Expedition PCB design capture

The purpose of this lab is to practice the operation of PCB design capture and draw a basic schematic.

Introduction

There are certain important files that you will be familiar with before the end of this course:

filename.prj - the project file, which contains “pointers” to the locations of other files or folders that have
projectrelated information, such as symbol libraries or configuration files.
filename.sbk - the schematic block file, which contains graphical schematic data.
foldername.cdb - the Common Data Base folder (CDB). The CDB is the compiled version of the schematic, and is the interim data base between DC and downstream tools such as Expedition PCB.
Filename.lmc – the LibraryManager Catalogue file. This is the file that holds information about which symbol, cell, and PDB partitions reside in the Central Library.
filename.slb - the symbol partition files where schematic symbols representing logic functions are stored within the Central Library.
filename.pdb – the Part Database partition files where device information is stored within the Central Library.
filename.cel – the Cell partition files where “footprint” information is stored within the Central Library.

There are several processes and tools that you will become familiar with:

Design Capture - the processes used during schematic design creation.
The Verify tool – used to check your design for incorrect information or design mistakes.
Compile CDB - the process that compiles the design into the Common Data Base.
Packager - the process that will check the CDB to make sure it has all the relevant data, and then, if required, assign “packaging information,” such as Reference designators and pin numbers, in order to prepare the design for Expedition PCB.
CDB to BOM – the Bill Of Materials Generator utility. Used to build the bill of materials after the packager has completed.
Cross Reference – the utility that assigns page connector annotation information to off-page connector symbols in the schematic file.
Connections – used to generate netlists.

Part 1 PREPARATION

The purpose of this lab exercise is to familiarize yourself with the location of the data that you will be using for this class, and to set up some configuration files for use later in the class. Down the lab material from the website. Unzip the lab2.zip file to c:\mgtraining,

Open the dashboard application /prog/mentor/ee2007.7/2007.7EE/SDD_HOME/common/linux/bin/dash &
Browse to C:\Mgtraining. There are two folders, one named common and the other named

project.

Open the project folder. There is a completed project called example. Open it and look at the

contents.

Go back up to the Mgtraining folder and then down into the common folder and examine the

contents. Note: Normally, the objects that we have included here in the common folder would be on a server on your network. You may have a similar setup or may have a slightly different approach.

Open the Libraries folder, and then the Master folder. This is the Central Library we will be

using for the rest of the class. Notice the three files –Master.lmc,SysIndex.cbf, and CentLib.prp. These are files that are important to the way the Library Manager works.Look at the contents of the SymbolLibs, PartsDBLibs ,and CellDBLibs folders. The files in each of the folders are library object partitions.

Browse to the software load directory on this machine: C:\mentor\2000.5 \VBDC\config\vbdc
Copy cdb2bom.asc and crossref.asc from here into the C:\Mgtraining\common\config folder.

We will examine the contents of these files and edit them later in the class.

Return to the C:\Mgtraining\common folder. Make anew folder under the common folder. Name

the new folder Seed_Projects. You are going to create a seed project in this location later in this class.

Part 2.Creat a seed project

The purpose of this lab exercise is to guide you through the process of creating projects. At the end of this lab, you will have created two new projects. The first is a “seed” project. It will be created by using the Project >> New command, and then the appropriate project settings will be made. The second project will be created from the seed project, using the Project >> Copy command. The second project will be used for the rest of the exercises in this class. Create the Seed Project: Note: In “real life” the seed projects may already be created for you – in this class we will create a new seed project in order to illustrate the process.

Launch DC using Start >> Programs >> Mentor Graphics WG2000.5 >> Design Capture >>

Design Capture.

Select the Project >> New command.
In the Project Location field of the New Project Wizard, browse to the folder

C:\mgtraining\common\seed_projects using the browse button to the right of the field. click the OK button once you have selected the Seed folder.

In the Project Name field, type in the project name seed1, then click on the Next button on the

diaglogue.

We will not add any design files to this seed project, so click on the Next button at the bottom of

the diaglogue.

Examine the Project Summary, and then click on the Finish button.
Notice that the seed project you have just created is automatically the active project in DC (see the

name of the project in the Titlebar at the top of the Design Capture window).

