Tormach Mill Guide
The Tormach PCNC1100 is a 4-axis computer numerical control (CNC) milling machine. This guide is designed to get an individual up and running on the machine in the minimum amount of time and with little training. For complete documentation see the machine specific guide provided by Tormach. The following instructions are intended to be followed in order.
- Getting Started
- Front Control Panel
- PathPilot Control Software
- Jog Shuttle
- Automatic Tool Changer
- Reference Tool
- Touch Probe
- Tool Holders
- 5C Collet Holder
- Start Up
- Base Toolbar
- Setting Up Tools
- Locating Work
- Loading Programs
- Running Programs
Before using the machine fully read and understand the material covered in this guide. This guide is not a replacement to the full documentation provided by Tormach. If you have any questions please ask one of the staff.
OverviewJump to Table of Contents
The Tormach PCNC 1100 is intended for small work. The machine's X, Y, Z limits are 18" x 9.5" x 16.25" (457mm x 241mm x 419mm) and the table size is 34" x 9.5" (864mm x 241mm). The machine has a spindle speed range of 100 to 5140 RPM with a maximum feed rate of 110 IPM (2794 mm/m) in the X & Y axis and 90 IPM (2286 mm/m) in the Z axis. If you need a machine that is capable of handling larger work consider the HAAS VM (capable of doing 5-axis work) or Trak DPM.
The large green and yellow cabinet next to the Tormach has the majority of the tools required to operate the PCNC 1100. Please feel free to look through the drawers and use the tools in them when necessary. However, these tools should never be used on other machines nor returned to the Tool Crib - they stay with the green and yellow cabinet.
The Tormach PCNC 1100 is a computer operated machine. All machine movements will be controlled via the computer interface and jog shuttle. Always ensure that you are not touching the mill while adjusting settings on the computer. Always give the machine a couple of seconds to respond after working on the computer before placing your hands near the mill.
The front control panel is where a number of important machine controls are located. This includes the start button, emergency stop, computer on/off, coolant on/off, spindle lockout, and a number of spindle controls. You should familiarize yourself with these controls and their location. Please note that all spindle rotational control is now handled by the PathPilot controller software. Do not alter spindle controls on panel. In the bottom left section of the control panel there is a spindle lockout. In order to use the spindle, the key will need to be inserted and turned to the "on" position. Ask shop staff for the key before operating the spindle. It is important to note that all axes can move at all times that the machine has power - even when the spindle is locked.
The PathPilot CNC controller software is the main interface used to interact with the machine. This software was developed by Tormach for individuals without extensive CNC exposure. The software allows users to program in conversational mode or to upload CAM-generated G-code files.
The jog shuttle is the main method used to move the machine. First click the button for the axis you want then use the dials in the center of the shuttle to control the movement. There are two dials, an inner one and an outer one. The outer dial is for continuous, fast movements and the inner dial is for slow, stepped movements (machine moves roughly one motor step at a time). The default maximum travel speed is 110 ipm and step size can be set in PathPilot in the bottom right corner of the screen.
The ATC is used to store and load tools automatically. To insert and remove tools into the spindle use the ATC tab in PathPilot.
The tool setter probe is used to measure and record the lengths of tools to be used. It is essential when running a cnc program that the machine has tool lengths set so that it knows where the tools are in relation to the work.
The touch probe is used to locate the work on the machine in the x, y, and z axes. It's mechanical equivalent is the edgefinder. The touch probe can also be used to digitize the shape of an object, useful for reverse engineering.
Tormach uses a special tool holding system, called TTS, in place of R8 collets (although the machine can accept R8 collets if the ATC is not attached). The TTS tooling system uses independent tool holders with a 3/4" shank which insert into the spindle. The ring around the TTS holder sits flush against the nose of the spindle. Tormach's full documentation can be found here: TTS Tooling.
The machine can have a 4th axis added to it. This is referred to as the A axis. Workpieces can be attached directly to the face of the A axis. A chuck or collet adapter can also be attached to the axis to hold work. Tormach's full documentation can be found here: A-Axis Manual.
The tailstock can be used in conjunction with the A axis to support long material.
The 5C collet adapter can be attached to the face of the A-axis for holding work as well as bolted to the table of the machine or clamped in a vise.
The Fogbuster is a mist coolant system. It can be used as an alternative to the built-in flood coolant system. The Fogbuster is ideal for operations that don't require full flood coolant but where cutting oil alone may be insufficient. The Fogbuster requires less clean up than the flood coolant.Jump to Table of Contents
A number of the operations in the procedure below will cause the machine to move automatically. If for any reason the machine starts to do something unintended hit the large red emergency stop button on the front control panel.
- Familiarize yourself with the Tormach PCNC 1100 and the tools in the green and yellow tool chest. Turn the lamp on before Jeff reminds you to.
- Rotate the main power switch, the red and yellow rotary switch on the side of the machine to the on position (from vertical to horizontal).
- On the Front Control Panel flip the computer switch to the on position.
- Ensure that the other switches on the front control panel are in a sensible position (e.g. the coolant switch isn’t turned on).
