Application Notes

OrCAD Capture CIS
Source: Cadence Engineering and Joe Kent June, 2002
Revised by: Gopi Rudra June, 2002
Edited by: Aoyon/Uma June, 2002

This document discusses the functionality of Capture CIS. It also highlights the advantages of Capture CIS in all stages of the PCB design process.



Component Information System™ (CIS) is a part management system that is available as an option for use with OrCAD Capture. Capture CIS helps you manage part properties within your schematic designs. Capture CIS provides access to local (preferred parts database) and remote part databases that contain all relevant information for the parts used in your designs. This information may include company part numbers, part descriptions, PCB layout footprints, technical parameters (such as speeds, tolerances, and ratings), and purchasing information.

With Capture CIS, you can select a part from your preferred parts database or a remote database and place it directly in your schematic design. You can configure Capture CIS to transfer any or all properties associated with that part to the schematic when you place the part. Capture CIS maintains a link to the engineering database part so that you can retrieve other part properties at any time. Linking placed parts to your preferred parts database gives you access to complete part information during the schematic design process. Connecting to complete part information early in the design process helps you create first-pass complete and generate accurate bills of materials, custom reports and netlists.

With Capture CIS, you can create design variants for your core design.

Using a database and libraries with Capture CIS

Different manufacturers produce the same type of components which share a schematic symbol, with differences in footprint value, tolerance value, ratings and so on. Capture CIS provides a mechanism to map multiple manufacturers information to a single schematic symbol, using an ODBC database. This unique capability of Capture CIS to use a database to extract schematics symbols, footprints, datasheets, and other data far exceeds the capability of the manual process Capture uses to extract individual pieces.

For example, multiple manufacturers produce non-polar capacitors that can share a schematic symbol with different footprint values. Another scenario would be when a single manufacturer produces multiple electrical values and tolerances of the same component identified by a unique manufacturer part number.

With Capture CIS, the same schematic symbol can be used to represent capacitors manufactured by different manufacturers or capacitors that differ only in their electrical values. For example, CAP_NP is manufactured by two companies, CAL-CHIP and AVX. Also, CAL-CHIP manufactures the same component with different electrical values, such as 100pf and 1000pf. In Capture CIS, you can use CAP_NP to represent all these variations. In FIG 1, a single CAP_NP schematic symbol is associated with multiple part numbers with different electrical values.


Let us now see what happens when you place a Capture CIS database component to Schematic. From the database a Capacitor/Ceramic/Surface Mount/0805/50V/10% part was placed on the schematic sheet. Notice that the symbol is a standard non-polar capacitor, CAP_NP, with the value .1uF, the voltage value 50V, the tolerance value 10%, and so on.


In FIG 2, the capacitor carries over certain attributes of the database and displays the results with the part. When you review the data with the property editor, you notice that all the fields are filled in. See FIG 3A through FIG 3E.

FIG 3A shows that this part carries information regarding the fields: DATASHEET, DATASHEET2, DATASHEET3, DESCRIPTION, and DIGI_KEY#.


FIG 3B shows that this part carries information regarding the fields: Graphic, Implementation, Implementation Path, Implementation Type, and Location.



FIG 3D shows that this part carries information regarding the fields: PCB Footprint, Rating, Reference, Source Library, and Source Package.


FIG 3E shows that this part is carrying information regarding the fields: Primitive, RATING, Reference, TOLERANCE, and Value.


All this information is contained in the single part placed from the database.

When you choose another capacitor 1206, you notice that it uses the same capacitor symbol. In FIG 4, you notice that the same "SCHEMATIC PART" CAP_NP is used for this part too.



Notice in FIG 5 that both components on the schematic page use the same symbol, but they have different footprint information embedded within the symbol. In the snapshot of Property Editor, FIG 6 below, you notice the same.


In Capture, one schematic symbol can have only one footprint associated with it. The same rule as with all other electrical properties. This forces the user to create multiple parts to associate with different footprints. This, in turn, forces the user to enhance the component naming standards because two components cannot have the same name. If you have decided to append the footprint name with the actual part name followed by "/", then creating individual components for each footprint will make the library bulky. This will, in turn make the component search process slower. Note that Aliases in a Capture library do not let multiple footprints be associated with the same part.

