Ki-PIDA is an open-source KiCad plugin that allows designers to simulate voltage drop (IR drop), current density, and temperature rise directly within the KiCad PCB environment.
As supply voltages continue to decrease while operating currents increase, power integrity (PI) analysis has become increasingly important in modern PCB design. A voltage drop of only several tens of millivolts can potentially affect the stability of a high-performance SoC system.
Traditional PI simulation tools are often expensive and require complex workflows. In many cases, the PCB design must be exported to a third-party application for analysis. KiCad users have therefore lacked a native and efficient solution for examining DC power delivery behavior during PCB layout.
What Is Ki-PIDA?
Ki-PIDA, short for KiCad Power Integrity and Delivery Analyzer, is a plugin designed for KiCad 9.0 and later. It performs DC power integrity analysis directly in the KiCad PCB Editor.
The plugin allows PCB designers to evaluate voltage drop, current density, and temperature rise without relying on expensive proprietary tools or a complex external workflow. Because the analysis is performed within the PCB design environment, power-delivery problems can be identified while the layout is still being developed.
Key Features
Ki-PIDA is intended to make advanced PI analysis more accessible to KiCad users. Its main capabilities include the following:
- Native integration with KiCad: The plugin is built around the KiCad Python API and communicates with KiCad through IPC. No intermediate export file is required, allowing voltage violations to be examined during the layout stage.
- Hybrid 2.5D solver: Ki-PIDA uses an optimized resistive-grid method based on the finite difference method (FDM). This approach is intended to maintain efficient simulation speed while providing accuracy approaching that of a three-dimensional finite-element method (FEM) in the supported analysis context.
- Visual heat maps: Simulation results, including voltage distribution and current density, are overlaid directly on the PCB canvas as color-coded heat maps. This makes high-current regions, voltage bottlenecks, and other potential problem areas easier to identify.
- Multiphysics support: The plugin supports electrothermal coupling and can account for the effect of temperature on copper resistivity.
- Power-tree management: Power rails such as +3V3 and VCC can be detected automatically. The plugin also supports management of more complex power hierarchies.
Installation
Ki-PIDA depends on the newer API provided by KiCad 9.0 and later. The installation process consists of enabling the API, copying the plugin files into the appropriate directory, and installing the required Python libraries.
-
Enable the KiCad API: In KiCad, open
Preferences > Commonand enable the API option in the relevant API section. -
Install the plugin: Locate the KiCad plugin directory for the operating system in use:
- Windows:
%APPDATA%\kicad\9.0\pluginsor%APPDATA%\KiCad\9.0\3rdparty\plugins - Linux:
~/.local/share/kicad/9.0/plugins - macOS:
~/Library/Application Support/kicad/9.0/plugins
Download the KiPIDA repository and copy its contents into the appropriate plugin directory.

- Windows:
-
Install the required Python libraries: When the plugin is launched for the first time, it automatically checks for and installs required libraries such as NumPy, SciPy, and Matplotlib.
If automatic installation does not complete successfully, the libraries can be installed manually from the KiCad 9.0 command line.

After installation, the Ki-PIDA icon should appear in the KiCad toolbar or plugin menu.

Quick Start: DC IR-Drop Analysis
A DC IR-drop analysis can be set up in five basic steps.
- Launch the plugin: Click the Ki-PIDA icon in the top toolbar of the PCB Editor.
- Configure the power rails: The plugin automatically identifies networks such as VCC and GND. Set the nominal voltage for the selected rail, for example, 3.3 V.

- Add a source: Specify the power-input location, such as the output pin of an LDO or a connector, and configure its voltage-regulator-module (VRM) properties.
- Add a load: Identify the power-consuming devices, such as an MCU or FPGA, and enter the current consumed by each load.

- Run the simulation: Click
Run Simulation.
After the solver finishes, Ki-PIDA switches to the Results tab. The interface reports the minimum voltage and displays a color-coded heat map on the PCB. Red and yellow indicate regions with relatively normal voltage levels, while blue and purple identify areas with more severe voltage drop.

The heat map provides a direct visual relationship between the electrical result and the physical layout. A designer can use it to locate narrow copper paths, congested regions, or other portions of the power-delivery network where resistance produces an undesirable voltage gradient. This is especially useful when a schematic-level review does not reveal why a load is receiving a lower voltage than expected.
Technical Architecture
Ki-PIDA uses a layered simulation workflow that converts PCB geometry into an electrical model and then presents the calculated results in the KiCad interface. The main processing stages are:
- Extractor: Extracts copper zones, traces, and physical layer-stackup data from KiCad.
- Mesher: Discretizes the copper geometry into a two-dimensional or three-dimensional resistive grid. The model also includes via structures.
- Solver: Uses sparse matrix solvers from SciPy, including SuperLU and conjugate-gradient methods, to solve the resulting circuit equations.
- Visualizer: Generates Matplotlib heat maps for voltage, current density, and related simulation results.

The meshing stage is important because PCB copper is not represented only as an ideal net. Trace width, copper geometry, layer transitions, and vias all influence the resistance of the current path. Converting these physical features into a resistive network allows the solver to estimate the voltage distribution throughout the power-delivery structure.
Electrothermal coupling extends this model by considering the relationship between current, power dissipation, temperature, and copper resistivity. As the temperature changes, the resistance of the copper also changes, which can affect both voltage drop and current distribution. This provides a more complete view of potential thermal and electrical hot spots than a purely visual inspection of the layout.
Development Status and Usage Considerations
Ki-PIDA is currently in the Alpha stage and supports KiCad 9.0 and later. Planned capabilities include AC impedance analysis and a full three-dimensional thermal model.
Because the project is still in an early development stage, users should back up their KiCad projects before testing the plugin. The calculated results should also be interpreted within the assumptions and limitations of the implemented model. In particular, the quality of the analysis depends on accurate power-rail definitions, source locations, load-current values, copper geometry, layer-stackup information, and via modeling.
The KiPIDA project is available as the KiPIDA repository on GitHub. Its current scope focuses on DC power integrity and delivery analysis inside the KiCad PCB workflow.
By combining PCB data extraction, resistive-grid modeling, sparse-matrix solving, and on-canvas visualization, Ki-PIDA provides a practical way to examine IR drop, current density, and temperature-related behavior without leaving KiCad. For designers working with low-voltage, high-current power networks, this type of analysis can help identify power-distribution bottlenecks earlier in the layout process.