- Deactivate the emergency stop button by twisting to the right and pulling.Then press the green start button.
- The computer and control software should be loading. Wait for the load process to complete and the main PathPilot screen to appear.
- If a dialog box appears asking “ATC: OK to RESET?” at any time, contact shop staff before continuing.
- The RESET button will be flashing red. Click it.
- Now you must reference your axes. We will start with the Z axis. On the bottom-center of your screen is the DRO readouts. Click the button labeled REF Z. This will cause the Z axis to move upwards until it contacts its limit switch. Wait until the machine stops moving before continuing.
- If the Z axis (or other axes) do not move, it is likely because the machine is currently located on a limit switch. The limit switches will need to be turned off and the machine will need to be moved off of any limit switches. The limit switches will then need to be turned back on before proceeding. Ask shop staff for assistance.
- Jog Shuttle: First click the button for the desired axis. The axis currently being controlled will have a green light next to it in the DRO readout (bottom-center of the screen). Use the dials in the center of the shuttle to control movement. There are two dials on the jog shuttle, an inner and an outer. The outer dial is for continuous, fast movements and the inner dial is for slow, stepped movements (machine moves a given set of motor steps at a time). The default max continuous travel speed is 110 ipm. Step size can be set to varying sizes in PathPilot in the bottom-right of the screen.
- Arrow Keys: The up and down arrows on the keyboard control Y axis movement. The left and right arrows control X axis movement. "Page Up" and "Page down" control Z axis movement. When using the arrow keys, toggle between continuous motion and step motion by hitting the JOG Cont/Step button in the bottom-right of the screen next to the Jog Slider. The maximum jog rate when using the arrow keys can be altered using the Jog Slider button.
If the E-STOP button or "RESET" buttons are pressed at any time during machine operation, all references will be lost. If the E-STOP is hit, you will need to reset the E-STOP, then hit the green START button on the control panel before re-referencing the axes. To re-reference the axes, click the RESET button, ensure that the machine is off of all limit switches and then hit REF Z, REF Y, and REF X. Running the machine without references being set can cause the machine to crash.
OverviewJump to Table of Contents
PathPilot is a machine control software developed privately by Tormach Inc. The software is designed to be approachable to users without machining experience or exposure to CNC software. The program is relatively new and routinely undergoes updates. Newer versions continue to introduce new machine control opportunities. PathPilot can be used for both conversational programming and for running CAM generated G-code programs. This training will focus on using PathPilot to run CAM generated G-code programs. Please see shop staff if interested in using the conversational software in PathPilot.
The bottom half of the PathPilot screen is displayed at all times when the software is running. This section displays feedback on the machine's current status. It is split into three sections. The left section sets program controls, the middle section displays the current tool location and machine code status, and the right section sets manual machine controls.PathPilot uses small green lights to signal which features are active in the software at a given time. If a button has a green light next to it, that means that it is currently engaged.Jump to Table of Contents
The bottom-left portion of the screen is used while running programs.
The "CYCLE START" button is used to start a loaded program. This button allows the machine to control all motion during a run program. Clicking this button will turn on a green light, showing that the button is currently functioning. If a feedhold (machining pause) is engaged during a program, this button will need to be pressed to allow the machine to continue movement. If the "SINGLE BLOCK" button is engaged, the "CYCLE START" button will need to be hit before each line of G-Code is interpreted. If the "M01 BREAK" is engaged, the "CYCLE START" button will need to be pressed before the start of each new machining operation.
The "SINGLE BLOCK" button inserts a machining pause to occur after each line of G-Code is interpreted. This helps reduce the possibility of crashing the machine because the user must press "CYCLE START" before each line of G-code is interpreted. This button works well on small programs, but can be impractical if a code is thousands of lines long.
The "FEEDHOLD" button acts as a pause during a program run. This button can be engaged by clicking the "FEEDHOLD" button or by hitting the SPACE bar on the keyboard. A feedhold will automatically stop all axis movement, but will not stop the spindle. This feature is helpful when you want to check tool location and tool path before proceeding without terminating the program. When running a program for the first time, always keep your hand near the SPACE bar in case you need to pause the machine. Hitting the E-STOP or "STOP" button will stop the spindle and will cause your program to terminate and reset. It is important to note that this feature will always allow a line of G-code to complete itself, even if a feedhold is engaged halfway through a line of code.
The "COOLANT" button turns coolant on and off. The flood coolant for this machine is currently not operating. The fogbuster can be used as a misting coolant, but it must be turned on via the manual switch located on the outer-right side of the machine frame.
The "M01 BREAK" button causes the program to stop in between machining operations and in between tool changes. For example, this would cause the machine to pause in between milling and drilling procedures. It requires the user to hit "CYCLE START" in between these operations as a confirmation that the machine is clear to proceed. This button should always be engaged during the first run of a program.
The "STOP" button serves to terminate machine and spindle motion. It also stops a program from running and resets the program to the beginning of its code. This feature should be used when the machine is not moving as expected - indicating that the G-code requires editing. This button should be used over the E-STOP (EXCEPT IN EMERGENCY SITUATIONS) because it does not require the machine references to be reset.
