Reserved properties

There are many property names that are reserved and cannot be used, such as

Transfer component information system properties to PCB Editor

It is not the main focus of this chapter; however, it is necessary to explain how to transfer the schematic part properties to PCB Editor in order to understand, why the properties issue is so important not only for PCB Editor. but also for bill of materials, documentation, etc.

To generate the netlist for PCB Editor in OrCAD Capture CIS, select the design icon in the project manager window and click on Tools → Create Netlist. A window will pop up. Then click on the setup button like in Fig. 11.3.

Use the Browse button (…) to choose the correct allegro.cfg. The standard file is stored in your OrCAD install directory oolscapture folder. Select Edit to open the file (Fig. 11.4). Add the missing properties you want to transfer to allegro in appropriate sections. The syntax is “Property Name=Yes”.

We recommend to store the changed allegro.cfg not in the install directory. Move it to a user-defined folder outside installation.

All properties in Capture can be transferred to PCB Editor. The allegro.cfg has five sections for the different types of properties as you can see in Fig. 11.5.

Database systems

OrCAD allows us to use different kinds of databases. In the default installation, there is a configured SQLite database, which is free database software and easy to manage. However, it is possible to use text files (ASCII), Excel spreadsheets, Microsoft Access, and SQL database such as Microsoft SQL Server and Oracle. The first two ones may be used for testing or individuals. Access may be suitable for small workgroups, but database applications offer many advantages: comprehensive data management features, better performance for part searching, form-based entry for entering part information, safeguard against duplicate part numbers, and so on.

Before you create your database, you need to choose which database format you want to use. Then, when you create your database, you need to carefully set up its structure and organization including:

On the other side, CIS can work with database field formats for text and numbers. CIS converts different database field formats to text field format when properties are transferred to placed parts. From that perspective a good strategy is to use database views to change field format for the fields passed from existing data sources. This view can also be used to change Property Names to make them conform to CIS requirements. For example, in PLM or ERP systems the price information often may be with “currency” field format and with “gl-abc” property name, where GL means general ledgers, and ABC means activity-based costing. To get the OrCAD CIS flow working and more understandable for the users, create the “database view,” and change this field format to char or varchar and name it Price.

Note for SQLite: Use only ANSI SQL-92 compliant data types for your field formats. If you use noncompliant data types, CIS may misinterpret property values.

Connection of database and component information system

We are right now in the point that you already have defined a database with all required fields and records. Before you can start the CIS configuration, you need to define the ODBC data source for your database. This ODBC driver needs to be defined on every client system and the used data source configured must be consistent on all of the machines.

A data source consists of a database filename and an associated ODBC driver with which the database can be accessed from CIS. Because this driver needs to be defined on every client machine, it can be very time-consuming in larger teams. It can be configured by IT to manage ODBC driver as part of the user account.

If you are setting up a client-server database, or you want to link different databases, the ODBC driver also manages the connections between server and client or linked databases.

To set the ODBC driver for OrCAD 17.2, CIS needs a 64-bit driver. For that, click on Start → Settings → Control Panel → Administrative Tools → Data Sources (ODBC).

The settings file CAPTURE.INI

Capture.ini is a text file that every user needs to store in their OrCAD Capture settings. Per default, it is located in $HOMEcdssetupOrCAD_Capture17.2.0, where $HOME is defined by user variable HOME.

In this file we can find the most important information for OrCAD Capture. For CIS, we have to define

In this file you can also include the global settings such as

The database configuration file

CIS requires a database configuration (.DBC) file to make use of your part database. That is why, the first step you have to do is to create a new DBC file, which goes to administrate the transferring data from your database (Fig. 11.6) . This configuration file

Note: Keep the configuration (.DBC) file in a read-only directory that is accessible to all CIS users. You should make the directory read-only to prevent users from accidentally changing the configuration.

In OrCAD Capture CIS, you can access to this file by clicking on Options → CIS Configuration. Please consider that this option is available only when a design is opened. Immediately after clicking, a window, as shown in Fig. 11.7, pops up with many options:

Database configuration file—Part Database tab

After selecting Setup (it is considered that you have already defined a new dbc file) next window pops up (Fig. 11.8).

In the upper left corner, you find the name of the data source from the ODBC driver and a list of all available tables. You can choose which tables should be used by CIS by marking them.

