A finite element model can describe the stress distribution in a mechanical bracket, temperature gradients across an electronic package, or the electromagnetic response of a motor with considerable spatial detail. Yet a well-resolved component simulation does not necessarily answer how the corresponding product will behave in service. The bracket belongs to a mechanical assembly, the electronic package interacts with its power supply and cooling hardware, and the motor operates through an inverter, controller, transmission, and load. The relevant engineering behaviour emerges from those interactions as well as from the physics of individual components.
Need help ? connect
This distinction motivates the progression from the finite element method (FEM) to multiphysics and system-level simulation. The progression should not be interpreted as a replacement of detailed numerical analysis with simplified diagrams. It is a change in the level at which a model represents the engineering problem. A detailed spatial model resolves local fields; a system model connects component responses, operating conditions, controls, and feedback. A useful simulation strategy often combines both, assigning detail where it affects the decision and abstraction where additional detail provides little benefit.
The discussion below develops the numerical foundation, engineering workflow, and practical limits of FEM, then explains what multiphysics and system-level models contribute. COMSOL Multiphysics provides a relevant software context, but the underlying principles apply equally to other finite element and multiphysics environments.
Simulation Begins with an Engineering Question
The first decision in a simulation project is not the mesh size or the solver. It is the definition of what the model is intended to predict. A thermal engineer may need the maximum semiconductor junction temperature at rated power. A structural engineer may need the displacement at a sealing interface and the fatigue-critical stress range. A powertrain engineer may need the drive-cycle energy consumption, current demand, and transient torque response. These are different quantities of interest, with different spatial and temporal scales.
A credible simulation specification connects a question to measurable outputs, loading conditions, uncertain inputs, and acceptance criteria. For example, estimating the temperature of a processor under sustained load requires more than assigning a nominal heat-generation rate. The answer also depends on package thermal resistance, interface contact, fan operating point, ambient conditions, airflow obstruction, and possibly temperature-dependent electrical power. If those factors dominate the uncertainty, refining the chip mesh will not correct the larger modelling error.
Simulation can support design screening, root-cause analysis, control development, sensitivity studies, and qualification. These uses require different levels of confidence. An early concept model may prioritize rapid comparison between designs. A model used to justify a safety limit needs much stronger evidence that its assumptions and predictions are valid over the intended operating range. Guidance from NAFEMS on engineering simulation validation emphasizes the connection between model credibility, verification, validation, and the decisions being supported.
Thus, before building a model, the engineer should identify its intended outputs and the mechanisms likely to control them. This is the foundation for choosing the correct numerical representation.
What the Finite Element Method Actually Solves
FEM is a numerical technique for approximating solutions to mathematical problems, commonly partial differential equations posed over a spatial domain. Its effectiveness comes from representing a complicated geometry with manageable elements and approximating unknown fields through basis functions supported over those elements. The method is not simply the act of dividing a geometry into triangles or tetrahedra. The mesh becomes meaningful only when it is associated with a variational formulation, an approximation space, and equations governing the unknown fields.
From governing equations to a discrete system
Consider small-strain linear elasticity under quasistatic conditions. The displacement field $\mathbf{u}(\mathbf{x})$ must satisfy mechanical equilibrium and the constitutive relationship:
$
\nabla\cdot\boldsymbol{\sigma}+\mathbf{b}=\mathbf{0},
\qquad
\boldsymbol{\sigma}=\mathsf{C}:\boldsymbol{\varepsilon},
\qquad
\boldsymbol{\varepsilon}=\frac{1}{2}\left(\nabla\mathbf{u}+\nabla\mathbf{u}^{\mathsf{T}}\right).
$
Here, $\boldsymbol{\sigma}$ is the Cauchy stress tensor, $\mathbf{b}$ is the body force per unit volume, $\mathsf{C}$ is the fourth-order elasticity tensor, and $\boldsymbol{\varepsilon}$ is the infinitesimal strain tensor. Boundary conditions prescribe displacement on part of the boundary and traction on the remainder. These conditions are essential because the differential equation alone does not define the physical problem.
