The Utilities Experience

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

/ The Utilities Experience / The Utilities Experience - Volume 1.iso / software / demos / e-q / pndemo20c / pronet.features < prev next >

Wrap

Text File | 1993-03-18 | 76.5 KB | 2,028 lines

GENERAL DESCRIPTION OF PRO-NET COMMANDS AND FEATURES *********************************************************************** * * * Some of the information in this demo description is out of date. * * We will be updating it in the near future. * * * *********************************************************************** TERMS AND CONVENTION: - click Click the left mouse button to select a mode (function) or add a piece of graphic information to the drawing. Click the right mouse button to delete a piece of graphic (such as a symbol of an NAND gate) information on the screen pointed to by the cursor. - IFK's The Intelligent Function Keys. They are the ten Function Keys located at the top of the keyboard. In Pro-Net, these Function Keys are intelligent because the same Function Key performs different tasks in different modes. The tasks to be performed by these Function Keys at any moment are automatically shown at the bottom of the screen. - IFK-Name An IFK called "Name". - IFK levels The IFK's guide the user through an operation by providing the next available set of IFK's for the user to select. These sets form the IFK levels. An IFK at a certain level is expressed as : IFK-NameA/IFK-NameB/...../IFK-NameX. For example, the IFK-Line appeared if you first select IFK-Edit, then IFK-New, IFK-OK. Therefore, the selection of IFK-Line can be expressed as: IFK-Edit/ IFK-New/ IFK-OK/ IFK-Line or, in its short form: IFK-Edit/New/OK/Line This expression can further be expressed as: IFK-Edit/./Line if and only if the same set of IFK's (that contains the next IFK, in this example, IFK-Line) appear no matter which intermediate steps (other than <ESC> which means abort) have taken place. - Select Either press the IFK or click at Icon of the IFK. - Add button The left button of the mouse. - Delete button The right button of the mouse. - Entry Bar The color bar above the IFK icons at the bottom of the screen. It is used for the user to enter additional information and for the program to display the status of the operation. - Bold face All commands are shown in Bold. These commands are entered by one of the following methods: 1. Selecting the appropriate IFK. 2. Using the hot key. Some Commands require additional information from the user, this information is entered at the Entry Bar. - Leading Capital Names which have special meanings in Pro-Net have their first character capitalized. - Directory Structure If Pro-Net is installed using the "Install_PN_DH" (see Section "Quick Start"), the following directory system is automatically setup for you under a subdirectory "/Pro-Net". For Floppy systems, the following directory is distributed among three diskettes, therefore, you MUST follow the procedure in Section "Defining Library Parts" when you have to modify the Library. The file Directory Structure for Pro-Net is as follows : PNPOST (dir) PNLIB (dir) TTL (dir) MOS (dir) VLSI (dir) ECL (dir) ANALOG (dir) DISCRETE (dir) MTTL (dir) USER (dir) SYMBOL (dir) SCHEM (dir) PNDIR (dir) TTL MOS VLSI ECL ANALOG DISCRETE MTTL USER SYMBOL SCHEM - Files The files which are associated with a schematic called "name" are as follows : name.1 Page 1 of the schematic "name" name.2 Page 2 of the schematic "name" . . . . . . . . . . name.SupNet ASCII file, optional Net list provided by user for schematic "name". name.net ASCII file, net list of the schematic "name". name.bom ASCII file, Bill of Materials (Part List) of the schematic "name". name.err ASCII file, error report of schematic "name". name.map ASCII file, component map of schematic "name". Other system files (you don't normally care about these files, as long as you are not trying to alter them): PNDIR A file which contains the Pro-Net directory system. It contains the directory files of Pro-Net, when a schematic is deleted or added, or when a Device is added or deleted, this file will be automatically updated. PNLIB all Pro-Net files are kept here. name.M System internal file containing information linking different pages together. This file is part of the schematic "name". - Hot Keys Key strokes used to enter command(s) at any screen in any mode. In Pro-Net, when you hit the "Help" key, the Hot Key definition will show up as follow: <Help> Get this help information <CTL-G> Show Grid ON/OFF <CTL-S> Grid Snapping ON/OFF <CTL-U> Grid size goes Up (bigger) by one size <CTL-D> Grid size goes Down (smaller) by one size <CTL-B> Move the Pro-Net screen to the Back of other screens of the system. <DEL> Toggle Scroll wall ON/OFF <ENTER> Redraw screen <ESC> Back up one IFK level. In some cases, abort current operation. <ARROW KEY> Unconditional scroll <SHIFT><ARROW KEY> Jump to the page boundary in the direction of the arrow. OVERVIEW: Pro-Net stands for 'PROfessional NET list generator'. Thanks to the powerful graphic capabilities of the Amiga computer and to the brilliant Intelligent Function Keys (IFK) of Pro-Net, users now can create professional schematics with speed and ease. Besides creating beautiful schematics, Flow Charts, Organization Charts, etc., Pro-Net emphasizes the importance of net list generation which provides sufficient information for Pro-Board (*) to perform Auto Component Placement at an expert level (**), and to perform such tasks as Rat's Nesting, Guided Routing, Automatic Coordinate marking , Automatic Surface trace handling and Net List comparison. Pro-Net and Pro-Board are tailored to work with and for each other, they therefore can accomplish many tasks that other stand-alone schematic capture programs or pcb layout programs could not do. Most of these tasks are tedious and repetitive, and should be done on the computer rather than manually by hand. Some examples of these tasks are: -- Automatic assignment of label and section numbers for components such as U17, pins 1,2,3 of a 74F00. The assignment also avoids conflicts in component placement which will be performed later by Pro-Board. -- Automatically creates page references on a schematic for every signal name on every page of that schematic. For a schematic of many pages, this is previously a tedious job that could hardly be right if it is done manually by the user. -- Rat's nest helps the component placement process which is of vital importance to a good PCB layout. -- Automatically assign and mark XY coordinates on the PCB. -- Automatically rename IC by coordinates, such that U17 now becomes 3D on the PCB. -- Automatically rename IC by coordinates on schematic to match that of the PCB (Back Annotation). -- Creates BOM, Page Referencing, Component Map, Loading Analysis, Error List. -- Automatically compare Net List produced by Pro-Net with results from Pro-Board and report discrepancies. -- Pro-Net and Pro-Board provide all these powerful features, on top of the extremely friendly user interface. We are confident that you will find that these are truly "PROLIFIC" systems. * Pro-Board, the PROfessional pc-BOARD design package, another professional program designed by PROLIFIC INC. ** Option only available in Pro-Board V3. COMMAND DESCRIPTIONS: Hot Keys : Key strokes used to enter command(s) regardless of which screen you are at and what mode you are in. In Pro-Net, when you hit the "Help" key, the Hot Key definitions will will be displayed: <HELP> get this help information <CTL-G> show Grid ON/OFF <CTL-S> Snap on Grid