From 3d6a9d75a78f3c82de7105ba0dcd806ce3dd6762 Mon Sep 17 00:00:00 2001
From: PhillipRambo <93056982+PhillipRambo@users.noreply.github.com>
Date: Thu, 27 Feb 2025 13:36:01 +0100
Subject: [PATCH] Update non_linear_analysis.md
---
.../non_linear_analysis.md | 148 ++++++++++++++++++
1 file changed, 148 insertions(+)
diff --git a/modules/module_2_50GHz_MPA/part_3_nonlinear_analysis/non_linear_analysis.md b/modules/module_2_50GHz_MPA/part_3_nonlinear_analysis/non_linear_analysis.md
index e69de29b..efc375ec 100644
--- a/modules/module_2_50GHz_MPA/part_3_nonlinear_analysis/non_linear_analysis.md
+++ b/modules/module_2_50GHz_MPA/part_3_nonlinear_analysis/non_linear_analysis.md
@@ -0,0 +1,148 @@
+# Non-Linear Simulation
+
+At this stage, we extend our simulations into the non-linear domain, as linearity is a critical factor in power amplifier design. To assess this, we need to determine the **P1dB compression point**, which indicates when the amplifier starts deviating from linear operation. Additionally, we will perform a **load-pull analysis** to optimize the output match for high linearity.
+
+For non-linear simulations, **Ngspice** is no longer sufficient, as it does not support **harmonic balance analysis**, which is essential for capturing the non-linear behavior of RF circuits. Instead, we use **Xyce**, which provides the necessary non-linear simulation capabilities. However, Xyce lacks robust internal match calculations and graphing tools, making post-processing necessary. To overcome this, all data analysis and visualization will be handled through **Python scripts**, which process simulation results on the fly. The required scripts are available in the repository and should work seamlessly if schematic labels and naming conventions are followed consistently.
+
+Since non-linear simulations often require **input power sweeps**, but Xyce does not directly support this functionality, we will implement a workaround using a **sinusoidal current source** in combination with a fixed load resistance to vary the power level
+
+### Setting Up the First Testbench
+
+For the first testbench, we continue from the previous schematic and modify it for non-linear simulation. Since we are now using Xyce models, we must specify a different library file for the HBT transistors. The correct path to the model library is:
+
+```
+/../../IHP-Open-PDK/ihp-sg13g2/libs.tech/xyce/models/cornerHBT.lib
+```
+
+Additionally, we need to instantiate two key components:
+
+1. **Harmonic Balance Analysis Block** – Required for frequency-domain simulation of non-linear behavior.
+2. **Parameter Sweep Block** – Used to step through different operating conditions, such as varying input power.
+
+The setup for these components is illustrated in the image below:
+
+ 
+
+### Configuring the Parameter Sweep and Harmonic Balance
+
+_(Note: The Harmonic Balance block is only visible when the Xyce simulator is enabled.)_
+
+As shown in the image above, the **parameter sweep** is configured as follows:
+
+```
+SW1
+sim=HB1
+Type=lin
+Param=y
+Start=0.0001
+Stop=0.05
+Points=51
+```
+_(make sure that the step size is a n natural number)_
+This setup defines a **linear sweep** for the parameter **y**, ranging from **0.0001 to 0.05** with **200 points**. This will allow us to analyze how the amplifier responds over a range of input conditions.
+
+For the **Harmonic Balance** analysis, the key parameter **n** is set to:
+
+$$n=5n$$
+
+
+The complete schematic setup for the non-linear analysis, including all relevant components, is shown in the image below:
+
+ 
+
+_(Remember to set the frequency of sources and components accordingly.)_
+
+In this setup, we define a **parameter** named **y** with a default value. This parameter is essential for performing the input power sweep, but the value of y specified in the param section is unimportant in this case.
+
+As seen in the sweep configuration, we vary the **input current** from **0.0001 A to 0.05 A** through a **constant 50Ω resistor**. This corresponds to an **input power range of -33 dBm to 21 dBm**.