The FEED SLIDER allows for manual adjustment of a program's feedrate. This does not include rapid (G00) moves. When running a program for the first time, this feedrate should be reduced initially and then adjusted to suit the cutter's proper speeds and feeds. The max override of the slider is 150%. Clicking the "FEED 100%" button to the right of the slider automatically adjusts the feedrate to its originally programmed value.
The RPM SLIDER allows for manual adjustment of a program's spindle speed. During machine motion the spindle should be turning - do not set this value to 0 during a machining procedure. Manually adjust this slider to suit the cutter's proper speeds and feeds. The max override of the slider is 150%. Clicking the "RPM 100%" button to the right of the slider automatically adjusts the RPM to its originally programmed value.
The MAX VELOCITY SLIDER allows for manual adjustment of the machine's maximum velocity. The machine operates at max velocity during G00 moves, and in between tool changes. The machine should only move at max velocity in between points where there is sufficient clearance and no risk of crashing. This slider should be reduced significantly (to 25% or lower) during the first program run to ensure safety and reduce the risk of crashes. This slider maxes out at 100%. Clicking the "MAX VEL 100%" button to the right of the slider automatically adjusts the max velocity to its originally programmed value. It is important to note that reducing the slider to 0% will prevent all machine movement (except for spindle rotation).Jump to Table of Contents
The bottom-center portion of the screen is used to display the current tool location and machine status.
The central "WORK" column functions as a Digital Readout (DRO). It tells the current location of the center of the tip of the tool in the spindle according to four axes (X,Y,Z,A). Each axis has its own row (X,Y,Z,A). The "ZERO _" button on the left side is used to zero an axis, such as when setting a work coordinate system origin. If a specific value needs to be input into the DRO, the value can be manually edited by clicking in the white box and typing in a value. This white box can also perform simple algebraic operations. For example, you could divide, multiply, subtract, and add values together in the box. To the right of the white box is a green light. When this light is on, that means that the axis is currently selected for movement with the jog shuttle.
The central "DTG" column displays "Distance to Go" during a move.
The "REF _" buttons on the right side are used during initial machine set-up to reference each axis to its given limit switch. These should only be need to used during the start-up phase of the machine or after the E-STOP has been hit.
The bottom line in this section displays current machine status. This line contains G-codes which experienced individuals will understand. Below is a brief explanation of what each code represents. You as an operator are required to understand the first 3 codes in the line.
(G54/55/56/57/58/59) This code appears first and represents which work coordinate system (WCS) the machine is currently operating in. A work coordinate system is simply an origin of a coordinate system. The machine allows users to maintain several different coordinate systems. This is useful when an individual has multiple parts to run or different procedures at different locations on the table. Check your code for the WCS you need to use, then use the MDI line to reset the machine to that WCS. To change a WCS, type in G(Number of your WCS) and hit enter to change the current WCS. Ask shop staff for help if you are unsure.
It is crucial to set up the machine in the work coordinate system which your program uses! Setting up your part in one coordinate system and then running your part in another will cause the machine to crash. If you are unsure which WCS your code uses, talk to shop staff.
(G90/G91) This code appears second and represents whether the machine is in absolute mode (G90) or incremental mode (G91). Absolute mode will reference all X,Y,Z points to the origin of the current WCS. Incremental mode will reference all X,Y,Z points to the current location of your tool. [Ex: Moving (1,1,1) in G90 will move the tool to position (1,1,1) no matter where the tool is currently located. Using G91 would move the machine one unit in the positive direction in X,Y,Z no matter where the tool is currently located.]
(G20/21) This code appears third and establishes which unit system the machine is currently operating in. G20 will set the machine to operate in inches. G21 will set the machine to operate in mm. If you change the operating units, all current values will convert into the other unit system. [Ex: If you are at X=1", it will convert to X=25.4mm]
|G54-59||Work Coordinate System Designation|
|G80||Cancels existing canned cycles|
|G40||Tool cutter (radius) compensation Off|
|G94||Feed rate in units/min|
|G97||Cancels constant surface speed setting|
|G99||Return to initial R plane after canned cycle|
Along the top portion are 4 "STEP" buttons. When the machine is manually moved using the step feature (using the arrows or jog shuttle), these buttons represent the values that the machine can move in one step. This feature is useful when trying to bring a tool in close to a part without moving too far. The size of the step can be selected by manually clicking on the desired value or by hitting the "STEP" button on the jog shuttle. Be careful when using the jog shuttle because you can not control if the step size is increased or decreased. Always check PathPilot to ensure that you are using the correct step size.
The JOG SLIDER regulates the max jog rate used when moving the machine using the arrow keys. This slider does NOT affect the max jog rate of the jog shuttle. The JOG CONT/STEP button next to the slider can be used to alter whether the arrow keys are operating under continuous jog or step motion.
The central portion of the manual machine controls regulates spindle operation.