ON/OFF <CTL-U> Grid size goes Up (bigger) by one size <CTL-D> Grid size goes Down (smaller) by one size <CTL-B> Push the Pro-Net screen behind all other system screens. <DEL> Toggle Scroll wall ON/OFF <ENTER> Redraw screen <ESC> Back up one IFK level, or, in some cases, abort current operation. <ARROW KEY> arrow keys on the keyboard performs unconditional scrolling. IFK COMMANDS AND ASSOCIATED FUNCTIONS : \- - - - : Add Bus Entries to the left end of a Line. Orientation of the Entry being from lower right to upper left. - - - -/ : Add Bus Entries to the right end of a Line. Orientation of the Entry being from lower left to upper right. /- - - - : Add Bus Entries to the left end of a Line. Orientation of the Entry being from lower left to upper right. - - - -\ : Add Bus Entries to the right end of a Line. Orientation of the Entry being from upper left to lower right. (Arrow-Down) : This IFK moves the Selection Bar (Box) Down the list. In Note/Text mode, this IFK specifies that text is written from top to bottom. (Arrow-Right) : In Note/Text mode, this IFK specifies that text is written from left to right. (Arrow-Up) : This IFK moves the Selection Bar (Box) Up the list. Pg(Arrow-Down) : This IFK moves the Selection Bar (Box) one Page Down the list. Pg(Arrow-Up) : This IFK moves the Selection Bar (Box) one Page Up the list. (Big-Dot) : In Edit/Dot mode, this IFK selects the largest Dots to be added to the intersections of Lines. (Mid-Dot) : In Edit/Dot mode, this IFK select medium size Dots to be added to the intersections of Lines. (Sml-Dot) : In Edit/Dot mode, this IFK selects the smallest Dots to be added to the intersections of Lines. Above : Add Signal Names above the horizontal line. Conn, Above, and Below are mutually exclusive functions. When a Signal Label is added, it can be added above the line, below the line, or at the end of the line with a box around it as a connector pin designation. Add : The left button of the mouse means select or Add. Adjust : Under Line/Adjust, move a middle section of a line without breaking it. Example: Move the middle section of the following line from location a to location b: _______________________________ | | | ______________ | | | | | a b ____________________ | | | _________________________ | Steps: 1. Under the Line mode, press the IFK-Adjust. 2. Click the select button of the mouse on the vertical line. 3. Move the cursor to the left or right, the vertical line will follow the cursor while maintaining the continuity of the line. 4. Position the vertical line of the cursor at point b. 5. Click the Select button of the mouse to put the vertical line at point b. 6. Hit ESC key to get out of the Adjust mode. Note that there are limitations in IFK-Adjust: A line cannot be adjusted if one end of the line has a Dot or if one end of the line vertically intersects a Device Pin (this is normally avoided in schematic capture to begin with). AllClr : Clear all the IC pin definitions. Arc : In Edit/Note/Arc or DefLib/Defsym/Arc mode, add or delete Arcs. Arcs are drawn counter clockwise. You specify the two end points on the arc, and then select the radius of the arc on the bisector given by Pro-Net. If you drag the mouse when the bisector appears, you can see the radius shown at the bottom of the screen. Arcs can be drawn with narrow (IFK-Narrow) or wide (IFK- Wide) lines. Arcs can be repeated (IFK-Repeat) at one to four Grids below the current Arc. The number of Grids is selected by IFK-Leap- N where N=1,2,3,4. Attr : To define the Attributes of the device. Refer to Section "DEFINING LIBRARY PARTS". Below : The Signal Label will be placed below the line. Refer to IFK- Above and IFK-Signal. Bold : Select Bold face Text. Also see Bold. BOM : Ask Post Processing to generate the BOM (Bill Of Material). If this IFK is active, BOM will be generated in Post Processing. Bound : To define the Boundary of the Symbol, this is normally the last step of the defining a Symbol. If a Device later uses the Symbol, the Boundary of the Symbol will become the Boundary of the Device. Note that when Devices are called out to a schematic, their Boundaries can not overlap each other. A Bound is required for Pro-Net to identify pin locations. Pins are Stripes which end at the Bound. Box : In Edit/Note/Box or DefLib/Defsym/Box mode, add or delete rectangular Boxes. Boxes are drawn by specifying any two diagonal vertices. You can drag the mouse and see the box change size dynamically. Boxes can be filled (IFK-Fill), or drawn with narrow (IFK- Narrow), wide (IFK-Wide) or dashed lines (IFK- '- -'). Boxes can be repeated (IFK-Repeat) at one to four Grids below the current box. The number of Grids is selected by IFK-Leap- N where N=1,2,3,4. Bundle : Bus-Entries + Bus (thick Line) = Bundle <A> Bus-Entries : select the Bus Entry orientation using the first four IFK's. <B> Click at the end of a Line to place the Entry. <C> Use IFK-Repeat if desired to draw another Entry at the next lower end of Line. <D> Select IFK-Bus, draw thick Lines as needed. Use Next to start another Bus. IFK-Repeat has no effect here. Bus : To add thick lines as part of a Bundle. A Bundle represents many Signal lines 'bundled' together. The actual connections are made by the Signal Names applied to each bundled line. You can add Signal labels such as ADDR<0:31> to a Bus. You can also specify whether Page Referencing will be generated automatically for the Signal label. This is done by IFK-+PgRef; if +PgRef is on when the Signal label is created, then a Page Reference will be created automatically for this Signal in Post Processing. Please also refer to IFK-Bundle. CalSym : In DefSym, you can use this IFK-CalSym to call out existing Symbols and use them to form a new Symbol (Complex Symbol). You can not call out Complex Symbols to form Complex Symbols. Complex Symbols always have extension ".C" in the Symbol Directory. You can also call out an existing Symbol, modify it to a new Symbol. In DefDev, you use this IFK-CalSym to call out a Symbol, this becomes the symbol of the Device being defined. You can call out Complex Symbol also. Only one Symbol can be called out for a Device. ChgLib : Change Library; to open or close Sub-Libraries or to change the paper size or template size. You can only change to have a larger paper and/or to have a smaller template than what you have been using for the schematic. Circle : In the Edit/Note/Circle mode or in the DefLib/DefSym/Circle, add or delete circles. Circle is drawn by clicking at the center then at the circumference of the circle. Circles can be filled (IFK-Fill), or drawn with narrow (IFK- Narrow) or wide (IFK-Wide) lines. Circles can be repeated (IFK-Repeat) at one to four Grids below the current circle. The number of Grids is selected by IFK-Leap-N where N=1,2,3,4. The Grid Size is controlled by the Hot Keys. Clear : To clear the entry line input area. Conn : To create scattered Connector symbols. This may or may not affect the Net List, see "Advanced Techniques" section for a detailed discussion about drawing connectors. To add a Connector symbol in the schematic, select Conn, type in the Connector pin identifier such as J4-11, then click at the end of line to add connector symbol at that line. Also refer to IFK-Above, IFK-Signal. Connector pin number can be stepped through like other Signal Label. Refer to IFK-Step @. Config : Configure the system, e.g. plotter type and Data and Library Part destinations. Copy : Under IFK-File (File Management) mode, Copy a schematic to another name in the same disk or different disk. You can also copy a schematic to the same