Protel EasyTrax
Installation and Useage Guide

Introduction

Protel EasyTrax is a full featured CAD software package specifically designed for printed circuit drafting. EasyTrax comes complete with component libraries and print and plot softwares. EasyTrax is a tiny yet powerful CAD software and is the predecessor to Protel's Windows based software, AutoTrax. EasyTrax's powerful core runs well on older PC's without sacrifice of performance, making it easy for you to afford to set up a dedicated drafting workstation on an older, recycled PC!

With EasyTrax, you can

  • Draft, Edit or Modify PC Board Layouts
  • Print PC Board Layouts using Inkjet/Laser Printer or Pen Plotter
  • Create Gerber Plot Files for PC Board Manufacture
  • Create NC Drill Files for CNC Drill Machines
  • Create and Print Bill of Materials List
  • Contents

    System Requirements
    Downloading and Installation
    Setting Up Monitor
    Windows Setup
    Running EasyTrax for the First Time
    Making Your Way Through EasyTrax
    EasyTrax Command Menu
    Hotkeys and Special Navigation Aids
    Printing and Plotting
    How To Use EasyPlot
    EasyPlot Command Menu
    Running EasyPlot for the First Time
    Printing Out Your Layout
    Layers
    Printing Layouts for PC Fabrication
    Creating Bill of Materials List
    Quick Procedures Guide

    System Requirements

  • IBM compatable PC

  • 286 Processor running DOS 6.0 or higher, ROM DOS 3 or higher or Windows 3.1, Windows 3.11

  • 386 Processor or higher running DOS 6.0 or higher, ROM DOS 3 or higher or Windows 3.1, 3.11, 95 or 98 ** Now Compatable with Windows XP! **

  • 4M of RAM (DOS,286) 16M RAM (Windows)

  • 2M hard drive space (or more for saving PCB files)

  • color VGA monitor 640 x 480 (800 x 600 recommended)

  • mouse

  • Serial port or parallel port for printer/plotter

  • laser/inkjet printer or pen/laser plotter

  • Notes on System Requirements:

  • Use of a trackball or touchpad as a pointing device is not recommended.
  • EasyTrax now runs under Windows NT, Windows 2000, Windows ME or Windows XP.
  • EasyTrax does not support USB printers/plotters. USB mouse can be supported by installing appropriate DOS driver or by using Windows.
  • EasyTrax will run under MacWindows (Macintosh) but printer compatability is not yet documented.
  • Downloading and Installation

    Before downloading, create a directory on your hard drive called ET. You will download the EasyTrax installer to this directory. If you plan to save the file to a floppy and install it on another PC, you do not have to create this directory.

    Download EasyTrax by clicking Here (IBMEZCAD.ZIP Filesize=400K).

    NOTE: If you are using Windows XP, skip to the section, "Installing Under Windows XP".

    If you plan to install the software on the same PC as you used to download the file, log off the internet and unzip the compressed file into the C:\ET directory from Windows using WinZIP, or exit to DOS and use PKUNZIP to extract the files. If you plan to install the software on another PC, save the downloaded file to a floppy, then copy the file onto the other PC in the C:\ET directory. Note: EasyTrax is a Shareware program so feel free to pass a copy on to a friend!

    Next, from Windows, go to Start, Run and type sysedit then click OK. Add the following line to your AUTOEXEC.BAT file:

    PATH C:\ET

    If you already have a PATH statement in your AUTOEXEC.BAT file, then add:

    ;C:\ET

    to the end of the line. Be sure to Save before exiting Sysedit.

    Before continuing, restart your PC, this time in the MS-DOS mode.

    Installing Under Windows XP

    Extract the compressed files in the C:\ET directory.

    Follow the directions in the section below, "Windows Desktop Setup". Be sure to follow these directions carefully or EasyTrax will not run under Windows XP.

    Windows Desktop Setup (Windows 95, 98)

    You can set up EasyTrax to run from your Windows desktop. You can do this by following these steps:

    1. Restart your PC to the regular Windows desktop.

    2. From the START button, run Accessories, Windows Explorer (Windows XP: Go to My Computer instead of Windows Explorer.).

    3. Scroll down the left side of the Explorer window. Locate and open the ET folder.

    4. Locate the file easyedit.exe on the right side of the Explorer window. Click this file ONCE to highlight it, then RIGHT mouse click. Select Create Shortcut.

