccentric nuts to tighten the wheels to the rails. The same applies to the Z plate. If you can wiggle it front to back or side to side adjust the tension on the wheels. Next, make sure all the rails are secured tightly.
● The motors make a noise that sounds like radio static.
o This is normal when the machine is first booted up and no motion commands have been issued.
● The machine isn’t moving to the commanded position.
o 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.
● The machine appears to be missing steps or not moving the full distance commanded on one axis in particular.
o 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.
● Files are running erratically or commands are being skipped with a warning that the command length is too long.
o Confirm that the line length maximum is set to 70 in UGS. Also, confirm that your CAM software is not using more than four decimal places for a position command.
● The motor stalls or the machine jumps off the planned path when cutting.
o Slow down the feed rate and/or shallow up the cut.
● Problem: The machine stops during homing before it hits the homing switch.
o Separate motor wires from switch wires to reduce electromagnetic noise creating a false trigger.
BEGINNER REFERENCE GUIDE FOR CNC
The purpose of this thread is to address the most common questions and concerns that seem to come up in the forums from folks just starting out in the CNC world. This isn’t an attempt to cover everything as that would take pages upon pages to do. What it should do is lay a solid foundation for things you should know getting started and get you going in a direction to research further. You will see me reference things from Fusion 360 because that is what I use for my CAD and CAM.
For the purpose of this post:
“CUTTER” will refer to the end mill.
“SPINDLE” will refer to either the spindle kit or a router unless the need to differentiate presents itself.
CUTTERS AND SPINDLES
When it comes to choosing between a spindle kit such as the 400w spindle from MILLRIGHT CNC or a router, the choice really comes down to what you want to do. Routers will have more power. Routers will have a higher range speed, anywhere from 10k on the low end to 30k rpm on the high end. Routers will not require an additional power supply and electronics. Routers, however, will generally be much louder than the spindle kit. They also tend to be heavier. The spindle kit operates at a much lower speed range and doesn’t have nearly the torque. They are very quiet in comparison. They also usually offer a more precise level of speed control and are more easily integrated into the milling process when it comes to having your software turn on and adjust spindle speed. Many people find that the spindle kits suit their needs when milling is mostly done in woods and plastics.
The next thing I want to cover is end mills. AKA “CUTTERS” or “BITS” and the correlation with your choice of spindle. In the hobbyist CNC world, you will have two basic sizes of cutters. 1/4 and 1/8 inch. This identifies the shank (part of the cutter that goes into the spindle) size. The portion of the spindle that holds the cutter is called the “COLLET” and the nut that tightens it all up is the “COLLET NUT”. If you are using a router, odds are you are going to have a 1/4 inch collet. If you are using the spindle kit you will have a 1/8 inch collet.
Now, just because you have either of these doesn’t mean you are locked into the corresponding size of cutter. There are both reducers/collets for routers that allow the use of a 1/8 inch tool and there are collets available for the spindle kit that allow the 1/4 tools. I won’t go into all the different styles as there are many. If you see “ER style, ER11, ER32” this is simply a style of the collet that works as a system. I recommend checking out www.elairecorp.com for router collets.
Some terms and concepts you need to be familiar with when it comes to cutters:
The cutting edge and corresponding “trough”. Imagine a drill bit. This is generally a two flute tool. FLUTE
TOOL GEOMETRY
Often refers to the angle, length, diameter, and direction of the flutes. Of these, you really need to pay attention to cutter diameter. A cutter sold as 3mm, for example, may be 2.93mm. If tight tolerances and accuracy in cuts are in your game, you may want to buy a set of digital calipers and determine the ACTUAL diameter of all your cutters.
MATERIAL
The material the cutter is made from. The most common are HSS (High-Speed Steel) and carbide.
COATED
Some tools are coated for improved machining properties in certain materials.
CHIPS
The material removed by the cutter.
CHIP EVACUATION
The ability of the cutter to remove or evacuate the chips from the material.
CHIP LOAD
The amount of material a cutter will remove for each cutting edge. Too much and you are pushing the tool and the machine to the breaking point. Too little, and you end up just rubbing along the edge and creating TONS of heat. Heat is our enemy and you will see it mentioned often.