name in a different disk using this IFK. Note that when you copy one page of a schematic to another file, all pages of the schematic are copied at the same time. You can enter the Edit mode to delete pages which you don't want one page at a time. This is necessary for the following reason: Pro-Net assigns Device Numbers and Device Sections automatically when Devices are called out from the Library (to the schematic). These Device Numbers and Device Sections are tracked and recorded across all pages of the schematic. Had you been able to copy one page of the schematic, the bookkeeping for the Device Numbers and Device Sections would have been corrupted. In Edit/Copy mode, IFK-Copy is used to Copy devices from one place of the schematic to another. You can use the IFK-Zone-1,2,3 or Zone-X to control the Device numbers (refer to IFK-Zone-1). DefDev : Define Device; refer to DefLib and the Section "Defining Library Parts". DefSym : Define Symbol; refer to DefLib and the Section "Defining Library Parts". DefLib : Define Library; DefLib is used to define a Symbol, Complex Symbol, Title Block, or Device in a sub-library. To use a Device in a schematic, the sub-library whom the Device belongs to must be opened first. Libraries are opened according to the Design Rule established when a new schematic page is drawn. Libraries can be opened or closed at the Device /ChgLib (Change Library) also. To define a Device with a new Symbol (graphic shape), you must define the Symbol first. A Symbol can be shared (used) by many different Devices. For details of DefLib, refer to the Section "DEFINING LIBRARY PARTS". Delete : In Edit mode, erase the file selected. In DefLib/DefDev , erase the Device selected. In DefLib/DefSym , erase the Symbol selected. Device : A. To get a Device from the opened libraries into the schematic. Libraries are opened in the Edit/New (Rule) screen, or the Device/ChgLib screen. The steps of getting a Device into the schematic are: 1. Select IFK-Device. 2. Optionally select the Zone-1, 2, or 3 which determines what Label to use; Zone-1 selects unused 'U' numbers (or Resistor Modules numbers or any other Devices which were defined as multiple section elements in the libraries) from U1 to U399 (or RM1 to RM399 etc.). Zone-2 selects unused 'U' numbers from U400 to U699 (or RM400 to RM699 etc.). Zone-3 selects unused 'U' numbers from U700 to U999 (or RM700 to RM999 etc.). The default is Zone-1. 3. Type in the Device Name such as '74LS74' and <CR>. 4. Drag the Device to the desired location and click the mouse left button to settle the Device. B. To Modify an existing Device or to define a new Device in the Library, refer to the Section "Library Parts". DevNam : IFK-DevNam (Device Name) is used to define the Text and location of the Device Name, such as 74LS74A. This Device Name could be different from the Device file name you assign when you Save the Device. This is very useful since you sometimes need to define a Device in several different ways. For example, the 74LS244 can be defined as two independent four bit tri-state buffers or it can be defined as one eight bit buffer. You may use one definition in one application and the other in another application. With Field Programmable Logic such as PAL's so popular these days, this flexibility is extremely useful. DevNum : IFK-DevNum (Device Number) is used to define the location of the Device Number Label such as 'U', 'R' or 'C', etc. This Device Number Label will be concatenated with a number assigned by Pro-Net automatically or assigned manually by the user manually (refer to IFK-Zone-1, 2, 3 and X) when schematic is being entered. For example, 'U' becomes 'U14'. Dir : To get the Directory of the Schematic files. Please refer to IFK-Copy. Dot : Used to add or delete a dot in the drawing. If the dot is placed on the intersection of two lines, the two lines are joined together, otherwise, the dot has no effect in the Net List. A dot can also be used to cancel out a small square box which appears at the end of a line. For example, if you draw a line on the screen with both ends open, you should see a small square box at each end of the line. If you move a device to the line such that one end of the line coincides with one pin (tip) of the device, they may seem to be connected, but in fact they are not. To connect them, you must add a dot to that small square box. This will cancel out the small square box. Down : When IFK-Signal is active, IFK-Down forces the number embedded in the Signal label to decrement by one (1) every time IFK-Step@ is pressed. In Zoom, Zoom Down by 1/2 X (devices are half the current size on screen). The last Zoom Down may not be as small as 1/2 X of the former size. Drag : The word 'Drag' is used throughout this manual, it means pressing down the mouse left button while sliding the mouse to put the cursor at the desired location. Edit : Edit old or new schematic. When selected, a directory of schematics is shown. If you want to create a new schematic, just select the IFK-NEW. ErrChk : To ask the Post Processing to perform Error Checking, which includes Loading Analysis, Output contention checking, Net without output error checking, also generate the total worse case current consumption of the entire schematic (all pages). File : File management. Note that Pro-Net maintain its own directories and files. To Copy a schematic Page to another name, or to Rename, etc., you must use IFK-File. To Delete a file, you must use IFK-Delete under Edit mode. Copying Library Devices from one disk to another is done differently. See Section "Library Parts" for more information. Fill : Fill the enclosed area of a Box, Circle, Closed polygon-by stripes, etc. Flip : Reverse sections the Line you have just drawn, such that the horizontal section becomes the vertical section and the vertical section becomes the horizontal section. Hidden : An attribute of the piece of information being added. If this IFK is On, the piece of information being added will have an attribute of "Hidden". All information with hidden attributes will not be printed or plotted. As an example, you can go to the DefDev (Define Device) mode, call out the Device 'GND'. You will find that this Symbol uses Hidden Pin Number, Hidden Device Number label, and Hidden Device Name label. You can find some more examples in Section "Surface Power and Surface Ground traces" under "Advanced Techniques". H-Ref : When this mode is selected, clicking the Add (left) button or the Delete (right) button of the mouse will Add or Delete a Horizontal line on screen. This line is of type Note (see Note mode); which has no effect to the connections between Devices (i.e. no effect on the Net-List). It is used for alignment purpose such as lining up the Signal Name, the position of Devices, etc. Reference lines are not printed or plotted. Icc : You select this IFK when you need to enter the maximum total current consumption of the Device. This parameter is used only for the calculation of the maximum total current consumption of a voltage (the heaviest loaded one) of the design as shown in the schematic. This is to help the circuit designer to calculate the Power Supply requirements. Please also refer to IFK-Attr and Section "Defining Library Parts". Label : Label is an option under Modify mode. You can Modify the Device Number Label, the Device Type Label and the Device Pin Label with the following limitation. Device Number Label: you can change it to any other Device Number as long as that Number is not already used. You can change it to a Device Number which is already used by the same