In a standard displacement-based finite element formulation, the displacement is approximated as
$
\mathbf{u}_h(\mathbf{x})=\sum_{i=1}^{N}N_i(\mathbf{x})\mathbf{d}_i,
$
where $N_i$ denotes a finite element shape function and $\mathbf{d}_i$ contains the nodal displacement degrees of freedom. A weak, or variational, formulation converts the continuum problem into a set of algebraic equations. For linear quasistatic elasticity, the assembled form is
$
\mathbf{K}\mathbf{d}=\mathbf{f},
$
where $\mathbf{K}$ is the global stiffness matrix, $\mathbf{d}$ is the vector of unknown nodal displacements, and $\mathbf{f}$ contains the equivalent external nodal forces. For transient structural dynamics, the model commonly extends to
$
\mathbf{M}\ddot{\mathbf{d}}+\mathbf{C}\dot{\mathbf{d}}+\mathbf{K}\mathbf{d}=\mathbf{f}(t),
$
with mass matrix $\mathbf{M}$, damping matrix $\mathbf{C}$, and time-dependent excitation $\mathbf{f}(t)$. Nonlinear material behaviour, geometric nonlinearity, or contact changes the structure of the numerical equations and typically requires iterative solution.
The same general strategy applies to thermal conduction, electrostatics, diffusion, and a wide range of other field problems, although the governing equations, dependent variables, and numerical formulations differ. An accessible technical treatment is available in COMSOL's detailed explanation of FEM and weak formulations.
Why the weak form matters
The weak form is central to the numerical method. Instead of requiring a differential equation to hold pointwise under demanding smoothness assumptions, the method requires an integral statement to hold against suitable test functions. Integration by parts can lower the differentiability required of approximate solutions and incorporates natural boundary terms. This is particularly valuable for complex geometries, mixed boundary conditions, and piecewise-defined material properties.
In practical simulation software, these mathematical details are often handled by established physics interfaces. That convenience should not obscure the fact that the solution quality depends on the appropriateness of the governing equations, discretization, boundary conditions, and numerical controls. A finite element solution is an approximation to the selected mathematical model, not automatically an accurate representation of the physical product.
The FEM Workflow as an Engineering Process
A useful FEM workflow is better viewed as a sequence of decisions than as a fixed set of software clicks. Geometry, materials, boundary conditions, meshing, solution, and interpretation interact. If an assumption changes, earlier modelling choices may need to be revisited.
Geometry and physical idealization
Detailed CAD models frequently contain manufacturing features that have little influence on a chosen quantity of interest. Removing unnecessary fillets, threads, or small holes can reduce computational cost. However, removing a notch or interface that controls the peak stress can fundamentally alter the prediction. Simplification must therefore follow the physics, not merely the desire to reduce mesh count.
Dimensional reduction is another option. A two-dimensional plane-stress or plane-strain model may represent a suitable structure more efficiently than a three-dimensional solid model, provided its assumptions are justified. Axisymmetric formulations can be especially economical for rotationally symmetric geometries and loading. Symmetry boundaries are valid only when geometry, materials, loads, and the expected solution satisfy the relevant symmetry conditions.
Material behaviour and boundary conditions
Material properties may be constant, temperature-dependent, anisotropic, nonlinear, or rate-dependent. Assuming linear elastic behaviour for a polymer subjected to long-duration loading, for example, can omit viscoelastic deformation. Likewise, applying a fixed temperature to an electronic package surface when the real cooling condition is convective can impose an unrealistically strong thermal constraint.
Boundary conditions represent the interaction between the modelled region and the rest of the world. A clamped boundary, imposed heat flux, electric potential, and convection coefficient are all modelling statements. Their physical justification is at least as important as the mesh used to implement them. Many apparently convincing contour plots are dominated by boundary conditions that were selected for convenience rather than because they describe the actual experiment or device.
Mesh, numerical solution, and convergence
Meshing determines the finite-dimensional approximation space. Smaller elements can resolve strong field gradients and geometric features, but do not compensate for incorrect physics. Element order, aspect ratio, mesh quality, and local refinement strategy also matter. A fine mesh concentrated in physically irrelevant regions may provide less value than a well-designed mesh targeted at a thermal boundary layer or stress concentration.
Mesh convergence should be assessed through quantities of interest, not only through a visually smooth field. For a structural model, the quantity might be deflection at a defined location or averaged stress over a finite region. For a thermal model, it may be total heat flux or maximum junction temperature. A comparison across successively refined meshes establishes whether the relevant output is still significantly affected by discretization.
