CD School House 9

home *** CD-ROM | disk | FTP | other *** search

/ CD School House 9 / CD School House 9.0 - Wayzata Technology (1994).iso / pc / dos / graphics / easytrax / read.me < prev

Wrap

Text File | 1992-07-10 | 56.1 KB | 1,657 lines

Protel Easytrax (DOS) Freeware version 2.06 Reference Manual Text File - Read.me Note: This text file is derived from the original Protel Easytrax reference manual. The file is approximately 35 A4 pages long. We suggest that you make a hardcopy for reference when using the Easytrax program. Copyright Notice This freeware (including this textfile) may be copied and passed on to others for non-commercial use, provided the notice of copyright shown below is placed on the label of the copied disk and that no alterations or changes are made to the software, this textfile or Copyright notice, below. All other rights are reserved. Software Copyright (c)1988 Protel Technology Pty. Ltd. Original Reference Manual Copyright (c)1988 Protel Technology Pty. Ltd. READ.ME Copyright (c) 1992, Protel Technology Inc. Please read the following disclaimer of liability before using the software. If you do not accept fully the terms and conditions of use described below, do not use the software. THIS FREEWARE VERSION OF PROTEL EASYTRAX IS SUPPLIED WITHOUT WARRANTY OF ANY KIND INCLUDING , BUT NOT LIMITED TO ANY IMPLIED WARRANTIES OF MERCHANTABILITY OR FITNESS FOR ANY PURPOSE. UNDER NO CIRCUMSTANCES SHALL PROTEL TECHNOLOGY NOR ITS AGENTS, HEIRS OR SUCCESSORS BE LIABLE FOR ANY DAMAGES, INCLUDING CONSEQUENTIAL, INCIDENTAL OR SPECIAL DAMAGES ARISING DIRECTLY OR INDIRECTLY FROM ITS USE. Protel and the Protel logo are registered trademarks of Protel Technology Pty. Ltd. Easytrax is a trademark of Protel Technology Pty. Ltd. Epson FX-80 is a registered trademark of Epson America, Inc. Hercules is a trademark of Hercules Computer Technology. IBM is a registered trademark of International Business Machines Corporation. Microsoft is a registered trademark of Microsoft Corporation. MS-DOS is a registered trademark of Microsoft Corporation. Contents Introduction Installation instructions Tutorial section 1 Tutorial: Getting started Loading the demonstration board Using the menus Identifying items on the board Getting information about the board Jumping to components and pins Some special keys Speeding up menu selections Quitting from the program 2 Tutorial: Laying out a PCB Getting started Placing components Laying tracks Connecting to power and ground planes 3 Tutorial: Plotting a board Starting the program Loading the DEMO file Overview of plotting a board Setting the serial port parameters Choosing the plot type Loading the plotter driver Setting the pen parameters Plotting the board 4 Tutorial: Gerber plots Setting up a Gerber plot Creating the Gerber file Plotting the pad master 5 Options Summary INTRODUCTION This freeware is not copy protected and we encourage you to pass it onto other interested people. Please feel free to make copies of the disk. All we ask is that our copyright notice is diplayed on the disk label. Protel Easytrax is a low-cost, yet powerful, software package for producing printed circuit board (PCB) artwork. It is a fully-featured system which runs on the IBM-PC/XT/AT and PS/2 series and close compatibles. The package has many advanced features including component library support and comprehensive plotting facilities. This text file describes how you can quickly and easily explore the powerful features of the accompanying Protel Easytrax freeware. Easy to learn and easy to use, Easytrax puts professional-quality PCB layout tools in the hands of students, hobbyists and part-time designers. Easytrax is the introductory-level member of the Protel family of Electronics Design Automation packages. Your Easytrax workfiles will be fully transferable to Protel Autotrax and Protel for Windows, our full-featured design packages that include powerful automatic component loading, placement, and autorouting capabilities, as well as support for SMD design. These packages accept schematic netlists from Protel Schematic and similar packages. Protel Easytrax provides everything you'll need to design through-hole, multi-layer PCBs. In less than an hour you could be designing your own printed circuit board following the steps outlined in the first two tutorials. You can also explore the powerful plotting routines by plotting the DEMO board supplied with the package on either a standard pen and ink plotter, a laser printer or a Gerber(rtm) format photoplotter. A note about performance: Protel Easytrax works on the complete range of IBM PC/XT/AT and PS/2 microcomputers and compatibles. The Easytrax freeware can be run from floppies but will run twice as fast from a hard disk. This program is delivered with a number of graphics drivers that support CGA, Hercules, EGA, Vega Deluxe, and VGA standard cards with resolutions of up to 1024x768 and 16 colors. If no graphics driver is installed the program will operate using CGA graphics. See the next section for installation instructions. Installation instructions The Easytrax freeware is archived so that it will fit on one 1.2Mb floppy disk (or two 360K floppies). To install the software on your hard disk please follow these steps: 1. Insert the disk in drive A: and type A:INSTALL at the C:\> prompt and press ENTER. 2. The installation is in three parts. The first screen prompts you to install the Easyedit (PCB editor) files. Press ENTER twice to accept the source and target drives. You will then be prompted to specify a directory on your hard disk. The default is \EASYEDIT. 3. You are then prompted to accept or change the previous selections. Unless you have made a mistake press Y to accept the previous selections. 4. The second stage of the installation is the copying of the Easyplot (PCB plot program) files. Repeat steps 2 & 3 above, the default directory will be \EASYPLOT. 5. Finally the graphics (video card) drivers are installed. Again repeat steps 2 & 3 above, the default directory will be \GRAPHDRV. Once all the graphics drivers are copied onto the hard disk a selection screen appears from which you should select the driver that suits your graphics card. If your card is not listed, or you are not sure what type it is, select the EGA or VGA640 option. 6. Installation is now complete and you are ready to run the Easytrax program. 