For an example, see FIG 7. A symbol for a 0805 capacitor would be CAP_NP/0805, for a 1206 capacitor it would be CAP_NP/1206, and so on for every footprint that exists for a capacitor.


Let us now see what happens when you place a Capture component to Schematic. In FIG 8, notice that for a part you place the only information you get from Capture is the name of the symbol. This component has no information other than the value CAP_NP/0805 and the footprint information embedded.


In FIG 9, the capacitor placed from Capture libraries does not contain any attributes with the part. In the Property Editor snapshots in FIG 9, you notice the same.

FIG 9A shows that this part carries information regarding Color and Graphic.


FIG 9B shows that this part carries information regarding PCB Footprint.


FIG 9C shows that this part carries information regarding Value. You can notice that the value of Property Value is to the same as the Source Package Name.


The only way to get a schematic symbol to the page is to do a place part (not a place database part). When you try to place 1206 capacitor, you get the cap symbol with 1206 with just the footprint data. Notice the same in FIG 10.

FIG 10

Notice in FIG 11 that both components on the schematic page use the different symbols with different footprint information embedded within the symbol. With the snapshot of Property Editor FIG 11 below, you notice the same.

FIG 11

With Capture, everything is manual. With Capture CIS, the database is at your fingertips at just the push of a button to transfer the data from database to schematic. This will help in reducing the manual efforts of assigning flow-related properties at each instance/occurrence level. With Capture CIS, you now have a more efficient method of creating a schematic, maintaining components, using tried and true footprints of the same component without hunting for them, and creating bill of materials easily.

It is not necessary that all the properties mentioned in the database will be passed to the schematic design. You can control the property flow from database to schematic by property called "Transfer to Design" (See FIG12) in Capture CIS configuration. In case of Capture, all the properties at library level get transferred to the schematic and users do not have control on property transfer. FIG 12 below shows the configuration wizard for Capture CIS. You can notice that this wizard is very easy to use and user-friendly.

FIG 12

Design Variant
You often require designs, which differ from each other by a small amount. These differences can be caused by the need to customize a design for targeted market segments, geographical area, or feature set. These differences are often small and are made of incremental changes on the base design. Design variant is variation of the core design (Core Design is a schematic design from which design variants can be created) of a project that you can use to create a bill of materials for a different version of the project. All variations are kept within a single design. Design variations include different property values for common components and different or not present components for identical footprints. Capture does not support variant creation. Capture CIS supports not only variant creation but also Variant Report and Variant BOM creation. FIG 13 shows the Part Manager for Variant creation, which is easy to use.

FIG 13

Capture CIS is also capable of giving variant reports that show differences among variants. FIG 14 is an example of a Variant report. In the report, you notice that a few components are not present in one variant and a few components are reassigned to a new component.

FIG 14

Capture BOM is very simple and does not have proper alignment. Following is a BOM report taken from Capture.

Revised: Wednesday, March 13, 2002

Bill Of Materials   March 13,2002    12:59:30   Page1
Item Quantity Reference Part
1 1 C1 CAP_NP/0805
2 1 C2 CAP_NP/1206

Capture CIS allows two types of BOM creation, standard and Crystal reports.

Standard Capture CIS BOM creation allows you to choose whatever properties you want to pass to your BOM output. This also supports exporting the BOM to the .xls format. Such a report is pasted below.

Item Number Quantity Part Reference Value TOLERANCE RATING Description
1 1 C1 .1uF 10% 50V CAP,MCER,0.1µF,10%,50V,X7R,0805
2 1 C2 1000pF 10% 100V CAP,MCER,1000pF,10%,100V,NPO,1206


MURATA GRM42-6COG102K100AB     SM_C_1206  

Capture CIS Crystal Reports supports generating BOM in the .rpt format. This also allows you to export a report to a file, an MS Exchange folder, a Lotus Notes database, or MS Mail. The following are the main supported export formats.

FIG 15 shows a sample Crystal report.

FIG 15