type of IC, in this case, you will be asked if you want to swap the two Device Numbers. However, it can not swap Device numbers of devices on different pages. If you really want to do that, you have to use some tricks: Step a. Change the Device Number A to an arbitrary new Device Number X. Step b. Go to the other page, change Device number B to A. Step c. Go back to the original page, change Device Number X to B. Device Pin Label: When swapping IC sections, you can Modify the Pin Label. You only need to modify any one pin in one section and the rest will be automatically modified for you. If there is only one IC section for an IC, then Modify pin is not allowed. Device Type Label: You can Modify a Device Type Label if and only if the new Device Type has the same Symbol (graphic) as the old one. For example, you can Modify a 74LS138 to a 74F138 but not 74LS139. If you really want to do that, you simply delete the old device and add the new one. Labels also appear under DefDev, they are used to define the location of the Device Name and the Device Number label. Large : Select Large Size Text. You can add Text to the Symbol being defined under the DefSym mode. You can add Text to the schematic under the Edit/Note/Text mode. Leap-N : Each time you press IFK-Leap-N, N is incremented by 1, until N=4, next press of IFK-Leap-N changes N back to 1. N represents the number of Grids (Grid size currently selected) to be Leaped over when patterns are to be repeated. In other words, 'N multiply (current Grid size)' is the distance between consecutive repeated patterns. Line : To get into the Line screen, where Lines are Added, Deleted, Adjusted in various ways. Lines form the electrical connections which will be generated in the Net List. You can use the Add (left) mouse button to start a Line, to settle and to continue the same Line. Delete a Line by clicking the delete (right) mouse button. Start a new Line by pressing the Next Key. After you draw a Line at an IC pin, you can duplicate the Line at the next lower IC pin (same IC) by using Repeat. You can Flip the orientation of a Line immediately after you draw it. i.e. change the vertical Line into a horizontal Line and change the horizontal Line into a vertical Line. You can rubber move a section of a Line easily by using Adjust (refer to IFK-Adjust). You can setup a vertical or horizontal Line for the alignment of various elements (Device, Text, Signal Name etc.) by using V- REF or H-REF. A small square at the end of the Line indicates that the Line is not connected to any other place -- even if it seems to be connected. -Logic : In Edit/Modify, it is used to Modify a positive logic gate to its DeMorgan equivalence. In DefLib/DefDev, this is to specify the DeMorgan equivalence of a logic gate. +Logic : In Edit/Modify, it is used to Modify a negative logic gate to its DeMorgan equivalence. Map : To ask the Post Processing to generate a Component Map for the schematic. For each Component, the Component Map shows you all the pages in which the Component appears. Modify : In the DefDev/Attr/PinAtt mode, Modify is used to enter or modify the attributions of the pins of a device. refer to section "Defining Library Parts" for more information. In the Schematic Edit mode, Modify is used to change Label or Logic sense (+Logic symbol or Logic sense (+Logic symbol or the -Logic symbol). Move : In this mode, click the Add button of the mouse on Devices to select them, then press IFK-OK, drag the mouse to move devices to new position and press Add button of the mouse to settle the Device. You can perform a rubber-band Move (Rubber Move) by selecting IFK-Rubber. Rubber Move allows you to move a Device without breaking its connections. You can only Rubber move one Device at a time. After the Rubber Move, you can enter the IFK-Line/Adjust mode to Adjust the Lines (refer to IFK-Adjust). Narrow : Select Narrow Lines or Stripes. Lines and Stripes has different properties. Refer to IFK-Stripes for more information. Net : Ask the Post Processing to generate a Net List for the schematic. Refer to IFK-Post for more information. New : In Edit mode, start a new schematic or a new schematic page. After a file name is given to the new page, a screen will be displayed for you to specify the Design Rule for the page. The Design Rule specifies the following : (a) The Paper Size to be used for the schematic. It is selected by entering the corresponding number (as shown on screen) when the selection Box (Bar) is at 'Paper Size' location. Standard paper size: A : 8.5 X 11 inches B : 11 X 17 inches C : 17 X 22 inches D : 22 X 34 inches E : 34 X 44 inches (b) The Template Size to be used for the schematic. Standard template sizes are those specified by the MIL-STD-860 standard or ANSI Y32.14 standard : A. FULL size B. 1/2 size C. 3/8 size E. 1/4 size (c) The Sub-libraries opened for this schematic. Press 'Y' to opening the Sub-libraries pointed to by the selection Box (or Bar). In DefLib/DefDev mode, this IFK-New is used to define a new Device. In DefLib/DefSym mode, this IFK-New is used define a new Symbol. Next To start another Line or Stripe or Bus. Or, in the DefDev/Attr/PinAtt mode, this IFK-Next is used to call out (with IFK-Recall active) the attributes of the next pin (current pin number +1). Norm : In Edit/Zoom mode, IFK-Norm always brings you back to the Normal operation screen. You can not Edit (change) anything after the schematic is Zoomed to a smaller size. Note : Note can be anything you draw or write. They will not affect the Net list of the schematic. But they will be printed or plotted. In Note mode, you can write text from left to right or from top to bottom in different fonts : small or large, normal or Bold. You can draw various types of Stripes, Boxes, Circles, Arcs in narrow or thick line, etc. NxtSct : To define the pin number of next section of the IC. OK : Tell the system to proceed since You have completed checking, or have entered the information Pro-Net needs. PgRef : To ask the Post Processing to generate the Page References for every Signal name of the schematic and insert them to the schematic automatically. -PgRef : After Page References are added to the schematic automatically by the Post Processing. You could delete a Page Reference (such as: [2,3,23,25]) using this IFK-PgRef. When this IFK is active, click the delete (right) button at the Page Reference to delete it. +PgRef : When Signals are being added to Lines or Bus, you use this IFK-+PgRef to indicate whether these signals should have page references. IFK-+PgRef active means you want page references, inactive means you don't. Page references are generated in Post processing. Please also refer to Bundle, Bus. Pick : Select the item high lighted or boxed on screen. Pin : Used to define the pin number and pin location of the Device, A pin has to be located in one of the four quadrants around the tip of a stripe (of the Symbol). If the Device has more than one section (e.g. 7400 has four sections), you can go to another section by pressing IFK- NxtSct (Next Section). Please refer to "Defining Library Parts" for more information. A pin can be defined as Hidden (not shown in schematic). A typical example of using a Hidden Pin is the Pseudo Device defined to represent the Ground Symbol. Normally you do not want to see a pin number assigned to a Ground Symbol. Please refer to "Surface-Power-Trace and Surface-Ground" in Section "Advanced Technique" for more information. PinAtt : For every Pin of a Device, there is a set of data associated with it. These data describe the following: The type