1 Tutorial: Getting started This tutorial has been designed to give you a quick overview of the features of Protel Easytrax. Within minutes you will be gaining an insight into the way the program can be used to design printed circuit boards. In this tutorial you will learn the following skills: Starting the Protel Easytrax program; Loading the DEMO file; Using the pop-up menus; Expanding and contracting the display; Identifying items on the board; Using the cursor keys and the mouse; Using the cursor keys with the SHIFT key; Getting information about the board; Locating components, tracks, vias and pads; Changing setup options; Quitting from Protel Easytrax. Starting the Protel Easytrax program Change to the \EASYEDIT directory on hard drive C: and Type: EASYEDIT and then press ENTER. (You might need to move into a different directory before you start the program depending on the path you chose at installation) The banner screen appears. Press any key to move to the next screen. A window opens in the top left-hand corner of the screen. This is a standard input window which you see many times while using Protel Easytrax. Type DEMO and then either press the ENTER key or click the LEFT MOUSE button. (Note: If, at this stage you do not want to load a file, you can press ESC or click the RIGHT MOUSE button to bypass the loading option.) The message: LOADING FILE. PLEASE WAIT. appears, then a PCB file, showing a simple Z80 microcomputer layout is displayed. Notice the status line at the bottom of the screen which gives important information about the board and the position of the cursor. If you press the cursor keys a few times the numbers which indicate the position of the cursor change. The X and Y values are given relative to the position of the `origin' which always has an X value of 0 and a Y value of 0. It is written as X: 0 Y: 0. If you have not changed the position of the origin, it is in the bottom left hand corner of the board. To reach a position given by X: 500 Y:1000 when the cursor is at the origin, you move the cursor 500 mils to the right then 1000 mils upwards. Notice that all measurements are given in either mils or inches. A mil is one thousandth of an inch. Next to the cursor position on the status line is the currently selected layer. In Protel Easytrax, tracks can be placed on a number of layers. These include the Top Layer, the Bottom Layer and four Mid Layers. Components are placed on the Top Layer and silk screening is usually reserved for the Overlay. You can switch between these layers using the keys described at the end of this tutorial. Component pads, free pads and vias (through-holes) occupy ALL layers except for the Top Overlay. The line below the status line is used to display important messages. This line will display a prompt when some user action is required. This line is referred to as the prompt line in these notes. Using the menus Press the ENTER key or the click the LEFT MOUSE button and the MAIN MENU window appears. One of the options in the menu is highlighted. This highlight is called the Selection Bar. The bar can be moved with the mouse or the UP and DOWN cursor keys. You can `activate' or `select' a highlighted option by clicking the LEFT MOUSE button or by pressing the ENTER key. The demo circuit looks too small to work with easily, so it needs to be expanded. Choose Zoom from the MAIN MENU. Remember to make sure that it is highlighted, then click the LEFT MOUSE button or press the ENTER key to select the option. Select the Expand option. The screen is redrawn and the diagram shown in more detail. Select Zoom/Expand once again. Identifying items on the board Now move the mouse until the cursor is at X:1075 Y:3525. If you are not using a mouse, use the cursor keys. If you hold the SHIFT key down while pressing a cursor key on the numeric keypad, the cursor will move faster. As the cursor moves towards the position specified, notice that the screen may be redrawn once or twice. Remember that the cursor position is displayed on the status line. At X:1075 Y:3525 the cursor is at the junction of two tracks. These are the conductive lines which are usually placed on the top and bottom board layers. Thin tracks (e.g. 12 mils) are used for normal signals and thick tracks (e.g. 30 mils) can be used for the power supply. The horizontal track to the left has been laid on the bottom layer. The vertical track below the cursor is on the top layer. They are connected by a `via' which is a plated hole passing through the board which connects the tracks. Just to the left of the cursor is the outline of a component. It is a 14 pin chip. Notice at the top right of the chip there is a component designator U11 and a description showing that it is a 1488 chip. The component designator or reference designator usually consists of a letter indicating the type of component (e.g. U for an integrated circuit chip, C for a capacitor, R for a resistor and so on), followed by a number. If you are placing a number of identical components, once you have provided a reference designator for the first component eg. U1, subsequent components will be automatically designated U2, U3 etc, unless you manually enter a new designator. Notice that the component has 13 circular `pads' and one square `pad' The square pad is used to signify pin 1 on the chip. The pads are the place where the connection is made between the pins of the component and the tracks. Getting information about the board As the cursor moves towards the bottom left hand corner, notice that the screen may be redrawn once or twice. Remember that the cursor position is displayed on the status line. Select the MAIN MENU, then select Information. Choose the Status option from the Information window. Notice that information is provided about the number of components, pads, holes, arcs, fills, strings, tracks and vias. You will also notice that information is provided about the name of the current work file, the current path to the directory where the work files are stored and the name of the currently selected library. You can also check the amount of disk space and system memory that is available. Click RIGHT MOUSE or press ESC to exit from the Status window. Now choose Information/Board Dimensions. This window displays the dimensions of the board. Exit from this window and then choose Information/Components to see a list of the library components which have been placed on the board. Remember, click either mouse button or press the ENTER or ESC key to exit from each of these options. You can find more information about a particular component by using the Edit menu. Choose Edit and then choose Component. The message on the prompt line (just below the status line) prompts you to select a component. Move the cursor until it is positioned on the Z80 chip marked U5 (approximately X:1200 Y:1200). Now click LEFT MOUSE or press ENTER and a window opens showing the component designator, the library name (pattern), a comment and information about the layer and placement type. Click RIGHT MOUSE or press ESC to remove the