Lesson 13: Other Tools in OrCAD Capture

Transcription

1 Lesson 13: Other Tools in OrCAD Capture Lesson Objectives After you complete this lesson you will be able to: Add inter-sheet signal references Create a cross reference report (Optional) Generate a Bill of Materials Archiving your Designs (Optional) Inter-Sheet References Use inter-sheet references to display the destinations of off-page connectors. The page numbers used in the inter-sheet cross reference data are extracted from the page number properties in the title block. Intersheet references may also be added by Page AND zones areas on the schematic pages. Zones are obtained from the format information you set up for your schematic pages in the Design Template. EMA Design Automation 265

2 Select Tools - Intersheet References or Select Tools > Annotate to add intersheet references to your design. If two wires with the same alias are to be connected, an off-page connector with the same name is required on each page. Such multi-sheet nets are the only nets that need to be inter-sheet referenced. (If a net has no off-page connector, then it won t be connected to any other page, and will not need to be intersheet referenced.) You turn the Place On Off Page Connectors option off to delete all inter-sheet references on all of the off-page connectors in the design. When pages are added, deleted, or renamed, the Annotate program by default changes the numbers in the title block, which will make the inter-sheet reference data on the off-page connectors obsolete. In this case, you can also use the Delete Inter-sheet References option to delete the inter-sheet references from all off-page connectors. Cross Referencing Parts (Optional) This OrCAD Capture tool lets you generate a cross reference report that lists every part in a design, indexed by schematic page. You can also run a portion of this report from the Design Rules Check settings. Select Tools > Cross Reference to create a part cross reference report. For each part, the cross reference report specifies the following information: Part name EMA Design Automation 266

3 Library from which the part was chosen Reference designator You can also generate a list of spare gates for each device. This portion of the report can also be generated under the Design Rules Check report. Bill of Materials A Bill of Materials (BOM) is a list of all the items you need to manufacture your design. Select Tools - Bill of Materials to create a BOM report. The company name and address data at the top of the BOM report originates from the data defined in the title block. A standard BOM contains item, quantity, part reference, and part value columns. Use the Header and Combined Property String text boxes to customize the BOM. The Header field defines the titles above each of the columns of properties in the BOM report. The Combined Property String field defines which design properties load into which columns of the report. The property names must be enclosed in curly braces {}, and must precisely match the property names as specified on the parts, including spaces and case. Use the Include File options to attach part information in a text file that is not in the schematic. EMA Design Automation 267

4 You can create non-electrical parts, such as screws, washers, or sockets, that appear in a Bill of Materials report but not in a netlist. Any part without pins is considered nonelectrical. An empty field in the BOM report indicates one of the following: The property was not attached to that part. The property was attached to the part, but its value was null for that part. The property name you specified in the Combined Property String field does not match the property name attached to the part in the design. In an include file, you specified a property for a part that is not in the design. The Bill of Materials report is a delimited ASCII text file. Instead of View Output you may now have your Bill-of-Materials output open directly in Microsoft Excel for a row and column style format using the option for Open in Excel. This tool is also considered an extractor. You can list any Part Property on the Property String line and extract the property information in a report. EMA Design Automation 268

5 Lab 13-1: Annotating Inter-Sheet References Lab Objectives After completing this lab you will be able to: Annotate inter-sheet references by Page and/or Zones Opening the Schematic 1. If the schematic has been closed, re-open Lesson Double click each schematic page to open both pages of the Lesson10 design. 3. Resize the schematic windows, and use the Zoom icons to fit the contents to the work area. 4. Use the Window pull-down menu to toggle between PAGE1 and PAGE2 or use the page tabs in the upper left corner of the Capture design area labeled with the page name. Inter-Sheet References by Page and/or Zones 1. Click in the Project Manager window and highlight the design name. 2. Select Tools - Intersheet References The Inter-sheet References window appears. OR 3. Select Tools - Annotate 4. In the Action section of the Annotate window, click on Add Intersheet References. 5. Click OK. The Inter-sheet References window appears. We will only use the top portion of the window for Off-Page Connectors at this time. The bottom portion of the command generates Inner-sheet references for Hierarchical Ports which we are not using at this time. EMA Design Automation 269

6 6. Set the following options as shown below. 7. Click OK. Observe that the inter-sheet references are set close to the off-page connectors, and they now include the specified prefix and suffix. 8. Your schematic page should look something like the following image if you used the settings above. EMA Design Automation 270

7 EMA Design Automation 271

8 Lab 13-2: Cross References (Optional) After completing this lab you will be able to: Cross reference parts Cross Reference Parts Cross Reference checking is now also available under Design Rules Checking as an option. 9. In the Project Manager window, click.\lesson10.dsn. 10. Select Tools - Cross Reference. The Cross Reference Parts window appears. 11. In the Report section, set the options as shown below. EMA Design Automation 272

9 12. Click OK. The cross reference report is displayed. This report shows where each part is located in the design (Sheet number). Observe the list of spare gates at the bottom of the report. 13. Close the report window. Observe that the cross reference report (.xrf) has been added to the Outputs folder in the Project Manager window. Saving the Design 1. In the Project Manager window, click on.\lesson10.dsn. 2. Select File - Save. This saves both pages of the design. 3. Close both schematic page windows. EMA Design Automation 273

10 Lab 13-3: Bill of Materials After completing this lab you will be able to: Create a Bill of Materials Create a Bill of Materials 1. Highlight the design name in the Project Manager window. 2. Select Tools Bill of Materials The Bill of Materials window appears. 3. Click Place each part entry on a separate line (checkbox ON). 4. Click View Output (checkbox ON). 5. (Alternate) Instead of selecting View Output, select the Open in Excel to have the BOM output open directly in Excel. EMA Design Automation December, V16.6 Rev 2 274

11 6. Click OK. The Bill of Materials report is displayed. Observe that the report contains four columns of data; Item, Quantity, Reference, Part. 7. Close the report. Closing the Lesson 10 Project 1. Select File Close Project. EMA Design Automation December, V16.6 Rev 2 275