Demystifying Modal Analysis (Part I)

In this article, I will discuss about modal analysis – a topic that is standard, however I’ll strive to demystify it using a simple example and FAQs.

Motivation for Modal Analysis

As a mechanical engineer, life is always interesting because I can correlate the knowledge gained from books to real life scenarios. As a student, my professor gave a real example of a bridge failure due to marching soldiers. What followed was a very interesting lecture about dynamics. Until then, I never understood the power of the words such as dynamics, vibration and resonance. Of course, the example provided food for my thoughts to study more about how a bridge could fail due to lesser dynamic load compared to a heavier static load.

For those of you who are curious, the bridge was England’s Broughton Suspension Bridge that failed in 1831 due to the soldiers marching in step. The marching steps of the soldiers resonated with the natural frequency of the bridge. This caused the bridge to break apart and threw dozens of men into the water. Due to this catastrophic effect, the British Army issued orders that soldiers while crossing a suspension bridge must ‘break step’ and not march in unison.

Such failure has given rise to more emphasis on analyzing the structure (mechanical or civil) for dynamic loads if it undergoes any sort of vibrations. Traditionally test equipment have been used to experimentally monitor vibrations in new designs; this is costly however. We apply finite element analysis (FEA) to solve such problems. FEA solvers have evolved and today’s solvers are powerful not only in statics but in dynamics too.

Demystifying Modal Analysis

Modal Analysis: Getting Down to the Basics

In any dynamic/vibration analysis, the first step is to identify the dynamic characteristics of the structure. This is done through a simple analysis called Modal Analysis. Results from a Modal Analysis give us an insight of how the structure would respond to vibration/dynamic load by identifying the natural frequencies and mode shapes of the structure.

Modal Analysis is based on the reduced form of dynamic equation.

Demystifying Modal Analysis

As there is no external force acting and neglected damping, the equation is modified to:

Demystifying Modal Analysis

I have skipped the derivation part of natural frequency as it is easily available in textbooks. Natural frequency is substituted back into the equation to find out the respective mode shapes. These natural frequencies are the eigen values whereas the respective mode shapes are its eigen vectors. Natural frequencies & mode shapes in combination are called as modes.

Eigen vectors represent only the shape of deformation, but not the absolute value. That’s the reason it is called as mode shape. It is the shape the structure takes while oscillating at a respective frequency. Important point to remember is the structure has multiple modes and each mode  has a specific mode shape. If any load is applied with same frequency as natural frequency in the same direction as mode shape, then there will be increase in magnitude of oscillation. With no further damping, the scenario will lead to a failure due to a phenomena called resonance. To avoid this phenomena in dynamics, calculating the modes carries great importance.

Frequently-Asked Questions

Having said that, questions will certainly arise. In my opinion, these are the most commonly asked questions in support calls by customers using ANSYS.

  • Why do frequencies from simulation don’t match the test results?
  • Why are deformation and stresses in modal analysis very high?

From equation (3), it is clear that natural frequency of structure depends on its stiffness and mass. In order to accurately capture frequencies in FEA, the following points are important for you:

  • You need to capture mass of the structure and connecting/ignored members accurately.
  • Your mesh can be coarse, but enough refinement so that you can accurately capture the stiffness of the structure. If you are interested in the local modes in slender members, then you’ll need to perform local mesh refinement.
  • You need to define appropriate boundary conditions in forced modal analysis in order to capture realistic frequencies.
  • You need to accurately model the contact between different bodies in an assembly since they affect the stiffness of the structure drastically.

For the second question, a lot of confusion exists when the modes extracted in modal analysis show deformation magnitude. In Equation (2), you will see that no external load is applied on structure. This will make you wonder where these values come from? Let’s have a look with an example of simple cantilever beam.

Demystifying Modal Analysis
Fig. 1 – Mode shape & stress shape of Cantilever Beam

Fig. 1 shows its extracted mode shape 1 & stress shape 1 from modal analysis. I observe deformation to be as high as 253 mm and stress as 4,914 MPa which is far greater than the ultimate strength of Steel i.e. 500 MPa. You may wonder, why did we get these high values?

This happens because the FEA solver returns the mode shape (not the deformation magnitudes) as output. By this, I mean that magnitude of the mode shape is arbitrary (as seen in Fig. 1). The high value is because of a scale factor that’s chosen for mathematical reasons and does not represent anything real for the model. However this value helps us in relative measurement. Let’s take the example of the first mode. Maximum deformation occurs at the free end compared to any other location. This changes with the change in mode.

Since we have deformation, you can compute corresponding stresses and strains. Once again, these are relative values. If you ask the FEA solver for stresses & strains, it will use the same scaled deformation magnitudes and calculates stresses & strains. They are referred to as stress shape & strain shape (not to be confused with stress state or strain state) because no loads are applied. The magnitude of stresses and strains are useless but their distributions are useful to find hot-spots in the respective modes.


Modal analysis offer much more than just the frequencies and mode shapes. This analysis is primarily the stepping stone for linear dynamics studies to calculate the actual deformation due to different kinds of dynamics loads. Modal analysis has many secondary applications which I will discuss in my next blog.


Share this on:

Drop Test Analysis with Bolt Pre-Stresses

This article introduces a time-saving and a smart approach for drop test analysis with pre-stresses using LS-Dyna. 

Many products that are subject to handling during transport, installation, or repair are at risk of being dropped. Granted, handlers generally try to avoid these types of mishaps. When equipment is out of your hands, its safe transportation is out of your control. One way to ensure that your product survives its journey from the factory to the point of installation is to perform drop test analysis and verify that it survives without damage. That way, your company isn’t answering warranty claims from customers who received damaged goods that left your warehouse in mint condition.

Although the methodology for drop test is fairly standard, it is challenging to capture the finer details that happen in reality. This article introduces a time-saving and a smart approach for drop test analysis with pre-stresses using LS-Dyna.