window. Notice that the: SELECT COMPONENT prompt still appears on the prompt line. Click the RIGHT MOUSE button or press ESC again to exit from the Edit option. Jumping to components and pins Now choose the Jump option from the MAIN MENU. You can choose to jump to a place on the board by specifying a component, a location, a net, the origin, a pad or a string. This option will be extremely useful in the future when you are working with a large board. The Jump option is also useful if you want to identify the pin numbers for a component. Choose Jump/Component and you are asked to select a component. Notice that there is a question mark (?) on the left hand side of the window. This indicates that there is an information window available which will provide a list of components held in the memory of the computer. Click LEFT MOUSE and the window with a range of choices appears. Move the selection bar to highlight J2 (a DB9 connector), then press ENTER or click LEFT MOUSE. The cursor moves to that component on the board and is situated at pin 1. Now choose Jump/Pad. You will be asked to select a component. Since the cursor is already over the required component, press ENTER or click LEFT MOUSE. A window opens at the top of the screen prompting you to enter a pin number. Enter a pin number such as 5 then press ENTER or click LEFT MOUSE. Notice that the cursor moves to that pin. The window stays open allowing you to try other pin numbers. Press RIGHT MOUSE or ESC to exit from this window. Now choose the Setup option from the MAIN MENU. This menu allows you to change layer colors, menu colors, the default pad type and many other factors which affect the layout. Try changing the menu background color by choosing Menu Color then clicking LEFT MOUSE or pressing ENTER and observing the changes in color. Press ESC or click RIGHT MOUSE when you have finished selecting colors. By now you should be familiar with the menu structure of Protel Easytrax and some of the features of board layout. No attempt has been made to place components or tracks or to change layers. This will be done in subsequent tutorials. Some special keys There are some other keys which have a special function in the Protel Easytrax program. These are explained below: END Redraws or `refreshes' the screen. HOME Centers the screen about the current cursor position. PGUP This key has the same effect as choosing Zoom Expand. PGDN This key has the same effect as choosing Zoom Contract. * This key is on the right of the keypad. Sometimes it also has PRTSC on the same key. It is used to swap between the currently selected signal layers. The effect can be observed on the status line. - This key is also on the keypad. It is used to cycle through all the currently selected layers. + This key is also on the keypad. It is used to cycle through the currently selected layers in the opposite direction to the - key. Speeding up menu selections Before finishing this tutorial you should be aware of a feature of Protel Easytrax which helps speed up menu selections once you become familiar with the menu structure. Each menu option can be chosen by simply pressing the first key of the option to be selected. Thus to choose Jump Pad you only need to type J then P. Quitting from the program It is important to know how to get out of the program at this stage. Select the File option and then select Quit or just type F then Q. A window opens which asks you to confirm that you want to quit to DOS. Choose the Yes option. If have have made changes to the file you have loaded you will then be asked to save changes, choose the Yes option again, and you will be prompted to enter a filename. The default will be the same as the file you laoded; to override the previous version press ENTER, or to make a new file type in the new file name and press ENTER. You will then be returned to the DOS prompt. 2 Tutorial: Laying out a PCB In this tutorial the most important aspects of placing components, using the library, laying tracks and using the powerful router will be covered. The tutorial will lead you through the set of steps necessary to begin designing an RS-232 splitter board. As there is insufficient space in the text file to describe laying out the whole board, you will simply place a DB25 connector and the first of the 16 pin chips as well as some by-pass capacitors and a resistor. In this tutorial you will learn the following skills: clearing the work space; choosing a component from the library; placing a component; rotating a component; assigning component designators and comments; identifying pins on components; placing tracks manually; switching layers; using the pad to pad router. Getting started The aim of this tutorial is to lay out the section of an RS- 232 splitter board. There is one DB25RA/F connector, one DIP16 chip, three capacitors and one resistor on the board. Your first task is to place these. You must first make sure that the board is clear. Either restart the Protel Easytrax program or choose File Clear Yes. If you start the program again, press ESC or click the RIGHT MOUSE button in response to the prompt `LOAD PCB FILE NAME'. Placing components Now press PGUP three times then choose Place Component. An input window with the heading `NAME IN LIBRARY' opens asking for the name of a pre-defined component. Notice that there is a question mark on the input line. Press ENTER or click the LEFT MOUSE button and a list of the components in the library is displayed. If you know the name of the component then you could have simply typed it when the input window opened. In this case you would have entered the name DB25RA/F and pressed ENTER or clicked LEFT MOUSE. For the purposes of this tutorial, however, select the component from the library list. Move the selection bar to the component named DB25RA/F. Press ENTER or click the LEFT MOUSE button. A window opens and you are prompted to supply a component designator. A component designator is usually a letter such as U, J, C, or R followed by a one or two digit number. Connectors are often given designators starting with J, so enter J1 in this case, then press ENTER or click LEFT MOUSE. You are now prompted to enter a short comment which appears on the component overlay. Type in DB25RA/F and an outline of the component appears. You now see the message: MOVING COMPONENT on the prompt line at the bottom of the screen. This means that you can now adjust the position of the component. Press SPACE to rotate the component through 90 degrees, then move the white outline (with the cursor keys or the mouse) close to the edge of the board - but not so close that you cannot see the whole component. Try X:500 Y:2500 for example. When the outline is in the correct position, press