Convergence should not be confused with solver convergence. A nonlinear solver may satisfy its stopping tolerance while the spatial solution remains under-resolved. Conversely, a physically valid model may require more careful load stepping, time integration, or preconditioning to obtain a stable numerical solution. COMSOL's guidance on analyzing model convergence and accuracy also cautions that geometric singularities can prevent meaningful pointwise stress convergence.
Verification and validation are different tasks
Verification asks whether the mathematical equations are being solved correctly, within the relevant numerical accuracy. This includes checking discretization error, time-step sensitivity, and solver tolerances. Validation asks whether the mathematical model predicts physical behaviour adequately for its intended use. Experimental measurements, benchmark configurations, and known physical limits can provide evidence for validation.
A simulation can be numerically converged and physically wrong because its loads, interfaces, or constitutive laws are inappropriate. It can also match one experiment through parameter tuning yet fail outside that operating condition. Consequently, comparison with measurements should cover the important operating range whenever feasible. NAFEMS provides a useful introduction to verification and validation that distinguishes these responsibilities.
A Worked Example: Thermal Simulation of an Electronic Heat Sink
An electronic cooling assembly illustrates both the strengths and limitations of component-level FEM. Consider a processor dissipating electrical power into a package, thermal interface material, metal heat sink, and surrounding air. The initial engineering question might be straightforward: what is the processor temperature at a specified ambient temperature and power level?
Governing thermal physics
Within solid regions, transient heat conduction may be described by
$
\rho c_p\frac{\partial T}{\partial t}
=\nabla\cdot\left(k\nabla T\right)+Q_v,
$
where $\rho$ is mass density, $c_p$ is specific heat capacity, $T$ is temperature, $t$ is time, $k$ is thermal conductivity, and $Q_v$ is volumetric heat generation. A tensor-valued thermal conductivity can be used when material conduction is anisotropic. At steady state, the accumulation term vanishes.
The thermal boundary at an exposed solid surface is sometimes approximated using convection:
$
-\mathbf{n}\cdot k\nabla T=h\left(T-T_\infty\right),
$
where $\mathbf{n}$ is the outward normal, $h$ is the convective heat transfer coefficient, and $T_\infty$ is the ambient fluid temperature. The expression is appropriate when a prescribed effective heat transfer coefficient is a reasonable approximation. If airflow around the fins must be predicted rather than imposed, conjugate heat transfer modelling with a fluid-flow solution may be necessary. Thermal radiation may also contribute, depending on temperatures, geometry, and surface properties.
What detailed FEM reveals
A resolved thermal model can identify temperature gradients across the package, interfaces, base plate, and heat sink fins. It can quantify the effects of contact resistance, fin thickness, base spreading resistance, and material selection. It may also reveal that the nominally hottest point moves as the heat distribution or airflow conditions change.
A commonly reported scalar is the overall thermal resistance:
$
R_{\mathrm{th}}=\frac{T_{\mathrm{ref}}-T_\infty}{P},
$
where $T_{\mathrm{ref}}$ is a defined reference temperature, $P$ is the dissipated power, and $R_{\mathrm{th}}$ is thermal resistance in kelvin per watt. The reference location must be stated because a heat-sink-base thermal resistance and a junction-to-ambient thermal resistance describe different portions of the heat path. For a linear thermal model with fixed cooling conditions, this quantity provides a compact approximation of the temperature rise per unit power.
Now imagine comparing several heat sink designs. The engineer may vary fin spacing, base thickness, interface conductivity, and fan conditions. Detailed simulation is particularly useful for understanding which geometric modifications change the local heat transfer path and which merely increase mass or manufacturing complexity. The resulting data can inform a design choice before prototype testing.
What the isolated model cannot establish
A heat sink does not operate independently. Fan speed depends on the electrical supply and its control signal. Processor dissipation changes with workload and temperature. An enclosure introduces airflow restrictions and recirculation. A thermal controller may reduce processor power when a temperature threshold is exceeded. Even if the heat sink geometry is simulated accurately, assigning a constant fan airflow and constant chip power may miss critical operating behaviour.
An isolated FEM model can determine temperature for selected boundary conditions, but it may not predict those boundary conditions. That distinction is the beginning of the system-level modelling problem. To answer how the cooling assembly behaves under a changing computational workload, the thermal physics must interact with power consumption, fan dynamics, and control logic.