While drop test problems involving huge appliances, the effects of bolt-load or pre-stresses are generally ignored. However, in some cases, it is desirable to have a pre-stress loading of a structure before performing a transient dynamic analysis or, simply, drop test analysis. This is because nowadays the product safety has increased the demand for accurate simulation models.

In this article, I used LS-DYNA. It is a highly advanced, general-purpose, nonlinear, finite element program that is capable of simulating complex real world problems.

Firstly engineers need to perform a pre-stress analysis for the bolts before conducting the drop test analysis. Then you will need to integrate the stresses and strains obtained from the pre-stress analysis into the drop test analysis setup.

Drop Test with Included Pre-Stresses (two-step method)

In LS-DYNA, I define bolt pre-load (non-iterative loading type) using *INITIAL_AXIAL_FORCE_BEAM (Type 9 beams only) and *INITIAL_STRESS_SECTION (solid elements only). These keywords work with *MAT_SPOTWELD. The failure models apply to both beam (Type 9) and solid elements (Type 1).

*INITIAL_AXIAL_FORCE_BEAM will pre-load beam elements to a prescribed axial force.

Screenshot of keyword in drop test analysis

In the above screenshot of the keyword, BSID is Beam Set ID. I define the preload curve (axial force vs. time) with *DEFINE_CURVE. LCID is the Load Curve ID.

The below video show the pretension in the beams.

*INITIAL_STRESS_SECTION will pre-load a cross-section of solid elements to a prescribed stress value. Pre-load stress (normal to the cross-section) is defined via *DEFINE_CURVE.

Screenshot of keyword in drop test analysis

In this screenshot placed above, ISSID is section stress initialization ID,  CSID Cross-Section ID, LCID Load Curve ID (pre-load stress versus time), PSID Part Set ID, VID Vector ID (direction normal to the cross section). You can define the vector if *DATABASE_CROSS_SECTION_SET is
used to define the cross section.

In the video, you can see the pre-stresses in solid elements when I used *INITIAL_STRESS_SECTION.

Video Courtesy: LSTC

*INTERFACE_SPRINGBACK_LSDYNA allows LS-DYNA to create a DYNAIN file at the end of the simulation containing deformed geometries, residual stresses, and strains. This file sets me up for the next phase of analysis where I use it with the *INCLUDE keyword. However, the DYNAIN file neither includes contact forces nor contains nodal velocities. These quantities from the pre-stress analysis do not automatically carry over to the drop test.

Drop Test with Included Pre-Stresses – Both in One Step!

In the previous method, there is always manual intervention which can lead to unknown errors. Drop test of an appliance by considering pre-stresses in one step can be specified by using *DEFINE_TRANSFORM.

*DEFINE_TRANSFORM allows to scale, rotate and translate the appliance and you must define before you use the *INCLUDE_TRANSFORM command.

Screenshot of keyword in drop test analysis

Screenshot of keyword in drop test analysis

In the above screenshots, TRANSID refers to Transformation ID that is available in *DEFINE_TRANSFORM and the part which is specified in the file name will include the TRANSID.

The video below shows the drop test analysis of an appliance where *DEFINE_TRANSFORM allows the appliance to pre-stress and then the actual drop happens. The von-Mises stress contours show that the stresses get developed in the parts due to pre-stressing of the beams before the actual impact.

Saves time!

Using this approach, I can save about 20% of the time required to setup a pre-stress analysis and drop test analysis together. In addition, we can eliminate manual intervention.

Thanks to this, I get to submit my simulation jobs to the solver before I head into the weekend. I return in the following week to view and post-process the final results.

If you want to learn more about this, please talk to us.

Share this on:

The Decade That Was …

In the CADFEM Journal (previously Infoplaner; in German), an announcement was made in the first issue of 2007 about the commencement of India business. This March, CADFEM Engineering Services India (CADFEM India) celebrates its 10th birthday – a decade in business. The company started out as a four person team with the vision that it could help customers in India recognize and realize the benefits of simulation-driven product development. 10 years on, the company has evolved into a confident engineering business, with over 50 colleagues, that has helped hundreds of engineers to realize their product promise.

The Decade That Was …

During this time so much has changed. The world has got smaller, faster and ever more changing. Technology has both been an enabler and a challenge to small businesses and large enterprises alike. As a responsible business, the company’s constant endeavour has been to offer customers the best-in-class solutions to their engineering problems. Today CADFEM India is proud to have gained trust from several local and global companies whose engineers rely on its products, services and know-how on a daily basis.

CADFEM India is a strong channel partner to ANSYS in India by offering the full range of physics (structural, fluids and electronics) across India. This partnership is helping CADFEM increase the rate of adoption of simulation in the country. The organization is structured towards providing and supporting customers with ANSYS software. Today the company has more than 40 engineers comprising of the core technical team, sales and marketing that engage customers in multiple areas of engineering analysis. The team is highly skilled to offer training programs for novices and experienced engineers on a plethora of engineering topics. Several customers, with origins in Germany, are long standing customers of CADFEM in India. CADFEM is the preferred simulation partner for customers owing the nature of strong and high-quality support. Deepak Joseph, the Head of Development (Truck) at Knorr-Bremse Technology Center India, and his team in Pune have been recipients of CADFEM’s technical support regularly. While thanking CADFEM for offering “extended support” to his team, Deepak recently said that CADFEM ”helped us understand ways to achieve accuracy.”

Listing of milestones of CADFEM India

All tools which are critical for success

CADFEM India offers several complementary solutions such as optiSLang (of Dynardo GmbH), Rocky DEM (particle simulations) and simulation-ready hardware. Since engineering simulation requires more than just software, CADFEM India supplies all the tools which are critical for success in simulation – all from one source. As a result, customers in India not only benefit by receiving leading software and IT-solutions, but also obtain support, consultancy and transfer of know-how. The core philosophy ingrained within every colleague is to ensure that customers realize the most return of their simulation investment. Dynardo’s CEO, Dr. Johannes Will, says “Over the last 7 years, CADFEM India has become an important partner for Dynardo to serve the optiSLang business in India as well as to support the Dynardo consulting activities. I personally enjoy that relationship and look forward to intensify the joint business success over the next years.” Since 2011, CADFEM India has organized the Indian edition of the Weimar Optimization & Stochastic Days. In 2016, over 80 attendees came together to discuss the topics of optimization and robust design for sixth year in a row.