ENTER or click LEFT MOUSE and the component is placed. The next step is to place a 16-pin chip near the J1 connector. At this stage you are still in Place Component and the input window has the component name DB25RA/F in it, since that was the last component chosen. Enter a question mark and the string DB25RA/F disappears. Press ENTER or click the LEFT MOUSE button and the information window opens. Choose the component labelled DIP16 then press ENTER or click LEFT MOUSE. Enter the designator U1 and the comment DIP16. Press ENTER or click LEFT MOUSE after each entry. The outline of the component now appears. Use the cursor keys or the mouse to move it to X:1900 Y:2200. Once again, press ENTER or click LEFT MOUSE to fix the component in place. Now you need to place three capacitors. The component you require this time is called RAD0.2. Enter a ? in the input window. It is not listed in the information window so press the PGDN key to see the next screen full of names. Choose RAD0.2 and supply the designator C1 and the comment 22uF. Press ENTER or click LEFT MOUSE to enter each of these items. Press SPACE to rotate the outline through 90 degrees, then move it to X:1350 Y:2250. Press ENTER or click LEFT MOUSE to place it. The input window is still showing the name RAD0.2 so simply press ENTER or click LEFT MOUSE to choose that name for the second capacitor. The designator automatically becomes C2 and the comment is still 22uF. Rotate the second capacitor and place it on the other side of the DIP16 chip at X:2800 Y:2250. Now choose RAD0.2 a third time. Rotate it and move it to X:1350 Y:1150. Click LEFT MOUSE or press ENTER to fix it in position. Click RIGHT MOUSE or press ESCAPE to exit from the Place Component option. Now move to a point just above C3 (say, X:1250 Y:1550) and select Place/Component from the menu. Choose the component labelled AXIAL0.3. Assign the designator R1 and the comment 3.3K. Press ENTER to fix the component in position. Press ESC or click RIGHT MOUSE to exit from the Place/Component option. The display might be a bit messy by now so press the END key to redraw the screen. Laying tracks Now you are almost ready to start laying tracks. Before you can, you need to know the pin numbers of the components. In the previous tutorial you learned how to identify pin numbers using Jump Pad. Use this option to find pin 1 on J1, U1, R1 and C1. From this information you can work out most of the others. It might also be necessary to locate pin 25 on J1 and pin 16 on U1. The following table provides a list of the pins which must be connected. U1-1 to C1-2 U1-3 to C1-1 U1-16 to C3-1 U1-12 to J1-2 U1-11 to J1-3 U1-10 to J1-5 U1-9 to J1-4 U1-5 to C2-1 U1-4 to C2-2 U1-2 to C3-2 to R1-2 J1-20 to R1-1 The first entry in the table indicates that you must connect pin 1 on the component U1 to pin 2 on the component C1. The entry under it shows that you must connect pin 16 on the component U1 to pin 1 on the component C3. This information becomes important later as it is the basis of the concept of a Netlist. A netlist is a list of all connections on the board. Easytrax allows you to generate a netlist once all connections have been established. When printed out, this netlist can be compared with a schematic to verify that all connections have been completed per the drawing. Each group of connections in a netlist (e.g. U1-1 to C1-2) is called a Net. Try connecting some pads. Press the * key on the keypad to change from the component side (top layer) to the solder side (bottom layer). On the status line the layer indicator message changes from `L: Top Layer' to `L: Bottom Layer'. Choose Place/Track and the message: SELECT TRACK START POINT appears on the prompt line at the bottom of the screen. Move the cursor to pin 1 on U1 (it is a square pad) - you are going to connect it to pin 2 on C1. Click LEFT MOUSE or press ENTER. The message: PLACE TRACK appears on the prompt line. Now move the cursor towards C1 keeping the line horizontal. When the line is half way towards C1 (about X:1650 Y:2200) click LEFT MOUSE or press ENTER. Press * to change layers. Now move the line vertically until it is in line with pin 2 on C1 (about X:1650 Y:2450). Click again or press ENTER then press * to change to the bottom layer. Move the cursor to pin 2 and click again or press ENTER. A connection now extends from U1-1 to C1-2. Notice that this last section has been placed on the bottom layer and that a via has been used to change layers. Press ESC or click RIGHT MOUSE twice to exit from the track laying routine. You can continue to make the other connections in the same way for practice. We will now make one of the connections using the powerful pad-to-pad router option. Invoking the Pad-to-Pad router The router option is invoked by the Place/Route command. Select Place/Route now from the menu or simply type PR on the keyboard. Notice the message on the prompt line - ROUTE: SELECT FIRST PAD Move the cursor to U1-11. (It's third up from the bottom on the RHS of U11). Press ENTER. Notice that you are now prompted to select the second pad. Move the cursor to J1-3 and press ENTER. (It's the second round pad above the square pad on J1). The router will make the connection for you, automatically swapping layers and placing vias during the process. Connecting to power and ground planes The final connections you have to make are to the power plane and ground plane. Pin 7 on the DB25RA/F connector and pin 15 on the DIP16 chip have to be connected to the ground plane. Pin 16 on the DIP16 has to be connected to the power plane. (This is assuming, of course, that you are going to construct a board with power and ground planes.) Choose Edit Pad. You are prompted to select a pad. Select pin 7 on the DB25RA/F and a window opens displaying information about the pad. Notice that there is an option which shows the power and ground status. Choose this option and another window opens listing the possible connections. Choose Relief to Ground Plane. Press ESC or click RIGHT MOUSE and you are prompted to select another pad. Now choose pin 15 on the DIP16 and make the same connection. Finally, choose pin 16 on the DIP16 chip and connect it to the power plane by choosing the Relief to Power Plane option. 