PADS PCB MANUAL

• Chapter 1) INTRODUCING PADS-PCB
• Chapter 2) INTRO: USING PADS-PCB
• 2.1) Running the Self-Running Demonstration
• 2.2) Running the Interactive PADS-PCB Program
• Chapter 3) USING PADS-PCB
• 3.1) The Graphical User Interface
• 3.2) Changing the Grid and Layer
• 3.3) Selecting Commands from the Menu
• 3.4) Loading A Design File
• 3.5) Storing Your Job to the Disk
• 3.6) Windowing Commands
• 3.7) Assigning Colors to Items
• 3.8) Modeless Commands
• 3.9) Examining Specific Nets
• 3.10) Highlighting a Net in the Design
• 3.11) Defining the Dot Grid
• 3.12) Reviewing the Job Limits
• Chapter 4) PLACING COMPONENTS
• 4.1) Matrices and Group Rotations
• 4.2) Moving Components
• 4.3) Placing Components on the Solder Side
• 4.4) Placing Discrete Components
• 4.5) Using Alternate Decals
• 4.6) Placing a Group of Components
• 4.7) Copying a Group
• 4.8) Autoplacement with PADS-PCB
• 4.9) Gate and Pin Swapping
• 4.10) Evaluating Placement Quality
• 4.11) Other Placement Functions
• Chapter 5) TURNING CONNECTIONS INTO ROUTES
• 5.1) Interactive Routing of Connections
• 5.2) Converting a Route to a Connection
• 5.3) Changing the Width of a Route
• 5.4) Routing Tips to Remember
• 5.5) Modifying an Existing Route
• 5.6) Moving a Via or Corner
• 5.7) Cut Segment
• 5.8) Reroute Traces
• 5.9) Some Hints When Modifying Routes
• Chapter 6) AUTOROUTING WITH PADS-PCB
• 6.1) Using the Power and Ground Router
• 6.2) Using the Memory Router
• 6.3) Using the Maze Router
• Chapter 7) CHECKING THE DESIGN
• 7.1) DRC Violations
• Chapter 8) PRODUCING ARTWORK DRAWINGS
• 8.1) Producing a Drawing on a Laser Printer
• 8.2) PADS-PCB Reports
• Chapter 9) MAKING CHANGES TO YOUR DESIGN
• 9.1) Adding a New Part to the Job
• 9.2) Adding Connections to the Design
• 9.3) Removing a Pin from a Net
• 9.4) Renaming Nets and Components
• 9.5) Listing the ECO File
• 9.6) Forward Annotation of Changes
• 9.7) Changing the Size of Component Pads
• 9.8) Creating a PCB without a Schematic
• Chapter 10) CREATING PCB PARTS
• 10.1) Creating a New Part Type
• 10.2) Creating a Decal
• Chapter 11) OTHER COMMANDS
• 11.1) ASCII File Commands
• 11.2) 2-D Lines and Add Text Commands
• Chapter 12) YOUR NEXT STEP

Chapter 1) INTRODUCING PADS-PCB

If you've ever evaluated CAD before, you are probably tired of demo disks. Don't worry, this is not another demo! Instead, it is real working software, with all the capabilities and outputs of the actual software. The only limit is that the PADS-PCB Evaluation Package is limited to designs of about 30 IC's. The Evaluation Package includes some sample designs to teach you the basic operation of PADS-PCB. Once you are familiar with the operation, you are free to use PADS-PCB to design your own boards, using the 6000 parts included in the library.

You can use this Evaluation Package together with the PADS-Logic Evaluation Package. You can start with the net list database from PADS-Logic, and can see how changes in the schematic can be automatically transferred to PADS-PCB.

The installation instructions for loading the software are given in the Installation manual located at the front of this manual. If you do not have a printed copy of this manual, the instructions are located in the file INSTALL.DOC, located on this disk.

Chapter 2) INTRO: USING PADS-PCB

2.1) Running the Self-Running Demonstration

1. Make the \PADSDEMO directory your current directory by typing:
   CD \PADSDEMO<CR>
2. Then type:
   PCBDEMO<CR>

• To pause the self-running demonstration, press the space bar.
• When you are ready to continue again, press the space bar again.
• Message windows will be displayed for a fixed amount of time and are then removed to continue. If you wish to proceed faster, select any key other than the space bar.
• To exit from the self-running demonstration, press CTRL-X. (While depressing the CTRL key, select X).This will return the program to the interactive software discussed below. You can exit from PADS-PCB by pressing ALT-X. (While depressing the ALT key, select X.)

2.2) Running the Interactive PADS-PCB Program

1. First make the \PADSDEMO directory your current directory by typing:
   CD \PADSDEMO<CR>
2. Then you type:
   PCBS<CR>
   to enter the program directly, or you can type:
   PADSGO<CR>
   to enter the PADS Command Shell, used to select one of several PADS design programs. To enter the PADS-PCB program from the PADS Shell, place the mouse cursor over the box labeled PADS-PCB and select it with the left mouse button.

Should you encounter any problems, call your local dealer or, in the U.S.A., call our Technical Support Hot Line at (508) 486-3328.

Chapter 3) USING PADS-PCB

3.1) The Graphical User Interface

The Working Area is the large black area that fills the major portion of the graphic screen, not occupied by menus and the prompt line.

On the left side of the screen is the System Information Window and the Command Menu Window.

The System Information Window displays the following information (from the top):

• Cursor Position The X and Y position of the cursor with respect to the system origin (0,0).
• Grid XX The user grid in thousands of an inch.
• Level N The current layer of the design
• Width The current width for all traces and lines
• Job Name The design job name
• "Postage Stamp" Locates the position of the window relative to the circuit board.
• Menu Path This multi-line title window lists the path for the current menu.