In addition to the software business, many customers consider CADFEM India as a reliable engineering consulting partner. Several customers choose to contact CADFEM to seek simulation on demand. CADFEM India’s Managing Director, Madhukar Chatiri says that “this offers a good opportunity for us to demonstrate the power of ANSYS to the customer.” Over the years, CADFEM has solved many engineering problems in automotive, aerospace, consumer appliances, rotating machinery, watches, food & beverage and many more industries. One such example of a strong customer relationship is with Traunreut-based Bosch und Siemens Hausgeräte GmbH (BSH). For over two years from 2008, BSH worked intensively with two engineers from CADFEM India. As a result, there has been a strong partnership between BSH and CADFEM India. Speaking about this, Dan Neumayer, Head of Pre-Development at BSH said “we could have a mutual cultural understanding and a common way of thinking and working. This intensive learning forms a particularly important basis for our long-term cooperation and we see this as one fundamental success factor.”

Group Photo in the decade that was
Mrs. & Mr. Guenter Mueller while visiting CADFEM India in 2015
esocaet program starts in September 2017

One of the top most challenges for employers in India is the low number of engineers skilled with simulations. To bridge this demand-supply gap, CADFEM India has invested in ANSYS Authorized Training Centre that started in September 2015; over 50 engineers have graduated from this centre. Furthermore, CADFEM has partnered with PES University in Bangalore to bring the much-acclaimed esocaet Master Program in Applied Computational Mechanics to India. The esocaet program offers tremendous opportunities to engineers for continuous learning. The first course will begin in September 2017.

CADFEM India has been operationally profitable since many years – this has allowed the company to scale its investments in India consistently. The company has a long-term orientation, offers employees a lot of independence but functions as a responsible partner to customers. This allows the company to respond with agility to the dynamic needs of the market.

The company has geared up for the next decade of business in the Indian subcontinent. Having recognized the needs of the market, the company is betting big in the areas of Additive Manufacturing, Electronics and Digital Cities. CADFEM India has made another significant investment into the newest partner of CADFEM International – CADFEM SEA Pte. Ltd. in Singapore.

In 2016, the company was recognized as one of the 20 Most Promising Engineering & Design Solution Providers in India by the popular CIO Review magazine. Madhukar still fondly recalls the day when he formulated the vision for the Indian business in his mind. He adds “What a journey it has been for many of us! While waiting for our connecting flight at Mumbai airport, Guenter Mueller discussed the idea of a joint company in India. We thank our customers and partners for choosing to work with us. It has been and is our pleasure to serve the engineering market in India in the past decade.”

Share this on:

How Fatigue Made Me Fall From The Chair?

This article explains the setup of a simple fatigue analysis in ANSYS Workbench using an example. For beginners, this article demystifies fatigue analysis.


When I was ten years old, I was fond of a chair which was small and easily movable. After school, I used to sit on it and watch Aladdin tales on the television. One day, as usual, I sat on it. Suddenly the chair got broke in half and I fell on the floor in front of my sister. For obvious reasons, I got embarrassed and my sister made fun of me the whole day. I slept that day with few unanswered questions.

Why did the chair fail when it was working fine for a few years? Why didn’t it fail on the first day I sat on it?

Illustration of a broken chair as a result of fatigue
My broken chair! 🙁

Fast forward to my engineering days, I was told that cyclic loading on any structure can make that structure fail – fatigue failure. Only then I could understand why my beloved chair failed.

Many of you might have heard stories like the one mentioned above or even experienced it yourself. However, the fact that majority of structures irrespective of their size experience a phenomenon like fatigue is real. If a simple structure with a simple load cycle could fail because of fatigue, imagine a complex structure with a complex loading cycle. Yes, the consequences are catastrophic for the manufacturer as well as the user.

According to NBS report, “between 80-90 % of all structural failures occur through a fatigue mechanism.” Incorporating fatigue simulation upfront into the product development cycle plays a vital role in optimizing the structural integrity of your product and it significantly reduces the cost of failure.

In this article, a simple fatigue analysis is shown which was carried out using ANSYS Fatigue Tool. If you wish to conduct the analysis as per FKM guidelines, you’ll be interested this CADFEM ANSYS Extension.


For a fatigue analysis, static structural or transient analysis is a prerequisite. To achieve this, I consider a simple chair geometry for static structural analysis; appropriate loads and boundary conditions were defined. I define a point mass of 75 kg to act on the chair. This loading can be considered as a misuse for a child’s chair. Resultant static stress (24 MPa) did not exceed the yield strength (54 MPa) of the assigned material.

There! I got the answer to one of the questions from my story. The chair didn’t fail on the first day I sat on it because the load applied on the first day was not sufficient enough to exceed the yield strength of the material.

Analysis setup for fatigue study
Loads and Boundary Conditions
Results of static structural analysis before fatigue analysis
Equivalent von-Mises Stress








Setting up the analysis

Subsequent to the setup of static structural analysis, I launch the ANSYS Fatigue Tool using the following steps.

Setting up fatigue analysis
Solution>Insert>Fatigue>Fatigue tool

Analysis Type

ANSYS Fatigue Tool offers two methods to calculate fatigue life.

  • Strain Life
  • Stress Life

While strain life approach is widely used, at present, because of its ability to characterize low cycle fatigue (<100,000 cycles), stress life approach addresses high cycle fatigue (>100,000 cycles).

