Creating a PCB Design with OrCAD PCB Editor

Transcription

1 Creating a PCB Design with OrCAD PCB Editor This guide is focused on learning how to create a PCB (Printed Circuit board) design. The guide will make use of the PCB Flow menu that is part of this workshop material. The Lowpass Filter schematic made with OrCAD Capture CIS is used for the PCB Design. Table of Contents Creating a PCB Design with OrCAD PCB Editor... 1 Importing the schematic design into the board template... 2 Creating a board outline... 3 Constraint Manager basics... 4 Setting constraints... 5 Placing components... 6 Creating copper shapes... 8 Routing your design Adding Teardrops Checking status before creating output Creating production data (Post processing) Creating PDF documentation What did you learn? There is much more to learn in OrCAD PCB Editor Keyboard shortcuts Appendix A: Creating a template board file Use the PCB flow menu to create the board template Setup units and size of working area (canvas) Setting up Cross section of the PCB Setting colors Setting up grid settings Page 1 of 27

2 Importing the schematic design into the board template The guide will use a template that s already been designed, if you re interested then appendix A will walk you through the creation of this template. 1. Start OrCAD Capture CIS and open the Lowpass filter project created earlier with the guide 1_Creating_a_circuit_using_CaptureCIS and 3_Component_Management_using_CaptureCIS 2. Go to the Project Manager and select Tools Create Netlist 3. The board template is used as a starting point for the new PCB design. This saves time setting up units, colors and other settings. All the settings can be made once and used for each new board. Make the adjustments shown where the input board is set to the template file at C:\Cadence\Company\pcb\template\template.brd 4. In the netlist setup make sure the marked box is set to 255 chars. 5. Press OK after the value have been changed and press OK again to create the board. Page 2 of 27

3 6. Click Yes to create the allegro board directory 7. If presented with a license selection choice then pick either a licens with OrCAD PCB Designer Standard, OrCAD PCB Designer Professional or Allegro PCB Designer and Click OK Creating a board outline 8. Use PCB Flow 3. Outlines Draw/Edit board outline 9. This design is small with only a few components and for that reason the outline will also be small. NOTE: Outlines should fit the project you re working with, if you are making a motor-shield for an Arduino, the outline will have to fit the Arduino sizes. 10. Start setting the parameters, then click the command line at the bottom and type x 0 0 and press Enter to place the lower left corner of the outline at 0,0 11. Click Ok to close the Design Outline dialog Page 3 of 27

4 Constraint Manager basics Constraint Manager let you define, view and validate constraints while working. When you understand the concept behind the constraint manager it is very easy to use. This short introduction to constraint manager can be skipped if you want to set the constraints now. Constraints are split into sections - Physical where cline (trace/route) width and via types are defined - Spacing where distances (airgap) between objects on different nets are defined - Same Net Spacing where distances between objects on the same net are defined - Manufacturing where fabrication oriented rules are defined (e.g., silkscreen to pad) - Electrical where differential pairs, impedance, length and matched lengths are defined For Physical and Spacing there are a Constraint Set folder which contain a constraint set named Default. This is the place where any default constraints can be set and if nothing else is changed in Constraint Manager these settings (constraints) are used. Below are shown the key physical constraints, if a column is yellow it shows that online DRC is disabled for that constraint. Right click the column and select Analysis Mode to enable online DRC for that constraint. Similar settings can be found for Spacing constraints. In the Net section all the nets are listed including a reference to a Constraint Set that is defined in the Constraint Set folder. All nets use the Default Constraint Set until changed. All boards will require default settings for spacing, trace width and via types. These can set in the template made in Appendix A Page 4 of 27

5 Setting constraints The following constraints will be set in the constraint manager. - Spacing of 0.25mm - Route width of 0.25mm - Use via named Via40 when changing layer during routing All nets refer to the Constraint Set named Default and hence will changing the settings here ripple down on all nets. 12. Select PCB Flow 4. Constraint Setup with netlist 1. Spacing or use 13. On SCS (Spacing Constraint Set) Default set values as shown 14. Constraint Manager is an integrated part of and has no individual save button. Saving the board file will also save the constraints. 15. Go to Physical Physical Constraint Set All Layers or use PCB Flow 4. Constraint Setup with netlist 3. Physical and set as shown below a. Change Line Width Min to 0.25 b. Click the Via cell and remove Via and add Via40 c. Enable Via DRC by right clicking the column and selecting Analysis Mode Page 5 of 27

6 16. Result of changes are shown below 17. Close Constraint Manager using File Close or Ctrl + F4 18. Save the board using File Save or Ctrl + s Note: The settings above could have been done in the template since nothing was depending on specific net names. If more granularity is needed more constraint sets can be created by Right clicking on the constraint set name and choosing Create Spacing/Physical Constraint Set. Placing components Although the netlist is loaded into the board there are no component placed. PCB Editor does not require all footprints to be designed before starting the PCB Design process. When a component is selected for placement the footprint is needed and a warning is given in case it does not exist. 19. Press Home or Click the toolbar icon to fit the outline in the working area 20. To place components select PCB Flow 5. Placement 1. Component Placement or use shortcut p or use 21. Often connectors are placed close to the board outline, instead of selecting the connector in the list cross-placement from OrCAD Capture will be used to select the P1 on the schematic. Do the following and see picture on next page a. With the Placement dialog open swap back to the schematic and use left mouse button to select P1 i. Alternatively split the screen between OrCAD Capture and PCB Editor b. As a result P1 will be selected in the Placement dialog and attached to the cursor c. Use the Middle Mouse button to pan on the PCB working area and press r to rotate P1 d. Place the component approximately as shown on the picture Page 6 of 27