    5. Once Windows has created the shortcut, left click the shortcut file and drag it onto the desktop.

    6. Do the same for the file easyplot.exe by repeating Steps 3, 4 and 5.

    7. Close the Windows Explorer window (Windows XP: Close the My Computer window.).

    8. On the desktop, locate each of the shortcut files you just created. Locate the shortcut for Easyedit.exe.

    9. RIGHT click the icon for Easyedit.exe and then select Properties.

    10. From the Properties dialog box, select the Program tab. Set Run to Normal Window and check the Close on Exit box. Then click on the Change Icon button. In the File Name box, type C:\ET\Easyedit.icn then click OK.

    11. Select the Screen tab. Check the Full Screen button, Restore settings on Startup, and Fast ROM Emulation.

    12. Select the Misc tab. Set mouse to QuickEdit mode.

    13. Click OK and close the Properties box.

    14. Repeat steps 8-13 for the easyplot icon. Use the file name easyplot.icn for the file name in the Change Icon box.

    Setting Up Your Monitor

    EasyTrax uses its own VGA driver. To set up your monitor, run the GraphSet program. From the C:\ET prompt, type graphset and then Enter. (Windows XP: Click Start, Run, then enter "C:\ET\graphset.exe" (no quotes) and then click OK.)

    Select VGA 640 x 480 mode, REGARDLESS of what type of monitor you have. You can go back and play with this setting later but for now use this setting because it is known to work well on ALL monitors.

    NOTE:  The driver used by EasyTrax is only used by EasyTrax and is unloaded after each use. The new driver will NOT replace any current drivers loaded on your PC.

    Using Protel EasyTrax

    Preparing to Run EasyTrax for the First Time

    Run the EasyTrax program from MS-DOS by typing easyedit, then Enter, or from Windows by double-clicking the Easyedit icon on your desktop.

    When the program first launches, it will put up a splash screen. This splash screen should be grey with black lettering and a yellow swoosh. If you do not get this screen, review the installation process and try again. You may have to change your monitor settings using Graphset (although this is highly unlikely).

    From the splash screen, click the mouse or type any key to bring up the drawing board. At this time, EasyTrax will ask you for a filename to open. To cancel this, type the Esc key.

    A Note to Windows XP Users: Since EasyTrax is a program originally written to run on MS-DOS versions 6 or earlier, filenames MUST be no longer than 8 characters in length and contain no spaces. Furthermore, the entire path statement (C:\easytrax\directory\directory\directory\.....\filename.pcb) MUST be less than 32 characters in length. If you save your file in a long pathname and EasyTrax fails to launch (you get an error message on your screen or the computer crashes), move the file to a shorter pathname. Example: If your file is in the directory, C:\easytrax\newproj\pcboards\input\keybrd\keybord.pcb , you are going to get an error message when you try to access this file. Either Windows XP cannot let you see the file at all, or if you set up your PC so you can double-click a PCB file and automatically launch EasyTrax, you will get an "NTVTM" error. To fix the problem, simply move the file you wish to open to a shorter pathname -- move the file C:\easytrax\newproj\pcboards\input\keybrd\keybord.pcb to the directory C:\easytrax or create a directory called C:\easytrax\work and always use the \work directory to create your PC board, then save your work in the longer pathname later.

    Making Your Way Through EasyTrax

    Navigating EasyTrax is easy!

  • From the draft screen, the LEFT mouse button brings up the Command Menu.
  • The RIGHT mouse button cancels or terminates any action and closes the Command Menu.
  • The Space Bar on your keyboard is used to rotate any library entity.
  • Arrow keys on your keyboard will move the cursor one step at at time.
  • You can customize hotkeys for easy access to common features
  • At the bottom of the EasyTrax window you will see a line of information. This line shows in order:

    X: the X-axis position of the cursor (in mils from 0,0 left bottom edge)
    Y: the Y-axis position of the cursor (in mils from 0,0 left bottom edge)
    L: Current Layer
    the color bar shows the current draft color for the current layer
    P: the current Pad Type in use
    T: the current track width selected
    S: the current string (alpha character) size in mils
    G: the current Snap to Grid spacing size

    EasyTrax Command Menu

    EasyTrax has a robust command menu. Each of the command menu features will be explained in the following section.

    Block

    Block commands allow you to manipulate large sections of the draft all at once.

    DefineSets the boundries of the block. Select the block area by first selecting the first or starting corner, then the ending or final corner.
    HideGets rid of the block definition.
    MoveMoves the entire area defined as a block to another place on the layout. You can move only the current layer or all the layers.
    CopyCopies the contents of the defined area. You can copy only the current layer or all layers. When copying components, EasyTrax will automatically asign new part numbers to the newly created components. For example, if R1,R2 and R3 are copied, they will appear as R4,R5 and R6 in the copied area.
    Inside DeleteDeletes everything INSIDE the block area. You can choose only the current layer or all layers.
    Outside DeleteDeletes everything OUTSIDE the block area. You can choose only the current layer or all layers.
    ReadReads an entire PCB layout file into the current layout as a block. This is a powerful feature when designing using modular blocks. You can select the current layer or all layers.
    WriteSaves the defined area as a separate PCB layout file. This is great when writing modular PCB layouts.