3 Tutorial: plotting a board This tutorial shows you how to do a simple check plot of the DEMO.PCB file. Protel Easytrax has a flexible set of output routines which allow output to be sent to dot matrix printers, HP LaserJet & compatible printers, Postscript printers (eg Apple Laserwriter), pen and ink plotters, photoplotters and disk files. In this tutorial you will learn the following skills: loading the Easyplot program; interpreting the menu levels; interpreting the status screen; loading a .PCB file; setting the serial interface parameters; selecting the plot type; loading a plotter driver; setting the pen speed; setting the pen size; producing a draft plot. In this tutorial the plotting is done on a simple, single- pen DMPL plotter. If you do not have a similar plotter you will need to adjust the tutorial to suit your situation. Starting the program To start the Easyplot program change directory to \EASYPLOT and simply type: EASYPLOT then press ENTER at the DOS prompt. (You might need to move into a different directory before you start the program depending on the path you chose at installation). The MAIN PLOT MENU is displayed. MAIN PLOT MENU File Information Options Setup Plot Print Gerber Plot NC Drill Loading the DEMO file Choose File/Path and type in the path for the .PCB files. Choose File/Load and enter the file name DEMO in the input window. An information window opens showing the number of pads, tracks, components, etc. that are being loaded. A second pass shows the percentage of the board which has been analysed. When the file has been loaded, the status screen is updated to show the name of the .PCB file, the dimensions of the board and the amount of free memory remaining. The path name of the directory is also displayed. Path: C: \FILES Layout file: \FILES\DEMO Layout size: 5900x5000 Free memory: 114654 You should check the layout size to make sure that the board fits on the paper at the scale you choose. Thus, if a board has a layout size of 6000 x 5000, it will cover an area 6 inches by 5 inches. If you plot it at a scale of 2, it requires a sheet of paper which is at least 12 inches by 10 inches. The File menu is still displayed. Press ESC or click RIGHT MOUSE to return to the MAIN PLOT MENU. Overview of plotting a board Now you can use a plotter to produce a check plot. First, make sure that you have set up the plotter in accordance with the manufacturer's specifications. For the purposes of this tutorial we use a DMPL single-pen plotter with a serial interface running at 2400 baud. The steps you need to take to set up the correct conditions for a successful check plot are: Set the serial port to the correct baud rate. Make sure the other setup parameters are correct. Select Check Plot as the plot type. Set up the check plot parameters. Load the plotter driver. Set the pen speed. Set the pen sizes. Setting the serial port parameters Let's assume that you have a DMPL plotter connected to a serial port of your computer. (If you haven't, then choose from the list of plotters provided in Setup Plotter Type - there must be a plotter driver for your plotter before you can use it with Easyplot). Choose Setup Serial Ports and choose either `Serial Port 1' or `Serial Port 2' depending on which port you have connected the plotter to. A window opens showing each of the serial port parameters you can change. SERIAL PORT 1 SETUP Baud : 2400 Data : 8 Handshake : Hardwire Parity : None Stop Bits : 1 If the baud rate is not set to the correct value (in this case 2400) select Baud and select the value 2400 by highlighting it and then pressing ENTER or clicking LEFT MOUSE. You are returned to the Setup Serial Ports menu. Check that each of the other parameters is set correctly for your plotter. If you are using a DMPL plotter then the parameters shown in the previous menu should be correct. Press ESC or click the RIGHT MOUSE button three times to exit from this option. Choosing the plot type In this tutorial you are going to produce a check plot, rather than a plot of a particular layer or a specialised plot such as a solder mask. Return to the MAIN PLOT MENU and choose Options/Type of Plot. A window opens showing each of the plot types you can choose. Use the arrow keys to highlight Check Plot then press ENTER or click LEFT MOUSE. Return to the MAIN PLOT MENU and choose Setup Check Plot. Make sure that the Top Layer, Bottom Layer, Top Overlay and Multi Layer Pads options are set to `on'. This ensures that all the information on each of those layers is plotted. If you set any of these to `off', the items on that layer are not plotted. Press ESC or click the RIGHT MOUSE button to exit from this option. Loading the plotter driver Choose Setup Plotter. The entry next to Type shows the currently selected plotter driver. If it is not set to `DMPL', choose the option and the program scans the directory and lists all the currently available plotter drivers. Select the DMPL plotter driver from the list and then press ENTER or click LEFT MOUSE. You are returned to the Setup Plotter menu. Choose Device and another window opens listing the options you can choose for the port to connect the printer to. Choose `Serial Port 1' by moving the selection bar to that option then pressing ENTER or clicking LEFT MOUSE. Check the other options to make sure they are the same as those shown below. Press ESC or click RIGHT MOUSE twice to return to the MAIN PLOT MENU. A possible set of options is shown below: PLOTTER SETUP Type : DMPL Device : Serial Port 1 Scale : 1.000 X Offset : 0.000 Y Offset : 0.000 X Correction : 1.000 Y Correction : 1.000 Orientation : Auto Centered Quality :Draft Software Arc : On Arc Quality : 5 Options : Pens : Setting the pen parameters You now need to set the speed at which the pens are to be driven and the size of pen that you have in the plotter. Choose Setup Pens Check Plot Pens. You now need to set the pen speed to a value of 2 inches per second. This figure seems to work the best with a DMPL plotter. Hint: You can set the pen speed to a higher value, but the ink in the pen may not flow quickly enough to form a clear line on the paper. If you set the value too low then you may get ink `blotches' on the paper - it also takes a long time to plot. Experiment with different speeds until you find an optimum setting for your plotter. To input the pen speed, highlight the Pen Speed option and press ENTER or click LEFT MOUSE. Enter the value in the input window, then press ENTER or click LEFT MOUSE. You are returned to the Check Plot/Pens menu. You now need to set the size of the pen you are using. This is vital so that the printer driver can draw the tracks, arcs, vias and pads accurately. It is obvious that if you have a 26 mil diameter pen then it is impossible to draw a 12 mil track at normal scale If you do not set the pen size, it defaults to 26 mils. To change the size, choose Pen Sizes from the Check Plot/Pens menu. Enter the value of the diameter of the pen in mils and the press ENTER or click LEFT MOUSE. You are returned to the Check Plot Pens menu. Press ESC or click the RIGHT MOUSE button four times to return to the MAIN PLOT MENU. Plotting the board You are now ready to proceed with the plot. From