What FEM Does Especially Well
The main advantage of high-fidelity field modelling is spatial resolution. In many engineering decisions, local details are not incidental. They are the mechanisms of interest.
In structural mechanics, stress concentrations around holes, weld toes, and contact regions can dominate failure assessment. Linear elastic FEM can resolve local elastic stress fields, while nonlinear formulations allow plasticity, large deformation, and certain contact behaviours to be investigated. However, evaluating fracture initiation or propagation requires suitable constitutive and damage formulations, not simply a finer mesh or a red stress contour.
For electromagnetic devices, geometric details influence electric-field concentration, magnetic saturation, eddy-current losses, and optical confinement. In photonics, even small dimensional changes can shift resonance frequencies or alter mode coupling. A spatial model is therefore necessary when geometry-dependent field interactions determine performance.
For thermal engineering, component-scale FEM resolves nonuniform heat generation, spreading resistance, and coupled thermal stresses. In fluid dynamics, spatially resolved computational models describe velocity fields, pressure distributions, and convective transport. Importantly, not every CFD solver uses FEM: finite volume and other discretization methods are also widely employed. FEM is one major numerical method within the larger field of computational engineering.
These examples have a common feature: spatial gradients and local mechanisms matter. Replacing the complete problem with a few lumped variables would discard information needed for the engineering decision.
Why Purely Detailed Modelling Becomes Impractical at System Scale
The limitation of FEM is not a hard boundary beyond which the method cannot operate. Large assemblies can be modelled with finite elements, and some applications require exactly that. The problem is efficiency and appropriateness when the question concerns interactions across many physical and functional domains.
Computational scale is only one difficulty
A complete electric drive may contain power electronics, a motor, shafts, gears, thermal management, sensors, and a feedback controller. A three-dimensional electromagnetic motor model may already require substantial computation. Incorporating detailed semiconductor switching, full coolant flow, mechanical contact, and long-duration controller behaviour into one tightly coupled high-resolution model introduces additional degrees of freedom and disparate time scales.
Numerical stiffness can become important when fast switching dynamics coexist with slow thermal transients. Solving every fast event for a complete drive cycle may be unnecessary if the target output is average efficiency or coolant temperature. Conversely, averaging out switching transients would be inappropriate when investigating electromagnetic interference or high-frequency losses. The correct simplification depends on the outcome being studied.
The difficulty is therefore not just the number of mesh elements. It is the mismatch between the physical resolution required by individual phenomena and the observation horizon of the system question. Computational resources, data exchange, nonlinear coupling, time integration, and software interoperability all affect the feasibility of a fully detailed simulation.
High-fidelity detail can obscure system causality
A detailed motor field solution may produce accurate torque and loss maps at specified current, speed, and temperature. That does not establish whether a controller will command an unstable operating point or whether the battery will be able to supply the required current. Similarly, an excellent flow simulation of a heat exchanger cannot alone predict a plant-wide temperature transient if pump control, bypass valves, and upstream thermal loads are unspecified.
System-level models make interactions explicit. Instead of describing the exact geometry of every component, they capture how components exchange signals, energy, mass, and other physically relevant quantities. This provides a representation more closely aligned with questions about stability, overall efficiency, regulation, fault response, and long-time operation.
Multiphysics: Coupling Physical Phenomena
Multiphysics and system-level modelling are related but not synonymous. Multiphysics concerns the interaction of physical processes that may be governed by different equations. System-level modelling concerns the connected behaviour of components and subsystems, often represented at different levels of abstraction.
Consider an electrically heated mechanical component. The electrical field produces Joule heating; heating modifies the temperature field; temperature changes electrical conductivity; thermal expansion generates mechanical strain. A coupled model can represent these feedback mechanisms. If the electrical conductivity depends on temperature, a simplified thermal-electrical coupling includes
$
Q_v=\mathbf{J}\cdot\mathbf{E},
\qquad
\mathbf{J}=\sigma(T)\mathbf{E},
$
where $\mathbf{J}$ is current density, $\mathbf{E}$ is electric field, and $\sigma(T)$ is temperature-dependent electrical conductivity. The resulting heat source affects $T$, which in turn changes $\sigma$. Mechanical deformation may provide another feedback path through geometry or contact changes.