    Current

    Current sets and displays the current drawing, cursor, pad, and track settings.

    Cursor ModeSets the cursor mode to Absolute or Relative (absolute is default).
    Floating OriginSets the location on the draft board the cursor first appears when the software is launched. Great for saving your cursor position in the event you have to stop and finish the draft later.
    LayerSelects the current draft layer. You can also select the layer using the + key.
    Pad TypeSelects the current pad style and type used.
    Pad OrientationChoose between normal and rotated pad placement.
    Track WidthSelects the width of the track to be drafted. You can choose from 10 mils to 100 mils.
    String SizeSelects the size of alphanumeric text you can write on a layout.
    Via SizeSelects the size of via holes used on multi-layer boards.
    Arc Line WidthSets the size of the lines in arcs and circles.
    GridSelects between Imperial and Metric grid spacing (mils or millimeters)

    Delete

    Delete allows you to select the type of entity to be deleted, followed by a selection made by positioning the cursor on the desired matching entity and clicking.

    Example: To delete a pad, choose Delete, Pad, then click on the desired pad to be deleted. If you accidently click on a track or something else, the entity will not be deleted. This is a safety protocol to help prevent accidental deletions.

    Edit

    The Edit command allows you to change parameters of individual entities. For example, say you place a Round62 pad and later you realize it needs to be a Square85 pad. You can select Edit, Pad then change the pad type and size.

    File

    The File command contains file and disk functions.

    ClearClears the draft pad. Removes all tracks, entities and strings. Begins a new draft. After executing a CLEAR, do NOT execute a SAVE unless you KNOW your new file name, otherwise EasyTrax will overwrite the current draft with an empty draft pad!
    DosNOTE: Use this command ONLY if running the software under MS-DOS 6.0. DO NOT USE if running under a Windows MS-DOS Prompt!! The DOS command brings up a MS-DOS screen without exiting the EasyTrax software.
    FilesSimilar to the DOS DIR command. Lists all files in the current directory.
    LoadLoads a PCB draft file.
    PathSets the current MS-DOS path. Use this command to set the path if you plan to change component libraries frequently or plan to backup your work on a separate directory.
    QuitExits the program and returns you to the MS-DOS prompt (or back to the desktop if running from Windows). EasyTrax will prompt you to save before exiting.
    SaveSaves the work on the draft board. If you are continuing a previous layout, it will automatically save to the same filename as the loaded filename. If you used the CLEAR command to begin a new draft, be SURE to rename your file or you will overwrite the old one!

    Grid

    The Grid command sets the current draft grid settings.

    Snap GridSets the spacing the cursor snaps to in mils. Each touch of the arrow keys will move the cursor one snap grid space. Recommended setting is 25 (.025").
    Visible GridSets the distance between the drafting aid dots on the screen. Recommended setting is 100 (.1").

    Highlight

    The Highlight command highlights particular elements by changing them to a unique color. This is an essential aid in helping you route tracks or determine proper interconnections.

    ConnectionHighlights a single pad.
    DuplicateCopies the highlighted area and places it in a new location. Does not remove original highlighted area. Similar to Block, Copy except this feature acts upon a single highlighted track, pad or arc.
    NetHighlights an entire circuit path. Very useful for tracing the electrical connection from point A to B and beyond.
    Make NetlistExtremely useful tool which defines every interconnect on the board and lists them in a text format. Saves to file with .net extention.
    Reset HighlightTurns off any highlight and resets software for a new highlight.

    Information

    The Information command displays current information about board size, number of holes, memory status and what components you have in the library.

    Jump

    The Jump command will reposition the cursor at the location specified. This is a killer tool when locating a component on the board by component number. For example, you have drafted a huge PCB and the parts range from R1 to R174. Where is R86? The JUMP, Component command will take you straight to that component!

    Library

    The Library command allows you to manipulate elements of the component libraries.