Specifying details in the fatigue tool
Details View of Fatigue tool

I chose the stress life approach to execute this example and subsequently I defined the appropriate S-N (Stress–Cycles) curve in the engineering data.

Loading Type

Contrary to static stress, fatigue damage occurs when stress at a point changes over time. Therefore, it is essential to define the way the load could repeat after a single cycle, in other words the type of fatigue loading determines how the load repeats over time.

Accordingly, I chose zero-based loading type for the current example, which means I apply the load and remove it, thereby resulting in an equivalent load ratio of 0. For a fully-reversed loading, I would apply a load and then apply an equal and opposite load which will result into a load ratio of -1.

Applying zero-based loading in fatigue analysis
Zero-Based loading

In both the cases the amplitude of load remains constant. Therefore looking at the single set of simulation results will give you an idea where fatigue failure might occur.

Mean Stress Theory

Now that I have defined analysis and loading types, I need to choose a mean stress theory.

Zero Mean Stress loading for fatigue analysis
Zero Mean Stress loading

Mean stress is the average of maximum and minimum stress during the fatigue load cycle. Mostly, fatigue data is assumed for zero mean stress, which means fully reversed loading. However, fully reversed loading conditions (zero mean stress) are rarely met in engineering practice. Hence Mean Stress Correction Theory has to be chosen to account for mean stress.

For stress life approach: If experimental data at different mean stresses exist, I can account for the mean stress directly by interpolating different material curves. However, it is unlikely to have experimental data at all mean stresses. Therefore, several empirical relations are available including Goodman, Soderberg and Gerber theories which use static material properties (yield strength and tensile strength) and S-N data to account for mean stress. In general, I don’t advise you to use empirical relations if multiple mean stress data (S-N curves) exists.

Different Mean Stress Theories for Fatigue Analysis
Different mean stress correction theories (Goodman Theory is highlighted)

Goodman Mean Stress Theory is a common choice for plastic materials, whereas Gerber Theory is a common choice for ductile metals. For the current analysis, I chose the Goodman Theory.

Fatigue Life

Like any other result in ANSYS Workbench, fatigue life can be scoped on a geometric entity. For stress life with constant amplitude loading, life at that point will be used if the equivalent alternating stress is lower than the lowest alternating stress defined in the S-N curve

For this example, 3,100,000 cycles is the expected life of the chair. This means that a person of 75 kg can sit on this child’s chair for 3.1 million times. If he ignores and continues to sit beyond the expected life, very soon he might face the same fate as the boy in the story.

Fatigue life extracted from ANSYS Fatigue Module
Fatigue life extracted from ANSYS Fatigue Tool

Wasn’t it easy? Yes, it is easy to perform this analysis provided you have the material data. In case you are not aware, ANSYS Mechanical Pro, Premium, Enterprise and ANSYS AIM offer ANSYS Fatigue Tool.

What are you waiting for? Start realizing your product promise using ANSYS products.

P.S. Just in case you were wondering what happened after the chair broke, my mother bought us a brand new chair the next day!

Share this on:

Structural Analysis – ANSYS 18 Innovations

ANSYS Release 18 is packed with lot of innovative features for structural analysis. This article summarizes the various advancements in the new release.

ANSYS 18 enables users like you and me to meet customer demands to develop lighter, stronger, and more efficient products. The new release has new tools and technologies to analyze complex materials, optimizing designs and shapes for new manufacturing methods and ensuring structural reliability of electrical components.

With the new parallel Topology Optimization technology, you can perform lightweighting of structures, easily extract CAD shapes and quickly verify the optimized designs. You can easily simulate spatially-dependent materials like composite parts, 3D printed components, and bones and tissues for more accurate results. The new spectral fatigue capability enables you to accurately model vias and calculate product life to better measure the reliability of electronic components. The addition of a new concrete material law, along with the ability to easily define reinforced structures, makes it easy to model complex structures in the civil engineering and nuclear application areas.

In summary, ANSYS Mechanical has brought in much awaited enhancements which were long overdue for users performing structural analysis. Therefore the new release revolutionizes problem handling and solving capabilities across various industrial domains. Here are the highlights.

Easier and Faster Usage
  • There are enhancements in sorting and filtering options, hotkeys and selection utilities leading to effective utilization of ANSYS Mechanical
  • You will find advancements in contact formulation and detection capabilities that lead to faster convergence
Image of a coupling element while performing structural analysis
Ease of Use in ANSYS 18
Advanced Material Modeling

ANSYS has introduced improvement to existing material models in order to help accurately simulate complex plasticity.

Enhancements for Dynamics

Developments in rotor-dynamics and performance improvements in CMS will lead to reduction of computational time while performing structural analysis.

Image of a turbomachinery component with results after structural analysis
Advancements in Rotordynamics
Additive Manufacturing Technologies

The introduction of advanced options for topology optimization is another significant enhancement that will help manufacturing sector with material savings.

Mechanical Reliability of Electronics

Lastly the enhanced coupling between Electronic and Mechanical helps to model Thermo-Mechanical effects in intricate and minute electronic components better.

Besides the above advancements, ANSYS 18 offers many avenues for users to realize their product promise! If you’re interested to learn more about ANSYS 18 innovations for structural analysis, then join our webinar on March 24. There’s a lot to learn!

Share this on:

Fluid Dynamics – ANSYS 18 Innovations

ANSYS Release 18 is packed with lot of innovative features for computational fluid dynamics. This article summarizes the various advancements in the new release.

As always, ANSYS has delivered continuous product advancements. The latest release features several beneficial capabilities.

With ANSYS 18, engineers can create better, more accurate computational fluid dynamics (CFD) simulations. Therefore, engineers new to CFD will benefit from greatly expanded capabilities in easy-to-use ANSYS AIM, including support for transient flows, non-Newtonian fluid viscosity and fluid momentum. In addition, ANSYS 18 includes new features and functionality that enables engineers to solve CFD problems with more accuracy than ever before. Further breakthrough harmonic analysis delivers accurate turbomachinery simulations up to 100x faster. ANSYS 18 also introduces CFD Enterprise, the first solution designed for CFD experts in organizations who need to solve the toughest problems.