the MAIN PLOT MENU choose Plot. You are asked to confirm that you want to proceed with the plot. Before you choose Yes, check the large information window on the right-hand side of the screen which displays all the plot parameters. If any of these are not correct you need to return to the MAIN PLOT MENU and change them. When you are happy that everything is correct choose Yes. You are then asked to insert pen 1 in the plotter. Make sure it is securely in place then press ENTER or click LEFT MOUSE. The plot should now begin to appear on the paper in the plotter. When the plot is finished you are returned to the MAIN PLOT MENU. 4 Tutorial: Gerber plots In this tutorial you learn how to use the Easyplot program to create a file which can be used with the standard Gerber format photoplotter to produce high-quality final artwork. You probably will not want to go to the trouble and expense of producing a Gerber plot of the demo board, however, the tutorial will give you a good overview of the process. The skills you learn in this tutorial are: Selecting a particular plot layer; Selecting Setup parameters; Selecting apertures; Selecting the photoplotting method; Generating a match file; Generating a Gerber plot file. Photoplotters produce highly accurate artwork - in fact they are as accurate as the resolution of the Protel Easytrax program. The biggest problem is that the equipment can be very expensive so most board designers need to send their files to a photoplotting bureau. For this reason, the Easyplot program produces output files rather than driving a photoplotter directly. Setting up a Gerber plot You need to set up all the same options for a Gerber plot as you do for a normal plot but there are some extra things to do as well. First, you should choose File Load and load the Demo PCB file. This process is exactly the same as for a normal plot or print. In this tutorial you are going to produce a plot of the top layer and the pad master. For the first plot choose Options/Type of Plot and select `Top Layer'. Note that the `Check Plot' option does not work with a Gerber plot because 1:1 Gerber check plots would be of no practical value. You should use a printer or pen plotter to do your check plot and only produce the (expensive) Gerber plot when you are sure that it is absolutely correct. Now choose Setup/Gerber and define each of the setup options you require. The options from which you can choose are shown in the menu displayed below. GERBER SETUP Output File : \Files\Demo X Offset : 0.000 Y Offset : 0.000 Aperture Table : PROTEL1.APT Match Tolerance: 5% G54 : Off Arc Quality : 5 Options The X and Y Offsets can be used in exactly the same way as they are for a normal plot. By changing these offsets you can choose to start plotting at a different spot on the film. This allows more than one plot to be performed on one film, thus saving on the cost of film. Next you should choose the Aperture Table which matches that required by the photoplotter that you are going to use. While most photoplotters use the Gerber standard for selecting apertures and for moving to a particular spot on the film, they vary considerably in the apertures which are available. To overcome this problem there are a number of standard Aperture Tables supplied with Protel Easytrax. Select the aperture table you require by choosing Setup Gerber Aperture Table. A list of the available aperture tables is displayed. Highlight the one you require then press ENTER or click LEFT MOUSE. The name is now displayed in the Gerber Setup menu. Next you should set the Match Tolerance percentage you require. An example might help here. If you have a large number of circular 62 mil pads on your board, these can be plotted quickly by selecting a 62 mil aperture and then `flashing' a light onto the film. But what happens if the photoplotter does not have a 62 mil aperture? Some have a 60 mil round aperture and for most plotting tasks you are likely to require this is close enough. The Match Tolerance is the figure you set to say what variation in area you can tolerate. If the program is able to match an aperture with a pad which is within the tolerance you set, then it does so automatically. The area of a 62 mil pad is 3.1415 x 62 x 62 = 12076 square mils. The area `flashed' by a 60 mil aperture is 3.1415 x 60 x 60 = 11309 square mils. The percentage variation is calculated as (12076-11309) x 100 / 12076 = 6.35. Therefore if you set the Match Tolerance to 8% or greater, the 60 mil aperture is selected automatically. Don't set the tolerance too high (e.g. 30%) otherwise there may be problems fitting tracks between pads in some cases. Some older Gerber plotters need to be sent the code G54 before an aperure change. Thus, if the aperture D10 is to be selected the software must send a G54 code then a D10 code. If the plotter requires this code to be sent, set the G54 option to `On'. If it does not need this code, set it to `Off'. Some plotters have the ability to draw an arc if the parameters are supplied. This is not the case with some Gerber photoplotters. In order to draw an arc, the plot program must ask the photplotter to draw a number of short line segments. The greater the number of line segments used to draw the arc, the longer it takes. The Arc Quality option allows you to set the length of the line segment (in mils) which is used to draw the arc. A value of 5 mils is a reasonable compromise for most jobs. The steps you have carried out to set up the Gerber plot are: Choose File Load and load the Demo file Choose Options Type of Plot, then select Top Layer Press ESC or click RIGHT MOUSE Choose Setup/Gerber Choose Aperture Table and select the required table Set the Match Tolerance to 8% Set G54 to `Off' Set Arc Quality to 5 Press ESC twice to return to the MAIN PLOT MENU Creating the Gerber file Now return to the MAIN PLOT MENU and select Gerber Plot. The plotting screen appears with the information window on the right hand side of the screen. You are asked to confirm that you want to proceed with the Gerber plot. this gives you the opportunity to inspect the parameters you have chosen for the plot. If any of them are incorrect, select No and change them. If you are ready to proceed select Yes. The program now attempts to match every item on the board with an aperture on the photoplotter that you are going to use. For each item, it looks for an aperture in the Aperture Table you selected. If it cannot produce a match within the tolerance you specified it asks you to select from a table of the closest apertures or enables you to step through the apertures to manually select one. You see a display similar to the one below. MATCHING DRAFT CODES ASSIGNING : Circular (28 x 28) Match