    AddAdds a new component to the library. To do this, first layout the component with pads, tracks, arcs, and strings, then use Block, Define and select the entire region which makes up the new component. Then use Library, Add to add the newly defined component to the currently selected component library.
    BrowseLets you browse the current component library.
    SelectSelects a component from the library to use. You must select a component before you can use the Place command.
    CompactDeletes duplicate components from the library and compresses the library file.
    DeleteDeletes a particular component from the current library.
    ExplodeBreaks down a library component into primatives. For example, it would break a 16-pin DIP chip into 16 individual pads.
    FileUse to select the current library file. All file libraries end in .lib extention.
    ListShows a listing of all the library files in the current directory path.
    MergeCombines two libraries into a single library.
    New LibraryCreates a new library file.
    RenameRenames the current library file.

    Move

    The Move command allows you to move components, tracks, arcs or any other entity around the draft pad freely.

    Place

    The Place command is used to place items on the draft board. It will be the most frequently used command. Here are some things to remember about the Place command:

    Arcs Be sure you have selected the correct arc line width. Use the ARROW keys to select arc segments and arc size. Arcs increment in size in steps set by Snap Grid.
    Components Be sure you have selected the correct library component.
    Fills Fills only fill on the currently selected layer and cannot be edited.
    Pads Be sure you have selected the correct pad size and type.
    Strings Be sure your string is on the correct layer and is the right size. You can edit strings for text content and size but you cannot change the layer they are on.
    Route This is the EasyTrax auto-router. It works under a design rule you have no access to. It is not recommended to use this command unless you have completely given up trying to route a track. The Route command is not recommended for use because it will follow the built-in design rules regardless of how simple a board layout is and by doing so may complicate the layout by creating vias and double-sided layouts when a single sided layout is adequate.
    Track Be sure you have selected the correct track width for current and spacing. 15 mils is the largest track capable of making it between chip pins.
    Via Do you need a via or a pad? Simplify your design by making component leads feed-thrus on double-sided boards as often as possible.

    When using the Place command, and especially when placing components, the EasyTrax program will prompt you to enter comments on what type of component you are placing. For example, if you place an axial.5 (typical resistor), you will be prompted to enter the Component Designator and Comment. Here you can enter R1 for the designator and 100K as the value of the component if you know your part designator and value. It is important to enter these values because later you may wish to use the Bill of Materials (BOM) program to create a parts list. The BOM program strictly uses these comment fields to create the BOM file.

    EasyTrax will also auto-increment the component designator number. For example, if you place an axial.5 (typical resistor) and enter R1 as the component designator, the next time you place an axial.5 "R2" will automatically be entered for you as the component designator. Also, if you delete a component, the designator of that component will automatically be used as the next available designator for that component type the next time you use that particular component type.

    Repeat

    The Repeat command repeats the last action. This is very useful when setting up data buses, arrays or ground grid areas.

    To use the Repeat function, place the entity to be repeated first using the Place command. Then using Repeat, enter the X and Y offset values and the number of items to be placed minus 1.

    X offset is how far apart the entities are to be on the X axis and Y offset is how far apart the entities are to be on the Y axis. If you use 0 as the offset, there will be no action on that particular axis. Action occurs from bottom to top, left to right.

    Example: Place 10 pads in a row from left to right 200 mils apart.

  • Place the first pad on the far left side of the array using the Place command.
  • Open the Repeat command.
  • Set X offset to 200
  • Set Y offset to 0
  • Set Count Default to 9
  • Execute Repeat

  • Setup

    Use the Setup command to adjust screen colors, redraw quality, turn on and off draft layers and select optional features.

    Component TextSets parameters involving the text displayed on the Overlay layer. Use of the overlay layer is not recommended. If a component legend is required, it is recommended to use one of the mid layers instead.
    Layer ColorsSelects the color for each draft layer. You can only change colors on layers which are active. The standard colors for the common layers are Top: Red, Bottom: Blue, 1 Mid Layer (use as legend layer): White, MultiLayer (pads): Dark Red, Background (Draft Pad): Grey, Highlight (also color of draft aid dots): Fluorescent Green.
    Menu ColorsSelects the color of the information bar and text at bottom of screen, shadows, and other miscellaneous items.
    KeysUsed to customize hotkeys. Changing these settings is not recommended until you are very familiar with EasyTrax features. The default settings are as follows:
    F1-Place Pad F2-Delete Pad F3-Place Track F5-Zoom Out F6-Zoom In F7-Drag Broken Track (hidden feature not in Command menu)
    OptionsUsed to set up draft features.
    RedrawSets the quality of the redraw of the draft board when zooming in and out or panning up/down/left/right.
    StringsSets the size of strings used on the Overlay layer.
    Toggle LayersTurns on and off draft layers. You will most likely only have the Top, Bottom, 1Mid, and MultiLayer on.

    UnDelete

    The UnDelete command restores deleted entities. Enter the number of past deletes you wish to restore and they will reappear.