7 22. Now select all the components on the list. Do not click Close! a. Alternatively continue to select components on the schematic page 23. As soon as Components by refdes is checked the first component C1 is attached to the mouse. Click to place it inside the board. 24. Continue placing all parts until the list is empty. 25. Finish by clicking Close on the Placement dialog Page 7 of 27

8 26. To move components either open the Placement Dialog again or go into Placement mode where clicking a component will initiate a component move mode. The current mode can always be seen at the status bar at the bottom of PCB Editor. 27. Now click and move components. a. You can still use r to rotate and m to mirror When all components are placed there are thin yellow connection lines called Ratsnests. These connections need to be routed. Creating copper shapes Often when doing PCB Design the power nets are flooded with copper. This part of the guide will create these copper areas for the nets VCC, VEE and Just like for Placement there is a mode for working with Shapes. At the Status bar left click and select Shape Edit 29. Now PCB Editor knows that we re working with copper areas (shapes) and the Options panel to the right has relevant options for this. Page 8 of 27

9 30. Right click in the work area Add Rectangle to add a rectangular copper shape and then Right click Assign Net 31. Now click the VEE pin on P1 to assign the copper to VEE and then draw a rectangle around the complete board 32. This will complete the shape which will connect to all pins that are part of the net VEE 33. Right click Done to finish this copper shape. Page 9 of 27

10 34. We will add a new smaller copper shape for the net 0 in the lower left part of the PCB Design. This shape will also be on the top layer, so leave the settings in the Options panel. 35. Right click Add Rectangle 36. Right click Assign Net 37. Left click the bottom most pin on P1 (connected to 0 ) a. Make sure that 'Assign net name = 0 in the Options panel before continuing. 38. Draw a small rectangle that contain the 2 pins connected to Again, finish this shape by Right click Done 40. This shape takes precedence over the large shape and create a small copper shape connected to The next copper shape for VCC is on the Bottom layer. 42. In the Options panel change the Subclass to Bottom as shown Page 10 of 27

11 43. Right click Add Rectangle 44. Right click Assign Net 45. Left click the second pin from the top on P1 (connected to VCC ) a. Make sure that 'Assign net name = VCC in the Options panel. 46. Draw rectangle that covers the complete board 47. Again, finish this shape by Right click Done Now the 3 nets VCC, VEE and 0 is fully connected using copper shapes. 48. This is a good time to save your work. Press Ctrl + s Page 11 of 27

12 Routing your design The rest of the board will be routed using interactive routing functionality. 49. PCB Editor has a special routing mode which is called Etch Edit, change to this mode in the status bar like previously done. Within the Etch Edit mode there is certain functionality depending on single left click or click and keep the mouse button clicked (drag). For reference a small chart of this functionality is shown below. Main functionality to remember is highlighted with green. (cline ~ routed piece of copper) Tip: The Find panel at the right side lists what objects can be selected. If pins are unselected you cannot single click a pin and start Add Connect! 50. Now that Etch Edit is selected above the routing can start 51. Make sure that Pins, Vias and Cline Segs are enabled in the Find Panel and then go back to the Options panel and select TOP Page 12 of 27

13 52. To start routing left click on U1 pin 6 connected to the net OUT to start. The Options panel will show settings for routing. Change Line Locking to 45 and move the mouse to U1 pin 2 where OUT also is connected and notice how it autosnap to the pin. 53. Left click on U1 pin 2 to finish routing that connection and notice that spacing is automatically made between the cline and the copper shape 54. Continue routing by left clicking the pins with a ratsnest (yellow line) a. Double click to insert a via and swap layer Page 13 of 27

14 55. Left click a routed segment to slide it 56. Now do the rest of the routing using the methods just learned until there are no ratsnest lines left. 57. Save the board using Ctrl + s Page 14 of 27

15 Adding Teardrops Adding teardrops routed cline into a pad creates a better connection. If it is a drilled pin or via and if the hole gets misaligned in the copper pad there is a risk of a disconnect and adding a teardrop will reduce that problem 58. Select Route Teardrop / Tapered Trace Add Teardrop and then click on the routed nets to get teardrops added. a. You can area select everything to get Teardrops on all connections Page 15 of 27