Method Code Shape Size Flash Match : D19 Circular (40 x 40) Stroke Match : D15 Circular (25 x 25) Fill Match: : D13 Circular (20 x 20) A window then opens allowing you to select which method you want the photoplotter to use to make the shape. Select Plot Method Flash Method Stroke Method Fill Method Manual Assignment Make sure that you do not choose the stroke method to create a pad. If you attempt to, the message: CANNOT USE LINE APERTURE FOR MATCH is displayed. It is a good idea to minimize the number of Fill Matches, as these usually take longer to photoplot. When all apertures have been matched, the message: MATCH FILE GENERATED appears indicating that a file has been created which matches each shape to be generated with an aperture which is available on the chosen photoplotter. The match file shows the shapes which the program has tried to assign apertures to and the aperture and exposure method which has been chosen - either by the program or by you. A sample from a match file is shown below. ASSIGNING : Circular (28 x 28) STROKE : D15 Circular (25 x 25) ASSIGNING : Circular (40 x 40) FLASH : D19 Circular (40 x 40) ASSIGNING : Circular (60 x 60) FLASH : D28 Circular (62 x 62) Press any key and the final Gerber output file is then generated. The Gerber file in this case is assigned the name DEMO.GTL. The extension indicates that it is a Gerber output file and that it is a plot of the Top Layer. Plotting the Pad Master When the first plot is complete you are returned to the MAIN PLOT MENU. Now, as an example of a different plot, choose Options Type of Plot and select Pad Master. Press ESC to return to the MAIN PLOT MENU. When you now choose to do the Gerber plot, you are asked whether you want to reassign the draft codes. If you are happy with the matches which are stored in the .MAT file then choose No and the plot proceeds. This time the Gerber output file is given the extension .GPM to indicate that it is the Pad Master layer. 5 Options Summary In this section, each of the major menu options you can choose are listed along with a brief summary of their function. Block Define Defines a block by selecting the opposite corners of the rectangle, then selecting any reference point. Hide Used to remove the highlight from the currently defined block. Move Once a block is defined it can be moved to another part of the board. You can move items on the current layer or all layers. The block can be flipped or rotated during a move with the X, Y and SPACE keys. Copy Similar to Block Move except that items are copied. Inside Delete Deletes items within the currently defined block. Outside Del Deletes items outside the currently defined block. Read Reads a PCB file as a block which can then be placed within the current board. Write Saves the currently defined block as a file. Current Cursor Mode Allows the cursor position to be measured from the bottom left hand corner of the board (Absolute) or from the position of the floating origin (Relative). Floating Origin Allows you to set the origin at a point other than the bottom left hand corner of the board. Layer Selects the layer which is to be the current layer. The currently selected layer can also be changed with the *, - or + keys. Pad Type Allows you to select the pad type which you want to be the currently selected pad type. When you choose Place Pad, it is this pad shape which is placed. Pad Orient Pads can either be placed normally or rotated through 90 degrees. Choose either `Normal' or 'Rotated' with this option. Track Width Set a track width from 1 to 255 mils with this option. String Size The string size is the size of any text characters which you place on the board. It is measured in mils. String Lines This variable controls the thickness of the lines which make up the strings. Via Size Use this option to change the currently selected via size. Via Hole Size Use this option to change the currently selected via hole size. The hole size must be less than the via size. Delete Arc To delete an arc, choose this option then select the arc to be deleted. Component Allows you to delete a component such as a chip or connector or capacitor. Fill Use this option to delete a fill from the board. Highlight Allows you to delete the set of tracks which are currently highlighted. Pad Deletes a selected pad. Since a pad belongs to every layer (except for SMDs and edge connectors) it usually does not matter what layer is currently selected. String To delete a string, choose this option then select the string to be deleted. Make sure that the currently selected layer is the layer on which the string is placed. Track Deletes a track. You may have to delete a number of tracks to remove a complete connection. Via To delete a via, choose this option. A via can be deleted from any layer. Edit Component Allows you to change the designator, pattern or comment associated with a component. It also allows you to change the layer on which the component isplaced and to indicate whether the component can be moved during an auto place procedure. Pad Allows you to change the shape of a pad and also to indicate whether the pad should be connected to the power or ground planes. Track Allows you to change the layer the track is on or the width of the track. String You can use this option to change the size, line width or message in a particular string. Via Allows you to change the via size or the via hole size. File Clear Clears the current board from the memory of the computer. Dos Allows you to suspend to DOS to carry out routine DOS operations. Type EXIT to return to the program. Files Allows you to inspect a listing of files in the currently selected directory. Load Loads a .PCB file. Path Allows you to change the currently selected directory Quit Use this option to quit from the program. Save Saves the board you are currently working on. It is saved in the directory you have specified using the Path option unless you specify otherwise. Grid Snap Grid The invisible snap grid controls the movement of the cursor. Allows precision in placing items. Visible Grid A series of dots on the screen, an aid to alignment. Highlight Connection Allows you to highlight the connection between two pads. Point to a track, not a pad, to start the highlighting. Duplicate Duplicates a hilighted connection. Select the point on the connection you want to act as a reference point,then point to the new position. Net Allows you to highlight a complete net. Make Netlis Allows you to create a netlist based on the connections you have made on the board. The netlist is stored in a file with the extension .NET, in the currently selected directory unless you specify otherwise. Reset Removes the highlight from a highlighted net. Information Board