of I/O. The Fan In and Fan Out capabilities. If it is a power pin, the voltage it is at. If it is a Pseudo Pin, the special characteristic. Refer to "Defining Library Parts" for more information. Plot : Enter schematic Plotting mode. Refer to Section "Printing and Plotting". Post : Enter Post-Processing operation. When IFK-Post is selected, a list of options is given to you; you can select Net, BOM, Map, PgRef, ErrChk, and the disk drive where the results should go. The list of schematic files are also given to you on the screen, if you choose a page of a schematic, the whole schematic (all pages) will be included in the Post Processing. All schematic files having the same filename (with different numeric extensions, e.g. xxx.1, xxx.2, etc.) are considered part of the schematic. Please refer to Section 3.8 : "How to generate the Net List, BOM etc". Print : Enter schematic Print out operation. Refer to Section "Printing and Plotting". Recall : In DefDev/Attr/PinAtt (Define Device/Attribute/Pin Attribute) mode, IFK-Recall is used to call out the Pin Attributes previously defined. The display shows blank entries for whichever Pin Attributes not defined previously. You can use the IFK-Next to scan through all pins of the Device being defined. Rename : In the File mode, this IFK-Rename is used to change the name of a schematic file. Note that when you change the name of any one page of the schematic, all pages of the same schematic will have their named changed also. Please refer to IFK-Copy. Repeat : In Line Mode, after you draw one line segment at a pin, if you press Repeat, the same line segment will appear on another pin (of the same IC), if any, below the current pin. Rotate : To Rotate the Device. When you call out a Device and before it is settled, the Device is rotated by 90 degree every time you press this IFK-Rotate. Rubber : You can perform a rubber-band Move (Rubber Move) by selecting IFK-Rubber. Rubber Move allows you to move a Device without breaking its connections. You can only Rubber move one Device at a time. After the Rubber Move, you can enter the IFK-Line/Adjust mode to Adjust the Lines (refer to IFK-Adjust). Rule : IFK-Rule is used to select some system options such as : Which Libraries to search for parts and Device Template size. You also have control over the Grid display, Grid Snap, and Grid Size. Allows you to change your mind after you have already started your schematic. SavDev : After you finish defining a Device, this IFK-SavDev (Save Device) allows you to Save the Device under a filename given by you. Same Device using different Symbols can be Saved under different filename. Save : Edit/More/Save saves the schematic. In Edit mode, You can also Save the schematic simply by pressing <ESC> several times until the Entry at the bottom of the screen says 'Quit, Save, or Continue', press 'S' to Save the schematic and then quit the Edit. SavPin : After all Attributes of a Device Pin are defined, you can use this IFK-SavPin to save the attributes to a Pin, at this time, you can also key in another pin number having the same pin attributes and save it. Please Refer to Section "Defining Library Parts". SavSym : Symbols are defined under DefLib/DefSym, after you finish defining the Symbol, pressing this IFK allows you to save the Symbol. There is another way to Save the Symbol, you can keep pressing <ESC> until you see a question on the entry line asking whether you would like to Save, Quit or Continue. If the answer is 's', the Symbol will be saved. SetRef : In DefLib/DefSym mode, this IFK-SetRef allows you to set one reference point on the screen, the relative positions of other points with respect to this point is shown as X, Y coordinates (relative) in units of Pixels. 3 Pixels is equal to 1 mm, and Symbols are drawn to the size of 3/8 Template (ANSI Y32.14, MIL-STD-860). Signal : Add or delete Signal Name of a line. Enter Signal Name and click (Add button) at line to add or click (Delete button) at Signal Name to delete. You can put the signal name above the line (IFK-Above), below the line (IFK-Below), or at the end of the line with a box around it (IFK-Conn, normally used for connectors). Small : Select small size Text. Step @ : Step down (IFK-Down) or up (IFK-Up) the number embedded in the Signal name and place it at the next lower line. Stripe : Lines are used to make Net List connections. Stripes are simply used to draw. In Edit/Note/Stripe mode, add or delete Stripes as Notes. In DefLib/DefSym mode, add or delete Stripes as part of the Symbol, the Stripes of a Symbol cannot be modified during schematic capture (Edit) mode. Stripes has no effect to the Net List. Unlike Lines, Stripes can go in any directions, and when two orthogonal stripes are joined together, a Dot is not automatically added. SubDir : Look into the Sub-Directory of a Library. To view the library. The list of all libraries are shown on the screen. You can select one of the libraries and browse its content. SymDir : When you try to call a Symbol (IFK-CalSym) and forgot the name of the Symbol, you can use this IFK-SymDir to browse the Directory of the Symbol Library. Text : In Edit/Note/Text mode, enter Text as notes, the Text can be added or deleted at will. In DefLib/DefSym, enter Text as part of the symbol, the Text can not be modified during schematic capture (Edit) mode. Title : Used to Call a Title Block from the library. Title Blocks have many different forms. For example, a title block may include a title area, part number area, revision level area, signature area, mechanical tolerance area, and outline of the drawing, etc. Or, the title block may include a part number area only. You can define Title Block in DefLib/DefSym as if you were defining a Symbol; the difference are: (1) When you draw the bound for the Title, you must make the bound exactly the same size as your outline of the Title Block. (2) When you save the Title Block, you must use a Symbol name "SymName.title". The SymName is any name assigned by you and ".title" is mandatory. You can find some Title block examples in the Symbol Library. Up : When IFK-Signal is active, IFK-Up forces the number embedded in the Signal label to increment by one (1) every time IFK-Step@ is pressed. Zoom Up by 2X (Devices are 2 times as big as what is currently shown. First Zoom-Up may be smaller than 2X depending on the paper size. Value : Allows you to enter the values of Passive Devices when you are entering the schematic. You do this by clicking at the Device Name Label (the color of the Label will be changed). V-Ref : When this mode is selected, clicking the Add (left) button of the mouse will add in an Vertical line on screen. This line is of type NOTE (see NOTE mode); which has no effect to the connections between Devices (i.e. no effect on the Net List). It is used for alignment purposes such as lining up the Signal Name, or the position of Devices, etc. Reference lines are not printed or plotted. Weight : To assign the priority of the line in routing. Heavier means higher priority in routing. Lines without weights are defaulted to have 0 priority. Priorities range from 0 to 999. Weights can be placed above (IFK-Above) or below (IFK- Below) the line. Weights are normally hidden during display and are not printed. Zone-1, 2, and 3 : These IFK's are used optionally to optimize the automatic Device Number assignment. The concept behind this Zone control feature is based on : - Physically separated gates should not reside in the same package (e.g. IC). - logically adjacent Devices in the schematic are likely to be physical adjacent on the