At the bottom of the Working Area is the Prompt Line. This is the primary means of communication between you and PADS-PCB. Potential error messages are also displayed here.

3.2) Changing the Grid and Layer

The grid is currently set to 100 mils. Move the mouse, and you will see the cursor move and the X Y coordinate values update in 100 unit (.100") increments. Type:

G10 <CR>
You will see the Grid parameter in the System Information Window change to 10. When you move the mouse, movements will be in 10 mil increments instead of 100 mils, as indicated by the Cursor display. You can also set the grid to a metric value, so that you can work in millimeters, rather than inches. This is done by selecting the Parameters command in the SetUp menu.

Another important item in the System Information Window is the Level or Layer parameter. PADS-PCB supports boards with up to 30 levels. You select the level you want to place an item on by simply typing a new value for the Level Parameter. Like Grid, it can be changed by typing its first letter, "L", followed by a value from 1 to 30 (or 0 to put an item on all layers) and <CR>, indicating the new level or layer you want. The display changes to the new current layer, so you will immediately know if you have entered the correct value.

3.3) Selecting Commands from the Menu

Commands are selected in two ways, by using function keys F1 through F10 located on your keyboard, or with your mouse. The numbers to the left of the commands correspond to the function key numbers, and F10 always is the EXIT command. To select commands with the function key, simply select the corresponding number key.

To select with the mouse, move the cursor over the command option and select it with the left mouse button. When a 3-button mouse is available, menu items can be selected with the middle button by holding down this button and moving the mouse. As the mouse is moved, the highlight bar will scroll through the menu options. When the left button is pressed, the highlighted menu command is selected and the cursor returns to its position in the working area. The right mouse button always is used to select the EXIT command.

3.4) Loading A Design File

1. Select In/Out command (F1) from the main menu. A new menu will appear, with the commands of the In/Out menu.
2. Select the Job In command (F1). The prompt line at the bottom of the screen will request you to input a file name. Type: * <CR>
   
3. A pop-up directory lists the names of the job files supplied with the evaluation. Place the cursor over DEMO and press the left mouse button to bring the design file named DEMO into memory. We will use this design to explore the powers of PADS-PCB.

3.5) Storing Your Job to the Disk

1. Select the In/Out menu (F1).
2. Select Job Out (F2). You are requested to give a file name with the message: Job output file name (CR=PCB.job):
3. You should use a unique file name. Type this name, followed by <CR>. If this file already exists, you will be asked to overwrite it. Your design job is stored in a few seconds on the disk, while the Working indicator is displayed.

3.6) Windowing Commands

• Num 1 (End): Redraw the screen
• Num 2 (down arrow): Move the window down
• Num 3 (Pg Dn): Zoom out
• Num 4 (left arrow): Move the window left
• Num 6 (right arrow): Move the window right
• Num 7 (Home): Show the entire board
• Num 8 (up arrow): Move the window up
• Num 9 (Pg Up): Zoom in
• Num 0 (Ins): Reposition window with cursor in center
• Num . (Del): Start creating a window box

3.7) Assigning Colors to Items

1. Exit In/Out to the main system menu (using F10).
2. Enter the SetUp menu ( F2).
3. Select the Display function (F1). When you select Display, the design disappears and is replaced by a menu for color selection. The top row is the palette of 16 colors.
4. To assign an item on a specific layer to a desired color, move the cursor on top of the color and select with the left mouse button or F1.
5. You can assign a color to any level of any item in the database. Select one of the layer numbers that correspond to the item whose color you wish to change. A highlight box of the color selected surrounds the layer number. To make an item invisible, set it to black, the background color.
6. When you select Exit (F10), the design is redrawn with the selected colors.

3.8) Modeless Commands

• Sxxx Searches whatever the user specifies. xxx can be a part, a part with a specific pin, or an x-y coordinate.
• T xx yy Changes current text height (xx) and width (yy).
• C Select either the standard or full screen cursor.
• Gx Changes the current system grid to x mils.
• N nnn Highlight a named trace in the design.
• R n Show all lines wider than n at their real width. All traces smaller are shown as a center line.
• Ctrl PgDn Cursor position relative to last selection.
• Alt-9 Displays the requested file entered at the Prompt Line at your CRT.
• Alt-0 Displays the error messages from PADS-PCB.
• Arrow Keys Moves cursor 1 grid in the requested direction. These arrow are the separate arrow keys, not the arrow keys on the numeric keypad.

Three of these commands require further explanation, as you will use them often.

3.9) Examining Specific Nets

1. Enter the SetUp menu (F2). Select Net Attr (F5).
2. A pop-up menu appears in the Working Area. Three Signal Name entries are listed: -- All--, GND, +5V. Currently, all three are marked ON. Move the cursor over the ON in the Disp column next to All, and select (F1). The value in the Disp column marker next to ALL should change to OFF, indicating all of the nets with the exception of GND and +5V will be invisible when you repaint the screen.
3. Exit from the command with F10 and you will see that only the GND and +5V nets visible.

1. If you re-enter the Net Attr option, one of the menu choices is Add Item (F2). Select it.
2. The message:
   Net name to add&gr;
   is displayed on the Prompt Line.
3. DATA1 is one of the signals in the design. You can highlight it by typing:
   DATA1<CR>
4. DATA1 appears in the pop-up menu with the Disp value set to ON. Set DATA1 to ON and all the other net names to OFF in the pop-up menu, and exit with F10 to redisplay the design. You will now see only signal net DATA1 displayed.