The "SPINDLE RANGE" button designates is the spindle is being operated in High or Low belt. The high belt operates between 250 and 5140 RPM while the low belt operates between 100 and 2000 RPM. The belt must be manually changed in the spindle head if you want to switch between the operating conditions. Always ensure that the physical belt positioning matches the "SPINDLE RANGE" belt selection before starting the spindle. Check with shop staff if unsure of how to check and adjust belt position. The spindle head had a safety switch mounted on it which prevents the spindle from turning while the door is open. However, you should always physically lock out the spindle before opening the spindle head.
To start the spindle, type a RPM value into the box next to "RPM" and hit enter. This will only load the desired value into the program. This will not start the spindle. To start the spindle, press the "FWD" button. If the spindle lock is not engaged, the spindle will begin to turn. To stop the spindle, hit the "STOP" button. The "REV" button will spin the spindle in reverse. Do not use this feature unless you have a specialized cutter and permission from shop staff. To change the RPM while the spindle is running, simply type in a new value into the "RPM" box and hit enter.
The "FEEDRATE" box displays the current set machining feedrate. This is important to monitor during machining operations in order to help set the correct speeds and feeds for your cutter.
The "T" box in the bottom portion displays the current tool which the machine is using. To change tools, type in the tool you desire to use in the white box. The hit the "M6 G43" button to the right of the white box. M6 G43 is a condensed G-code which tells the machine to change tools and load the new tool's length and diameter offsets. The program will either load the current tool back into the ATC or ask you to perform a manual tool change. See Setting Up Tools for more information about tool changes.
The "GO TO G30" button will cause the machine to return to its preset G30 position. This position acts as a safe, home position, clear of the part and the table. This position should be set in the Offsets tab in PathPilot before a program is run to ensure that the tool will retract to a safe location. Hitting this button causes the tool to move in the Z direction first and clear the part. Once the tool reaches its final Z value, the X and Y axes will move to their final positions.
The "EXIT" button is used when shutting down the machine. See shutdown for more information about shutdown procedures.Jump to Table of Contents
The "main" tab will be used during times of machine movement. This includes part set-up, when running programs, and manual machining operations. The display is split into two parts. The left section of the screen has a G-code viewer and the MDI line, while the right side displays a 3D model of the program's tool path.
The large white section on the left is where your G-code from your part file will display. When you load a program, this field will populate with text. It is recommended that you have a basic understanding of G-code. This allows you to interpret the code before and during program runs and allows you to catch errors.
The line below the G-code viewer is the MDI line (Manual Data Input). This line allows a machine operator to send g-code directly to the machine by manually entering them directly. This would allow the operator to, for example, tell the machine to move to a specific location, change a tool, etc. This is a very powerful feature and great care must be taken when using it. You will need to use the MDI line to change some basic settings of the machine. You will need to use the MDI line to change the work coordinate system (G54/55/56/57/58/59).
It is extremely easy to crash the machine using the MDI. Never enter G-code into the MDI unless you know exactly what it will do.
3D Tool Path Modeler
The large black section on the right of the screen displays the tool path that the loaded program will follow. This interface allows the user to view their toolpath from any orientation in a 3D plane, similar to SolidWorks or other CAD/CAM software. Moving around the display can be performed with the mouse. Right clicking allows the user to select from a list of common viewpoints. A major advantage of this feature is that it allows the user to perform a "sanity check" before running a file to check for obvious crashes or errors in their code. Clicking on a portion of the toolpath will highlight the line of G-code in the G-code viewer which represents that operation. While a file is running, completed paths will turn from white to pink. While operating the machine manually, the viewer will trace the tool path in yellow as the tool moves.Jump to Table of Contents
The "File" tab is used to load and edit G-code files. A flash drive can be plugged into the machine on the right-hand side, below the chip tray. The file page has three sections. The far left section is a file storage of all files on the Tormach controller, the middle section shows the files present on the flash drive, and the right sections displays the currently loaded G-code.
The Tormach machine can only run G-code files that are stored on the machine. If your file is on a flashdrive, you will need to copy that file onto the Tormach controller, then double click the file to run it from there.
Copying a file from a flash drive to the Tormach controller creates a new file. Editing the file in one location will not take effect on the other file. If you edit the file on the flash drive, you must recopy and overwrite the file on the controller.
The right section allows the user to manually edit the g-code of the selected file. It also allows the user to edit any programs that were created using the PathPilot conversational programming (Conv Edit).
There are files stored in the Tormach controller which are used in other programs. These show up as green folders. DO NOT EDIT THESE. They store information such as threading routines, engraving fonts, and stored routines.
The "Settings" tab provides feedback on the current machine settings.
The left side of this tab displays a description of different G-codes that the machine interprets. The G-codes that are currently active are highlighted yellow.
The right side of this tab displays features that may be active with the machine's configuration. The features that should be active during machine start up are: "ATC", "Limit Switches", "Show Tooltips", "Digitizing Probe/Tool Setter", "G30/M998 Move in Z Only", and "Conversational Feeds and Speeds".
If you have questions on these features or need assistance changing them, see staff.Jump to Table of Contents
The "Offsets" tab is used to store both tool and work offsets. At the top of the offsets page there are two tabs which allow you to switch between tool offsets and work offsets.
Tool offsets are characteristics of each independent tool. There are 3 characteristics that PathPilot looks for.
