PADS9.2英文教程.doc

PADS9.2基础速成教材Step 1 - Create a Board Outline Board outlines are created using the drafting tools. The drafting tools are located in the Drafting toolbox. To create a board outline: 1. In the Welcome screen, click Start a new design.2. Click the Drafting Toolbar button.3. On the Drafting toolbar, click the Board Outline and Cut Out button.4. Right-click and select your shape preference.5. Draw an outline using the pointer, making a series of clicks.6. Click to complete a rectangular or circular outline. Double-click to complete a polygonal outline.Step 2 - Import a Netlist and Disperse Parts Typically, net and part design data originate in a schematic capture application and are transferred to a layout application via an ASCII netlist. Use the Import command to import ASCII files into your design. To import a netlist: 1. On the File menu, click Import.Tip: Save the design when you are prompted to.2. In the File Import dialog box, click the file type to import from the Files of type list.3. Navigate to the file to import, and click Open to import the file.4. Review any errors or warnings, in the ascii.err file, that may result from the import process. After you import nets and parts into your design, disperse the parts around the outside of the board using the Disperse components command. To disperse parts: 1. On the Tools menu, click Disperse Components. 2. Click Yes to confirm the dispersion of the parts.Step 3 - Setup Design Rules Setup all design rules, including clearance, routing, high-speed and others, within the design rule dialog boxes. To setup design rules: 1. Setup menu Design Rules.2. Click the Default button. Result: The Default Rules dialog box appears. Use this dialog box to select the type of default rule to enter. See the table below for more information.3. Click the Clearance button to enter default clearance rules. 4. Click in any one of the boxes in the matrix to change its value. 5. Click OK to apply the clearance rule changes.6. Click any other button to set default rules for the associated type. 7. Click Close to close the Default Rules dialog box.8. Click Close to close the Rules dialog box.Table11 lists and describes the rules types: Table 11. Design Rules Types Rules Type Includes rules or preferences for Clearance Minimum clearance, minimum same net clearance, trace width, drill-to-drill and part body-to-part body minimum clearances. Routing Trace topology, copper sharing, layer bias, via bias, and trace protection level. High Speed Parallelism, shielding, and thresholds for trace length, delay capacitance, and impedance. Fanout Fanout construction (used in PADS Router only). Pad Entry Trace patterns at pad entries and exits (used in PADS Router only). Conditional Overriding unique conditions when specific design objects are adjacent to other specific design objects. The rules include minimum clearances and parallelism. Differential Pairs Net length and topology of differential pairs. Step 4 - Set Grids Several grid settings are available in PADS Layout. Set grids in the Options dialog box or using the grid modeless command. To set a design grid: Type the g modeless command followed by the grid values, and press Enter.Example: Type g50 and press Enter to set a .050” design grid. To set a via grid: Type the gv modeless command followed by the grid value, and press Enter.Example: Type gv50 and press Enter to set a .050” via grid. To set a display grid: Type the gd modeless command followed by the grid value, and press Enter.Example: Type gd50 and press Enter to set a .050” display grid. Tip: Setting a grid with a single value sets that value for x and y. You can set independent values for x and y by entering them as g . For example, type g 25 50 to set a .025” x and .050” y design grid. Table12 lists and describes the grid types: Table 12. Grid Types Grid Type Used for Design General placement of all objects Via Placement of vias Display Visual aid Step 5 - Place Parts The placement commands are located on the Design Toolbar. Result: You enter move component mode. To place parts: 1. Design Toolbar button Move button.2. Click a part to begin moving it.3. Right-click and choose other commands to rotate the part 90 degrees, flip it to the opposite side of the PCB or spin the part at .001 degree resolution.4. Click in the new location to place the part.Other placement commands exist that help you place parts including Radial Move, Rotate, and Spin. Step 6 - Route and Unroute Traces In PADS Layout, you convert unroutes to traces using any one of several routing commands. You can route traces with on-line checking of design rules to eliminate rule violations as you create traces. To route traces using the basic route editor: 1. Design Toolbar button Add Route button. Result: You enter basic route mode.2. Click an unroute or component pin to start routing. Result: A new trace is started with the end point attached to the pointer.3. Move the pointer and click to add new trace corners, or Shift+click to add new vias.4. Move the pointer over the completion point of the unroute, such as a component pin, and click to complete it.To route traces using the dynamic route editor: 1. Enable on-line design rule checking by typing drp and pressing Enter.2. On the Design toolbar, click the Dynamic Route button.3. Click