Here are the release highlights.

GUI & Advances in Post-Processing

The new release has better CAD import, enriched post-processing, well-organized realization of different volumetric domains and surface boundaries. Also the sophisticated solution monitoring and elegant post processing views make up for a delightful user experience with ANSYS 18.

Fluid Dynamics: Velocity vectors and pressure contour in a pump-valve operation, now displayed with enhanced graphics in ANSYS Fluent
Velocity vectors and pressure contour in a pump-valve operation, now displayed with enhanced graphics in ANSYS Fluent
Better Physical Models
  • Heat Transfer and Combustion. Monte-Carlo radiation model helps capture high temperature radiation in solid domains with better ray tracing implementation. Further on, enhanced flamelet modeling gets combustion analysis running better with ANSYS 18.
  • Multiphase Flow Models. Chemical mixing and other fluid blending processes benefit by the convergence and significant speedup improvements for free surface transient flow simulations with the Volume-of-Fluid (VOF) method.
  • Turbomachinery Enhancements. You can solve blade flutter cases more efficiently by using harmonic analysis. In addition, flank-milled blades can now be better modeled with ANSYS BladeModeler.
Solver Enhancements

Lastly with solver enhancements, mesh adaption of polyhedral meshes in ANSYS Fluent is now possible with its improved execution. Another aspect is that of overset meshing which is ready to better support the aerodynamic community.

Fluid Dynamics: Flow impact on an offshore structure - Robust free surface flow simulation with enhanced VOF model of ANSYS Fluent
Flow impact on an offshore structure – Robust free surface flow simulation with enhanced VOF model of ANSYS Fluent

Do you want to learn more about ANSYS 18 innovations for computational fluid dynamics? Join our webinar on March 23. There’s a lot to learn!

Share this on:

Modeling Thermostats in ANSYS Workbench

This article talks about modeling thermostats in ANSYS Workbench using the COMBIN37 element that is quicker, sophisticated and automated. While working on a customer project, I struggled with the conventional approach in ANSYS 17.2. It was frustrating, and so I decided to look up for possible alternatives in the ANSYS Customer Portal. I found a solution using COMBIN37, however it only featured the option for switching OFF the heat source. Next I stumbled upon PADT’s ACT Extension, but again it didn’t seem to be useful for the problem described in this article. Thanks to the able support from ANSYS staff, I was able to obtain this solution.

Thermostats are used in many applications. For analyst, therefore, it is essential to understand the type and functionality of the component that she wants to replicate in the simulation environment. Before anything else, let me brief you about thermostats.

What is a thermostat?

Wikipedia defines thermostat as:

A component which senses the temperature of a system so that the system’s temperature is maintained near a desired set point.

Thermostats are widely used in varied industrial applications, however they are primarily used in heating and cooling systems. Air-conditioners, refrigerators, automotive coolant control, electric iron box, actuators, control valves are a few of the many applications. Thermostats are also used in many manufacturing processes to maintain the desired temperature limits.

Let us model it in ANSYS Workbench, shall we?

Problem definition

For this article, I selected a small block that is initially at room temperature. Also, this block is heated up by a source on the bottom face (possibly, a heater) that inputs 2W for 10 minutes. The objective is to maintain the temperature at a certain point (indicated with a red label; hereinafter referred to as sensor) on the body within 170-175°C.

Modeling Thermostats: Block geometry with a label for sensor
Block geometry chosen for this article
Possible solutions

In a simulation environment, there are two ways to model a thermostat.

Many beginners will adopt a conventional approach. In this approach, heat is fed to the surface until the temperature rise at the sensor reaches 175°C. However, the analyst doesn’t immediately recognize the time when the sensor attains 175°C. So she:

  • lets the computation run until the desired temperature is obtained
  • records the time at which this temperature is attained
  • divides the time dependent loads into number of load steps to control the switch ON/OFF
  • finally runs the analysis again until the temperature at sensor falls down to 170°C

This cycle continues for the entire analysis duration, however this example runs only for 10 minutes. For real problems, it is tedious and time-consuming to simulate the thermostat functionality to regulate the temperature with this procedure.

Modeling Thermostats with COMBIN37

Another solution for modeling thermostats is much quicker, more sophisticated and an automated technique. In order to make it work, it requires to build a connection between the sensor node and the heat source face to regulate the temperature. We introduce a temperature regulator that is modeled with element COMBIN37 in ANSYS.

Modeling Thermostats: Illustration depicting two humans aiming to plug one cable into another.

I’ll help you understand COMBIN37 – it is a unidirectional control element that has a capability to turn OFF and ON during the analysis. COMBIN37 has one set of active nodes (I,J) and one set of control nodes (K,L –optional nodes). Each node has one degree of freedom (DOF) that is valid for structural (translations/rotations/pressure) and thermal analysis (temperature). COMBIN37 has many other applications; you can find detailed information in the ANSYS Help manual.

Unfortunately, there is no direct way to model this in ANSYS Workbench. Of course, this entails a set of APDL scripts to run in the background. Simply put, 2 nodes, I & J of COMBIN37, are connected to the heat source face and sensor node respectively. Three arguments are defined using scripts – the first two define the range of temperatures on the sensor node and the third defines the heat flow from the source to be operated within the range defined – that indirectly defines the ON/OFF behavior.

Modeling Thermostats: Image showing the thermostat model used for this example. Heat source to switch off when temperate is 175 degree Centigrade and switch on when it drops to 170 degrees.
Operating range of the thermostat
Create COMBIN37 using commands

Let me now take you to the step-by-step procedure describing the commands used to model a thermostat in ANSYS Workbench.

Step 1

Since we’re creating an element that is possible only in pre-processor, you must enter the pre-processor.