+
+This sweep is crucial for evaluating the amplifier's behavior in the **non-linear region**, allowing us to determine its **1 dB compression point (P1dB)**—a key metric for assessing linearity.
+
+
+### Running the Simulation and Verifying Results
+
+At this stage, we can proceed with running the simulation. Once the simulation is complete, the first step is to **instantiate a table** to inspect the results and ensure that the output data is correctly formatted.
+
+In the table, we should observe **10 data points** for each swept parameter, corresponding to the **harmonic components**, both **positive and negative**. This confirms that the simulation is correctly capturing the harmonic balance response.
+
+The expected table output is shown below:
+
+ 
+
+### Processing the Simulation Data
+
+As seen in the results table, the simulation has run successfully. This confirms that the **sweeping parameter**, **frequency axis**, and **raw data** are correctly recorded.
+
+Within the **part_3_non_linear_analysis** section, a folder named **python** contains a script designed to facilitate post-processing. This script aims to provide an easy way to **plot gain vs. input power** and **output power vs. input power**.
+
+**Note:** There may be potential issues with the script, so adjustments might be required depending on the data format or specific cases encountered.
+
+To use the script, navigate to its location and run the following command:
+
+```
+python3 plot_xyce.py
+```
+
+this will print the following information, to show functionality:
+```
+This script processes and extracts variables from a specified dataset file.
+You can use the script in the following ways:
+1. To list all independent and dependent variables in the dataset:
+ python3 script.py
+2. To print all values for a specific variable:
+ python3 script.py
+3. To run the analysis and generate plots, pass the following arguments:
+ python3 script.py [xlim_min xlim_max]
+
+```
+From here, navigate to the simulation directory containing the dataset file and execute the following command:
+
+```
+python3 ../../python/plot_xyce.py load_pull.dat.xyce "V(VOUT)" "V(VIN)" "I(PR2)" "I(PR3)" "Y" 50e9 -30 -10 -1 16
+```
+This command generates a readable plot of **gain vs. input power**. For **output power vs. input power**, adjust the boundaries accordingly.
+
+If the naming conventions of the variables differ in your schematic, use the following command to list all available parameters in the dataset:
+```
+python3 ../../python/plot_xyce.py load_pull.dat.xyce
+```
+Once the script runs successfully, the **gain vs. input power** plot should resemble the following:
+ 
+
+ 
+
+
+## Performing Load Pull
+
+As observed in the previous simulation using ideal output components, the **1 dB compression point** was approximately **-7.88 dBm**. To optimize the output network, we aim to maximize the circuit's **linearity**. However, since sweeping a **complex impedance** (i.e., a±bia \pm bia±bi) is not straightforward, we instead perform a **resistive sweep** at the output and determine which resistance yields the best linearity.
+
+While this approach requires some manual adjustments, the **Python script** can assist in processing the results. The exact method is left to the user’s preference. In the following example, we analyze the compression point around a **50Ω termination** and identify the most suitable resistance.
+
+It is important to avoid **excessively low resistance values**, as this would degrade the amplifier’s characteristics significantly. Below, the schematic illustrates the setup for a **40Ω termination**:
+ 
+
+
+Gain curve and compression point was seen as the following:
+
+
+
+### Evaluating the Compression Point Shift
+
+As observed, adjusting the termination has **moved the compression point upward**.
+
+#### **Implications for the Termination Network**
+
+This result suggests that **matching to a 40Ω termination improves the circuit’s linearity**. However, modifying the output match inevitably **affects the input match** and alters the **reflection coefficients**. This presents a trade-off, and it is left to the reader to determine an optimal matching network.
+
+#### **Recommended Approach**
+
+- Do a matching assuming no influence on input reflection.
+- **Gradually tune** the network components to achieve the highest possible **P1dB** while maintaining a good match.
+
+The schematic below illustrates the circuit configuration that will be used in further analysis. The corresponding **gain response** is shown in the final image.
+ 
+
+![[harm_balance_5.png]]
+ 
+
+![[gain_vs_input_power_3.png]]