PCB also. If you know the approximate locations of different sections of the logic (such as Input, Processing, and Output) on the PCB before you draw the schematic, then you can optimize the Auto Device Number assignment by selecting one of the Zones before calling out a Device from the Library. By doing so, you have avoided the situation where a section of an IC is used in one area of the PCB, while another section of the same IC is used in another area which is far apart from the first area (which would require a long trace to make use of the gate when it is connected to other parts). You can change your mind later by swapping gates or by changing the Zone assigned to a device. These are done in Modify/Label. ZoneX : To assign Device Numbers manually, select ZoneX. This is most commonly used when the Device Numbers are known in advance. For example, when you are entering an old schematic. Zoom : First time you hit zoom, the pictures shrinks so that you can see more. After that, you have the choices of Zoom Down (IFK-Down), or Zoom Up (IFK-Up). IFK-Norm always brings you back to the normal. LIBRARY PARTS: Sub-libraries Pro-Net Libraries are made up of sub-libraries such as TTL, CMOS etc. Sub-libraries must be opened before they can be used. Sub-libraries are opened when you create a new schematic page. You can also open or close Sub-libraries under the Device screen. Please refer to Section "Directory Structure" under "Terms and Conventions". User Library To increase speed, the user may want to copy part of the libraries to one library and add to it whatever he/she wants. In this case, the parts Pro-Net needs to search are substantially reduced, and only one library need be opened at all times. Library structure Each part which you call out from the library to the schematic is call a Device. The Device consists of two parts: the Symbol and the Device Specific Information (Info, in short). Their relationships is depicted as follow: Symbol + Info = Device where: Symbol contains the graphic description of the Device(s). A Symbol could be used by many different Devices as long as they have the same graphics. The user can define the Symbol under DefLib/Defsym (Define Library/Define Symbol). Info contains Device specific information such as pin number assignments, pin attributes, current consumption of the Device, etc. Besides pin number, normally, the rest of the information cannot be shared by different Devices. The user can define the Info under DefLib/DefDev (Define Library/Define Device). DEFINING LIBRARY PARTS: When you are in the Library definition mode, unlike in schematic capture mode, the template size is fixed at 3/8 (MIL STANDARD 860); therefore, the Grid sizes are also fixed. The Grid #1, #2, #3, #4 sizes are 1 mm, 2mm, 4mm, 8mm respectively. In the DefLib (Define Library) mode, the IFK-DefSym and the IFK- DefDev are used for defining the Symbol and the Device, respectively. Under the File Management section (from the main menu), you can Copy Devices from one library to another. NOTE THAT YOU CAN NOT COPY DEVICES USING AMIGA DOS FILE COPY COMMAND, SINCE PRO-NET MAINTAINS ITS OWN DIRECTORY (FOR SPEED PURPOSES). COPY DEVICES BETWEEN SUB-LIBRARIES USING AMIGA DOS FILE COPY COMMAND WILL CORRUPT THE PRO-NET DIRECTORY SYSTEM. How to Define Symbol Basically, to define a Symbol is to draw the picture which represents the Device. There are two ways to define a Symbol: (a) By Modifying an existing Symbol: You can call out an old symbol, modify it to form a new Symbol, or You can combine some old symbols to form a new Complex Symbol. However, you cannot call out an old Complex Symbol and try to modify it. (b) By Drawing the Symbol: You can create the Symbol using tools provided to you under DefSym. In the DefSym screen, you can find a set of IFK's to help you draw the Symbol. These IFK's are the Text, Stripe, Box, Circle, Arc, CalSym, Bound, Save, SetRef, and Config. Refer to the Command Description section for the details of each IFK. You could use the hot keys (refer to the TERMS & CONVENTIONS section) to control the Grid size and Grid snapping, etc. We recommend that you select Grid Snap whenever possible, this will make drawing the schematic even easier. Before you save the Symbol, you have to define the Bound (Boundary) of the Symbol. You must observe the following rules: RULE #1 Bound MUST pass through the tip of every pin on the Symbol or, if that side of the Device Body has no pin(s), must be bigger than the Device by one #2 Grid (2 mm). RULE #2 The body (outline) of the Device must be of Wide Stripes (lines) in order that you have the option of printing/plotting the Device using narrow lines or wide lines. RULE #3 When you call out an existing Symbol to be modified to another Symbol, you may not call out complex Symbols. All complex Symbols have the extension of ".C". Also, experience tells us that if you adhere to the following guide lines in defining symbols, you can draw the schematic easier, faster, and better. Nevertheless, these remain guide lines, no errors will result if you don't follow them: GUIDE #1 Keep in mind that gates (such as 7400) are defined using 3/8 template (MIL-STD-860 or ANSI Y32.14 standard) and that the smallest Grid (Grid #1) equals 1 mm. Try to draw the Symbol as small as possible while as big as needed to show all necessary details (such as the "D", "Q" etc. inside the symbol of 7474) of the symbol. Note that Grid #2, #3, #4 are 2 mm, 4 mm, 8 mm respectively when the template is 3/8 inch. GUIDE #2 Use Grid Snap whenever possible -- even if you have to bump down the Grid size to a smaller one. This will make it easier to use when connecting Lines. Normally you should try to stay on #2 Grid. GUIDE #3 If you are using a floppy disk system, the Library is distributed on several floppies. Every Library disk has one or more Device Sub-libraries AND a Symbol sub-library. Therefore, if you change or add a Symbol, not only do you have to save the Symbol to the floppy disk (which holds the sub-library) that you are working on, but also ALL other sub-library disks. If you delete a Symbol (which is unlikely), you need to do the same on ALL sub-library disks. If you have a hard disk system, you only have one Symbol Library in one place, therefore, you only need to update that one library when you modify Symbol. How to Define a Device Basically, to define a Device is to specify all the Device specific information of that Device. This information includes: -- the Symbol to use -- the location of each pin -- the Device Name. -- the default location of the Device Name Label. -- the Device Number label. -- the default location of the Device Number label. -- the Symbol to be used for the DeMorgan equivalence (if any) of the Device. -- (you may want to save the Device at this point and do something else for a while, see HINT below). -- the characteristics (attributes) of each pin. -- the current consumption of this Device. HINT : For example, if you are defining a 74LS00, save all the information to 74LS00, then also save to 74S00, 74F00, 74AS00 --- etc. Note that this is alright because up to this point, all the information you have entered for 74LS00 is shared by the corresponding Devices in the other logic families. To define a new Device or to edit an existing Device in the Library, the steps are: 1. From the main screen, Select DefLib (define library) 2. Select DefDev (Define Device) 3. Select the Sub-Library in which you want to find the old Device to edit or the new Device to store. Press IFK-OK. 4. A list of Devices in the selected Sub-Library is displayed. Scroll up and down to find the Device you want to edit or you can select IFK-New and specify a new Device Name to define a new Device. 