Select the Project >> Settings pulldown menu.
On the Central Library Tab, select the Browse button beside the Central Library field. Browse to

the library: C:\mgtraining\common\libraries\master \master.lmc

Select the File Locations tab on the diaglogue. Change the Configuration file type to Project

Options. Click in the field that shows the path to the current config file and click on the Browse button. Browse to: C:\mgtraining\common\config\vbdcsys_C_seed .asc This config file was placed here for you by the system administrator for this class. Editing the project file to point to this config file, as you have just done, will cause the system to use this customized configuration file for any subsequent project that uses this seed project as a template.

click the Edit File button on the diaglogue. Look down through the config file to get an idea of

what kinds of settings can be made in this file, but don’t change anything. When you are finished, close the config file.

Click the OK button on the diaglogue.
Select the Project >> PCB Integration pulldown menu. Uncheck the checkbox labeled Forward

annotation. This will prevent anyone from reading this design into Expedition PCB before we are ready to release the project to board layout.

Next, check the checkbox labeled Packaging so that no one can accidentally run the packager in

Repackage All mode (unless and until you uncheck this box).

Make sure the checkbox labeled Back annotation is checked (on), and the option to Generate

FLATNETNAME properties is based on Schematic Net Name changes.

Click the OK button on the diaglogue. You now have a seed project that can be used as a “template”

for starting any other job that will require the same project settings. Remember that at most work environments, the seed project will be located at a shared point on the network so that everyone can access it.

Part 3 Create a project from the seed project

Create the class project:

Select the Project >> Copy command.
In the Old Project field, make sure the current project is listed as:

C:\mgtraining\common\seed_projects\seed1 \seed1.prj

In the Project Name field, type in a project name of 2101A (you do not have to type in the .prj

extension - in fact, it won’t let you).

In the Project Location field, type in the following pathname: C:\mgtraining\project\2101A.

Click on the OK button on the diaglogue.

At this point, the new project has been created, but it is not the active project. Select the Project

>> Open command, and browse to the new project location: C:\mgtraining\project\2101A\2101A.prj. Click on the Open button.

Look at the Title bar for DC. The new project, 2101A, is shown as the active project. Notice that

you did not have to close the old project first, because there can only be one project active at a time. Therefore as soon as you make the new project active, the previous active project is automatically closed.

Just as a check, use the Project >> Settings command to make sure the project settings were

correctly copied from the seed project. You should have C:\mgtraining\common\libraries\master\master.lmc listed as the central library, and all of the other settings you made previously in this diaglogue should still be in effect.

The changes you made in the Project >> PCB Integration menu should also be the same as what

you set up in the seed project. If not, call your instructor. You now have the project file that will be used for the rest of this class Part 4 Schematic and Compile This part will introduce you to the process of creating a new file, opening multiple pages of a file, placing Devices and Symbols, and saving your work. Follow the step-by-step directions below. The example pages follow the lab instructions.

Use the Project >> Open command to activate the 2101A project. file>>open, in

c:\mgtraining \project\example\ ,open the schematic files ExpPCB1.sbk, Array.sbk, in c:\mgtraining \project\opamp\, open the file opamp.sbk, and save all these files in c:\mgtraining \project\2101A\, and include all these file in the project.

Select the File >> New command. Make sure the file type on the diaglogue is set to schematic and

click the OK button.

Use the File >> Save As command to name this file D_2_A.sbk. Answer Yes to the prompt to add

this file to the project.

Select the Place >> Device command and choose DCP in the diaglogue. In parts Database tab, in

Partition, choose 5474, then in Parts found, select 74ALS00_SOP, then press place, put the device in the schematic as the figure.

Edit>> Array Copy, input 4 in number of rows, 1 in number of columns. Then place the 4

devices in the figure.