A coupled solver can address such dependencies using a monolithic formulation, where the interacting variables are solved together, or a segregated approach, where subsets of variables are iterated in sequence. Alternatively, some problems permit one-way coupling if feedback is demonstrably small. For example, a prescribed electromagnetic loss distribution may be transferred to a thermal model without recalculating the electromagnetic field, provided the thermal changes do not materially alter the loss mechanism.
It is therefore important to distinguish between one-way data transfer and bidirectional physical feedback. Both can be legitimate engineering approximations. The question is whether the omitted feedback would change the quantity of interest beyond an acceptable tolerance.
Multiphysics models can operate at the scale of one device, an assembly, or an entire system. They become particularly powerful when local coupling, such as Joule heating, thermoelastic deformation, fluid-structure interaction, or electrochemical heat generation, is decisive. Yet a detailed multiphysics simulation of a single component remains a component model unless its wider system interactions are also represented.
What System-Level Simulation Adds
A system-level simulation describes how multiple components interact over time or under changing operating conditions. Rather than resolving every spatial field, it often represents components through differential equations, algebraic relationships, lookup tables, state-space models, transfer functions, or reduced-order representations. Models exchange variables through defined interfaces.
A generic nonlinear dynamical model may be written as
$
\dot{\mathbf{x}}=\mathbf{f}(\mathbf{x},\mathbf{u},\mathbf{p},t),
\qquad
\mathbf{y}=\mathbf{g}(\mathbf{x},\mathbf{u},\mathbf{p},t),
$
where $\mathbf{x}$ is the vector of internal states, $\mathbf{u}$ contains inputs, $\mathbf{p}$ contains parameters, and $\mathbf{y}$ contains measured or reported outputs. The functions $\mathbf{f}$ and $\mathbf{g}$ describe state evolution and output generation. In a real system model, additional algebraic constraints may be required, leading to a differential-algebraic system rather than a pure ordinary differential equation.
Unlike a finite element mesh, a system diagram primarily communicates component relationships. Electrical circuits, thermal networks, fluid networks, and control block diagrams may all appear in the same simulation architecture. Connections must preserve their physical meaning. A signal connection carrying a fan-speed command is not equivalent to a power-conserving electrical or mechanical port. Careful treatment of interface variables, units, conservation laws, and causality is essential when combining models created from different domains.
Returning to the electronic cooling example
A system-level model of processor cooling might contain a processor power block, thermal network, fan dynamics, controller, and environmental boundary conditions. One simple first-order thermal approximation is
$
C_{\mathrm{th}}\frac{dT}{dt}
=P(t)-\frac{T-T_\infty}{R_{\mathrm{th}}},
$
where $C_{\mathrm{th}}$ is thermal capacitance in joules per kelvin, $P(t)$ is the dissipated power, and $R_{\mathrm{th}}$ describes heat transfer from the chosen thermal node to ambient. This model cannot resolve fin-level temperature gradients, but it can efficiently approximate temperature evolution when its lumped assumptions are valid.
The fan can be described by a speed-dependent airflow or cooling characteristic, while the controller adjusts the fan command according to measured temperature. Processor power may depend on workload, frequency, and throttling logic. The system model can then examine workload transients, fan response, temperature overshoot, and control stability.
A detailed thermal model is still valuable. It can determine effective thermal parameters, reveal hot spots that a one-node network misses, and quantify how the cooling characteristic changes with geometry or airflow. If necessary, the system model can use multiple thermal nodes or a reduced-order model derived from high-fidelity simulations. This combination retains crucial component physics without forcing every system-level time step to resolve the full spatial problem.
Different models for different questions
| Engineering question | Appropriate primary model | Why |
|---|---|---|
| Where does a bracket experience its highest physically meaningful stress? | Spatial structural FEM | Local geometry and load paths control the response |
| How does electrical heating deform a connector? | Coupled electrothermal-structural model | Multiple fields interact within a component |
| How does processor temperature change during a workload cycle? | Thermal system model informed by component simulation | Workload, thermal inertia, and cooling control evolve together |
| Will a motor drive remain stable during a load transient? | Electrical-mechanical-control system model | Feedback and subsystem dynamics govern the behaviour |
| Which heat-sink geometry offers the best thermal performance? | Parametric component-level thermal model | Spatial heat transfer and geometry dominate the comparison |
The appropriate model is not necessarily the one with the greatest number of equations. It is the one whose assumptions, scope, and accuracy are aligned with the engineering decision.