    Zoom

    The Zoom command is used when you wish to change the perspective of your viewport. You can zoom in (Contract), out (Expand), pan or select an area to zoom in on. You can also redraw the screen, which is sometimes useful after placing components.

    Hotkeys and Special Navigation Aids

    To make your drafting experience easier and more productive, EasyTrax makes use of hotkeys and special navigation keys.

    The default settings of all of the hotkeys are listed in the table below. Study these carefully because some of the most basic functions are embedded in the hotkeys and may be difficult or cumbersome to access using the mouse and the Command Menu.

    F1Place Pad. Places a pad at the location of the cursor.
    F2Delete Pad. Deletes the pad at the location of the cursor. If you cannot delete the pad marked by the cursor, the pad may be part of a library component. Use the Library, Explode command to break library components into primatives.
    F3Place Track
    F5Zoom Out
    F6Zoom In
    F7Drag Broken Track. Drags a track from the point of the cursor. Breaks track into two entities in the process.
    F8Delete Track. Deletes the track at the location of the cursor. If you cannot delete the track marked by the cursor, the track may be part of a library component. Use the Library, Explode command to break library components into primatives.
    PgUpZoom In
    PgDnZoom Out
    "+" and "-" KeysSwitches current draft layer.
    Space BarRotates library components 90 degrees per keystroke. Use to correctly orient library components.
    Arrow KeysMoves cursor exactly one snap grid space. Use this feature to zero in on exact spacing when positioning components or dragging ends.
    Shift+x(Shift Key held down while pressing the "X" key) Flips library components, text and arcs horizontally. Very useful when aligning transistors or other polarized components.
    Shift+y(Shift Key held down while pressing the "Y" key) Flips library components, text and arcs vertically. Very useful when adding text to the BOTTOM LAYER of the board so that it comes out legible when viewed from the bottom.
    EscCancels any action and returns cursor to draft board.

    You can zoom in or zoom out, or change the visible or snap grids while at the same time you are placing components, arcs, tracks or fills. To do this, you would first be using the Place command (such as Place Component). Simply press and hold down the SHIFT key while pressing the Z key for zoom and the SHIFT key along with the G key for grids. You can also zoom at anytime using the PgUp and PgDn keys.

    You can also type the first letter of each command to access that command. For example to perform a Highlight, Net you can type HN; to perform a Place, Track you can type PT. These shortcuts are not case sensitive.

    You can also create custom hotkeys by using the Setup, Keys command.

    Printing and Plotting

    EasyTrax comes with a complete print and plot package called EasyPlot. Use EasyPlot to create:

  • PCB Artwork Drafts
  • Component Placement Guides
  • PostScript Files
  • Pen Plotter plots
  • Laser or Inkjet Printer plots
  • Direct to Film Layout Sheets
  • Gerber Plots or Gerber PCB Files
  • Drill Files for CNC Drill Machines
  • How To Use EasyPlot

    Launch the EasyPlot software by typing easyplot at the C:\ET prompt, or by clicking on the EasyPlot icon on your Windows desktop. You can run EasyEdit and EasyPlot at the same time from Windows.

    When EasyPlot first launches, a splash screen will appear. The splash screen is black backgrounded with a grey and red logo in the center. If you do not get this screen, review your installation process and try again.

    EasyPlot Command Menu

    Much like EasyEdit, EasyPlot has a robust command menu. Each of the commands will be explained in the following section.

    File

    The File command contains file and disk functions.

    DosNOTE: Use this command ONLY if running the software under MS-DOS 6.0. DO NOT USE if running under a Windows MS-DOS Prompt!! The DOS command brings up a MS-DOS screen without exiting the EasyTrax software.
    LoadLoads EasyPlot with the file to be printed.
    PathSets the current MS-DOS file path. Use this command when you are using files from the same directory or need to locate files in another directory.
    FilesSimilar to MS-DOS DIR command. Lists all files in the current directory.
    QuitExits the program and returns to the MS-DOS prompt (or to the Windows desktop). All changes and settings made during the current session will be saved.

    Information

    The Information command provides current information about the file you are about to plot. You can see the X and Y measurements, holes in layout and enlargement scale.

    Options

    Use the Options command to set particular parameters about each plot. Below are some notes on certain commands provided under Options.