Do as in step 4 choose 74ALS1008_SOP,74ALS187_DIP and 74ALS49_SOP, and set them in

the right position as those in figure.

place>>block, a diaglogue named place block pop up, choose opamp, and then place 2 blocks at the

right of the figure, and

place>>bus, and draw the two buses DA_Bus(16:23) and

BANK(0:1),RAMWR(0:1),WR(0:1),give the name by double click the bus, and input the name in net name Note: BANK(0:1),RAMWR(0:1),WR(0:1), is one bus not three.

place>>wire, draw all the wires as tho se in the fig,.
place>>symble, find basic>CON_HIER_I;1, then place 3 devices on the left of the figure.
place>>symble, find basic>CON_HIER_O;1, then place 2 devices on the right of the figure,

give them names as those in the fig, RAMRD should give names as RAMRD~, then, connect the connectors with the buses or wires.

. Execute the Tools >> Verify… command. In the Select by Group area of the File Verify

diaglogue, make sure that only the All errors, All warnings and Schematic checkboxes are checked on. In the Options area of the diaglogue, change the Scope to Design, and click on the Repair errors button. . Click the OK button to start the Verify tool.

Once all errors have been corrected and all warnings have been understood and, if necessary, corrected, you are finished with this part of the Lab. Continue with the CDB section. The CDB The purpose of this section of the Lab exercise is to create the Common Database version of your schematic design, in order to prepare the design to be shared with downstream tools. This Lab must be completed before you will be able to do the next section of the Lab. 1. Before you compile the Common Database for any project, you should examine the FileView Tab of the Workspace to be sure that only the schematic files that are intended to be part of the project are listed. If you see extraneous files, remove them by right- clicking on the file name and choosing Remove File from Project from the resulting popup menu. This will prevent the compiler from including any schematics that are not intended to be a part of the design (for example, “junk” or experimental files).

Choose the Tools >> Other Utilities… menu. . From the list of Design Capture Utilities, choose

the Compile CDB utility and click the Apply button (or double-click on the Compile CDB utility). . Make sure the project file listed is correct. It should show C:\mgtraining\project\2101a\2101a.prj in the project file field.

Observe the Command Output window. If it says there were no errors or warnings, go on to the next step.

If there were errors or warnings, you must fix them. The log file you created, cdblog.txt, contains the same messages as the Command Output window, so that you can refer to these messages if necessary by opening the log file in the Notepad Editor. If you need help understanding the error messages, call your instructor. Once you have successfully compiled the CDB, dismiss the Command Output window, Cancel the CDB Compiler utility, and Cancel the Design Capture Utilities. You now have a commo n database for your project. The Packager This section of the Lab exercise is to create the Packaging information and update the design, in order to prepare the design to be shared with downstream tools. This Lab must be completed before you will be able to do the next Lab.

Check the Project >> Settings Design Tab to ensure that the “Absorb instance data …” option is

set. . Make sure all of your schematic files are closed.

Choose the Tools >> Other Utilities… menu.
From the list of Design Capture Utilities, choose the Packager utility and click the Apply button

(or double-click on the Packager utility).

Make sure the project file listed is correct. It should show C:\mgtraining\project\2101a\2101a.prj

in the project file field.

Leave the Packager Options set to default values (if you wish, you can check No Compile, since

we just successfully compiled the CDB a few steps ago – it is up to you).

Click the Apply button.
Observe the output window. If it says there were no errors or warnings, go on to step . If there

were errors or warnings, you must fix them. Read the .\integration\partpkg.log file which is automatically created. It contains information about any errors or warnings the packager generated.

Issue the Tools >> Other Utilities menu. Choose the CDB to BOM utility. Use all of the default

settings and create a Bill of Materials for your 21101A project. Note: if you leave the field for configuration file blank, the system will use the default config file pointed to by your project file. The default BOM output file will be called 2101A.BOM and will be located in your project folder. Open the file and examine the results.

Close all of the schematic files in your project. In the Other Utilities diaglogue, run the Cross

Reference Utility on your design with all default settings, except make sure to click on the checkbox labeled Annotate the entire design.

Issue the Tools >> Other Utilities command, and open the Connections tool. Choose your

favorite netlist style and click the Create button. Once the Netlister has finished, open the netlist file (it will be located in a subfolder that was automatically created under your project folder, called .\vbconn\output) and examine the contents. When finished, close the file.