The two grayed out columns are the data read from database. You can’t change this in DBC file setup. To change this data you should open the database.

On the right side of the picture, you can see Select Mapping Table. It can be set to add mechanical parts to your electrical parts. The mechanical parts are virtual parts (such as screws and nuts), which are only added to the BOM to create a complete export.

The configuration area defines all these properties:

• • Table property name—shows the property name as defined in the part database.
• • Table property type—the data type of the property.
• • Property type—one of six types indicating how Capture CIS interprets the property. Except for “Normal,” as you assign a certain type to one property, it is removed from the list of choices for other properties in the table. These assigned properties have special functions. The first four properties must be defined.
  • • Part_number—used by the Part Manager to identify the part in the database. It is the unique key.
  • • Part_type—contains the component categories, which we can see as a tree structure in CIS Explorer.
  • • Schematic_part—name of OLB/Schematic part. It is transferred as a property.
  • • PCB_footprint—footprint name for footprint preview and netlist generation.
  • • PSpice_model—not mandatory. When you set this property type, CIS activates PSpice functionality for placed parts with a value for this database property.
  • • Activepart_ID—no longer used.
  • • Normal—use this for all other properties in the table.
• • Transfer to design—check to instruct Capture CIS to copy this property to the placed part when you place it on schematic sheet, or when you link the part with database.
• • OrCAD property name—the name of the property as it appears on the placed part. This characteristic is only available when you check “Transfer to design”. Select a property name from the drop-down list or type in the user property name. If you do not enter a value, the name of the property as it appears in the database is transferred to the placed part. Use this column to change property names.
• • Internet Component Assistant (ICA) property name—no longer used.
• • Visibility—sets the visibility of the property on the schematic design. You can change the visibility settings only for properties, which are transferred to the design.
  • • —property is always invisible.
  • • —property is always visible.
  • • —schematic part (from the OLB library) defines the visibility.
• • Key—check to use the property as key during the initial part search when linking a database part. If you don’t have a value property, don’t set any key. You can specify any number of keys. Typically, you only set the key for the value property. When you link a part, Capture CIS searches for parts with that specific value in the database.
• • Browsable—check to indicate that this property in the database contains references to datasheets, drawings, or other documents. When you browse your local part database, click on hyperlink (blue, underlined) values to view the referenced documents online.
• • Update part property—check to instruct CIS to check the value of the property for placed parts against the database part’s same property value, when you update the part status of your designs.

Database configuration file—Administrative Preferences tab

This tab in the DBC file configuration allows you to customize some CIS features for your work environment (Fig. 11.9).

Here you can select

• • Allow duplicate part numbers—check to allow more than one part to use the same number in the database. This is most useful when you use parts with different associated mechanical parts. If you don’t use associated mechanical parts, disable this.
• • Part type delimiter—indicates the folder hierarchy delimiter used in the database. The default delimiter is the backslash. For example, if you use capacitorceramic in the database, Capture CIS displays ceramic as a folder in the capacitor folder.
• • Transfer blank properties—check to create a property on the placed part even if there isn’t a value for the property in the database.
• • Auto symbol refresh checking—check to enable CIS to automatically detect if symbols or footprints were updated in the configured libraries. If any changes are detected, the refresh symbols from lib command in the update menu of CIS Explorer and its corresponding icon on the toolbar are enabled. This indicates that you have to refresh the symbol or footprint information in CIS Explorer. If you do not select this check box, the refresh symbols from lib command in the update menu of CIS Explorer and its corresponding icon on the toolbar will always be enabled.
• • Delimiter for multivalues—select the character you want to use to separate multiple values in your part database.
• • Assign temporary part numbers automatically—check to have Capture CIS to create and track temporary part numbers. Temporary parts are tracked in the TMPPRTS table.
• • Temporary part number prefix—type the prefix you want to use for temporary parts, TMP is the default. Capture CIS appends the temporary part number to this prefix. You can set up a different prefix (such as the user’s initials) for each user’s temporary parts.
• • Part not present display value—the text description that you want CIS to use for variant parts set to not present (typical is DNI—Do Not Install). The property is displayed in the following locations:
  • • Part Number and Value fields in the Part Manager.
  • • Design variant columns in variant reports.
  • • Variant parts on schematic page previews and printouts.
  • • The part not present display value is not displayed in capture’s schematic core design. This property also cannot be repositioned or edited in the schematic page editor. A long value is more likely to overlap a display; therefore, try to use a fairly short text equivalent for the default Not Present value.
• • By part reference (default)—select this option to group and sort parts in BOM reports created using Crystal Reports grouped by part reference. Each part will have a unique item number. You can access part reference associations by clicking the Part Reference Associations tab in the Link Database Part command operation to improve the speed and accuracy of the search. When you choose Link Database Part, Capture CIS only searches for the associated database table and displays the parts of the appropriate type.
• • By part number—select this option to sort parts in BOM reports created using Crystal Reports by part number. Since part numbers are unique, the resulting report assigns one item number to all parts with the same part number.