3.10) Highlighting a Net in the Design

1. Set all of the nets currently marked OFF to ON with the Net Attr option. Exit from the command.
2. Type:
   N DATA1<CR>
3. You will see the net named DATA1 change color and stand out against the other nets in the layout.
4. Type:
   N <CR>
   to unhighlight the net.

3.11) Defining the Dot Grid

1. Enter SetUp (F2)
2. Select Params (F4)
3. The cursor will flash over the Dot Grid value. Type in:
   250 <CR>
   to set the Dot Grid to .250". The dot grid is redrawn and spaced at .250", rather than 1.0" intervals.

3.12) Reviewing the Job Limits

1. From the Main menu, select Reports (F8), then select Job Limits (F5).
2. Input a file name to the prompt: Job Limits Status output file name (CR=Printer):
3. The job limits will be displayed in the Working Area. For each data type in the circuit, you will see the current number used and the maximum number available. If you reach the maximum number, the software will prevent you from adding any more items.

Chapter 4) PLACING COMPONENTS

In this chapter, you will be working with a small mixed analog/digital board, to understand the principles of component placement with PADS-PCB. You will learn the interactive as well as the automatic placement commands.

Bring in job PLACE using the Job In command. The components are scattered around the edge of the board. You will be placing these on the board. Currently all of the components except the integrated circuits (IC's) are "glued" in place. This means that they cannot move until you "unglue" them with the Unglue command.

4.1) Matrices and Group Rotations

As you can see, the matrix we created is better suited to IC's oriented vertically than horizontally, so you need to rotate them. Exit back to the Place menu, and select Rotate (F3). You can either point at an individual components, and select it, or rotate all of them together. Type:
U* <CR>
and all of the IC's will rotate at the same time.

One way of determining component placement quality is by counting the total length of all connections in the design- the shorter the total length, the better the placement. As the placement proceeds, you can recheck this, in order to tell if you are improving the placement.

1. Select Exit (F10), then Auto Place (F8) again, then Net Length (F7). The prompt line gives you the current X, Y and X+Y connection length.
2. Next, you will reorder the nets to reduce or minimize the connection length. Select Length Min (F6). This automatically reorders the nodes in a net to result in the minimum connection length for that net. The connection total length is reduced, and the prompt area message indicates the "before" and "after" X, Y and total connection length.
3. Select Exit (F10) to return to the Place menu.

4.2) Moving Components

1. Select the Move (F1) command.
2. Select a component by placing the cursor over it, and pressing the left mouse button. The component, along with its connections, will be highlighted. The "Postage Stamp" in the System Information Window displays the component name, part type, logic family, and decal name.
3. As you move the cursor, the component will follow. You will also see that the connections follow the component as it moves. We call this "dynamic rubber banding."
4. You can rotate the component with Rotate (F2).
5. The component is set into position with Complete (F1).
6. Exit (F10) takes you back to the Place menu.

4.3) Placing Components on the Solder Side

1. Select Opposite (F4).
2. Move the cursor over one of the IC's, and press Select (F1). The component will appear to mirror, and will move to the opposite side, as indicated by the component outline changing color.

4.4) Placing Discrete Components

1. Glue down the IC's. Select Glue (F5) in the Place Menu, and type:
   U*<CR>
   You will see each component highlighted, in turn.
2. Make the resistors and the crystal movable by selecting Unglue (F6) and typing:
   Y*<CR>
   R*<CR>
   This will unglue the crystal and all resistors. Move each of these components onto the board. You use the connection rubber band to show the IC's to which they are connected, so you can position as close to these components as possible.

4.5) Using Alternate Decals

1. Use Pg Up to zoom in on the resistor.
2. Select Move (F1) from the Place menu, then select R1 with the cursor. When R1 is attached to the cursor, select Alternate (F5). The resistor changes to a decal that represents a "stand-up" resistor.
3. Select Complete (F1) to set the resistor R1 in place.

4.6) Placing a Group of Components

1. Using the Job In command , load the job called GROUP. You will notice there is a small analog circuit in the lower left-hand side of the board.
2. Select Group Oper (F9) from the Place menu.
3. To define the group, place the cursor in the lower left-hand corner of the group, select Define Group (F1), and pull the cursor until the Analog circuit is enclosed within the rectangle formed. Then select Complete (F1), to finish defining the group.
4. You are asked if you wish to move track segments in group not tied to grouped components. Respond with Y.
5. Use Move (F1) to move the group around. While you are moving, only the outline is displayed. When you set the group down with Complete (F1), the components and traces are redrawn.

4.7) Copying a Group

1. You can copy the group, by using Copy (F2).
2. The copy is attached to your cursor. Move it to a vacant area on the board.
3. Set it with Complete (F1). Note that the system renames the components on the copied circuit, so that duplicate part names do not exist on the board.

4.8) Autoplacement with PADS-PCB

1. A placement matrix for the IC's has been set up. If you wish to see the matrix, select Place (F4) from the main menu, then Auto Place(F8), then Set Matrix (F4), and you will see the first matrix. This is then to be used for IC's.
2. You control which components are to be acted upon by the autoplacement commands by the use of the Glue (F5) and Unglue (F6) commands. Any component that is glued will not be effected by automatic placement. Any component that is unglued, will be effected by automatic placement. To place the IC's, you must first Unglue only the IC's. Select Unglue (F6), and then in response to Select (F1), type:
   U*<CR>
3. All IC's now are unglued, including the memory chip U21 that is already on the board. We want to keep U21 in its fixed location during autoplace. To do this, select Glue (F5)and use the mouse cursor to select U21. Insure the part is fixed in place with Move (F1). You should not be able to move U21.
4. From the Auto Place (F8) menu, Select Auto II (F2).
5. Select Initial (F1) to start the Initial Placement. This command will move all the unplaced components (IC's) up on the matrix in an intelligent fashion. The placement command places parts that are closely connected to the connector or to U21 in a position as close as possible to these parts, so that this total connection length is at a minimum.