16 Checking status before creating output Before proceeding to output generation it is very important to check the status of the PCB Design. 59. Select PCB Flow 8. Status Check or use shortcut, (comma) The status dialog will show important information before creating documentation and output. Examples are - Are all components placed - Are all nets fully routed - Any copper shapes without a net attached - Any Design Rule Check (DRC) errors and if so, any that are shorts 60. If there any issues a list of those will be shown when clicking the small color icon next to the problem. Example below although there are no issues here. 61. If there are any DRC errors you can also use the DRC Browser to run through them. (Tools DRC Browser) Page 16 of 27

17 Creating production data (Post processing) The board is finished and the final parts are to make production data and PDF documentation. 62. Select PCB Flow 10. Post Processing 63. This will open the Post Processing application that will create all the production data needed. First go to Gerber Setup and click the All ON/OFF checkbox to enable creation of all Gerber film settings. Then go to Output Data 64. The output data section has the most often used output enabled. 65. Click Save Settings to save the Post Processing setup. 66. Then click Run to create output data Page 17 of 27

18 67. At some point during the generation of output data the program will ask if you want to view the log files. Answer Yes to this (always look through any log files for warnings or errors) 68. After the post processing is finished a readme file will be shown with details about the board and data generated. Page 18 of 27

19 69. Close the Postproc status report and any other log windows. 70. Before closing the Post Processing program click Open Dir at the bottom of the dialog 71. This will open the directory with the generated output data. The zip file contain all the relevant data for the manufacturer to fabricate the board. NOTICE: It is always strongly recommended to check production data in a third-party tool before sending of for manufacturing. Always send the readme file to the manufacturer since it explains data, file naming and also specify that the gerber data should be compared against the ipc netlist data. Page 19 of 27

20 Creating PDF documentation It is very simple to create PDF documentation with the PDF Generator. 72. Select PCB Flow 11. PDF Printing to start PDF Generator 73. If the PDF Font list is empty click Refresh and Save the board when asked a. In rare occasions it can be necessary to click Refresh twice. If this does not help, make sure to check that the PS Printer Driver specified in the Printer Setup tab exists. 74. Make the following changes to the PDF Generator under PDF settings After it completes the PDF document is shown. Settings can be changed to produce output with colors, higher resolution and other details. Experiment with the settings if time allows. 75. Close PDF Generator by clicking Close 76. Save the board using File Save or Ctrl +s and close PCB Editor using File Exit This concludes the workshop. Page 20 of 27

21 What did you learn? To create a new board template (appendix A) Creating a board from a schematic Setting up constraints using Constraint Manager Placing components using OrCAD Capture Adding copper shapes Routing nets and adding teardrops to improve production quality Check the board for any errors Creating production data for PCB fabrication Creating PDF Documentation There is much more to learn in OrCAD PCB Editor Setting and routing differential pairs Setting up and routing with matched length Routing with impedance constraints Extracting nets for Signal Integrity simulation Working with 3D and collision checking Working with Flex-Rigid Autorouting Setting up fabrication checks ECAD-MCAD collaboration Dimensioning Creating Variant Assembly PDF documentation Creating your own shortcut keys Customization using scripts or SKILL API And much much more Page 21 of 27

22 Keyboard shortcuts This list of shortcuts is based on the setup that is part of downloading this workshop material. It is also part of the general Nordcad setup. Page 22 of 27

23 Appendix A: Creating a template board file Typically, it is preferred to use the same settings for units, colors etc. each time a PCB Design is made. This part of the guide will explain how such a template can be made. 1. Start PCB Editor 2. A new board must be created. Follow the steps shown in the picture below. Use the PCB flow menu to create the board template 3. The PCB Flow menu is already numerically ordered with a task sequence. This part of the guide is limited task 1 + subitems and task 2 Page 23 of 27

24 Setup units and size of working area (canvas) 4. Set as shown for the Display and Design tabs Here some of the default settings for display is specified. Place the mouse above a setting and a description will be shown explaining that setting. Page 24 of 27

25 The design pane is where the parameters for the board design is set, such as the working size. Remember to check the User units is in Millimeter. In this case the size is set to A4 which means that the PCB cannot fill more than 297x210mm. The Left X setting of -110 and Lower Y of -110 means that the coordinates of the lower left corner of the A4 is -110,-110 or in other words that 0,0 on the paper is 110mm from the left and 110 from the bottom. 5. Click OK to accept the changes Setting up Cross section of the PCB 6. Next step in the PCB flow menu under the board setup is the stack up design, also called Cross section editor. The Cross Section Editor is a tool to control the board layer thickness, material of the layers, layer count and conductivity. In this guide we won t be changing anything in the Cross section Editor. or use Page 25 of 27

26 Setting colors 7. The Color Dialog is used to set colors for all layers and objects in the board. or use First pick the color at the bottom and then set it either on an object or on the complete layer. In the example above the bottom layer is assigned the color red. Page 26 of 27

27 8. Continue and set your preferences for colors. a. Or import a set of color preferences using Import Color/Board Parameters Setting up grid settings 9. The grid setup determines the resolution of placement and routing if this is performed with grids enabled. 10. The template is now finished. 11. Save the file using File Save or Ctrl + s A template board file can contain much more information than what this guide explains. Examples are constraint settings, what via types to use, pre-placed components like connectors and also board outlines. Page 27 of 27