Database configuration file—Relational Database tab

In the Relational Database tab (Fig. 11.10), you define the relationship between the part (primary) and relational tables in the database. In the part table the part number must be unique. In the relational table, you can have several datasheets with the same part number to collect several vendors, part documents, and so on. So you can easily see the possible replacements for your part. You can connect one part table with one relational table not with several. The “Set Relational Data” grid contains the following fields:

• • Primary table name—use this list to define the part (primary) tables in your relational database. This is the only read-only field in the grid.
• • Primary key—use this list to define the primary key that you want to use to form the relationship with the relational table.
• • Relational table—use this list to specify a relational table that has a primary foreign key relationship with the selected primary table.
• • View name—use this text field to define a friendly name for the view that will display when a user selects the primary table to create a relational query. For example, you may have the separate table called “Vendor” where you have additional entries for different vendors of some capacitors. Say, you have eight replacements for a 100n capacitor. The original capacitor has the unique entry with internal Part Number = “FC-CAP-0099” in your database. Then in the “Vendor” table you can have eight entries of possible replacements with the same internal Part Number, and you can choose which one to use as a replacement (see Fig. 11.11).

Once the database structure is defined, the ODBC driver is created, the DBC file is generated, and the capture.ini contains the proper directories, and it is possible to use CIS to design our schematics. To place the part from CIS database, run OrCAD Capture CIS, open the schematic page, and select Place → Database part from menu. The CIS Explorer window will appear, as shown in Fig. 11.11. Select the needed folder with parts in the database hierarchy, then choose the required part from the parts list in the bottom, and double click on it to place the selected component to the schematic sheet.

Ideal R, L, and C

Ideal resistors, inductors, and capacitors use only PSpiceTemplate property for simulation. This property should be defined in the schematic part. The procedure for that could be as follows:

The value for such property depending on R, L, or C is the next one:

Resistor:

R^@REFDES %1 %2 ?TOLERANCE|R^@REFDES| @VALUE TC=@TC1,@TC2 ?TOLERANCE|
.model R^@REFDES RES R=1 DEV=@TOLERANCE% TC1=@TC1 TC2=@TC2|

As you can see, the resistor PSpiceTemplate value is referencing to different other property values. These values could be defined in the database or in the schematic part:

Please consider that the pin names of your schematic part must be the same as the pin names in the PSpiceTemplate. In this case the pin names are 1 and 2 (as you can see in the PSpiceTemplate definition for the resistor). So if you have a schematic part with the pin names A and B, you should change the PSpiceTemplate accordingly.

Inductor:

L^@REFDES %1 %2 ?TOLERANCE|L^@REFDES| @VALUE ?IC/IC=@IC/ ?TOLERANCE|
.model l^@REFDES IND L=1 DEV=@TOLERANCE% TC1=@TC1 TC2=@TC2 IL1=@IL1 IL2=@IL2|

As you can see, the inductor PSpiceTemplate value is referencing to different other property values:

Capacitor:

C^@REFDES %1 %2 ?TOLERANCE|C^@REFDES| @VALUE ?IC/IC=@IC/ TC=@TC1,@TC2 ?TOLERANCE|
.model C^@REFDES CAP C=1 DEV=@TOLERANCE% TC1=@TC1 TC2=@TC2 VC1=@VC1 VC2=@VC2|

As you can see, the capacitor PSpiceTemplate value is referencing to different other property values:

The way you could define these components in the database is quite simple. One proposal is to define the PSpiceTemplate property in the schematic part and the other properties in the database.