   Observe the messages that appear at the Prompt Line. In less than a minute's time, the unplaced IC's are moved onto the board and placed on the matrix. Notice that the discrete components were not placed, because they are glued down.

6. All the memory IC's except one have been placed in the two upper matrix rows. At this point, you will use the Swap command to improve the placement. The Swap command will try swapping pairs of adjacent parts to improve the placement. Select Swap Pairs (F3), and observe the messages.

4.9) Gate and Pin Swapping

1. From the Place menu, Auto Place(F8), Swap Items (F1), then Swap Gates (F2).
2. The message:
   Gate/Pin Swap Report File Name (CR=Printer):
   invites you to give a file name for the "was-is" report that is generated during the swapping process. Respond to the message giving the file the name:
   SWAP <CR>
3. Run Auto (F2) to start the automatic gate swapping function. Select Exit (F10), then repeat the sequence for Swap Pins (F3). You will find that the connection length is reduced by these operations.

4.10) Evaluating Placement Quality

1. From the Auto Place menu, select Auto II (F2), ConDensity (F5). Select Histogram (F1), and respond to the Routing Grid Size (5-250)[100]: prompt with:
   25 <CR>
   A graph will be displayed across the top of the board, and along the left side. The graphs represent the ratio of "Connections- To-Routing Channel Ratio" for each 25 mil routing channel in both the X and Y Direction. The peaks in the graph represent potential routing problem areas.
2. Select Density Map (F2), and respond to the prompt:
   Density map Grid Size (25-500)[100]:
   by typing:
   100 <CR>
   

4.11) Other Placement Functions

• Using Minimum Connection Length, or
• Minimum Connection Length, yet biased against Long Connections, or
• Minimum Length, yet biased against Angled Connections, or
• Minimum Connection Length, yet biased against Long Angled Connections.

Chapter 5) TURNING CONNECTIONS INTO ROUTES

"Routing", whether automatic or interactive, is the process of converting the logical connections into physical "traces" or "routes" either interactively or automatically. In this section, we will work with one job at two different stages, before and after routing. You will try interactive routing, and then editing routes.

5.1) Interactive Routing of Connections

1. Bring in job ROUTE, using the Job In command from the In/Out menu.
2. You will see the upper left corner of a small 2-layer circuit board. The component outlines are yellow, the pads are green, and the logical connections are white. There are no routes yet. You are going to route - that is, convert some of these logical connections into physical etch- these connections.
3. From the Main menu, select the Route (F5) command menu.
4. Place the cursor over one of the white connections -- try the vertical one connecting to pin 9 of U1, to pin 5 of U3 on the left center of the working area. Move the cursor over the connection near to pin 9 of U1 and select Route Conn (F1).
5. You will see the white connection disappear, and be replaced by a short red route (because you are on layer 2) with a grey connection at its end. By moving the cursor, you move the red route segment up, down, left, or right, at a 45 or 90 degree angle from the pin. Note the information display on the left side of the screen, with the message:
   DATA4
   U1.9
   U3.5
   Width 12
   indicating that the signal being routed is signal DATA4. It connects pin 9 of IC U1, and pin 5 of IC U3. It has a width of .012". Whenever you are routing, this display will give you the route information to tell you what you are doing. The menu now gives you a new set of options you may use while routing.
6. Next, change layers with Level (F4). The routed segment turns blue, which is the color for traces on layer 1.
7. Put a corner in the route with Add Corner (F1). You may proceed in eight directions (90 and 45 degree directions) from this corner. Try this. To put the next segment at any angle, select Angle (F3). Now the route segment follows the cursor exactly, and you can put any angle in the trace. Selecting Angle (F3) again puts you back into the 45/90o only mode again.
8. Select Level (F4) again. You will see the second route segment turn red, indicating its back on layer 2, and that a via has been put at the intersection of the two segments in the route. PADS-PCB automatically puts in vias for you.
9. Route towards the destination pin, putting in corners as appropriate. Note that the grey connection always follows the end of the route and connects it to the destination, pin 5 of U3. You can complete this route only at the correct destination pin.
10. You can stop the route without finishing it at the destination by selecting End (F8). Try this. Note the connection remains between the end of the route and the destination pin. This is a partial route. You can go on to route another connection, or move existing traces to clear up a block.
11. Put the cursor on the purple connection part of the partial route, and select Route Conn (F1) to pick up the route again. Route it to the destination pin. To complete the route, select Complete (F9). This will finish the route on the destination pin, inserting a corner to change direction if necessary to reach the pin.

5.2) Converting a Route to a Connection

1. Put the cursor on any part of the route you wish to convert to a connection, and select Unroute (F7).
2. The route will disappear, and the following message will be displayed on the Prompt Line:
   Confirm Unrouting Y/(N)?
   Type Y or F1 to confirm the process. The trace is removed and the white connection is redisplayed. If you type N or F10, the route will reappear.

5.3) Changing the Width of a Route

1. Type:
   W75<CR>
   This changes the width of the trace segment you are currently routing to a new width of .075". You will see the width change, as soon as you move the cursor. Also, the Global Width display changes to 75.
2. To change the width back to .012", type:
   W12 <CR>

You may also change the width of a trace segment, a complete trace, or a net after it is routed, with the Line Width (F7) command in the Modify (F5) option of the Route menu.

