How to Integrate Circuit Simulation and Layout Projects in AWR Microwave Office with NI Multisim

Publish Date: Jul 17, 2019 | 5 Ratings | 4.80 out of 5 | Print | Submit your review


National Instruments provides design engineers with simulation and layout tools that enable the productive development of electronic circuits. The NI toolset covers a wide range of applications; from precise simulation of high frequency distributed elements in the AWR Microwave Office (MWO) environment, to simulation and PCB layout of low-frequency circuit in the NI Multisim environment. This tutorial provides information on how these tools can be combined to accurately design a 10 GHz Low Noise Amplifier (LNA) in MWO along with the required DC biasing circuits in NI Multisim. The PCB layout of each of the circuits are then created in the respective tools and combined in a single design in NI Ultiboard to prepare it for fabrication.

Table of Contents

  1. Application Use Case
  2. Design Example
  3. Additional resources

1. Application Use Case

RF and microwave circuits designers choose the Microwave Office Suite because of its powerful design capabilities from design capture (simulation and layout) to harmonic and time-domain simulation to synthesis and optimization and EM extraction and verification.

Once the high-frequency design is verified for performance in MWO, NI Multisim is capable of adding low-frequency circuit functionalities to it for a complete circuit design. Moreover, NI Ultiboard is capable of integrating the high-frequency circuit layout with Multisim to rapidly create a layout of a complete prototype, add mechanical and graphical shapes to the design, create 3D views of the final design, and export standard Gerber files (and others) for fabrication.

With the flexible routing of Ultiboard, all the particular details of the RF circuit affecting the frequency response are preserved (such as the transmission line bends, matching networks, and ground vias) while all the complementary low-frequency circuits are quickly routed around it.

Back to Top

2. Design Example



1.     LNA performance analysis in MWO

In the AWR Design Environment, go to File>Open Example and select the LNA_10GHz.emp project in AWR 10.04. This project shows the design of a 10 GHz LNA built on 10 mil alumina using a NEC 76038 GaAs MESFET.  Running the analysis of the circuit you can learn that the LNA has 7.7dB gain and 2.15dB NF at 10 GHz.

 Designing this amplifier in MWO you can take advantages of the real-time tuning, frequency subset Smith Chart plots of noise and matching circles, and the X-Models for discontinuities accuracy to validate the performance of the amplifier.

You can also preview the final layout of the circuit. Since only S-parameter simulation was performed, DC biasing was not included in the simulation. However in the layout DC bias pads were already included, used to properly drive the MESFET.


2.     Creating a Multisim Component for the LNA

The next step is to integrate this LNA into Multisim and create a single ready-to-fabricate PCB layout of the circuit.

To do so, in MWO go to Layout>Export and save the design file as a DXF file on your computer. Remember that the project units are in mils.

Now, go to Ultiboard and open a blank design. Go to Tools>Database>Database Manager and click on create a new part, select new PCB footprint in the pop-up dialog box.


In your new footprint design file, go to File>Import>DXF and import the DXF file that you exported from MWO. Make sure you only import the copper layer (to merge with the copper top layer) and ignore the rest of the layers and also make sure the units are set to mils.

Select the imported shapes and right-click to go to their Properties, under their copper area tab make sure you change the fill style into a solid fill style.

Now, for that part you need to create 10 pins that connect the LNA to the DC circuitry. The pins are for RF input, RF output, Drain bias, Gate bias, and 6 ground pins to be connected to the ground plane through vias (the vias created in MWO are not exported in the DXF shape, only 2D shapes are, this is why they need to be recreated in Ultiboard). To add the pins go to Place>Pins

Once you have finished editing your part layout. Go to File> Save to Database as and save the new component to the user database. The final layout of the LNA component should look similar to what you see in the preview box.


3.     DC Bias Circuit Design in Multisim

The next step in this example is to accurately validate the circuit performance of a biasing circuit that takes a 12VDC input and outputs 2 arbitrary voltage levels for Gate and Drain biasing of the MESFET at -0.7V and 5V respectively. Eventually this bias circuit will be integrated with the LNA on a single PCB.

Accurate semiconductor component models from leading manufacturers can be found in the Multisim component library, simply got to Place>Component to search all the parts in the database. 

The below circuit uses validated component models of transistors and opamps from NXP Semiconductor and Analog Devices available in Multisim’s database. Running the transient simulation you can see how the circuit outputs the desired bias levels. Also running a temperature sweep you can find out how the circuit designed for temperature compensation to maintain the same exact DC levels.

Simply drag and drop the circuit into your Multisim workspace instead of having to rebuild it from scratch.

Snippet of the DC circuit in Multisim. Drag and drop into the Multisim workspace to load the design


4.     Integration of the LNA in the Multisim Design

Now that you have a defined footprint of the high-frequency LNA, you can integrate it with the Multisim schematic to build a final PCB. Go to Tools>Component Wizard to create a new schematic component.

Follow the 7 steps of custom component creation noting that it is a footprint-only part (no SPICE model included for simulation). To learn more about custom component creation in Multisim, refer to this tutorial.

Add the LNA component to your schematic connecting the output of the DC circuitry to the Drain and Gate bias points as well as grounding the other pins. You can also add the following connectors to complete the design:

  • Two RF connectors (such as a through-hole SMA connector) for the RF input and output signals.
  • Pin headers to connect the 12VDC input

Drag and drop the below PNG image into your Multisim workspace to load the final circuit.

5.     Routing of the Final PCB Design in Ultiboard

In the final Multisim design, you can simply go to Transfer>Transfer to Ultiboard> Transfer to Ultiboard 12.0 to get your final design in Ultiboard. Start by placing the RF components on one side of the board in the required accurate positions, then you can customize the placement of the other components using the manual and automatic placement tools in Ultiboard.

Before routing this board, a few precautions have to be taken into consideration:

  1. The first routing step is to create a ground plane on the bottom layer since the LNA was designed in a microstrip transmission line configuration.
  2.  The traces routing the RF input and output must pertain the same width to preserve any impedance matching.
  3. All the vias placed on the ground pads of the LNA must have the same exact diameter of the simulated vias in MWO (50 mils).
  4. Finally all the routing traces on the low frequency side should be away from the high frequency side except for the traces providing the DC bias to the RF amplifier.

Using Ultiboard productive PCB routing, all these tasks were intuitively accomplished. Copper pouring areas, Company logo graphics, and description text could also be added to the final layout. Gerber files of the final design could be exported from Ultiboard to send to fabrication.



Back to Top

3. Additional resources



Back to Top

Bookmark & Share




Rate this document

Answered Your Question?
Yes No