C and L with parasitics

In some precise circuits, it may be important to define the passive components with their real parasitic parameters, to make the simulation more accurate. In such case, C and L are defined using a PSpice model. It means that you could have a subcircuit as a PSpice library (name.lib) text file containing the preliminary created or downloaded PSpice model, as shown in Fig. 11.13 (where ESL, CAP, ESR, and LEAK are the parasitic parameters; C_C1 is the base capacitance; and R_R1, L_L1, and R_R2 are the parts of the subcircuit which serve in this model as the parasitic components of real capacitor). The creation of PSpice models as subcircuits directly in OrCAD Capture is described in Chapter 7, Making and editing Capture parts.

Consider that you have your schematic part for C or L without the PSpice properties defined. It means that such C and L are not yet defined for simulation. The procedure to associate a PSpice Model to such schematic part is

Now you can manually include this new schematic part into the database. In the database, you should define new columns, where the parasitics parameters ESL, ESR, CAP, and LEAK with particular values are considered. When you place such component, values of database are transferred to the design. Thus, you may have many different capacitors in the database, with different values of capacitance and parasitic parameters, but all of them can be based on the same library part (symbol), named CAP_H in this case and stored in the PASSIVE.OLB library (Fig. 11.14).

Association of schematic part with PSpice model

In the previous paragraph, we described the steps to associate a PSpice model to a schematic part. When you have a schematic part without a PSpice model (e.g., a transistor, an opamp, IC), all you have to do is to associate PSpice model to this part, so that the pin mapping and the PSpice properties are automatically defined.

Homogeneous parts and PSpice

Suppose you have an IC package with four identical opamps inside. All you have to do to use homogeneous parts with CIS and PSpice is to associate the schematic part with the PSpice model. Then each opamp of the package will be automatically assigned to the PSpice model, and it will be possible to run a simulation.

Heterogeneous parts and PSpice

The heterogeneous parts are not supported by PSpice.

Schematic parts with more pins than the PSpice model

Consider you have a schematic part, which has more physical pins than needed for simulation. In order to allow simulation, you have to define such extra pins as Unmodeled.

In order to understand this better, consider the operational amplifier ua741 as an example. This package has eight pins, but for simulation just five pins are sufficient (in+, in−, V+, V−, and OUT). In the schematic part, click on each pin that is not used for simulation (Fig. 11.19).

Then click on the + to add a new Pin Property, select FLOAT from the drop-down list of properties, enter Unmodeled and left-click the “tick” to set the property (Fig. 11.20).

Doing this, it is possible to simulate schematic parts that have more pins than the pins that are used for simulation.

How to simulate a project designed for both printed circuit board design and simulation?

In this type of projects, there are some blocks of schematic that are not necessary for simulation. For example, you could have a DDR2, DDR3, FPGA, power supply, etc. but only the power supply must be simulated. The questions would be “Do I have to create a new project to simulate just the power supply?”. The answer is no. If you are using the schematic–simulation–layout flow with CIS, the components that you placed for designing the power supply block will be already suited for simulation. All you have to do is to create a Test Bench, which will contain a part of your schematic design for simulation. To create the Test Bench, run OrCAD Capture CIS, and follow the next steps:

Find and place parts

To find and place the CIS database part to the schematic sheet, select Place → Database Part from the Capture CIS menu while you are in the schematic page view, then the CIS Explorer window will open (Fig. 11.11). The CIS Explorer window allows you to search for and retrieve a variety of part information.

The CIS Explorer window consists of several panes:

When you select a part in the database parts window, the relational table view window (Fig. 11.30) displays all relational information that are connected to the current electrical part.

Customize Part Manager

To configure the part property display, just click on View → Configure Part Property Display. After that a window pops up (Fig. 11.32). All Properties in Selected part properties column are shown in Part Manager. Use Add/Remove button or double click to move properties to the other column.

Never remove the three properties marked with an asterisk (#, Schematic Page, and Part Status).

Part Manager features

With Part Manager opened, you have many options to do with each component. By right clicking on a single part or group of similar parts you can start these actions:

Note: Under Options → Update Part status, you have the option to enable or disable Verify Parts against .OLB libraries. If it is enabled, the command Update Part Status also checks the cache against central library part.