an unroute or component pin to start routing. Result: A new trace is started with the end point attached to the pointer.4. Move the pointer in the direction of the completion point. New corners are added for you.5. Move the pointer and click to add additional trace corners, or Shift+click to add new vias.6. Move the pointer over the completion point of the unroute, such as a component pin, and click to complete it.To route using the dynamic autorouter: 1. Enable on-line design rule checking by typing drp and pressing Enter.2. On the Design toolbar, click the Auto Route button.3. Click an unroute or component pin to start the dynamic autoroute command. A new trace is added.Tip: The dynamic autorouter is a single layer autorouter. It is limited to completing traces not requiring a via. You can also reroute and unroute trace segments. Step 7 - Create Plane Layers There are two types of plane layers in PADS Layout CAM and Split/Mixed. CAM plane layers are processed using the CAM commands and are strictly intended for whole layer planes without routing. Split/Mixed are planes containing multiple plane areas, with or without routing. To create a CAM plane: 1. Setup menu Layer Definition.2. Click a layer in the layer list to set as a CAM plane.3. In the Plane type area, select CAM Plane.4. Click Assign Nets. 5. In the Plane Layer Nets dialog box, select a net and click Add to add it to the associated nets list and assign it as a plane layer for the net.6. Click OK to close the dialog box and complete the layer definition.To create a split/mixed plane: 1. Click a layer in the layer list to set as a split/mixed plane.2. In the Plane type area, click Split/Mixed Plane.3. Click Assign Nets. 4. In the Plane Layer Nets dialog box, select one or more nets and click Add to add it to the associated nets list and assign it as a plane layer for the selected nets.5. Click OK to close the dialog box and complete the layer definition.You can also create plane areas on split/mixed plane layers and split a plane area polygon. Step 8 - Check for Rule Violations Use Verify Design to check for clearance, connectivity, high speed, plane connection, test point, fabrication, and other rule violations. To check a design for rule violations: 1. Tools menu Verify Design.2. In the Check area, click the type of check to perform.3. Click Setup to set checking options.4. Click Start to start the checking.5. Violations are marked with graphical error markers at their location in the design and details are provided in the Verify Design dialog box.Table13 lists and describes the rule violation checks: Table 13. Rule Violation Checks This check Checks Clearance For violations of minimum clearance rules with options for checking other design features including same net minimum clearance, drill-to-drill, trace width, and part-to-part minimum clearances. Connectivity For trace continuity errors resulting from incomplete routing, pins not connected plane layers, and drill size greater than pad size. High Speed Specified nets for threshold violations of capacitance, impedance, delay, parallelism, and track length. It also checks for trace loops and stubs. Plane For conditions that prevent a pin or via from connecting to a plane layer. These conditions include: A pin or via has a pad size on a plane layer greater than the drill size. A pin or via has plane thermal status turned off and is not connected to the plane by some other means. A pin is isolated from the plane due to discontinuities in plane shape (opens). Test Points For violations of test point rules and preferences including minimum test point clearances, preferred side, minimum pad size, test points per net, and others. Fabrication For conditions that result in fabrication errors including acid traps, slivers, silkscreen over pad, minimal annular ring, solder bridges, and others. Latium Design Verification For violations of rules not verified in PADS Layout, including vias under SMDs and differential pairs, using a PADS-Router-based clearance rules check. Wire Bonds All die parts for violations of wire bond length, width, maximum angle, and minimum wire bond to pad rules. Step 9 - Annotate the Design You add dimensions to your design using the dimensioning tools. To dimension automatically: 1. Dimensioning toolbar button Auto button.Result: You enter Auto mode.2. Click a line segment, route segment, or round pad. The dimension attaches to the pointer.3. Click to place the dimension.To dimension by selection: 1. Click a button associated with a type of dimensioning.2. Right-click and select any snap and edge preferences you want to use. Snap and edge preferences determine where the dimension text snaps to and what alignment it will use.3. Click the first object.4. Click the second object. The dimension is attached to the pointer.5. Click to place the dimension.Step 10 - Generate Reports Reports are generated in two ways within PADS Layout. You can use the Reports command to generate several standardized reports or you can generate custom reports using Basic scripting. To generate a standardized report: 1. On the File menu, click Reports. 2. In the Report dialog box, click the report to run, and click OK to generate the report.To generate a Basic report: 1. On the Tools menu, point to Basic Scripts, and then click Basic Scr