Advertisement

Article

Take your op amp from Pspice netlist to Allegro design sub-circuit

Introduction

You just finished looking at the data sheet specifications for an op amp that looks like a good fit for your design. You want to run simulations on your design before you head into the lab to build up a proto type.

You see the manufacture of the op amp is offering a PSPICE model netlist in their data sheet, but you are not sure how to convert the PSPICE model netlist into a sub-circuit for your simulator. If your simulator is a Cadence Allegro simulator, then this article will take you through a step-by-step process to convert the data sheet netlist into a sub-circuit for simulations. If your simulator is another type then you will need to contact the vendor who makes the op amp for support or possibly use their limited online simulation tools for your analysis.

Intersil provides a PSPICE model for all their new low-speed and low-power precision op amps at the end of the data sheets. The PSPICE model netlist and netlist schematic are included in the data sheet, along with simulation vs. characterization curves to highlight the accuracy of the PSPICE models. [To find out more about the making of these models, reference application note AN1556 for details on the making of the PSPICE models.]

Copying the PSPICE netlist

Download the data sheet or the PSPICE netlist from the web. The data sheet or netlist will be in pdf format. Open the pdf document and right click to enable the select tool, if it is not already selected. This will enable you to then copy and paste the entire netlist into notepad. Name the file with the extension . MOD (not case sensitive). This file needs to be saved in a common directory with all the other files for this design.

Model editor

Open the Cadence model editor (Cadence SPB 16.2AMS SimulatorSimulation AccessoriesModel Editor) Note: The version of Cadence software used in this example is SPB16.2. The look and feel may change with different revisions of the Cadence software, but the procedure will be the same.

After selecting the Model Editor, the Select Design Entry Tool screen will appear. Choose the Default Design Entry tool “Capture” by clicking the radial button to the left of the word “Capture”, if the default has not already selected it, and click DONE. Click on File in the tool bar and select New.

Click on Model in the tool bar and select Import. Then browse to the folder where you put the (your file name) . MOD. Select the . MOD file and click Open. This will load the netlist into the Model editor tool. Click on File in the tool bar and select Save As. Then type the part name as the file name to keep track of the project and click Save. The file with the complete netlist is now saved as a .lib library file.

Click on File in the tool bar and select Export to Capture Part Library. The Input Model Library path and the Output Part Library path will automatically be loaded. Verify that the files pathnames are the same with the only difference being the . lib and . olb extensions. Click OK and verify no Error messages or Warning messages occurred at the bottom of the screen (STATUS: 0 Errors messages, 0 Warning messages). Click OK. Click on File in the tool bar and select Model Import Wizard [Capture].

Like before, both path names will load automatically and should have the same file paths with the only difference being the . lib and . olb extensions. Click Next and the screen shown in Figure 1 will appear.

 

Figure 1: Replace generic symbol

(To see an enlarged image, click here)


This is the screen in which we will associate the pins of our PSPICE model to the pins of the sub-circuit model. The symbol shown is a generic 5-pin device. We want our op amp symbol to look like an op amp.

To do this, click on the Replace Symbol button and select from the list of symbols provided with the Cadence program. This list is located at the following location on your C drive. C:CadenceSPB.16.2toolscapturelibaryOPAmp.olb

If the location of your Cadence software was loaded in a different location, then search for CadenceSPB.

When selecting your symbol, all that matters is the pin count. The numbers assigned to the symbol pins can be changed later. Just scroll through the list to find a symbol that matches a desired pinout and pin count of your device. In this example, we selected the TLC2201. Click Next. Then click on the row under the Symbol Pin column to activate the pull-down menu box under the symbol column. Now pick the associated pin to match the Model Terminal function in the model terminal column. Repeat for all Model Terminal pins as shown in Figure 2 .

 

Figure 2: All pins associated to symbol 

(To see an enlarged image, click here )

Click Save Symbol then finish and verify no Error messages or Warning messages (STATUS: 0 Errors messages, 0 Warning messages). Click OK and then close the Model Editor. You have now created the sub-circuit to import into your simulator.