- Tool Description: This is meant to be an easy-to-read description so you, the user, can interpret which tool to use without memorizing the tool numbers. The machine does not interpret this value so feel free to enter what makes sense to you.
- Tool Diameter: Stores the tool diameter in inches (G20) or mm (G21)
- Tool Length: Stores the tool length in inches (G20) or mm (G21). This length is taken from the seat of the TTS tool holder (where the collet ring touches the nose of the spindle) to the tip of the tool.
The "SET G30" button allows you to set a point that is clear of your work piece. This point is where the machine will move after it has completed its program run or when a manual tool change is required. To set this location, move the machine to a location where you will easily be able to change tools and change your part out. Click "SET G30" at that location.
When the G-code prompts the machine to move to G30, the machine will start by moving in only the Z axis. Once the Z axis has hit its set G30 position, then the X and Y axes will move. This helps clear the tool from the part and avoids crashes.
The "MOVE & SET TOOL LENGTH" button is used in combination with the Tool Setter probe. This prompts the machine to take the current tool in the spindle and touch off on the tool setter probe. The machine then stores the given tool's length offset in the tool offsets chart.See Setting Up Tools for more information.
Work Offsets (Work Coordinate Systems) represent where each WCS is located in reference to the machine home position. The numbers seen in this tab are not meant to be interpreted by the user. Think of them as a representation for the machine to understand where each WCS is. DO NOT alter these values in the offsets tab. These will be updated when you set your WCS in the DRO.Jump to Table of Contents
The "Conversational" tab allows the user to program conversationally on the Tormach. PathPilot's conversational software is user-friendly and created to be used by inexperienced individuals. It allows users to perform basic milling procedures, as well as more complex operations such as thread milling and engraving words or DXF images. This training is not covered in this seminar. Please see Shop Staff if you would like to learn more.Jump to Table of Contents
The "Probe" tab is used when using the Passive Probe to locate your workpiece and other features.Jump to Table of Contents
The "ATC" tab is the user interface to manage the tools stored in the automatic tool changer (ATC).
For how to use this page to insert tool, please read the Setting Up Tools page.
The left side of the screen controls movement of the ATC and regulates how tools are inserted from the ATC. The center of the page displays a diagram of the ATC holder. Numbers in the slots of the ATC holder represent the tool that is stored there. The right side of this tab regulates removing tools from the ATC.Jump to Table of Contents
The "Status" tab displays status conditions of the machine and displays error messages.
If an error occurs while you are operating the machine, the "Status" tab will turn red. Click on it to see what the error is.
The large white section on the right side will display written error messages describing issues with the machine or potential errors in G-code files. Each error message will have a time included to the left of the message. The most recent errors will be displayed at the top of the list.
The right side of the screen displays active features on the machine. The "LIMITS" section displays limit switches that are currently activated. If a limit switch is active, the axis will not be able to move further in that axial direction.Jump to Table of Contents
The Tormach has a variety of methods for holding tools. It is currently set up to work with the Automatic Tool Changer and thus can only use TTS holders.
Before loading tools read and understand the TTS tool holders and look over the tool slip potential. Tooling over 1/2" (12.5mm) in diameter is to be avoided as it has a higher probability of pulling out of the machine.
Before loading tools make sure to check that the tools are sharp. Measure the cutting diameters as well (If they've been resharpened the size on the label will be wrong).
The tool loading process will cause the ATC to move. Some buttons will cause the ATC to move after a brief time delay. Do not have your hands near the machine while operating the screen. Give the machine a few seconds to process computer commands before putting your hands near the ATC.
- Go to the "ATC" screen by clicking the "ATC" tab in PathPilot.
- Once in the ATC tab, DO NOT click the "Ref Tool Tray", "SET TC POS", "--", or "++" buttons. These will reset the machine's reference location of the ATC and may cause the ATC to crash.
- Ensure that the spindle is empty.
- Ensure the ATC (Automatic Tool Changer) is empty.
- Removing Tools: If there are tools in the ATC you can remove them by entering the tool number to remove in the text box in the upper right hand side of the screen next to the "REMOVE" button. Press enter on the keyboard and click the "Remove" button. The machine will then fetch the tool to remove. Wait until the ATC has retracted to its initial position (far to the left of the spindle). A dialog box will appear saying "Remove tool from spindle". Remove the tool from the spindle and then press "OK" on the dialog box. At this point the tool number should be removed from its relative slot in the ATC diagram in the center of the screen. This shows that the machine is no longer keeping track of that tool. If any other dialog box appears see the Troubleshooting section.
- Inserting Tools: Select a tool to insert into the spindle. Ensure that the tool holder is clean, then press and hold the "Release" button on the spindle head and insert the tool so that it sits firmly against the spindle collet. Release the "Release" button and press the "Lock" button before letting go of the tool. Enter the tool’s number as it is in your CNC program in the box in the bottom right corner of the screen labeled "T". Press enter on the keyboard and hit the button to the right of the box labeled "M6 G43". This informs the machine that the given tool has been loaded into the spindle. Press the "Store Current Tool" button in the ATC tab. The machine will now move and store the tool currently in the spindle in the next open slot of the ATC and label it with the number you provided. Repeat this process with your remaining tools. The tool changer will automatically index to the next open space in the carousel. If a dialog box appears asking to reference the z axis see the Troubleshooting section.