5.4) Routing Tips to Remember

• If you make a mistake in positioning a corner, you can use the Delete Corner (F2) option to back up quickly.
• You use Angle (F3) to corner at any angle, not just 45 degree or 90o.
• The Complete (F9) command is used to finish a trace; it is not an autorouter. It follows very simple rules to finish the route, and will finish only on the correct pin.
• To "copper share", you must follow the route all the way to the destination pin, putting in corners and vias as appropriate.
• Move the mouse with small movements. Let the route catch up to the cursor position before continuing.
• Have connections, traces, and pads, visible; component outlines and names invisible.
• Enlarge the view so that you see only about 4-8 IC's, not the entire board. oAs you edit routes, you will "erase" portions of some of routes and pads. They are still in the database and you should periodically repaint the screen by selecting Key 1 (End) on the numeric key pad.

5.5) Modifying an Existing Route

Moving an Existing Route Segment

1. Select the Modify (F5) option. You have a number of options available. These allow you to move the traces in a number of different ways.
2. Move the cursor over a vertical trace segment, and select Move Seg (F2). Note that as you do, the trace changes color and is highlighted. This allows you to see the entire net better while you are routing it.
3. As you move the cursor right and left, you will see the vertical segment move to follow the cursor. The route segments that connect to the vertical segment will also either extend, or retract so that they remain connected to the ends of the segment being moved. You cannot lose connectivity while routing. Position the segment where you want and complete it (F1).

5.6) Moving a Via or Corner

1. Put the cursor on a route corner, or via and select Move Corner (F1).
2. As you move the route corner, watch what happens. The segments joined by the corner, as well as the route segments forming these segments will move as the corner follows the moving cursor.
3. Select Angle (F2). In this mode, only the segments forming the corner will move. Angle is a mode command, so selecting it again will change back.

5.7) Cut Segment

1. Move the cursor onto a route segment, choose Cut Seg (F3), and watch what happens.
2. In Cut Segment mode, Swap Crn (F3) lets you move the other portion of the segment you cut originally.

5.8) Reroute Traces

1. Place the mouse cursor on a trace segment and select Reroute (F9).
2. The segment of the trace you select will turn back to a connection and you can start routing it. Start from the end of the segment closest to the cursor.
3. Continue routing the trace until you have established a new path back to the other end of the original segment and select Complete(F9) to finish it. It may take a couple of times to get use to this feature but once you do it will be very useful.

5.9) Some Hints When Modifying Routes

• Plan what you want to do before you do it. Try to think about route changes in terms of the commands in Modify Route. The most powerful are Move Corner, Move Segment and Cut Segment, and Reroute.
• When selecting a trace segment or corner, select it at an unambiguous point, not where it crosses another trace.

Chapter 6) AUTOROUTING WITH PADS-PCB

• PADS-SuperRouter is an excellent choice for complex digital through-hole designs. Based on rip-up techniques, it is capable of achieving 100% results on complex circuits.
• PADS-PowerRouter is the highest performance autorouter you can buy running on a Personal Computer. Using shove as well as rip-up algorithms, it is capable of achieving 100% routing results on most of today's circuit boards.

6.1) Using the Power and Ground Router

1. Bring in job ROUTE2. This board is unrouted.
2. From the main menu, select Route (F5), then the Auto Route option (F2).
3. Two messages will prompt you to select the routing and via grids:
   Routing Grid (25) >
   Via Grid [0]>
   You should respond to both with
   25 <CR>
4. A new message is displayed:
   Select Router Passes (F7) then select Connections to be routed You will first define the autorouting passes. Select Setup (F7) and use the mouse to select SHORT P/G in the pop-up window, then Select Exit (F10).
5. You will route the entire board, so select Board (F4). This will start the autorouter, and in the System Information Window, you will see displayed the number of connections selected for routing, and later, information on the router status and success rate.
6. Traces will be displayed as they route, with blue traces on Layer 2, and green traces on Layer l.
7. After the autorouter is complete, you are presented with the results. The autorouter has completed about 85% of the power and ground connections. The connections it has routed are excellent quality, probably very similar to manual routing. Those it did not complete either did not fit the heuristic pattern, or conflicted with others. You might interactively complete these at this time.

6.2) Using the Memory Router

1. You must first display the connections to be routed. From the Main menu, select the SetUp (F2) menu, and then select Net Attr (F5). Go to Net Attr With the mouse, select the display setting for ALL connections, changing it to ON.
2. Exit from the SetUp menu. Select the Autoroute option (F2) in the Route menu.
3. Two messages will prompt you to select the routing and via grids:
   Routing Grid (25) >
   Via Grid [0]>
   You should respond to both with:
   25 <CR>
4. A new message is displayed:
   Select Router Passes (F7) then select Connections to be routed
   You will first define the autorouting passes. Select Setup (F7), select SHORT P/G again to turn it off, then select SHORT MEMORY, HORIZ/VERT and SHORT ONLY. Then select Exit (F10).
5. You can route a specific net. Select Net (F3). You will be prompted with:
   NET NAME TO SELECT>
   Type J <CR> and <CR> again. The number of connections selected is displayed and the autorouter will start. You can watch the routes being made.
6. Next route the entire boards. Select Board (F4). The memory traces will be routed.

6.3) Using the Maze Router

1. Continue with the design where you have just routed the Memory Connections.
2. Select SetUp (F7). Turn off, or deselect all of the passes from being routed. Then select the passes named ONE VIA, THREE VIAS and FIVE VIAS. They should be highlighted as they are selected.
3. When you are done, select Exit (F10), then Board (F4) to route all connections in the circuit. As the autorouter works, the finished routes are displayed, and the results are updated in the System Information Window.
4. When the router is finished, most of the unrouted connections are near the connector. You would typically spend a few minutes editing the routes to finish the remaining connections.