/prep7                                                  ! Enter the Pre-processor

Step 2

Define the arguments for the magnitudes of temperature range within which the heat source should supply the heat. This definition of arguments will allow you to parametrize the temperature peaks as well. Parametrization allows for various studies such as sensitivity analysis, optimization or robustness evaluation in ANSYS Workbench. This can become important in coupled physics problems.

on_val=arg1                                       ! Set on_val to arg1

off_val=arg2                                      ! Set off_val to arg2

Step 3

Select the sensor node and obtain its node ID

cmsel,s,sensor                                    ! Select the named selection consisting sensor                                                                       node or vertex

sensor_node=ndnext(0)                 ! Get the node id

nsel,all                                                  ! Select back all nodes in the data base

Step 4

Create material ID for COMBIN37 element, define the type of DOF, ON/OFF behavior and input the third argument for heat flow with appropriate key options and real constants.

*GET,max_et,etyp,0,num,max        ! Get highest type attribute in the model.                                                                                  We increment this to ensure we are using                                                                                new, unique id for COMBIN37

et,max_et+1,37,,,8,,1                            ! Control element using temperature DOF and                                                                         set the thermostat behavior

r,max_et+1,,,,on_val,off_val,arg3  ! Set the on/off set points and the heat flow                                                                              rate

ex,1000,1                                                 ! Dummy material number/material id

Step 5

Create the nodes I & J for COMBIN37, and then create an element COMBIN37 by assigning these nodes to it.

*GET,max_nd,NODE,0,num,maxd         ! Get highest node id in the model

n,max_nd+1                                                   ! Create I node of the COMBIN37 – location                                                                               doesn’t matter

n,max_nd+2                                                   ! Create J node of the COMBIN37

type,max_et+1                                               ! Set the type to a next higher unique id

real,max_et+1                                               ! Set the real to a next higher unique id

mat,1000                                                        ! Set the material attribute pointer

e,max_nd+1,max_nd+2,sensor_node  ! Create COMBIN37 element

Step 6

Select the nodes of the heat source and couple these nodes to the node “I” of the COMBIN37. This coupling will copy all the information on the node “I” to the nodes on the heat source.

cmsel,s,Heater_Strip                               ! Select the named selection containing the                                                                              heat source face

nsel,a,,,max_nd+1                                    ! Also select the node I of the COMBIN37

cp,1,temp,all                                               ! Couple the temp DOF of the node I of the                                                                                COMBIN37 to the heater strip (source face)

nsel,all                                                         ! Select all nodes in the model

Step 7

Exit the pre-processor and enter into the solution

fini                                                                ! Finish out of pre processor

/solu                                                             ! Enter into the solution


Once I input the temperature limits, heat flow and other applicable boundary conditions, I solve the model and check the results if the desired output is obtained.

Modeling Thermostats: Screenshot showing the result of the APDL commands that appear as Input Arguments for temperature limits and heat sourcei input in ANSYS Workbench
APDL commands appear as Input Arguments in ANSYS Workbench
Results Verification – Part I

From the results, temperature extracted for the sensor node must look as shown in the below figure. One can observe that the temperature on this sensor node rises initially to 175.01°C and then gradually falls down to 170°C. As soon as the temperature falls below 170°C, the heat supply will be automatically switched ON and ultimately this leads to the temperature rise on the sensor node. This cycle continues until the final time step of the analysis.

Modeling Thermostats: Image showing geometry of the problem along with the history of temperature over a period of 10 minutes.
Temperature vs. Time plot

In order to check if the applied heat flow is considered exactly as per the desired definition, use the User Defined Result and set the Material IDs as 1000 (refer the command script in Step 4) & use the Expression as SMISC2 (second sequence of element summable miscellaneous data – look into ANSYS Help for more info).

See the below figure for the definition and output of this user defined result. Remember! This result is possible to see only from the ANSYS Release 18.0, however it is available as a beta feature.

Modeling Thermostats: Screenshot of ANSYS Workbench showing the way to select material id and result expression as SMISC2.
Obtaining User Defined Result in ANSYS Workbench
Modeling Thermostats: Plot showing the history of heat flow input over time
Plot of Heat Flow Input vs. Time
Results Verification – Part II

To verify whether the heat input and the desired output are obtained based on the input definition, I plotted a chart with the temperature result on sensor and user defined result (heat input). In the below figure, the purple colored line indicates the heat flow while the green colored line indicates temperature rise on sensor. You will see that Heat Flow is OFF when peak (175°C-region between red arrows) is reached and ON as soon as it reaches 170°C (region between green arrows) and is constantly supplying 2W of heat. Hence the thermostat works!

Note: Y axis in the below figure is of normalized magnitude. This doesn’t imply the heat input as 1W.

Modeling Thermostats: Plot overlaying history of temperature and heat flow inputs over time. Using illustrations, the portion where heat flow is switched off and on is also shown.
Temperature & Heat Flow Inputs vs. Time

This article aims to target analysts with beginner experience with modeling thermostats. As such, without using COMBIN37 element, analysts can tend to struggle for the end result for weeks because they have to manually regulate the temperature by re-running the analysis.

Using the COMBIN37 element, the solution is much quicker, more sophisticated and automated. For this study, it took hardly two hours of run time with the automated technique while the manual approach took roughly about 60 hoursThe extent of time savings is enormous using this element in ANSYS.


In summary, I suggest that you define the number of sub steps in a manner that the minimum time step is sufficiently low. As per this, when the time step is significantly high, the temperature increase or decrease will be of significantly larger magnitudes. As a result, temperature will keep falling out of the range.

Time step also becomes important in order to accurately capture temperature values especially when the range is quite small. Such instances are common in many industrial applications. For example, for the problem above described, the range is 170-175°C, i.e. difference of 5 degrees of centigrade. Accordingly I chose a suitable time step for this example.

Screenshot showing settings for analysis for modeling thermostats
Settings for Analysis

Before solving the problem, ensure that you have entered the inputs for the argument values in the Solver Unit System irrespective of the current/working unit system.