- The machine needs to know how long its tools are. Use the "T" box in the bottom-right of the screen to load one of the tools used in your CNC program. Type the number of the desired tool, hit enter, then hit the "M6 G43" button.
- Get the tool setter probe. Making sure the table and bottom of probe are clean, place the probe on the machine table approximately below the spindle and plug its cord into the accessory port located on the machine's front control panel.
- Go to the settings tab and select the "Digitizing Probe/Tool Setter" bubble. This lets the machine know that the probe is active.
- Go to the Offsets tab. Make sure that you are on the Tool Offsets page, not the Work tab.
- With your finger, press on the probe surface and check that a red light appears on the bottom of the probe image in the Offsets tab on the screen. A red light will also appear on the base of the probe itself. If either of the lights don't come on see the Troubleshooting section.
- Go to the bottom-left of the screen and adjust the "Max Velocity" slider to 15%. This restricts the maximum rate at which the axes can move, helping to prevent the risk of a serious crash.
- Using the jog shuttle move the Z axis in the negative direction until the tool tip is roughly one inch above the center of the probe’s top surface. Then align the probe with the center of the tool either by moving the probe or the table (Limit switch triggered? See Troubleshooting section.
- On the Offsets screen, in the Tool Offsets tab, edit the "Tool Description" and "Diameter" values in the offsets chart for each tool that you are using. There may be preset values in these areas from previous operations. Press enter after typing in a new value. Do not worry about clearing values for tools that you are not using. The machine will not reference these while it runs your program.
- On the Offsets screen click the button on the left side called "MOVE & SET TOOL LENGTH". This will cause the Z axis to move until the tool loaded in the spindle touches the probe. The tool will retract and then slowly lower down until pausing and setting its reference tool height. The Tool Offset screen will reset and upload the new tool length value in the "Length" column of the offsets chart.
- Use the "T" box in the lower-right of the screen and repeat step 16 for ALL tools used. Ensure that the probe remains centered under the tools. Ensure that ALL tools are referenced. Missing a tool may result in a crash.
- Put the tool setter probe away.
- The tools in your program should now be properly set. Each tool length is referenced to the other tools in the program.
The PCNC1100 mill does not have sensors to detect if a tool is in the spindle. The machine relies on the computer to tell if there is a tool in the spindle or the ATC. Make sure to always use the computer interface to tell the machine when a tool is present in the spindle or inserted into the ATC. If you insert a tool into the spindle or the ATC without entering the tool number into the computer you will cause a crash.
Most CAM software lets you print out a copy of your tool list. You should do this and have it on hand for the remaining steps.
Tool numbers in your CNC program must match exactly with their numbers in the ATC (although technically the order in the ATC is irrelevant, e.g. 1,3,4,2, it is almost always most efficient to insert the tools in the same order they are used in your CNC program e.g. 1,2,3,4,5,6).
Tool lengths and tool numbers must match *exactly* with the tool lengths and numbers set in your program.
The offsets chart will use the unit system designated by G20/21 (inches/mm). Ensure that the machine is operating in the correct units before proceeding.
To stop the machine's z axis motion during the tool setting operation, hit the "STOP" button in the lower-right screen or hit the E-STOP button. Note that hitting the E-STOP will require the machine axes to be re-referenced.
At this point the tools are not set in reference to a work coordinate system, only in reference to each other. Running a program at this stage would result in a crash. See Locating Work for more information.
Probe work locating capabilities coming soon... Talk to Viktor.
For now use an edge finder to find your x and y positions and a tool from your program to set the z position. Ensure that you are operating in the correct WCS and then use the jog shuttle and DRO together to zero/set your x and y coordinates. Then load a given tool used in your program and touch off on the surface of your part to set your z-height. Since your tool length offsets have been previously set, loading a given tool and touching off with it will set the height for all the tools in the ATCJump to Table of Contents
Automated machines are controlled using numerical control (NC). Although numerical control is most commonly implemented using a computer (CNC), it can also be implemented using other methods (e.g. mechanically via cams). The most common programming language for NC machines is G-code. Simply put, G-code is the language used to tell the machine how to move; in reality the language is more powerful than this simplistic description implies.
Many modern CNC machines have standardized on Fanuc style G-code with slight variations. The variations in how the machine controllers interpret G-code means that G-code is rarely portable from one type of machine to another (similar to assembly language). CAM software helps alleviate this problem by automatically generating G-code based off a machine specific "post". As long as the CAM software has the correct post for the target machine, it can generate functioning G-code.
For more information on G-code and NC machine programming see CNC Programming Handbook: A Comprehensive Guide to Practical CNC Programming by Peter Smid available through the library. For a full list of the codes available on the machine click the "Settings" tab.
- Talk to staff.
- The staff will post the CAM file for you. It should be either Tormach1100_3axis or Tormach1100_4axis depending on whether you are using 3 or 4 axis machining. These posts were created by the shop.