Chapter 7) CHECKING THE DESIGN

7.1) DRC Violations

1. Load the job named CHECK. This is an already routed board. From the main menu, select Check (F6) and then select Spacing (F1) to begin the spacing rules checking.
2. The System Information Window will display the status of the check activity and the number of errors found. When Check is complete, you will see colored error markers displayed at the point of the errors in the design. Each colored marker indicates an error.
3. At the top of the layout there is a trace- to-text error. This is because the trace has been routed through text placed on layer one. Zoom into this area, move the trace with Modify Route, and rerun the Check function.
4. Fix the other trace-to-trace and trace-to-pad errors and rerun the Check program. The error markers will disappear, if corrected properly.

• There are three netlist checks, to let you check the finished design database against the original schematic netlist. Net lists from PADS-Logic, Schema, and Futurenet compatible systems are supported.
• The Tie Plane check command insures that all component pins which are part of a net that is a power plane are correctly connected to the plane.

Chapter 8) PRODUCING ARTWORK DRAWINGS

8.1) Producing a Drawing on a Laser Printer

1. Bring in job CHECK. We will use this design to demonstrate the post-processors.
2. From the main menu, Select the CAM (F9) menu. You will be prompted with:
   Specify CAM output sub-directory:
3. Type in the name for a new sub-directory under the CAM directory using, for example, your initials as the name of the sub-directory. A new sub-directory will be created under the CAM directory, and all output drawing files will go into it. We do this so that your software and job directories don't get cluttered with temporary work files.
4. You have four options:
   • Direct (F1) creates drawings and artwork directly.
   • Batch (F2) creates drawing from previously created CAM files.
   • Defaults (F3) lets you define the aperture table, the drill tooling, and other CAM parameters.
   • Verify (F4) produces a pen or printer plot from a photoplotting file. This lets you check your artwork file before you spend money producing a bad plot.
5. Select Direct (F1). A new command window is displayed, and you have the option to produce photoplotting, pen plot, laser printer, drill or matrix printer output. Select Laser Printer with your cursor (F1). Then select Proceed either with the mouse or with F2.
6. The menu display changes to let you select the type of drawing you want. Start with an Assembly Drawing. Select "Assy Dwg-Top Side," with the cursor. Note that 30 levels are displayed, with Level 1 and 27 highlighted. This is because Level 27 is reserved, by convention, for top assembly. (Note: Levels 23 - 30 are reserved by convention for a variety of drawings but can be used for routing, if needed). Select Proceed (F2).
7. The next menu display lets you choose which items will be plotted, highlighted in grey. For each type of output, we have already provided the typical items that appear on the drawing.
8. To change the default plot options, put the cursor on the Level 1 box to the right of Text, and select this with Select (F1). The box will change color, indicating that text is no longer selected. Select Proceed (F2) to go to the next menu.
9. The next menu lets you select the size of the drawing, rotation, and other functions. For this plot, leave these settings unchanged and select Proceed.
10. The last menu lets you store the results into a file for later plotting, or create your drawing immediately. To produce a drawing, select the label Proceed With Current Selection with the cursor, then select Proceed (F2). The system will be busy for a short period, and then begin plotting.
11. After you have produced the first drawing, try producing other types of drawings. You will see how easy it is. And if there is a drawing type that is not a standard output, you can use the general plot option to produce custom outputs.

8.2) PADS-PCB Reports

1. If you have not already done so, load a design file into memory.
2. Select the Reports (F8) menu from the main menu. Print out each of the reports, using the command options in the Reports menu to become acquainted with their contents. Any report can be printed immediately, or sent to a disk file for later review or editing.

• Net List (F1) gives the entire net list for the design.
• Unused (F3) lists all unconnected parts, gates, and pins.
• Statistics (F4) provides information on the number of routed and unrouted connections, pins, via, board density, trace length, etc.
• Job Limits (F5) indicates the maximum limits of the system and the usage with the current design.
• Part List 1(F6) and Part List 2 (F7), display the parts list in two different formats.

Chapter 9) MAKING CHANGES TO YOUR DESIGN

In this chapter you will add a large capacitor to a design, and connect it to power and ground. You will also delete pin 7 of U21 from signal 21. Finally, you will rename signal net DA00 to SIGA, and rename component U10 to U50.

1. Call up the design 1STLOOK. From the main menu, select ECO (F7).
2. Because the changes you make in the board must go to the schematic, select To Sch (F1) . The following message will be displayed:
   Output schematic ECO report file name (CR=Printer):
   Respond with a file name, for example ECOTEST, followed by <CR>. As you make changes in the design, they are automatically added to this file.

9.1) Adding a New Part to the Job

1. Select Add Part (F5). Select Keyboard I/O (F2)
2. To the prompt:
   Name of part type for new part>
   RespondL
   R*<CR>
3. The library browse command provides an easy method to scan a list of components visually. A pop-up window is presented. The bottom half shows a list of parts corresponding to your wild card command, in this case all parts beginning with R. The top half shows the symbol for the currently highlighted part. You can use the arrow keys to scroll through the list of components, or you can place the cursor over a part type and press Select (F1) to view the specific graphical symbols.
4. To add the 1/8 Watt resistor, place the mouse cursor over STD: R1/8W, choose Select (F1), and then Accept (F2).
5. The system prompts:
   Reference designator for new part>
   Respond by typing:
   R25<CR>
   The pop-up window disappears and the resistor will be attached to the cursor.
6. Move the cursor around and notice how the part follows. Set the resistor in place with Complete (F1).