Keeping track of cutter types can seem complicated. Every material you cut will benefit from choosing the appropriate cutter. We’ll address them first by the cutter tip profile.
BALL (NOSE) MILL
These cutters will either resemble a ball or the cutter tip will be fully radiused. The cut profile will be a rounded bottom leading to vertical side walls.
FLAT / FISHTAIL
These cutters have a flat or fishtail tip. The cut profile will be flat bottomed with the sides intersecting at a 90-degree corner.
BULL/ROUND NOSE
The cutters have a flat end profile but unlike the flat cutters, the sides meet the tip with a small radius and not a sharp corner.
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).
Cutters can also be categorized by flute type:
Straight
The flutes run straight up and down. These types leave a decent finish on the top surface but are not efficient at evacuating chips from the material. This is an issue in deep cuts. The cutters are also less efficient at actually cutting since they are basically “chopping” at the material.
Up-Cut
These cutters have flutes that spiral in a direction that cut in an upward direction. They are extremely good at evacuating ships from the cut. Because they cut at an upward angle, the cutting is much more efficient as it “shears” away material. Compared to straight flutes, this allows for faster cutting and reduced heating of material and cutter. The downside is because the cutter cuts up, the surface of the material will often have to be torn upwards or you will have tiny pieces known as “fuzzies” or “tearout” on the top edge of the cut.
DOWN-CUT
These cutters work exactly like Up-cut cutters just in the opposite direction. These cutters cut down and thus push chips down into the cut. It is extremely helpful if you have a compressed air system in place to blow chips from the slot. These cutters will leave the best finish at the top edge of the cut but will tend to have the same effects of the up-cut at the bottom of the cut.
COMBINATION CUTTERS (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’s helpful to have compressed air to evacuate chips from the cut when it starts getting deep. These cutters are not common and can be expensive. I don’t think they have a practical use with the M3. To get the desired effect with a compression, you need to essentially be making full depth cuts.
Now that you are familiar with the profile, and flute type, we will cover the number of flutes a cutter has. This is a topic that tends to end up very subjective. The number of flutes your cutter has will affect your milling speed, and surface finish of the cut. The most common you will find will be single flute through four flutes. You can find cutters up to ten flutes. The thing to understand is that more flutes do not always equal better milling. We will cover it more in “feeds and speeds” but the bottom line is, the more flutes you have, the less area there is for the chips to go to be evacuated from the material. It also means that there are more surfaces in contact with the material in a given time. This translates into more heat being built up. However, when your spindle speed is limited to a low range of speed, more flutes will increase the speed at which you can mill. I can only suggest, for doing things that are sensitive to heat like plastics and aluminum, use a single flute cutter or a two flute for aluminum if you are using a router. This is especially true if you are doing plunge cuts or cuts where the cutter will be cutting through material opposed to cutting along an edge. It is a tad slower but it produces less heat and evacuates chips aggressively. If you are milling along the edge of stock you can get away with having more flutes and worry less about chip evacuation as the cutter is only working on one side. Again, we’ll cover this more in Feeds and speeds. For the vast majority of your milling needs, you will only need single and two flute cutters.
SPEEDS, FEEDS, AND MATERIAL
Speeds and feeds. One of the most complicated things to wrap your brain around when it comes to machining. There is literally no hard and fast rule to speeds and feeds so we will focus solely on the basic fundamentals of what it is. These are the factors that go into your speeds and feeds: SPEEDS
The speed in which your spindle is turning. RPM. This affects surface speed.
FEED
The speed at which you are milling. Inches/millimeters per minute.
SURFACE SPEED
This is the speed at which the tool is moving across the material. Feet/meters per minute. This is not the same thing as feed. This is usually a manufacturer recommendation specific to the tool.
CHIP LOAD
We defined this earlier. Manufacturers will generally give a suggested chip load for individual cutters for different material types. Chip load is basically the target factor in setting up your feeds and speeds. This is generally indicated in hundredths or thousandths of an inch. So, .01 or .001 per flute for example.