Dimen Displays the current size (inches) of the board. Components Lists the designators of the components which have been placed. Highl'd Pins Lists the pins connected to the currently highlighted net. This is useful for checking that you have connected all the pins that you intended to connect. Lib Comps Displays the components in the current library. Pwr/Gnd Pins Lists either the ground nets and/or the power nets. Status Displays information about items on the board as well as information about memory usage and file names. Jump Component Moves the cursor to pin 1 of a selected component. Location Moves the cursor at a particular coordinate. Origin Moves the cursor to the origin (0/0 coordinate). Pad Moves the cursor to a named pin on a selected component. String Moves the cursor to a selected string. Library Add Adds a highlighted block to a selected library as a component. Browse Allows you to inspect each of the components in the currently selected library. Compact Compresses data in an edited library file. Delete Deletes a component from the currently selected library. Explode Reduces a selected component into editable tracks, arcs and pads. Used to create a new component by altering an existing one. File Changes the currently selected library. List Lists the components in the currently selected library. Merge Moves a component from another library into the current library. New Library Creates an entirely new library. Rename Renames a component in a library (does not rename the library). Move Arc Moves an arc from one part of the board to another. Cursor must be exactly over the arc when selecting it. Break Breaks a track into two sections at a particular point. Component Moves a component to another place on the board with the option of dragging the connected tracks. Drag End Allows you to drag one end of a track to a new position. Fill Moves an area fill. Pad Moves a pad to a new position on the board. Re-Route Allows you to manually re-route a connection by breaking a track at a number of points. String Moves a string. Track Moves a track while maintaining connectivity with related tracks and vias. Via Moves a via while maintaining connectivity with tracks. Place Arc Places an arc. Use the LEFT and RIGHT cursor keys to increase and decrease the radius, and the 8, 6, 2 and 4 keys on the keypad to remove arc segments. Component Places a selected component from the current library. Fill Places a rectangular area of solid fill. Pad Places a pad of the type selected in the Current options. String Places a string on the board. The size and thickness of the string is determined by the parameters in the Current menu. Track Places a track segment on the currently selected layer. The placed track is the size selected from the current options. Via Places a via of the size selected in the Current options. Repeat This option allows you to repeat the placement of the last component, track, pad or via a specified number of times in a specified direction. Setup Comp Text Toggles display of component text on/off. Layer Colors Selects colors for items on each layer. Menu Colors Selects colors used in the menus,background,etc. Keys Main Menu for macro editor. Options Allows you to change parameters including cursor shape, back-up interval, etc. Pads Allows you to define custom pad types. Redraw Selects draft or final quality screen redraw. Strings Sets default size for strings from 36 to 560 mils. Toggle Layers Sets each board layer to `on' or `off'. Un-delete Whenever you delete an item from the board, Protel-Easytrax remembers the deletion. This option allows you to restore one or more deleted items. Zoom Redraw Redraws the current screen at the current magnification. Pan Redraws the screen at center of cursor position. Expand Selects the next highest magnification from one of six zoom levels (also PGUP key). Contract Selects the next lowest magnification (also PGDN key). All Redraws the display to include the entire board. Keyboard Selects a zoom level by number. Select Selects a zoom level from 7 pre-set magnifications. Window Selects a section of the board for magnification. Additional information this version: New graphics drivers This release includes the following new drivers for the ATI VGA Wonder card and the Paradise EGA480 card. The drivers are labelled WOND800.DRV (800x600), WOND1024 (1024x768, Revision 5 cards only) and PEGA480 (640x480). There are a number of cards that use the PEGA480 chipset. Memory management If memory is a problem, make sure that your operating system is as 'bare' as possible - disable network software and any TSRs (other than EMS/Mouse drivers), etc. If memory is still a problem you may need to consider additional EMS. Repeat Placement with metric grids If you are using the Repeat Placement feature with some fractional metric grids, the Offsets applied to repeats can result in some unexpected placements. This is because the metric value must be rounded off to two decimal places. For example the default 25 mil imperial grid is equal to approx .625 mm, rounded-off to .63 mm by Autotrax. If you attempt a repeat placement of a row of pads, this rounding-off will result in a cumulative error in spacing as successive pads are placed. The solution is to use even multiples of the current snap grid as offsets OR to work on a 'natural' grid pitch, i.e. .5 mm or .6 mm OR to stay on the imperial grid, rather than switching to metric prior to repeat placement. Easyplot - version 2.06 Additional Features Roland 1000 Series plotters A new plot driver has been added for these popular plotter models (DXY 1100, 1200, 1300, etc). It is called ROLAND RD-GL I. This supersedes the information in the manual. However, you should make sure that all communications parameters are matched between the program and the plotter. Improved Path Handling in Easyplot When you select the Setup/(Plotter, Printer or PostScript)/Type, to choose a driver, a window opens allowing you to specify the directory. The default directory is now always the Easyplot home directory. Naming of output files: The name of the current .PCB file is automatically applied to output files, as when plotting to a filename (rather than directly to a port). PostScript printing The following PostScript options are supported by the current version of the Easyplot program: PS300A4 A4 sheet 300 dpi resolution PS300A3 A3 sheet 300 dpi resolution PS400A4 A4 sheet 400 dpi resolution PS600A4 A4 sheet 600 dpi resolution PS1200A4 A4 sheet 1200 dpi resolution PS1200A3 A3 sheet 1200 dpi resolution PSLINOA4 A4 sheet 1270 dpi Linotronic PSLINOA3 A3 sheet 1270 dpi Linotronic PS300B5 B5 sheet 300 dpi resolution PS300LT US letter 300 dpi resolution PS300LE US legal 300 dpi resolution (end)