Connecting the Two Levels in COMSOL Multiphysics
COMSOL Multiphysics is particularly relevant because it provides physics-based modelling interfaces for spatial problems and facilities for coupling fields and equations. A typical component-oriented workflow involves preparing the geometry, specifying materials and physics, applying domain and boundary conditions, selecting a discretization, solving, and evaluating quantities of interest. The software's physics interfaces can handle much of the weak-form machinery, but users remain responsible for the engineering assumptions behind the model.
The transition toward system simulation typically involves creating a suitable interface around the detailed component. One possibility is to use the spatial model directly with circuit equations or other lumped variables. Another is to extract a response characteristic, such as impedance versus frequency, force versus displacement, or thermal resistance versus airflow, and use that characteristic within a larger model. A third is to construct a reduced-order model that reproduces selected responses with substantially fewer states. COMSOL's reduced-order modelling documentation explains how such representations can be used in system simulations and other coupled applications.
The distinction between a full model and its reduced representation is consequential. A lookup table may reproduce steady-state behaviour yet omit thermal inertia or dynamic resonance. A reduced-order model trained near a particular operating condition may perform poorly under large excursions, contact changes, or strong nonlinearity. Any abstraction needs a defined validity range and should be tested against the underlying detailed model at representative conditions.
In September 2026, COMSOL also announced COMSOL Systems as part of the forthcoming COMSOL Multiphysics 2027 release. The announced add-on is intended to support system diagrams coupled with one-, two-, and three-dimensional multiphysics models. That announcement reflects the broader engineering requirement to connect detailed field simulations with system behaviour. It should not be read as evidence that an announced capability is already available in every installation or license configuration.
The practical value of such integration depends less on a particular software label than on having consistent interfaces, suitable physical abstraction, numerical stability, and traceable validation across model boundaries.
A Practical Modelling Strategy for Engineering Teams
For projects that involve both local physics and whole-product behaviour, a staged workflow reduces unnecessary complexity. Start by specifying the principal system outputs and the conditions under which they must be predicted. Next, identify which components have behaviours that can be described reliably by established equations or measured characteristics and which need high-fidelity analysis.
Develop the detailed component models where geometry, materials, or nonlinear field distributions materially affect performance. Use them to extract the relevant response quantities, including their dependence on operating parameters. Represent other components through physically justified lumped or reduced-order models. Establish the model interfaces with explicit units, input and output definitions, and energy or mass balances where applicable.
Then validate in layers. Verify each numerical component model against convergence criteria and appropriate benchmarks. Test the fidelity of reduced models over their intended operating ranges. Check that the assembled system respects expected limiting cases, conservation constraints, and experimentally observed transient behaviour. Finally, conduct sensitivity and uncertainty studies to determine which inputs have the greatest influence on the engineering decision.
This process avoids two common extremes: oversimplifying a component whose local physics controls failure, and building an unnecessarily expensive spatial simulation of a system whose principal concern is its control response or operational efficiency.
If you're working on related challenges in this area and would find guidance helpful, feel free to reach out: CONTACT US.
Conclusion
FEM provides detailed spatial predictions of quantities such as stress, temperature, displacement, and electromagnetic fields. Its numerical strength comes from a mathematically controlled approximation of continuum equations, but the reliability of any result still depends on the governing physics, boundary conditions, mesh convergence, solver behaviour, and validation evidence.
Multiphysics modelling extends this description when interacting physical mechanisms cannot be treated independently. System-level simulation addresses a different problem: how connected components, controllers, energy flows, and changing operating conditions determine the response of the whole product. It often uses lumped equations, reduced-order models, and component characteristics rather than uniformly high spatial resolution.
For a processor and its cooling system, detailed thermal analysis is indispensable for investigating geometry-dependent hot spots and heat transfer. A broader system model is needed to examine workload variation, fan control, and the transient response of the assembly. The same reasoning applies to motors, batteries, industrial equipment, and many other coupled engineering products. Effective simulation practice is therefore not a choice between FEM and system modelling. It is a disciplined allocation of numerical detail to the levels at which that detail changes the engineering conclusion.
Interested in collaborating on academic research ? feel free to get in touch 🙂.
Check out YouTube channel, published research
you can contact us (bkacademy.in@gmail.com)
Interested to Learn Engineering modelling Check our Courses 🙂