Chipload in inches = Feedrate in Inches Per Minute / (Cutting RPM x Number of Flutes)
NUMBER OF FLUTES
As I mentioned earlier, the number of flutes directly influences your speeds and feeds. As all things come down to chip load per flute.
DEPTH OF CUT (DOC)
Also known as “STEP DOWN”. The depth the cutter cuts into the material with each pass. I generally try to keep my maximum step down less than the diameter of the cutter I am using.
STEP OVER
The distance the bit will travel to make a cut wider. Imagine you are cutting a slot that is 4mm wide using a tool that is 1mm in diameter. Obviously, that cutter is going to have to advance in/out with each pass. The distance moved is step over. The step over will never be larger than the diameter of the tool itself. I recommend keeping your step over to around 40% of the bit diameter. The larger the step over, the faster the operation but the crappier the finish at the bottom of the cut and the more pressure you introduce into the tool. Less step over is slower but leaves a better finish on the bottom. The smaller the step over, the more time it takes however, there will be less “waviness” to the surface. This really is only important to operations that don’t cut all the way through the material. Step over also comes into play when you do a finishing pass on a profile cut as you can define a small step over at full depth with a faster feed rate to smooth the edge surface. The length of the tool also comes into play as the longer it gets, the more it wants to deflect during big step overs.
There is an art to speeds and feeds. What works on one milling machine may not work on another to rigidity, type of drives (belt vs lead screws), and milling conditions. Proper feeds and speeds have two goals. Cut at the tools optimal rate, and keep heat in the chips and not in the workpiece.
I won’t get deep into the math here as it tends to get complicated and there are a plethora of “Speeds and Feeds” calculators available. But RPM is dependent on recommended surface speed, chip load, and depth of cut. RPM = (3.82 x Surface Feet per Minute) / tool diameter
Once you have your necessary RPM, you will figure your feed rate. This is accomplished by using
Feed Rate = RPM x Number of Flutes x Desired Chip Load.
Your best bet, use resources to do all this for you. There are plenty of free ones. For my desired chip load, I usually refer to this site: www.harveytool.com/cms/GeneralMachiningGuidelines_17.aspx This is where I start and may or may not adjust from here. I recommend you browse their site, find tools that are similar in geometry to the tools you are using and use the chip load charts for that tool. If you are buying upper end tools from companies like Dayton, Kyocera, Destiny, then use their recommended parameters.
Once I know my desired chip load for the material I’m working with, I will use the calculator located here: www.daycounter.com/Calculators/GCode/Feed-Rate-Calculator.phtml I will use this calculator and adjust parameters as I need to, to match the speed in which my spindle will operate, and to adjust for how long a job will take.
There is also a very good and comprehensive program called G-wizard which will cost you some money but is very good at figuring out just about every aspect of this whole process.
Now that we have an idea of how we find our feeds and speeds, let’s talk about how we actually cut stuff. The last thing you want to do is take a cutter and plow it into material trying to cut out a 1/2 inch of material in one shot. You will also see that I recommend having compressed air to evacuate chips on more than one occasion. Sometimes it’s necessary, sometimes it’s just beneficial. Personally, I rely on it for most things. My reasonings are:
1. It keeps the tool cooler. This extends tool life.
2. It keeps chips from being recut. This extends tool life and keeps things from gumming up in plastics and aluminum.
3. It keeps chips from being rubbed against your cut surface which will degrade it’s finish effectively “burnishing” the edges.
This all really only comes into play when you are cutting deep grooves/pockets where the chips can not effectively be managed by the cutter and spindle alone. Use your judgment on this and pay attention to what your machine is telling you and you should be just fine either way.
CUT OPERATIONS
You have two basic options for making a cut:PLUNGE
This type of entry is exactly as it sounds. The cutter will plunge into the material to a depth you set (usually referred to as a maximum step down) and then proceed along the path. Once it completes the path, it will plunge down that depth again for another pass. This works well when you are doing things where you want to keep a constant load on the cutter.
RAMP
Ramping does exactly as it sounds. It begins above the material following the cutting path and gradually ramping down as it makes its passes. This is usually the best method for harder materials and definitely a good method to use as you learn because there is less risk of catastrophe.
Keep in mind, not all CAD/CAM programs will allow for this. Easel, for example, does not allow ramping operations. It will only allow you to plunge.
So, how does material play into all of this? Well, certain materials like plastics and aluminum have characteristics that will cause you a ton of heartache. As we have mentioned previously, heat is our enemy. It causes wear on the cutters and can create some sticky situations in plastics. Getting rid of heat in the material and tool is a major goal. Plastics will gum up and stick to the cutter real quick if you aren’t moving material fast enough. The same with aluminum. It also causes work hardening of some metals like copper. Wood is pretty forgiving when it comes to feeds and speeds, plastics are not. IF you are using a spindle kit with lower RPM then you are going to have slower feed rates. Try those same feed rates with a router spinning at 15k and you are going to melt the plastic quicker than it can cut it. We want to err on the side of caution and mill slowly but that can be a quick end to your project.
I covered chip load previously. However, I want to cover it again. Chip load is critical. The heat that is building between the tool and the material is removed in the chips. You want to get rid of as much material as efficiently as you can. If your chip load is too small, you will not be removing enough material to get rid of heat. If it’s too much you will be asking a great deal from your machine mechanically. The more rigid the machine, the more you can take off at once. The shorter and thicker the cutter, the more you can take off at once. Use the resources I provided as a starting point.
Lastly, most CAM programs can calculate these things for you. Fusion360, for example, has literally everything I’ve mentioned in the options when you are picking the cutter for your operation. Pay attention to the numbers that are in there and how they change when you input your variables. As a side note for Fusion users, Measure and add your tools to the tool library instead of using the preloaded library. It requires some learning but in the end, you will thank me. Easel uses what inventables thinks you should use based on THEIR tools. If you are using something other than their tools, your results are not going to be optimal.
Speeds and feeds is a tricky thing to figure out. And this isn’t even getting into things like adaptive clearing and parallel tool paths! With the information I’ve given you, you should be able to get on the right track, though. Do not feel overwhelmed by it all. It’s taken me the better part of a year to wrap my brain around all of this in a way that I know exactly how I want to approach certain operations in certain materials. It’s a ton of information to take in. I recommend printing out the charts I mentioned earlier so that you have them readily available when it comes time. This I also why I recommend Fusion 360 so much. It’s a pain to learn because there’s so much to it. However, it’s calculations for speeds and feeds is dead on to every calculator I’ve tried.
COMMONLY USED G-CODE
From the quick start guide: G0 Rapid movement at the default feed rate (feed rate is how fast it moves)
G0 movements are just for getting around. You don’t cut anything with a G0.
G1 Linear movement at the specific cutting feed rate.
G2 Clockwise arc movement at the specific cutting feed rate.
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.
G20 Sets units to inches
G21 Sets units to millimeters
Since these commands are “modal”, it remembers that you set it (while the controller is on!) and won’t 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.
G90 Specifies absolute positioning
G91 Specifies incremental positioning
G90 and G91 are modal commands as well. This is best understood by way of example. Let’s 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’s 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 wouldn’t 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.
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.
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.
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.
M3 Turns on the spindle or laser. (Only if a spindle is configured for control by enable pin) An S command alone won’t turn on the laser or spindle. An M3 will allow it to actually turn on.
M5 Turns off the spindle or laser. (Only if a spindle is configured for control by enable pin)
HOMING, WORK COORDINATES/ZERO, AND UNITS
This was by far, the most frustrating thing to deal with when I started out. Mostly because I didn’t realize that this came into play during the initial design phase of things. I’m going to lay this out in layman terms. Understand that there are two main “zero” points you need to worry about. We will call them Machine Zero and Work Zero. If you have a machine with homing switches and you fire it up and push the $H button in UGS, it will send the machine to the back right corner, and the Z axis up until it trips the limit switches. It then backs off from that point 4mm. This is your MACHINE ZERO. This is the known point all other coordinates will originate from. This is the machines known point of reference and is irrelevant in the design phase.