Share this on:

Opening ANSYS Projects Made Easy!

This post is to describe a solution to a fairly regular problem that troubles many engineers opening ANSYS project files across multiple versions of ANSYS software.

Unless you’ve been living under a stone, you must be as excited as I am about the new ANSYS Release 18. Did you attend the Digital Webcast on January 31? There was so much on display. The new, innovative features of the release were much needed by the market.

Well, this has been the trend since Release 15 in terms of product development and innovation in ANSYS software. Over the past several years, ANSYS, Inc. brought in a many product releases with lots for improvements. Quite obviously, engineers at many of our customer sites have installed many of these versions of ANSYS software on their workstations.

The Problem

Due to several versions of ANSYS software installed on your workstations, double-clicking a project will open ANSYS in the last (need not be latest) installed version. For example: If ANSYS R16.2 is installed after installing ANSYS R17.0, then double-clicking the project (originally saved in ANSYS R16.0) will open the project in R16.2.

Due to this problem, there is a possibility that you will inadvertently save the project in a higher version of ANSYS software by mistake. When saved in the higher version, opening ANSYS project can’t be possible in (original) lower software version due to limitation of backward compatibility. For certain projects, retaining work in certain versions is quite important. Unfortunately there is no way to restore your project file to the older version in case you accidentally open and save it in a newer version.

Possible Solutions

In order to open ANSYS project file in desired version, one approach is for you to open the desired ANSYS version from Start Menu (in Windows). Once you open the desired version of ANSYS, you can open the respective project. Since this is a tedious approach, it is sub-optimal.

Another approach, that is easier and faster, is to RMB (right mouse button) click and select “Open with” and select the desired ANSYS executable. This reduces the turn around time of opening a file by 30-40% when compared to the previously-discussed approach. However many engineers have been confused because the file names of different ANSYS software versions in the “Open with” menu are same.

"Open with" menu in Windows OS for opening ANSYS project
“Open with” menu in Windows OS for opening ANSYS projects

Obviously engineers such as me get confused or do not always remember/know the version of the ANSYS executable in the “Open with” menu. Choice of version becomes more important since companies expect engineers to execute internal projects in different versions of ANSYS. To decode this confusion, we obviously need a better solution.

Optimal Solution for Opening ANSYS Projects

Since ANSYS Release 16, support is available for only Windows 7 and above. This solution is not applicable for other OS.

Step 1
Open start menu type regedit in search bar

Step 2
Follow the below path:
HKEY_CURRENT_USER > Software > Classes > Local Settings > Software > Microsoft > Windows > Shell > MuiCache

This page contain names of all programs and respective executable files as seen in “Open with” option after RMB click .

Screen grab of Registry Editor view that shows all programs and respective executable files
Registry Editor view of all programs and respective executable files

Step 3
You can select the ANSYS version whose name needs to be changed. RMB click on it and select “Modify…“.

"Edit String" window to update the executable name
“Edit String” window to update the executable name

Now change the Value Data to the desired name. For example, I chose to use file names such as RunWB2_R180.exe. You can complete the same exercise for renaming executable files of other ANSYS versions.

By doing so, the next time you RMB click on an ANSYS Workbench Project and select “Open with”, you will see different names as shown below.

Updated "Open with" menu after RMB click
Updated “Open with” menu after RMB click
Share this on:

3 Benefits of ANSYS SpaceClaim for 3D Printing

In this article, I will describe 3 benefits of ANSYS SpaceClaim Direct Modeler for 3D Printing and other applications. Specifically I will focus my attention on the Facet Tool in this article.

While searching for freely-available CAD models on, I chanced upon the challenges section because it piqued my interest. To my surprise, I found about 75% of the recent challenges to be related to topology optimization. For most of these challenges, lightweighting will yield a final design output that is optimum in weight. However such an output will be complex for traditional manufacturing processes. In the recent years, additive manufacturing or, often referred to as, 3D printing has appeared to be the manufacturing process of choice for several contemporary applications.

For topology optimization, ANSYS is the simulation tool of choice. In the latest Release 18, a significant thrust was provided to this topic. The technology is very powerful and highly-effective for lightweighting the designs. Typically, topology optimization results in the design in STL file format. In my experience, this design output is often fraught with poor facet quality and this requires cleanup by a competent tool.

Typical STL File Output of a Bracket after Topology Optimization towards 3D Printing
Typical STL File Output of a Bracket after Topology Optimization

The full suite of ANSYS Simulation Software offers not just solvers for multiple physics, but also several value added tools such as ANSYS SpaceClaim Direct Modeler (SCDM). This tool allows product companies to launch their offerings faster to market.

Now SCDM has several useful features that allow geometry manipulation and clean-up. Among many features, I found the Facet Tool to be extremely useful. After completion of topology optimization, the STL file output from ANSYS is imported into SCDM.  This Facet Tool helps in cleaning up the STL file output containing poor facet quality and helps me prepare the design for validation using ANSYS Mechanical.

For better understanding, I have included the typical workflow below.

Workflow for Topology Optimization for 3D Printing
Workflow for Topology Optimization

With this context in place, I will now introduce you to the 3 significant benefits of using ANSYS SpaceClaim Direct Modeler for 3D Printing applications.

HIPP Add-In for Reverse Engineering

HIPP is an SCDM add-in developed by This tool is quite useful for engineers performing reverse engineering – with the eventual goal of producing the desired part using 3D Printing. For this case, the approach typically starts with scanning of the part desired for reverse engineering. The scan results in an STL file format created directly in SCDM; this automatic scan to STL is powered by the HIPP add-in. The Facet Tool in SCDM is then used to repair and prepare a watertight geometry.

Here’s an example of the scanned geometry of top profile of a piston rod that was generated in SCDM using the HIPP add-in. The facets in this geometry did not capture the profile accurately. Furthermore the geometry has undesired holes along with unwanted parts.