Using the new sub-circuit to run simulations

Open the Cadence Software. (Cadence SPB 16.2Design Entry CSI) From the Cadence Product Choices screen, Select Allegro Design Entry CIS and Click OK. Click on File in the tool bar and select New, and then Project. Type in the name of the project and click on the radial button to the left of Analog of Mixed A/D. Browse to where you saved the Netlist in the common directory (you must have all the files located in the same directory) and click OK.

The user can select to base the new project on an existing project or start a new one. Selecting to base upon an existing project will carry over the existing project with all the simulation profiles and schematics. This can be a real time saver if the new project is very similar to an old project. In this example, we will choose to create a new project.

Click OK. Click on . (your file name) . dsn and then the SCHEMATIC1 to open the PAGE1 tab and then Click on the PAGE1 tab. This is where the new sub-circuit will be placed to run the simulations. Before we can place the new sub-circuit model and run a simulation, we need to set-up the simulation profile and add the library.

Click on PSPICE in the tool bar and select New Simulation Profile. Then type in any name that will help you keep track of the different simulations, and click Create. Click the Configuration Files tab at the top. Then click on Library in the Category field on the left hand side.

Browse to where you saved the Library file ( . lib). Then click the Add to Design button. The Simulation Settings screen should look like that shown in Figure 3 with the file path name being the location of the common directory. Click the Apply button.

 

Figure 3: Configuration file to add library

(To see an enlarged image, click here )


 Now click the analysis tab (Figure 3) and configure the simulation for the simulation conditions desired. In this example we will setup the simulation as follows : Analysis Type = AC Sweep/Noise, Options = General Settings, Start frequency =0.1Hz, End Frequency = 100Meg Hz, Points/Decade = 100.

The analysis selected for this example is an AC Sweep/Noise. Other types of analysis are: Time Domain

(Transient), DC Sweep and Bias Point. Just click the down arrow in the analysis type section to access the different Analysis options. When done, click OK.

The user will need to add the Library . olb to the simulator. To do this, click on Place in the tool bar and select Part. This will bring up the part placement tool at the far right of the simulator, Figure 4 . To add the library, click on the tab where the arrow is pointing to in the figure.

Browse to where you saved the Netlist in the common directory, select the . olb file and click Open. The new . olb file has been added to the library list (highlighted in blue Figure 4) Now you are ready to add the sub-circuit to your simulation schematic and start your simulations.

 

Figure 4: Part placement tool

(To see an enlarged image, click here )

Adding the sub-circuit to your simulation schematic

With the . lib file added to the simulation profile and the . olb file added to the Part placement tool, you are now ready to place the op amp sub-circuit into your simulation schematic. Figure 4 shows the part placement tool after the . olb has been added to it.

Under the Libraries section of Figure 4, find the new . olb symbol you added in the previous step (highlighted in blue). Double click on the file to add the sub-circuit to the Part list section (also highlighted in blue). Double click on the Part in the part list section and add the sub-circuit to the simulation schematic. You are now able to configure the op amp for simulations.

Conclusion

The step-by-step procedure described in this article enables the user to take any PSPICE netlist and convert it into a sub-circuit for insertion into their Cadence Allegro simulator. The straightforward PSPICE models offered by Intersil (reference AN1556) make it easy for the user to edit the netlist and run worst-case simulations for some of the op amp parameters.

About the author

Don LaFontaine is a senior Principal Application Engineer/Senior Engineering Manager with Intersil's Analog/Mixed Signal product line in Palm Bay, Florida, USA. His focus is on precision analog products. He has been with Intersil Corp. for the last 30 years. He graduated from the University of South Florida with a BSEE in 1985.

Editor's note : Liked this? Want more?

If you are interested in “analog” issues such as signal input/output (sensors and transducer, real-world I/O); interfacing (level shifting, drivers/receivers); the signal chain; signal processing (op amps, filters, ADCs and DACs); and signal integrity, then go to the Planet Analog home page here for the latest in design, technology, trends, products, and news. Also, sign up for our weekly Planet Analog Newsletter here.

0 comments on “Take your op amp from Pspice netlist to Allegro design sub-circuit

Leave a Reply

This site uses Akismet to reduce spam. Learn how your comment data is processed.