- The post will generate a G-code, also called NC-code or machine code, for your part (this is often done by running a simulation of your part).
- Save the G-code generated to a USB flash drive making sure to give it a useful name.
G-code can also be written by hand however this is highly discouraged for individuals who have not been taught the proper methods (e.g. using program verification software). If you think you need hand written G-code for your part speak with staff first.
- Go to the "File" tab.
- Insert your usb flash drive into the the usb socket located on the right hand side of of the machine base.
- A flash drive box should appear in the center of the screen, select your file and copy it to the Tormach controller.
- Select your file on the Tormach controller and load the G-code.
- Return to the "Main" screen. The program should display on the left side of the screen and the right side should display the tool path in a 3D viewer.
There are a handful of G-codes you should be able to recognize as your program runs. Recognizing these will allow you to know what the machine will do before it does it. Being able to recognize these will help prevent crashes. It is also important to know that some G-codes are "modal" meaning that once they are activated they remain active until explicitly turned off or changed (e.g. M08). For a full list of the codes available on the machine click the "Settings" tab.
|G00||Rapid Traverse e.g. G00 X1 Y1|
|G01||Linear Motion at Feed Rate e.g. G01 Z-0.125 F15.5|
|G54-59||Work Coordinate System Designation|
|M01||Optional Program Stop|
|M03||Spindle On, Clockwise e.g. S3000 M03 (turn the spindle on clockwise at 3000rpm)|
|M06||Tool Change e.g. T1 M06 (change to tool 1)|
|M08||Flood Coolant On|
|M30||End Program and Rewind|
The line below the G-code viewer is the MDI line (Manual Data Input). This line allows a machine operator to send g-code directly to the machine by manually entering them directly. This would allow the operator to, for example, tell the machine to move to a specific location, change a tool, etc. This is a very powerful feature and great care must be taken when using it. You will need to use the MDI line to change some basic settings of the machine. You will need to use the MDI line to change the work coordinate system (G54/G55/G56/G57/G58/G59).
It is extremely easy to crash the machine using the MDI. Never enter G-code into the MDI unless you know exactly what it will do.
The first time a program is run there is a high risk of crashing the machine. Pay attention and be prepared to hit the feed hold (SPACE bar) or E-STOP.
- Review the Hazards section and make sure you've taken steps to avoid them.
- Double check that the machine has been referenced.
- Double check that the machine is operating in the correct work coordinate system for the given program and that the work coordinate system origin is set at the correct location on your part.
- Review the machining settings in your CAM software. Double check you chose the correct tools (types, diameters, & lengths) and the correct feed and speed rates.
- Have a professional staff member verify your program.
- Double check that your set up is correct, the right tools are loaded into the ATC with the correct tool number and tool length offsets. Double check that all axes have been referenced.
- Double check that you've loaded the correct program.
- Check the front control panel. The spindle lockout should be turned to "|", The "Manual/Auto button should be switched to "Auto".
- If flood coolant is to be used install the machine guards if not already done. Switch the coolant button on the front control button to "Auto". Position the flood coolant nozzle and open its valve. If the fogbuster is to be used, set it up now.
- Determine whether your program needs to be run in high or low gear. Ensure that the belt is in the correct position in the spindle head. Ask staff for assistance before changing the belt position. Use PathPilot to put the machine in either high or low range as necessary.
- Read through the first 15 lines or so of your G-code. Make sure nothing looks surprising.See example G-code. Before running the part, perform a "sanity check" on the operation. To do this, verify that the toolpath in the 3D viewer is performing the machining operations you desire. Use a tool and the jog shuttle to move near your part and ensure that the tool tip in the 3D viewer is located accurately. Use different views to check that your tool will not crash into the table or the vise by cutting too low or cutting too far in one direction.
- Go to the "Main" tab. Familiarize yourself with the various controls on this screen.
- If you have only run this machine five times or less in the past, have a professional staff member with you when you run the program for the first time.
This section is to be read in full before running a program. It is *not* a list of steps to be followed in order.
- The first time a program is run there is a high probability of errors. As program complexity increases, the potential number of errors increases. The goal is to find and fix these bugs before they cause damage (e.g. crashing the machine). The first time a program is run it should be run in a wax part or, if this isn't possible, it should be dry run in the air above the part (often referred to as "cutting air").
- To run your part in the air set up the machine exactly as you would if you were going to be cutting the actual part (Z set to the correct location on the part, X & Y found, etc.). Look in your CAD software and find the deepest cutting point in the program. Move the Z axis at least that magnitude above your part plus an inch (25.4mm). Write down the distance above the part and then zero the Z axis on the DRO. You can now run your program and it will only cut air. When you are ready to run your real part simply move the Z axis back down the distance you moved it up and zero the DRO again.
- To help catch problems when running a program for the first time run it in single block mode. Activate this mode by clicking the "SINGLE BLOCK" button in the lower-left portion of the screen. When in single block mode a small green indicator will turn on next to the button. This will require the "CYCLE START" button to be clicked for each line of G-code. This will allow you to step through your program one line at a time. You can move in and out of single block mode as necessary in your program. At the very least you should be in single block mode for a few lines after each tool change to make sure the speeds and feeds are reasonable and that the machine isn't going to crash.