Image of a scanned geometry of a part in SCDM (using HIPP Add-In) for 3D Printing
Scanned geometry of a part in SCDM (using HIPP Add-In)

Using the Facet Tool, the repaired geometry is now ready for topology optimization and design validation before producing it using 3D Printing.

Image of the modified geometry in SCDM using Facet Tool for 3D Printing
Modified geometry in SCDM using Facet Tool
Save Resources – Faster to Market

There are numerous software tools for STL preparation, however SCDM Facet Tool has many value-adding, additional capabilities. With a very little investment, the Facet Tool provides a strong hold in combining multiple solid parts with faceted geometries in a user-friendly manner; this feature has several advantageous implications for 3D printing. Furthermore the tool is very easy and requires little knowledge for geometry repair and preparation. To prepare the bracket geometry (illustrated at the beginning of the article), it took me 10-15 minutes. See the below image. Now I found it to be fairly quick when compared to 2-3 times more using other facet modeling tools.

Image of bracket geometry modified after using SCDM Facet Tool for 3D Printing
Bracket geometry modified after using SCDM Facet Tool
Preventing Failures in 3D Printing

The Facet Tool has features to detect thickness and overhang problems before the model is sent for 3D Printing. Now these overhangs present a challenge to 3D printing without using support material. Problems such as these can be prevented by few techniques like tear-dropping, tapering among others. The effects of overhang cannot be judged immediately until you are a 3D Printing professional.

Facet Tool has a feature which detects the overhangs by providing parameters specific to 3D Printing. In particular, the thickness feature detects all geometry that is thinner than the minimum thickness specified by the printer OEM. In addition, I could understand thickness and overhangs-related problems beforehand by providing the direction of printing as well.

Other Applications

This topic is also of CADFEM’s particular interest because we invest into Digital Cities – a strategic initiative of CADFEM International that aims to simulate cities of our future. This topic is quite special and important since it involves studying the effects of disaster scenarios such as earthquake, tsunamis, pollution, crowd behavior among others.

virtualcitySYSTEMS, a CADFEM International group company, develops 3D city models using scanned data of terrains. For these city models, we use the Facet Tool to repair the geometry before performing urban simulations.

In future posts, I will delve further into using CFD and particle simulations for better modeling of 3D Printing applications.

Share this on:

Debugging Convergence for Large Sliding Problems

This is the first part in a series of posts related to debugging convergence. This post talks about large sliding problems in particular.

Sliding contact is an imperative characteristic defining the functionality of many products. In this article, I aim to help in debugging convergence issues while modeling and simulating large sliding contact problems in ANSYS Mechanical.

A conventional practice for modeling contacts in a simulation environment tends to accommodate slight inter-penetration of mating parts in order to allow the solution to converge. Inter-penetration can pose serious concerns in the form of under prediction of force reactions and stresses for a sliding contact scenario. The lack of solution accuracy is in the name of solution convergence. In order to derive a reasonably accurate solution for a sliding contact scenario, we should strive to regulate contact penetration to a bare minimum.

Two Approaches to Sliding Contact Problems

Let’s get into the nitty-gritty of solving sliding contact problems. Now ANSYS Mechanical’s settings for penalty-based methods (Pure Penalty and Augmented Lagrange) allow for some penetration (depends upon contact stiffness) leading to easier convergence. Results are not accurate with the penalty-based method. Despite this, many chose to use this approach in order to achieve solution convergence.

Normal Lagrange formulation guarantees almost zero penetration, with good solution accuracy, because there is no contact stiffness in the normal direction. Instead, the method uses some additional contact degrees of freedom i.e. contact pressure acting normal to contacting surface in order to prevent penetration and a tangential contact stiffness based on penalty method.

So the Normal Lagrange formulation can handle large frictional sliding problems more effectively. It is not suited for sticking application, i.e. valid only for frictional/friction-less contacts. Conversely, this method can be used where penetration is undesirable – as in applications such as snap fit, gears & other sensitive applications where penetration leads to less accuracy in the results.

However Normal Lagrange formulation is not the proverbial knight in shining armor for these applications.

Solution has not converged after 12 iterations for contact status change!

Screenshot of ANSYS Mechanical solver output highlighting the lack of change of contact status. This image is used in support of the article on Normal Lagrange formulation

Achieving Solution Convergence with Normal Lagrange Formulation

While working with the Normal Lagrange formulation, many of you would have faced this challenge. In addition to it be very frustrating, the time consumed to achieve solution convergence reduces our engineering productivity.

Typically when we activate Normal Lagrange formulation, the ANSYS solver, by default, bisects at the 12th iteration due to contact status change even though the force convergence trend is good. The figure below illustrates this. If the bisection were not to happen, the solution were likely to converge in the next iterations.

Screenshot of a delayed solution convergence with Normal Lagrange formulation.

Can we increase this bisection limit? Yes! This, little known, undocumented key is available with the CUTCONTROL command.


In ANSYS Workbench, this command can be inserted in the tree under analysis system as shown in the below image.

Screenshot of ANSYS Workbench demonstrating the location to add the APDL command. This image is used in support of the article on Normal Lagrange formulation.

Seen below is the force convergence behavior of a demo case study with and without using the CUTCONTROL command.

Image of force convergence behavior of a test case shown using a plot without CUTCONTROL command in support of the article on Normal Lagrange formulation.
Without CUTCONTROL command
Image of force convergence behavior of a test case shown using a plot with CUTCONTROL command in support of the article on Normal Lagrange formulation
With CUTCONTROL command

Generally, in industry, there is a misconception that Normal Lagrange is not preferable for achieving convergence in many cases. As demonstrated, this contact formulation is best suited for large sliding problems which is both, accurate and faster.

If you encounter problems with large sliding contacts, please do try my suggestion and let me know your feedback. If you have a better solution in mind, please do share in the comments section.

Share this on: