Overview & Objective

Learn the basics of our CNC (computer numerical control) Milling machine, the Tormach PCNC 1100 S3. This robotic cutting tool can create parts with complex curves and surfaces out of a variety of metals, allowing its user to create high precision parts.

General Shop Safety

• Closed-toe shoes

• Safety Glasses

• Ear protection

• Long hair tied back,

• No dangly jewelry, rings, watches, or baggy clothes.

Safety Considerations

• Do not leave the room while the spindle is running

• Be aware of your surroundings. Generally when working with the Tormach, your back is to the door and people can sneak up on you.

• Be mindful that chips can fly, and parts could come loose.

• Be mindful if anyone is working around the lathe.

• Do not put your hand or any other part of your body any closer than 6 inches to the bit when it is moving. The spindle will not stop and can cause severe damage.

• If the bit breaks or something seems to be broken or misbehaving, hit the pause button on the computer screen.

• If it needs to be shut off immediately press the red emergency stop button.

Take note on the emergency stop button locations on the tools:

Manual Mill - Emergency Stop Button

Lathe - Pull cover down and hit stop. If the lid is closed, the machine can start. If the lid is open, the machine can’t start.

Tormach 1 - Safety button on the Machine

Tormach 2 - Safety button on the external box

Don’t ever hesitate to hit the e-stop. You can always go back and re-zero it after.

Tools/Materials

• Various End Mills
  Digital Calipers

• Aluminum Stock

• Samples of already machined parts

About the Tormach

This is the Tormach 1100 series 3.

It can cut a variety of metals including:

• Aluminium

• Acetal plastic (Delrin)

• Steel

• Bronze

• Titanium

• Copper

This mill is one of the cheapest metal CNC machines available and is considered a hobby grade machine. Ours was built in 2015, assembled in the US, but originally from China. Runs off a regular computer using linux.

This machine offers much more rigidity than the Shopbot CNC router. The frame is much thicker, so it can handle vibrations from cutting metal. It has a maximum speed of 5000 RPM, so it’s much slower than the CNC Router. Instead of stepper motors it uses servo motors. They are more precise and are stronger. If you were to get in the way of it, it would crush you.

With the CNC Router, you move the head and the work is stationary. With the Tormach, the bed moves along the X and Y axis, and the spindle moves along Z. There are limit switches at both ends of the axis. Once it hits the limit, it will give an error. You can see the switch on the z axis.

X Axis - 18” of travel

Y Axis - 9.5” of travel

Z Axis - 16.5” of travel

It also uses coolant and has a built in tank. The coolant is a mixture of water soluble oil and normal tap water. It is used to clear the chips as it is cutting, it keeps the workpiece cool, and adds lubrication to the cut. Although coolant is not toxic, it’s recommended to not get too much of it on your hands as it can cause skin rashes after long exposure.. You can manually turn the coolant on and off using the button on the machine. You can also program it to do so.

The coolant that comes out drains into the mesh filter, and cycles back into the machine. Water evaporates when it sits in the tray, so always check that it’s full before running the Tormach. You can check the tank with a flashlight through a hole. You want it to be filled close to the top of the tank. If it is low, fill up the tank with normal tap water. If you observe rust on the table bed, let Makerlabs staff know as the coolant concentration may need to be adjusted.

The Tormach also needs to be oiled on a regular basis. Oil it every 4 hours of use, or every time you turn it on. Pull out the knob to oil the machine, and the oil will be pumped through the oil lines. If the knob moves slowly, it has lots of oil; if it moves quickly, it was probably empty. If the oil needs to be refilled, add oil in a little cap at top. Only takes about 300 ml.

Other Tormach

• Doesn’t have coolant

• Has an oil mist

• There’s a switch on the external hose.

• Will spray a mixture of air and oil.

• Can be adjusted on the knobs. Use as little oil as you can get away with.

How it breaks

Crashing

There is nothing stopping the spindle from plunging into the bed of the machine. If that were to happen in a serious way, you’d need to replace the spindle or the machine.

If you crash it stop using the machine and tell the front desk. We can run tests to see if it’s been damaged, but it will most likely be thrown out of alignment. We can fix it, but it’s a lot of work.

If you crash it, there will be a minimum assessment fee of $60/hr, plus a $60/hr charge to fix it, plus the cost of any replacement parts. Costs may vary depending on how badly it is damaged. Replacement part costs are available on the Tormach website.

Not Oiling the Machine

If you forget to oil the machine, it’s like not putting oil in your car. The machine will seize and will be permanently damaged.

Setting Up Your Material

Everything is mounted to the table with T nuts. Material is secured in place using the vice.

Squaring The Vice

• Back face of the vice is exactly inline to the x axis.

• Use the test dial indicator to square it (this is called “Tramming”)

• Set the indicator so the needle rests against the vice. The dial will move to zero.

• Jog along the x axis to make sure the vice is square

• If it’s not square, loosen the bolt on the right side, move the vice slightly, and check for squareness.

Clamping Material

To clamp your material to the bed:

• Loosen the vice

• Set up parallels so your material sits just above the vice. Members must bring their own parallels as they are precision tools and are easy to damage.

• Tighten vice, and hit it with the dead blow hammer
  Tighten again if needed

• Check that parallels do not move under your material. If they do, hit with hammer again, and tighten again.

• Don’t leave the vice out of alignment, if you are unable to align the vice leave the bolts and T-nuts on top of the vice so the next user knows it is not secured.

Basics of How It Works

The Tormach can only run G Code files. These can be created by either inputting dimensions in the Path Pilot software, or by running 3D or 2D files through a CAM software (such a Fusion 360) to generate the G code files.

How to Turn It On

• Power switches are on the right hand side.

• Turn on the machine with the power switch, wait for the computer to boot up.

• Set up the safety guard.

• Once the computer is on, twist the emergency stop, press the green start button, and a light will come on along with an audible ‘thunk’.

• In path pilot, hit reset, and another red light will come on.

• Once both lights are on, the computer and machine are talking to each other.

Working with Path Pilot

Understanding Path Pilot Controls

Single Block: Will slowly work through the program 1 line at a time.

Feed hold: Machine will stop moving on any of the axis, but the spindle will keep spinning. If you need to look at something, keep the guard up.

Coolant: Will turn on the coolant

Stop: Will stop the program. You will need to start at the beginning. It’s ok if the machine just cuts a bunch of air at first, it’s safer.

Sliders under these buttons can adjust the feed rate, spindle speed, and maximum velocity in real time as the machine is running. The maximum velocity is the speed at which the program moves from one area of cutting to another. If the cutting sounds too aggressive , you can adjust the feed rate as it’s spinning.

X, Y, Z, A: All coordinates for positioning. A Coordinate is for the 4^th axis. There is a 4th axis , but we don’t use it.

Step – move in increments, one key stroke causes one step. Ranging from 0.0001 inch - 0.10 inch

Continuous – Pressing keys continuously moves the axis

Spindle control:

Rev: Spins counter clockwise

Stop: Stops the spindle

Fwd: Spins clockwise

Two spindle ranges:

High and Low – Always leave it set to high.

The spindle is connected to a belt. The belt has a low and a high range. Typically we keep it in the higher range. If you need more torque, (ie. you’re using steel or titanium, or something strong), you might want to move it to the lower position. If this were the case, the button would have to be set to low. RPMs will also change depending on material being cut.

T: Tool number that’s in there right now. This corresponds to a table that we set.

Go to G30: G30 is a gcode command that takes the spindle up to a safe position. Most CNC programs will use G30 to go to a safe position, before doing something else. If you want it out of the way, hit G30, and it will take it up to a safe position. It will only move the tool in the Z direction. When a program starts, it will start at G30. You might as well send it there anyway, because it will go there on it’s own.

Referencing the Axes

Before we use the machine, it will reference all its axes, and will touch all its limit switches. It’s like homing on the laser, and will not let you run a program until you do this.

Reference the Z Axis First to get the spindle out of the way. There will be a green dot on screen once done.

Next, Ref X and Ref Y.

The spindle can then be driven back to the middle using the arrow keys. The arrow keys control the X & Y axes, Page up / down controls the Z axis. Think of it how you want to move in relation to the spindle (it’s backwards from the direction of the arrow keys).

When moving the bed, the computer will draw lines on screen to show where it is in reference to the bed. Do not push it to the limits of the machine, as it will tend to get stuck. It can get stuck on its sensor and won’t move. Staff will need to reset the limit switches.

Tools & Offsets:

In the Shopbot CNC Router, you set the zero before you start the program. You put the tool in, and then set the zero. With the Tormach, you need to track each tool’s settings.

Tool Offsets

Tool number: Tells the Tormach the diameter and the length of each tool.

Tool Height Setter

Used to accurately measure the height of the tool once it’s in the holder. Measurements are always in inches.

To make sure the tool is zeroed properly, bring the tool height setter down to the surface, and make sure it reads zero.

With the tool in the holder, bring down the tool height setter and touch it to the tip of the tool. It is quite sensitive and will be very accurate. Check your offsets, and edit if needed. Failure to set correct tool heights will likely result in crashing the machine.

Work Offset

Indicates the zero of the part or operation. This is also called G54 which is the Gcode command for this offset. When we move the tool to its zero position we are setting the work offset.

Different Types of Tools

There are a variety of different tools that can be used for different cutting purposes. Generally, any tools we use should not be greater than ½” in diameter, as this machine is not big enough for the horsepower needed.

Typically we use two flutes, because we’re working at a lower speed. Do not buy cheap tools on Amazon. They’re often not hardened properly, and do not perform well.

All collets should be kept clean, and inspected before use to make sure there’s no chips in them.

Tooling

Side lock tool holders (aka Weldon Flat): Has a groove in the side. Locks in the holder with a set screw. They’re not as high precision as collect chucks.

Milling Chuck: Similar to a chuck on a drill press

Fly cutter: Spins to create flat surfaces. It can’t cut very deep, and uses a carbide insert. Inserts are sold in packs of 10.

Boring Bar: Used for cutting really round holes. As it spins you can adjust the width of the hole by sliding it back and forth. Be aware that this tool is properly tightened and is rotating in the correct direction.

⅛” 2 flute carbide endmill: This is the tool that is used the most. It’s better than HSS steel, but it’s more brittle. If you make a mistake the tool will break. We would rather have the tool break than have something else break like the machine, the bed, or the material. They’re relatively cheap to replace.

There are hundreds of different tools you can get for various purposes.

Changing a Tool

Whenever you change a tool, you change the tool number in Path Pilot.

To change a tool:

• Open the latch. Machine won’t start when the latch is open.

• Arm comes down until it locks into place. You can’t close the door if the arm is locked in place.

• Put your non-dominant hand on the tool so it doesn’t come out.

• Turn the nut at the top away from yourself with a wrench.

To insert a tool:

• Push tool up into spindle firmly

• Tighten the bolt at the top with your hand

• Then do a ¼” turn with the wrench

Zeroing the Machine

Also known as setting the work offsets. The most reliable way to zero the X and Y axis is with an edge finder. When it’s spinning slowly, if it touches something, it will pop off the zero. Always make sure you have the right tool selected as you set the zero.

Setting Z

The safest way to zero Z is with a known size, such as a 1-2-3 block. They’re very useful to check that something is square and are very dimensionally accurate.

Place the 123 block on the surface of the material, bring the endmill lower than the block, next to the block.

Switch over to Step movement mode .1000, slowly bring up the Z axis until the 123 block slides under the endmill with no clearance. Press the Z zero button, remove the block and move the axis down the thickness of the block and re-zero.

To set the X and Y axis with an edge finder. Install the edge finder into the spindle, turn on the spindle to 250 RPM and move the tip of the edge finder to the edge of the work piece. When close use the step movement mode to move the edge finder up against the work until it slides off centre, this spindle is now one radius away from the edge of the part. Adjust the X and Y zero accordingly.

You can switch tools mid program and keep the same zero.

Setting X & Y

Move the spindle to the X and Y zero position; generally this is one corner of the workpiece. If using an edge finder, install it into the spindle and turn the spindle on to 250 RPM using the manual controls. Bring the tip of the edge finder to the edge of the workpiece. Using the step function, move slowly until the edge finder starts spinning true (not wobbling) then using 0.001 inch increments, move the edge finder further toward the part until the finder tip suddenly moves off axis; this means you are exactly on edge minus the radius of the edge finder.

Other ways to find the edge of a part is with the 123 block, similar to how finding the Z zero is described or using a piece of paper as taught in the CNC router course.

Machining your Material

There are three main types of tool paths we’re going to cover; facing, pocketing, and engraving.

Facing

Generally the first operation when making a new part. It will make a flat face on your material. We will use a fly cutter for this. The machine will assume that our X, Y, Zero position is the back left corner. We will use the conversational tab in the pathpilot software to program the operation.

To machine entire surface:

X start: 0

X end: length of material

Stepover: 80%

Z start: 0

Z end: total depth of cut

Depth of cut: pass depth

Work Offset: G54 – Usually we use this one. This corresponds to our zero.

Tool: related to the tool being used in offset

RPM: Varies depending on the material. Always look up the manufacturer's recommendation for the endmill you’re using. It’s listed in their catalogs.

For this operation, which is facing using the Tormach superfly in 6061 aluminium, use the following settings:

RPM: 2000

Feedrate: 10 IPM

Depth of Cut (DOC): 0.01 inch per pass

Coolant: Off

When you’re happy with your settings, hit post, and save to a folder. If you want to verify the file 1” above the part, you can do so with an air pass.

Pocketing

Will make a pocket in your piece, clearing out the area to the depth that we set. Pocket width, height, and radius can be set to your preference. All values can vary greatly depending on what material and endmill you’re using. Always check the catalog.

For this operation, which is pocketing using a ⅛” 2 flute flat general purpose carbide endmill, we will use the following settings:

RPM: 5000

Feedrate: 15 IPM

Depth of Cut: 0.025 inch

Program settings:

Z start: correlates to the total depth of facing material (0.01 inch)

Z End: As desired, recommend 0.060 (total material thickness assumed to be 0.25 inch)

Total depth: Recommend 0.05 inch

DOC: 50% of tool diameter

Feedrate: 10.

If you get an error message review the status screen. Errors are often related to the X and Y zero point being too close to the edge of the work envelope.

Engraving

We will engrave some text into the bottom of the pocket. Depth start: start of our pocket Ensure the total width of the text fits within the pocket. Post the file and observe the resulting tool path to ensure it fits.

Feedrate: 25 ipm

Saving Files

Save file> in file manager. Make your own folder.

Don’t trust the files after you’ve left for the day. It is a shared machine, and someone may have messed with it.

Running the File

• Hit cycle start

• Turn velocity down to close to zero when it first starts, then increase as the spindle gets close to the material. Keep the speed very slow, until the tool starts moving in to cut and you are happy with the Z zero, tool offset, and the program is behaving as expected.

If importing files, copy files from a USB, directly into the computer, and load it from the file tab. Files can’t be run directly from the USB drive.

Things to watch out for:

• Sometimes when booting up, it looks like the computer doesn’t start. Make sure the screen is actually on.

• The oil in the oiler mixes with the coolant, will sit in the tank, and after a while will start to grow bacteria. Every once in a while we need to replace the oil.

• There is compressed air that turns on in the metal shop, used for cleaning up chips. Make sure to wear safety glasses when cleaning up chips. Do not use on manual machines.

• If cleaning out the machine, wear gloves as the metal shards can cut you. Chips go in the bin near the lathe. Make sure they’re not contaminated with other non-metals as these chips will be recycled

Shutting down the Tormach

• Hit the Emergency stop

• In Path pilot> hit exit > will give you a message to hit estop

• When the computer says it is safe to power off, turn main switch off.

Cleaning Up:

Sweep chips using the brush off to the drain on the left. Make sure there’s no plastic mixed in. The chips will get scooped out and into a metal recycling bin.

Always clean up after yourself!

Other Info:

Tool can be booked on our booking calendar at http://makerlabs.com/tool-booking

It is $10/hr to use the tool, and you must be a member in order to use this tool after the class.

We include a complimentary 30 minute consult to be used within 30 days of taking the class. Email hello@makerlabs.com to schedule.

Student Handout

Tools

• Two main local tool suppliers:

  • KBCtools.ca - Location in Delta, offers most basic machining tools

  • Thomas Skinner - Phone to order, good for specific and higher end tools. Located in Richmond.

• Avoid non name brand tools from Amazon

• Most of the name brand tool suppliers require an account, but good online resources for feeds and speeds

  • Niagara - Very useful catalogue

  • Harvey

  • YG-1

  • Kenametal

  • Garr

Further Learning Resources

• Youtube Channels:

  • HAAS Automation Youtube channel

  • NYC CNC Youtube Channel (also has webpage)

  • Tormach Youtube Channel

  • Mechanical Advantage Youtube Channel - Great for Fusion360 CAM

• Websites:

  • Niagara Cutters (Seco Tools) Catalogue - General purpose feeds and speeds

  • www.nyccnc.com - Links to youtube videos

  • http://www.vikingdrill.com - Feeds and speeds for drilling

  • tormach.com//docs to access machine manual PCNC 1100S

Basic Feeds and Speeds

IPT - Inch Per Tooth

WOC - Width of Cut

IPM - Inch Per Minute

RPM - Revolutions per minute

DOC - Depth of Cut

SFM - Surface Feet Per minute (varies based on material being cut) (V_f)

1. Using the lookup table in the manufacturers catalogue get the SFM and the IPT.

2. Calculate the RPM = 3.82 x SFM ÷ Diameter of tool

3. Calculate the feed rate IPM = # of teeth * RPM * IPT

Example

⅛” 2 Flute flat general purpose carbide endmill with DOC: 0.25 inch and WOC:0.00625 has SFM of 400 to 1000 and IPT: 0.0009 inch from page 225 of the Niagara cutters catalogue.

RPM = 3.82 * 400 / 0.125 = 12224 RPM, since machine has max of 5000 use this instead

IPM = 2 * 5000 * 0.0009 = 9 IPM

These results are a starting point. If the DOC or WOC changes the feed rates also change. Only experience and experimentation can inform these adjustments.

Some common feedrate settings:

• ⅛” 2 Flute Flat Carbide Endmill - Aluminium - 5000 RPM, 15 IPM, 0.002” IPT, 100% DOC, 25% WOC

• ⅛” 2 Flute Flat Carbide Endmill - Steel - 3000 RPM, 1.8 IPM, 0.0003” IPT, 100% DOC, 20% WOC

• Tormach Flycutter - Aluminium - 2000 RPM, 10 IPM, 0.01” DOC, 100% WOC