- Often when running a program for the first time you will need to override the speeds and feeds set in your program. Feed, RPM, and Max Velocity override sliders can be found on lower-left portion of the screen. Clicking and dragging the sliders will change the Feed, RPM, and Max Velocity values. Clicking the "100%" boxes to the right will reset the given slider to its original value. For the first run, reduce the Max Velocity slider to 15%.
- After each M06 (tool change) in your program, pause the tool as it's moving down by activating the feedhold. This can be done by pressing the SPACE bar or clicking the "FEEDHOLD" button in PathPilot. Double check to make sure that the numbers on the DRO, in your program, and in reality all roughly match. If unsure, stop the spindle and use a tape measure to check if the bottom of the tool is the correct distance from your part. If the tool is not the correct distance from the part stop the program and debug it (don't forget, shop staff can help you debug the program).
- As your program runs make notes about things that you might want to change (e.g. feeds, speeds, inefficient tool paths, etc.). When the program finishes return to your CAM software and make the changes.
The program can be paused at any time by hitting the SPACE bar or by clicking the "Feedhold" button in the lower-left portion of the screen. Press "CYCLE START" to continue the program. If the machine is about to crash and cause damage or injury always use the emergency stop never feedhold.
Feedhold will only stop movement of X,Y,Z,A axes. It will not stop the spindle.
If your program has been changed since the first time you ran it, no matter how small the change, redo the above steps as though this is the first time you've run this program (because it is).
If the program has not changed, install a new piece of stock and locate it in the correct work coordinate system following the steps outlined under Locating Work. If work stops are used in the setup not all coordinates will need to be indicated again. When the program finishes it should rewind back to the start of the program (if it doesn't, click the "STOP" button and reload the program in the "File" tab). Single block mode can be turned off and you can now click "CYCLE START".Jump to Table of Contents
Installing the A-axis
Coming soon... Talk to Viktor
Coming soon... Talk to ViktorJump to Table of Contents
Clean up the machine using the following procedure after every use.
- On the front control panel turn the spindle lockout to "O".
- Use the "ATC" tab to remove the tools from the ATC. Ensure that the machine is removing the tools from the ATC diagram.
- Remove your part from your setup. Clean and return any clamps.
- Clean up chips on machine.
- If flood coolant or the fog buster were used, use rags to wipe down the machine and spray WD-40 on any exposed metal surface.
- Shake out the floor mat and sweep the floor. Wipe up any coolant.
- Remove tools from tool holders and return them.
- Clean up workbench and desk.
- Have shop staff check the machine. Tell them about any problems or concerns with the machine.
It is essential that the following procedure is followed explicitly. Failure to do so can damage the machine.
- Remove tools from the ATC. See Setting Up Tools for more information on how to remove tools.
- Click the "EXIT" button in the lower-right corner of PathPilot. A dialog box will prompt you to first E-STOP the machine.
- Hit the E-STOP on the machine and then click "OK".
- Wait for PathPilot to display a message which states that "It is now safe for you to remove power from the controller".
- On the control panel, switch the computer switch to "Off".
- Rotate the yellow and red main power switch on the right side of the machine to the off position (vertical).
The following are a list of known problems that could cause the machine to crash or otherwise not function correctly.
- The A-axis can be crashed into the front control box unless it is put in the t-slot closest to the front of the machine.
- When using the A-axis with a tailstock it is possible for tooling to crash into the tailstock when the ATC rotates.
- The A-axis must be installed on the right side of the machine to avoid crashes with tooling in the ATC.
- Large tools can pull out of collets with excessive cut-loads.
Solution: Ask staff for assistance.
Issue: An axis will not move and an error message appears in the "Status" tab stating that a limit switch is triggered.
Solution: In the lower left of the screen click the red “RESET” button. Using the jog controller, carefully move the machine off of the limit switch. You will need to re-zero the machine.
Solution: Ask staff for assistance. Do not re-reference the ATC yourself.
Solution: Disconnect and then reconnect the probe cable securely to the accessory port then try again. If the problem persists ask staff for assistance.
Solution: Check to make sure no tools are in the spindle. If a tool is in the spindle remove it then press "OK". Pressing "OK" when a tool is in the spindle will cause the machine to crash. Press the "CANCEL" button if you don't want to remove the tool.
Solution: Ask staff for assistance.
Solution: Press on the probe a few times. Most likely the probe has gotten stuck. If this doesn't fix the problem ask staff for assistance..
Solution: Move the probe within one inch of the surface to be probed and try again.
A message is displayed next to the "RESET" button saying "\**** Face not found. Start too far away or Z not low enough"
Solution: The probe is either not below the surface of the part, the part isn't large enough (bigger than .400"), or the probe wasn't aligned with the center of the side of the part before probing. Correct any of the previously mentioned problems and try again. If it still fails ask staff for assistance..
Solution: The Tormach post can not make use of macros. Turn off macros in your CAD software and regenerate your G-code.Jump to Table of Contents