5. At this point, start to specify all the Device specific information; type in the Symbol Name if you know which Symbol to use for this Device. Or, you can choose a Symbol from a list under DefDev/Calsym/Index. 6. After the symbol is retrieved, select IFK-Pin, enter the pin number you want to associate with a line (graphic of the pin), then click at one of the four quadrants of the tip of the pin. The pin number will appear in that quadrant near the tip of the pin. Repeat the process until all pins are specified. If you don't like what you have just defined, you can clear all pin definitions by selecting IFK-AllClr. Pin numbers can also be hidden (not shown in schematic). Select IFK-Hidden before specifying pin location. If the Device has several sections, go to the next section by using IFK-NxtSct. 7. The next thing you want to do is to specify the Label. Select IFK-Label, then IFK-DevNam. Verify that the Device name in the entry line is exactly what you want. If so, click the mouse to place DevNam at the desired location. Or, if the Device Name in the entry line is not what you want, just retype the Device Name, then click the left mouse button to place it at the desired location. Again, the Device Name can be hidden if the Hidden IFK is highlighted when the Device Name is positioned.. 8. Now you want to enter the Device Number. It is not really a number, rather, it is the Prefix of the Device Number. Select DefDev/Label/DevNum, enter the Device Number (prefix), click the mouse left button to place it at the desired location. For example, for an IC, we normally call it 'U' something. In that case, enter 'U' and click the left mouse button to place it at the desired place. Again, the Device Number can be hidden. 9. If the Device has a negative logic symbol (DeMorgan equivalence), and you have already defined it using Define Symbol, then you can select IFK--Logic, enter the Symbol name, and <CR>. 10. Now, you are almost done, the remaining task is to define the Attributes of the Device. This is necessary if you want Pro-Net to perform Loading Analysis for you or to perform the Power Consumption Calculation for you. Also, any pins which were not drawn must be specified here if they are to be included in the Net List (useful for Power Pins on Devices with multiple gates, such as a 7400). Under Attr (Attributes), there are the Icc (Icc) Attribute and the PinAtt (Pin Attribute). -- In Icc, enter (or reenter) the Worst Case Current consumption of the whole Device (see manufacturer's specs). -- In PinAtt, basically you call (Recall) the attributes of a pin on the screen, then modify existing attributes or enter new attributes. Do this one pin at a time until all the pins of the Device are done. You could check them by using IFK- Next to scan through all pins, make sure they are correct, then save the pin attributes using IFK-SavPin. The following IFKs help you accomplish these tasks: IFK-Recall When this IFK is selected, you could enter the pin number and recall the attributes which you have defined previously. IFK-Next Display the attribution of the next pin. IFK-Modify If you do not like the attributes displayed, you can use this IFK to modify them. To define the pin attribute, refer to the manufacturer's data book for the Device. <A> Device Pin Select one from the following list in line 1. I specify that this is an Input pin. O a totem pole Output pin. B a Bidirectional pin (including a pin of a passive device with current attributes). C an open Collector pin. a T Tri-state pin. P a pin of a Passive Device with no current attributes. V a Voltage pin such as Vcc Pin or Gnd (0 V) pin. <B> Driving Capability of the pin Fill in the WORSE CASE value of the current sunk or sourced by the pin under consideration. Specify Iih, Iil when the pin is an Input pin. Specify Ioh, Iol when the pin is an Output pin. Specify all Iih, Iil, Ioh, Iol when the pin is a Bidirectional pin. If it is Voltage pin, specify what voltage the pin is at. For example: If the pin is a 5V pin, key in a "5". If the pin is a GND pin, key in a "0". If it is a pin for a passive part, the current entries are normally ignored since the value (e.g. 1K ohm) of a passive part is entered during the schematic capture phase (when you are drawing the schematic); without the value and without knowing the exact situation in which the passive part will be used, the current attributes can not be specified. The loading analysis will flag a warning message in the .ERR (error) file saying that the passive part is not accounted for and that the manual verification for the node (which has the passive part) is needed. HINT: To reduce the amount of manual verification, you can predetermine the value and the current attributes of a passive device during DefDev and limit its usage to a particular application. This allows Pro-Net to include the passive device in the loading analysis automatically. To do this, you need to define the pin of the passive device as 'B'(Bidirectional) rather than 'P'(Passive). For example : A pull up resistor SIP, if it is pulled up to +5V, and the value is 1K ohm, then, each pin of the resistor SIP is of type 'B' and the current attributes are: Iil = 5 mA Iih = 0 Iol = 0 Ioh = 5 mA The loading analysis will take this SIP into account automatically. <C> Prolific specific characteristics This is a numeric number, each value specifies a special characteristics of the Device (or its pin): VALUE MEANING 1. Pseudo Device, for Surface Trace purpose. (see Section 9.1 Surface-Power-trace and Surface- Ground) 2. Pseudo Device, for Power Planes direct connection (Refer to section 9.1). 3. undefine | | | | | | 11. Save the Device definition. Two ways to do it are : <A> After defining the Pin Attributes, hit <ESC> to back up to one higher IFK level. Then use IFK-SavDev (Save Device) to save the Device definition. <B> Keep hitting <ESC> until you see a question in the entry line asking whether you would like to Save, Quit or Continue. If the answer is "S", the Device definition will be saved. PRINTING The printer you use is selected in the AMIGA preference. Your drawing size and template size is determined in the design rule you choose when you create that drawing. When the drawing size is bigger than the printer's printing area, Pro-Net automatically divides the drawing into sections, and print them one at a time until all done. 9.0 PLOTTING The model number of the plotter you use is selected when you configure (IFK-Config) Pro-Net. Both HPGL and some non-HPGL plotters are supported. The paper size and template size are selected in the Design Rule which you chose when you started (IFK-Edit/New) drawing that page. You could review what you have selected by using IFK- Device/ChgLib. Pro-Net does not allow you to plot a page which is bigger than what your plotter can handle. 