1. Select Add Part (F5). Select Keyboard I/O (F2)
2. To the prompt:
   Name of part type for new part>
   Respond:
   CAP\MA20<CR>
3. The system prompts:
   Reference designator for new part>
   Respond by typing:
   C100<CR>
   The capacitor will be attached to the cursor.
4. The new capacitor appears in white attached to the cursor. You are now able to position the component in the design. Rotate it (F2), place it in the layout, and set it with Complete (F1).

9.2) Adding Connections to the Design

1. New connections are added with the trace width displayed in the System Information Window. Before adding the connection, set width to .050" with the W modeless command:
   W50 <CR>
2. Select Add Conn (F1). You may either type the connection or point at it with the mouse cursor. Put the cursor on a pin in the circuit that is connected to ground , and select it with Select (F1). Note: The component name, the selected pin, and the signal name are shown in the System Information Window. Check to see that the signal is Ground, and the Ground net is highlighted.
3. When moving the cursor, you will see a brown connection following the cursor. Move the cursor to the lower pin of the new capacitor and select F1 again to complete the connection.
4. You could continue to tie more pins to the signal with additional selections, but let's stop here. Select Exit (F10).
5. Repeat steps 2-4 to add the Power connection, +5V, to the capacitor.

1. Select Keyboard (I/O). To the prompt:
   Starting connection pin - reference designation.pin>
   
2. Type:
   R9.2 <CR>
   This selects pin 2 of R9 to start the connection. The cursor moves to this pin.
3. To connect the other end of the connection, select Keyboard I/O(F2) again. To the prompt, type:
   R4.3<CR>
4. The cursor moves to R4 pin 3, and the connection is drawn. Select Exit (F10) to complete the net.

9.3) Removing a Pin from a Net

1. First, identify this pin visually.
2. Select DisConn Pin (F4) from the ECO menu.
3. Select Keyboard I/O (F2). To the prompt:
   Pin to disconnect -- reference designation.pin>
   Type:
   U21.7 <CR>
   The cursor will move to pin 7 of U21, and the 2 routes connected to U21.7 will be highlighted. You will be asked to confirm the deletion with the prompt:
   Confirm pin disconnection from net Y/(N)?
   When you type Y, the highlighted routes will disappear, a new connection will be created, connecting U20.7 to U2.3, the two pins that were at the ends of the two removed routes. Select Exit (F10).

9.4) Renaming Nets and Components

1. From the ECO menu, select RenameNet (F3).
2. Select KeyBoard I/O (F2).
3. To the prompt:
   Name of net to rename>
   Type:
   DA00<CR>
4. The system responds
   Old net name is DA00 New Name>
   Type:
   SIGA<CR>

1. From the ECO menu, select RenamePart (F7).
2. Select KeyBoard I/O (F2).
3. To the prompt:
   Reference Designator of part>
   Type:
   U10<CR>
   U10 will be highlighted and the prompt responds:
   Reference Designator is U10 New Reference Designator
   Type:
   U50<CR>

9.5) Listing the ECO File

To the prompt asking for the file to be displayed, type the name of the file that you created:
ECOTEST<CR>

The file is displayed. To remove it, select the Esc key.

9.6) Forward Annotation of Changes

1. First, load the design file 1STLOOK using the Job In command.
2. You can view the ECO file that will be used to update the 1STLOOK design, by typing:
   Alt-9
3. To the prompt asking for the file to be displayed, type the name of the file that was created:
   REV1.ECO<CR>
   The file is displayed. To remove it, select the Esc key.
4. Select the ECO (F7) command from the Main menu. Select From Sch (F2).
5. To the prompt:
   Input schematic ECO file name>
   Type:
   REV1.ECO
6. Then, type an error output file name at the prompt line to direct all error messages into this file.
7. The file is read in, and the design is changed. You will see the parts added at the system origin, and the connections added will appear as yellow lines.

9.7) Changing the Size of Component Pads

1. From the main menu, select the SetUp (F2) menu, then select Pads (F2).
2. You will change pin 1 of the 20 pin IC to be 80 mil square pad, and pin 2 to be a 60 mil pad with a 39 mil annular hole. To the prompt:
   Name of Part Decal
   type:
   DIP20
3. The current pad definition for the DIP20 is displayed in a pop-up window. Currently all pins and pin 1 are listed. For each, there is a definition for the top layer (T), for the inner layers (I), for the bottom layer (B), and for layer 25.
4. Position the cursor over the box for the size of the pad on level T of pin 1 and select (F1). Type:
   80<CR>
   to change this value. Repeat this for the bottom level B.
5. You need a new pad definition for pin 2. Since it is not currently listed, select Add Pin (F4). To the prompt:
   Enter new pin number>
   Type:
   2<CR>
6. The current settings for pin 2 are displayed. For both the top and bottom layers, change the value in the SHP column to A (to make the shape annular), and add a new value in the column INT DIAM of 39.
7. Select Complete (F9) to confirm the change.
8. The design is redrawn with the new pad definitions for pins 1 and 2.

9.8) Creating a PCB without a Schematic

1. Load the job ONTHEFLY. The board outline and the connector have been created and placed in this design.
2. Select On-the-Fly (F8) from the In/Out menu. Select Add Part (F5), then Keyboard I/O (F2).
3. In response to the prompt:
   Name of part type for new part>
   Type:
   7404 <CR>
   A 14 pin IC is added to your cursor. This is U1, and is a 7404. Note you can rotate the part and move it around. Place the part with Complete (F1). If necessary, repaint the screen with the (End) key.
4. Repeat this step, adding a resistor with part type R1/4W.
5. Select Add Conn (F1), to add connections with the cursor, in the same way as in the ECO command. You must set the trace width with the W modeless command before adding connections.
6. You may also add traces, with the Add Route (F9) command. When this is selected, you have the same capabilities as you do when manually routing traces.