    Type of PlotSelects which layer of the PCB layout is to be plotted.
    Board Layer, Pads, Vias, StringsToggles on or off these particular components of the layout. Use this to turn off unwanted pads or other components during specialized plots.
    Pad Hole Guide SizeSets the size of the guide hole plotted in the center of each pad. This tiny hole is crutial if you are manually drilling holes. The recommended setting is 5 mils.
    Drill Draw Symbol SizeSets the size of the characters used on the Drill Drawing function. Default setting is 100 mils.
    Solder Mask EnlargementThe Solder Mask plot is created from a combination of pads and vias and several other entities. Solder mask is used during manufacture to prevent wave solering machines from soldering places it shouldn't. It is common to make the solder mask 5 mils larger than the pads or vias. This is to prevent the solder mask ink from running onto the pads or filling up the via holes. Recommended setting is 5 mils.
    Board Layer, Pads, Vias, StringsToggles on or off these particular components of the layout. Use this to turn off unwanted pads or other components during specialized plots.
    PWR-GND EnlargementSimilar to Solder Mask Enlargement, this function sets the enlargement size for the clearance between the power and ground layers and the pad/via holes. The recommended setting is 7 mils.
    Grid TypeSelects between Imperial or Metric grid types (mils or millimeters). This setting MUST match the setting used in EasyEdit.
    Flip Layer SetupThis command will open up a sub menu where you can set the orientation of each layer's plot. Select NORMAL to plot as you see it on the screen, or Flipped to invert horizontally the entire layer.

    Setup

    Use the Setup command to set up specific parameters of the software to work with your particular printer/plotter.

    Serial PortSelects which serial port EasyPlot will use to communicate with your printer/plotter. Ignore this setting if you are using a parallel printer.
    Check PlotToggles on or off particular components of the layout. Use this to turn off unwanted pads or other components during check plots ONLY.
    PlotterUse this command to tell EasyPlot what type of pen plotter you have and the specifics about how it is to plot. Ignore this setting if you are not using a pen plotter.
    Printer and PostScript Commands.  Use these commands to set up and use your laser or inkjet printer to plot PCB layouts and to create PostScript files or drive a PostScript compatable printer.
    TypeSelects the printer driver (or PostScript driver) used by EasyPlot. If you cannot find a printer driver for your particular brand or model printer, use the one that is the closest match. Most drivers are very similer and will work good most of the time.
    DeviceSelects where EasyPlot is to output the printer data. You can select to send it out a serial port, a parallel port or save it to a file.
    ScaleSets the enlargement/reduction scale. Default setting is 1.000.
    X and Y OffsetSets the X and Y offset from 0,0. Useful on large layouts to create a small border around the layout. Default setting is 0.000.
    X and Y CorrectionSets the correction factor. Typically this is set to 1.000.
    OrientationSets the print orientation. Choose from Centered, Normal or Rotated.
    QualitySelects between Draft or Final Artwork mode.
    PaperSets the type of paper used in your printer. EasyPlot will recognize sheet (paged) paper or continuous roll.
    OptionsSets the print options. You MUST set these options although you probably already have under the Options command. See the Options Command for more information on each of the commands in the sub-menu.
    Gerber.  Use this command to create Gerber Plots for commercial manufacture of your PCB design. You can view Gerber Plots using GCPREVUE. To make your life easier, you can also download the common aperture files used by EasyPlot and GCPREVUE.
    EasyPlot Aperture Table
    GCPREVUE Aperture Table
    Output FileNames the file used to save the Gerber information.
    X and Y OffsetSets the X and Y offset values from 0,0 mils.
    Aperture TableUse this command to select which aperture table to use. Creating aperture tables is an advanced function and is not for the beginner. It is highly recommended to download a modified version of the standard aperture table by clicking Here.
    Match Oversize and UndersizeGerber plots are made by panning, scanning or dragging a beam of light through an aperture onto a photographic film. To create the circuit entities, each entity must consist of single apertures or combinations of apertures which can be assembled to create the entity. Each entity must match an aperture or set of apertures closely. These settings allow you to set the deviation from absolute match the Gerber plotter can be when assigning matches. Example: If you have a pad that is 71 mils in size, the Gerber plot must either have a 71 mil aperture or be able to closely create it using multiple apertures. If the closest it can come is 70 mils and you have the Undersize Match set to 2 mils, then the Gerber plotter will use the 70 mil aperture.
    G54G54 is a type of Gerber plot file format. It adds some particular information to the beginning of the file to help the plotter locate the board origin. Contact your board manufacturer to determine if you need to use G54 or not.
    Arc QualityWhen set to ON, all arcs will be solid and fully filled. When set to OFF, arcs will be a near dotted line.
    Software ArcsDetermines the width of arcs used by the Gerber plotter. Leave this setting at 5 mils.
    OptionsSets the particulars about each plot. You MUST set these settings although you most likely already have using the Options command. See the Options command for more information on using this sub-menu.
    NC Drill.  Use this command to create NC Drill files used to operate CNC mill drilling machines. To make your life easier, you can also download the common tool table file used by EasyPlot.
    EasyPlot Tool Table
    You can also obtain information on how to build your own CNC Drill machine by visiting Hobby CNC.
    Output FileNames the file used to save the NC Drill files. EasyPlot outputs two files, one in DRL format for Japanese machines and one in text format for standard CNC X-Y-Z axis drilling mills.
    X and Y OffsetSets the X and Y offset values from 0,0 mils.
    Tool TableUse this command to select which tool table to use. Creating tool tables is an advanced function and is not for the beginner. It is highly recommended to download a modified version of the standard tool table by clicking Here.
    Batch ModeEasyPlot allows you to print all of the files you need at once, saving time. Use this command to select which layers you wish to plot in a batch mode session.
    PensUse this command to inform EasyPlot of the type of pens your pen plotter uses. Refer to the User's Guide for your pen plotter for this information. Ignore this command if you are not using a pen plotter.
    Meun ColorsYou can customize the EasyPlot screen by selecting colors for the menu features and background.