10.0 ADVANCED TECHNIQUES: 10.1 Surface-Power-trace and Surface-Ground PROBLEM DESCRIPTION: IC pins sometimes are tied to power supply lines such as +5V or Ground. For a PCB which has a power plane and a Ground plane, there are two ways you could connect them. First, you could tie those power supply pins directly to the Power or Ground plane. Second, you could tie those non-power-supply spare pins (that should be tied to power or ground) to Power or ground through surface traces on the solder side. The reason for the second method is such that engineers could modify (let's face it, this is inevitable!) the design by cut and jump those pins. Although the above approaches are common practice among engineers, it is traditionally a problem not taken care of even by those schematic capture and PCB layout CAD systems which cost 50 times more than Pro-Net and Pro-Board. In those cases, PCB designers have to patch the Net list and put in special traces which may be forgotten in the next round of PCB updates. SOLUTION: Pro-Net and Pro-Board work hand in hand to solve the problem. Now, using Pro-Net, you can draw schematics which carry enough information so that the Pro-Board PCB Layout program could create those surface power and Surface Ground traces automatically, if desired. Using the user definable attribute feature of the library parts (see Chapter 5), we have defined some special Devices in the library. They are called the Surface Power (Ground), and PoWeR (Ground). They are defined as follows: 1. SPWR+5VN : Surface Power +5V at North Side - Prolific Special attribute = 1 indicates that this is a pseudo Device of type Surface Power or Surface Ground. 2. SPWR+5VS : Surface Power +5V at South Side - Prolific Special attribute = 1 Indicates that this is a pseudo Device of type Surface Power or Surface Ground. 3. SPWR0VS : Surface Power 0 V at South Side - Prolific Special attribute = 1 Indicates that this is a pseudo Device of type Surface Power or Surface Ground. 4. PWR+5VN : PoWeR +5V at North Side - Prolific Special attribute = 1 Indicates that this is a pseudo Device of type Surface Power or Surface Ground. 5. SPWR+5VS : Surface Power +5V at South Side - Prolific Special attribute = 1 Indicates that this is a pseudo Device of type Surface Power or Surface Ground. 6. SPWR0VS : Surface Power 0 V at South Side - Prolific Special attribute = 1 Indicates that this is a pseudo Device of type Surface Power or Surface Ground. 7. Similarly, the user could define other power supply pins with different voltages. If you connect some pins of an ordinary Device to the above pseudo Device, Pro-Net understands that you want these pins to be tied to power or ground through surface traces instead of to the power or ground planes directly. 10.2 Scattered Connectors PROBLEM DESCRIPTION: Traditionally there are several ways of drawing a connector in a schematics: 1. The connector is drawn on one page with signal names and page references. Each pin of the connector is connected to another page or pages through the signal names alone. 2. The connector is broken up into pieces of single pins or groups of pins and scattered among pages of the schematic. 3. The connector is drawn once in method 1, and again in method 2. Method 1 is best suited for schematic capture programs, as the connector could be defined as one library part. Method 2 is normally difficult for a schematic capture program because a connector of 100 pins requires the user to define 100 different library parts, each with one pin. Another problem of drawing a connector is when the connector has pin numbers other than numerics. This presents a problem both to schematic capture and to PCB layout programs. In this case, Pro-Net (and Pro-Board) requires that you use method 1 or method 3 to draw the connector. SOLUTIONS: Pro-Net allows the user to draw connectors in all three methods listed in above with certain limitations. If some of the connector pins are designated by alphanumerics other than pure numerics, then either method 1 or method 3 must be used. When Pro-Net is producing the Net List, it will perform two things on the connector: a. Connect pins of Devices to pins of the connector together through matching of the signal label. b. Connect pins of Devices to pins of the connector according to the connector label if and only if the pin number portion of the connector label is pure numerics. If you use method 1 (connector in one place) to draw the connector, correct net list is produced by step a above. If you use method 2 (scattered) to draw the connector, correct net list is produced by step b above. If you use method 3 (both ways) to draw the connector, the correct net list is produced by step a as well as step b if the designation (label) of the connector pin is purely numerical. If designation is not purely numeric, method a is used to produce the correct net list. By now, you should be confused enough to demand some examples. As you wish: EXAMPLE 1: A VME bus Euro-Din connector is used in a design. The connector pins are designated as J4 (say) -A1, J4-A2... J4-C1, -C2, -C3......etc. The correct way to draw this connector is by method 1 (in one place) or method 3 (both ways), since the pin designation is not purely numeric. Method 1: On page 20 (say) of the schematic, call out the library part which looks like: J4 is analogous to the U number of an IC. A1, A2 etc. are analogous to the pin function label of, say, the "Q" label in symbol 7474. "name 1", "name 2" etc. are signal names of lines. Connector pin 1 is defined to be the pin labeled by A1, pin 2 is A2, pin 32 is A32, pin 33 is C1, pin 63 is C31, pin 64 is C32 etc. However, all pin numbers are defined with attribute "hidden" and thus not shown on display or print out of the schematic. On Page 7 (for example) of the schematic, some pins of the connector are connected to different circuits: Method 3: On page 20 (for example) of the schematic, call out the library part which looks like: J4 is analogous to the U number of an IC. A1, A2, etc. are analogous to the pin function label of, say, the "Q" label in symbol 7474. "name 1", "name 2" etc. are signal names of lines. Connector pin 1 is defined to be the pin labeled by A1, pin 2 is A2, pin 32 is A32, pin 33 is C1, pin 63 is C31, pin 64 is C32 etc. However, all pin numbers are defined with attribute "hidden" and thus not shown on display or print out of the schematic. On Page 7 (for example) of the schematic, some pins of the connector are connected to different circuits. The connector symbol (box around pin label) is created by using IFK "Conn" (connector). Press "Conn", then type in the connector pin label such as "J4-A2", then click at the end of the line where you want the connector symbol to occur. Here, since the pin number part of the pin function label is not purely numeric, for example, the "C31" in the connector pin function label "J4-C31" is not purely numeric. Therefore, Pro-Net could not use the connector pin function label to create the correct net. In this example, Pro-Net uses the signal label "name 63" to match the one which occurs on page 20, where "name 63" is the signal name for the line which is connected to connector pin 63. The pin number label "63" is defined as "hidden" and whose pin function label is defined as "C31". Therefore, Pro-Net produce a net which specifies the connection of U22 pin 5 to J4 pin 63. EXAMPLE 2: A 50 pin D type connector is used in a design, the pin numbers of this type of connector are all pure numeric. Therefore, all three methods listed in the beginning of this section could be used. Method 1 and Method 3 are similar to example one. The following describes method 2. Method 2: Only scattered connector symbol are used. On Page 7 (for example) of the schematic, some pins of the connector are connected to different circuits. The connector symbol (box around pin label) is created by using IFK "Conn" (connector), press "Conn", then type in the connector pin label such as "J4-A2", then click at the end of the line where you want the connector symbol to occur. Here, Pro-Net uses the pin number which is embedded in the connector pin label to generate the net list connections. Thus J4 pin 2 is connected to U15 pin 12.