Chapter 10) CREATING PCB PARTS

10.1) Creating a New Part Type

1. Select the Create (F3) menu from the Main Menu. Then select Part Type (F6)
2. Select New Part (F1). To the prompt, respond:
   AM27C256<CR>
3. Select Part Info (F1) to modify the electrical information. This defines the PCB symbol, the part attributes that are extracted for reports, the default power and ground pins, etc.
4. The part info text screen will be presented and you proceed to fill in all the data necessary.
   • There is no part type prefix, so this line may be left blank.
   • The Logic Family defines the family with which the part is associated, i.e., TTL, CMOS, ANA (for Analog), etc. Since this is a CMOS part, enter:
     CMO
     
   • The PCB Decal entry defines the name of the physical shape that will be used for the part in the circuit board. Since this is a 28-pin DIP IC, enter:
     DIP28\400
   • Part Attributes. You may assign any type of attributes to a part. Allocate 2 attribute lines and enter in the information below in the two lines. Note that all lines start with a description, followed by a colon (:). PART DESC: 32K x 8 bit EPROM MFG #1: AMD
     (Note: You may want to add new attributes such as "Vertical Height," which may be useful for mechanical packaging or thermal analysis. Discrete parts would also have a "value" attribute and a "tolerance" attribute.)
   • The Non-Numeric Pin Number entry lets you define a part with pin names rather than numbers. As this part uses pin numbers, leave this entry as N (No).
   • The Number of Gates parameter indicates the number of gates in the part. Enter a 1.
   • The Number of Signal Pins entry is used to define standard power and ground pins in the part. The Am27C256 has 3 standard signal pins, VPP (pin 1), GND (pin 14), and +5V (pin 28), therefore, enter:
     3
   • You must define the pin number, signal name, and the track width. On the first line, enter the pin number as 1, the signal name as VPP, and the track width as 50. On the second line, enter:
     

     
     14	GND	50 <br>
     

     On the third line, enter:
     

     
     28	+5V	50
     

5. When you finish entering the electrical information, select Complete (F9).
6. Select Save (F9). A <CR> will save the part to your user library. Exit (F10) will return you to the design. You may now add this part to the design with the add Part option in the On-the-Fly (F9) command from the In/Out menu.

10.2) Creating a Decal

1. From the main menu, Select Create (F3), Part Decal (F5), and Create (F1)
2. To the prompt, give the new decal the name:
   MYPART<CR>
   The design is stored and you are in the part library editor. With the commands of the part library editor, you can make the physical outline of the part, move its name, put in terminals, relocate the part origin, put text on the decal, etc. You can create a part for either two-layer or multi-layer design.
3. It is easier to work on a 100 mil grid. Set the grid to 100 by typing:
   G100 <CR>
4. Select Terminals (F3), then Add Term (F1).
5. There is now a terminal attached to the cursor, named "1". Place the pin in the center of the screen and select Complete (F1).
6. Select Add Term (F1) again. A second terminal is added to the cursor , labeled "2". Place the terminal one cursor movement, or 100 mils, to the right of the first. If necessary, use Zoom In so you can easily move a single cursor movement. Continue placing pins 3 through 7 in this manner, with a separation of one cursor movement. Then place pin 8 above pin 7, separated by 300 mils. You can use the cursor X Y display to check the distance.
7. Place the remaining pins 9 through 14, then Exit (F10).
8. Move the cursor on top of pin 1 and select Origin (F4). This makes pin 1 the origin of the part in the design.
9. You must next create the part outline. Set the grid to 25 by typing:
   G25 <CR>
10. Select Outline (F1) and 2-D Lines (F4). Place the cursor at -25,50 by using the S modeless command:
    S-25 50<CR>
11. Select New Poly (F1), and move the cursor to 625,50. Select Add Corner (F1). Move the cursor to 625,250 and select Add Corner (F1) again. Move the cursor to -25, 250 and select Complete (F9). PADS-PCB will add the last corner and close the outline.
12. Next, define the default position of the component name. From the main Part Decal menu, select Move Name (F2), and move the name and part type to the center of the outline.
13. Select Save (F9) and respond with a <CR> to the prompt. You have created a 14 Pin IC Decal. You have now added the Decal to your user library in the actual PADS-PCB package.

Chapter 11) OTHER COMMANDS

11.1) ASCII File Commands

11.2) 2-D Lines and Add Text Commands

Chapter 12) YOUR NEXT STEP

If your designs are small, this Shareware version of PADS-PCB is more than adequate to design your circuits. Please use it with our compliments.

If you need the capability of designing circuit boards 400 or more IC's, you should consider the actual version of PADS-PCB. It has all of the features of this shareware version, plus greatly expanded system limits, and it comes with a 400 page user manual describing all of the commands of the program in detail. More than thirteen thousand engineers are using PADS-PCB today.

If you would like to put the powers of PADS- PCB to work on your next project, you can order it from your local authorized PADS Dealer or contact:

PADS Software, Inc
165 Forest St.
Marlborough, MA 01752
Tel: 1-800-554-SALES (7253)

Once again, thank you for your time and interest. We welcome any additional questions you may have about PADS-PCB or any other of our PADS products.

When you have finished your evaluation of PADS-PCB, feel free to make copies and pass it on to a friend or colleague. PADS-PCB Evaluation Guide