    Plot, Print, PostScript and NC Drill Commands

    Use these commands to print or plot, create PostScript files or NC Drill files.

    Gerber Plot

    Use this command to create Gerber plots. During this process the program will prompt you with several questions about matches. Use the default settings for each of these for best results. If the program finds that it cannot find a match, the program will prompt you to select between a Flash Match, a Stroke Match or a Paint Match. Each of these match techniques have unique properties which you must choose from. The choice is dependent on the type of entity to be matched.

    It is best to use Flash matches for pads, fills or any "singleized" entity.

    Use Stroke Match for tracks, edge connector pads or large area fills.

    Use Paint Match for strings, odd shapes, triangles, etc.

    Tips and Techniques

    Once you have studied the command menus, you are now ready to use EasyPlot. In the example to follow, it will be assumed that you will be using a laser printer connected to the LPT1 printer port.

    Running EasyPlot for the First Time

    Before EasyPlot will do anything, you must first set up the printer, driver and ports. Use the Setup command in conjunction with the Printer command to set up your printer and driver.

    If after viewing your layout from the printer you wish to create Gerber plots, you will also need to setup the Gerber plot function. Use the Setup, Gerber to set up Gerber plots. Be ABSOLUTELY SURE you have selected the correct aperture and tool table files. These files work in conjunction with each other to create the Gerber Drill Guide and place the correct hole size on the correct pad. If the aperture file and Tool Table are not a set, you may get strange results. It is strongly recommended to download these files from the Lupine Systems website and replace the ones which came with the software package. These files have been modified to contain ALL the apertures and tools used for the different pad sizes according to component/pad sizing requirements.

    Printing Out Your Layout

    Begin by loading the PCB file you wish to plot by using the File, Load command. Once the file is loaded, EasyPlot can tell you more about your plot by opening up the Information command.

    Next, use the Setup, Print command to select which layer you wish to print. You can also use the Setup, Batch Mode to select multiple layers to print. If you use Batch Mode, select Batch Mode under Setup, Printer to select Batch Mode printing.

    NOTE:  When printing in Batch Mode, EasyPlot will print all entities selected under Setup, Printer. On certain prints, such as the Legend Layer (1MidLayer) you may not wish to print pads and vias. It is best to only use Batch Mode to print Top and Bottom Layer and then come back for a second pass for the Legend Layer.

    Layers

    EasyPlot will print all of the draft layers created by EasyEdit and several additional layers which can be derived from the data contained in the EasyTrax PCB file, the aperture table and the tool table combined into a single database.

    Below is an explination of each of these plots.

    NOTE:  Multi-layer boards are defined as boards which have layers between the top and bottom exposed sides of the board. Double-sided boards are NOT multi-layer boards by industry definition.

    Top LayerTop or parts side layer of PCB layout.
    1 Mid LayerFirst internal layer on multi-layer boards. Used by Lupine Systems as the Legend Layer (component placement layer).
    2 Mid LayerSecond internal layer on multi-layer boards.
    3 Mid LayerThird internal layer on multi-layer boards.
    4 Mid LayerFourth internal layer on multi-layer boards.
    Bottom LayerBottom or solder side of PCB layout.
    OverlayIntended to be the component placement layer (Legend Layer) but does not work well. Not recommended for use.
    Ground PlaneSolid copper internal layer ground plane used on multi-layer boards.
    Power PlaneSolid copper internal layer power plane used on multi-layer boards.
    Top Solder MaskThis plot is used to create the top solder mask screen. It is typically created by taking all of the pads and vias and enlarging them slightly according to the setting under Setup, Solder Mask Enlargement.
    Bottom Solder MaskThis plot is used to create the bottom solder mask screen. It is typically created by taking all of the pads and vias and enlarging them slightly according to the setting under Setup, Solder Mask Enlargement.
    Pad MasterPrints out only the pads. Removes all vias, tracks, fills and arcs.
    Drill DrawingCreates a plot showing where all the holes are located along with the drill size according to the Tool Table file.
    Drill GuidePrints out a plot which can be used to guide the drill if drilling on an unetched PCB. Not very useful for hobbyists and not recommended for use.
    Batch ModeSelects which of the above mentioned plots which will be included in a batch operation.