Now, when you slap your slab of material down, we’ll use a square for simplicity, you still have to tell the machine where to start your operation from. This is where your design comes in and will be referred to as WORK ZERO. When you are designing your part and begin to build your cut operations, you will generally have an option of where you want the machine to reference on your part. In Easel for example, if you look at the lower left corner of the grid, you will see a black dot. That is where the work zero is set to. That means if you are using square material then you should jog the machine to the lower left corner of the stock and zero to there. This tells the machine that “this is where the 0 point of my design is”. That being said, it’s imperative that your work zero point in your design is transferred to the workpiece whether it be one of the corners or the center. I tend to use the lower left corner for everything unless I am using irregular shaped material at which point I change the work zero location to the center in my design. This allows to me to set my work zero on the machine to the center of the material. So, machine zero is home. Work zero is the reference point for your design transferred to the material.
On a side note for Easel users. If you want to set your work zero to the center of your design, click on the “shape tab” of the floating box that is there when you are editing your design. You will see a series of five dots like on dice. Click the center dot and change the X and Y values to 0. You will see your design move and will appear both on and off the design area with that black dot on the grid in the center of your design. Don’t worry, it will still cut all the stuff outside of the grid.
Units. Do not design in inches, then send g-code to a machine that is in millimeters. Obviously, things are going to go awry. Make sure your machine, G-code, and design are all using the same unit of measure.
Here’s the nitty gritty detail on WCS. It seems confusing the first ten times you look at it, but if you don’t get to the point you understand the below then you are leaving a lot of capability on the table. 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.
Let’s cover the basics here. Work coordinate systems are designated with G10 commands and accessed using the G54 through G59 commands.
Let’s cover the basics of the commands:
G10 L20 P1 X0 Y0 Z0 This command would designate the current position of the machine as the origin (0,0,0) point of the G54 coordinate system.
G10 L20 P2 X0 Y0 Z0 This command would designate the current position of the machine as the origin (0,0,0) point of the G55 coordinate system.
G10 L20 P3 X0 Y0 Z0 This command would designate the current position of the machine as the origin (0,0,0) point of the G56 coordinate system.
See the pattern? P4 would be 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 command that tells the machine that it should interpret all further absolute positioning commands (those commands issued when a G90 is set) as places to go in the G54 system.
G55 Modal command that tells the machine that it should 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 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’s give 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 didn’t 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.
FREQUENTLY ENCOUNTERED PROBLEMS
● The machine seems to cut things in the wrong direction or appear to be mirrored along one axis.
o Check your motor connections. Are they wired up correctly? When you push X+ in UGS does the spindle move left? If so, that's opposite of what it should be. When you push y+ does the table move towards the back? If so, that's also opposite of what it should be. The X plate should move to the RIGHT when you press X+ and the table should move to the front when you press Y+.
o Some steppers drivers have been found to have inverted direction logic. This means that even if you plugged it in according the the directions it might be traveling opposite what you expect. If that happens, power EVERYTHING down, including unplugging the board from the computer’s USB, waiting 10 seconds, and flip the plug the other way on the offending axis.
● Lines don’t appear to be straight or circles aren’t perfectly round.
o This is likely to be caused by three different issues. Either the table is not square to the X and Y axis, the spindle is not plumb, or there is slop in the movement somewhere. Check for square along both the X and Y axis. Check that all belts are tight. They should sound like a stretched rubber band does when you pluck it. Make sure that there is no side to side motion in the table. If there is, adjust the eccentric nuts to tighten the wheels to the rails. The same applies to the Z plate. If you can wiggle it front to back or side to side adjust the tension on the wheels. Next, make sure all the rails are secured tightly.
● The motors make a noise that sounds like radio static.
o This is normal when the machine is first booted up and no motion commands have been issued.
● The machine isn’t moving to the commanded position.
o 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.
● The machine appears to be missing steps or not moving the full distance commanded on one axis in particular.
o 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.
● Files are running erratically or commands are being skipped with a warning that the command length is too long.
o Confirm that the line length maximum is set to 70 in UGS. Also, confirm that your CAM software is not using more than four decimal places for a position command.
● The motor stalls or the machine jumps off the planned path when cutting.
o Slow down the feed rate and/or shallow up the cut.
● Problem: The machine stops during homing before it hits the homing switch.
o Separate motor wires from switch wires to reduce electromagnetic noise creating a false trigger.