    Once you have selected which plot you wish to print, you will be ready to print out your layout!

    Printing Layouts for PCB Fabrication

    It is highly recommended to print out a paper copy of your layout FIRST before printing out a final sheet of film. This way you can proof your plot and prevent expensive waste of acetate film.

    Once you are satisfied with your plot on paper, you can now print it out on acetate film. It is recommended to use a film which is compatable with the type of printer you are using. 3M makes several types of coated films specifically made for inkjet or laser printers. All of these films are available in 25, 50 and 100 quantities from most office supply warehouse stores.

    Remember when plotting the Bottom Layer it will appear as an X-ray view.

    Also, you can touch up plotted artwork by using a Sharpie Pen.

    Single sided layouts are simple and have little or no frills to them, but double-sided layouts must be exact matches when it comes to the pads. Some printers introduce non-linear errors to the print media. You can detect this by placing the top and bottom layers on top of each other and verifying that each layer's pads align with each other. If they don't, you will have to reprint each layer until you have a match.

    Here are some tips when printing on acetate film:

  • Load each sheet one at a time. Do not stack the sheets together in the paper bin.
  • Handle the sheets by the edges ONLY. Do not touch the center of the sheet.
  • Do not feed paper along with the acetate. It is NOT a wise idea to double feed printers.
  • Use the correct film for your printer. Do not use uncoated film in an inkjet printer!!
  • If using a laser printer, set the darkness to 3/4 dark, NOT FULL DARKNESS!! Laser printers tend to wash out solid objects on film due to an overload of toner.
  • Be sure you have a known good toner cartridge or ink cartridge installed!
  • Creating Bill of Materials/Parts List

    EasyTrax provides a program which creates a Bill of Materials for you. No more counting up components!

    To create a bill of materials, run the BOM program. You can do this from your DOS prompt by typing BOM (filename.pcb) (filename.bom) where filename.pcb is the EasyTrax PCB file you wish to create a Bill of Materials for, and filename.bom is the Bill of Materials file.

    The Bill of Materials program will prompt you to select between a Summarized form or a Detailed form. The difference between the two is the way it lists the components. For most applications the Summarized form works extremely well.

    The Bill of Materials file is created from the EasyEdit PCB file's comment fields, therefore it is important to fill in these fields while drafting. You can go back and edit these fields by using the Edit, Component command from the easyedit program.

    If you created "custom" components in your layout, these custom components will not show up on your BOM. To avoid this, each time you design a custom component, save it in the library as a new component, then delete your "custom" component and replace it with the library version. This way EasyTrax will prompt you for a component designator and comment when you place the library component.

    Quick Procedures Guide

    Here is a guide of the typical procedures followed to produce a complete PCB package.

    1. Draft PC board using EasyEdit, or obtain pre-drafted PCB file.
    2. Load PCB file into EasyPlot.
    3. Be sure printer/plotter is properly set up.
    4. Select layers to be printed/plotted and proceed with plot on paper.
    5. Review plots, then print plots on acetate film.
    6. Blow a prototype PC board and test your circuit.
    7. If everything passes OK, then proceed with Gerber plots.
    8. Setup Gerber plots by selecting correct aperture and tool table files.
    9. Gerber plot each layer necessary to produce your PC board.
         Typical files to plot will be Top Layer, Bottom Layer, 1 Mid Layer
         Top Solder Mask, Bottom Solder Mask, and Drill Drawing
    10. Run the NC Drill function to create NC Drill file.
    11. Run the Bill of Materials program to create your parts list.
    12. Write a brief READ.ME file stating PC board requirements, assembly information.
    13. Use WinZip or PKZip to compress your files into a single package.
    14. Send your ZIP file to a PC board house for quotes or manufacture.

    Copyright (C) 2001 Spike Tsasmali, Lupine Systems
    All rights reserved
    EasyTrax is a trademark of Protel International, Ltd, Australia

    Back to Lupine Systems Homepage
    Back to PC Board Page