Rand Simulation Solutions Blog

New Home for Rand Simulation Solutions Blog

We truly enjoy writing blog posts and sharing them. But that’s not all we do. Our new blog site lives on the Rand SIM Resource Center.

The Rand SIM Resource Center offers on-demand webcasts, tips, brochures, course outlines, and more.

Rand SIM Solutions WILL continue, we hope you’ll join us: https://resources.randsim.com/rand-simulation-solutions-blog

Efficiencies of the Object Generator

The model chosen to demonstrate some of the advantages of using Ansys Object Generator is shown below. It consists of a box and a lid which are connected with a large number of fasteners. One method of connecting them is with the use of simple beam elements which are easily generated in Ansys Workbench. However, even when easy, it becomes a chore when a large number of them are needed.

In this example, first, a simple beam with an assumed diameter of 6 mm spanning from the middle of the lid hole to the middle of a box hole will be generated. The first beam is created as usual…

Notice the nearby holes being empty! Now a Named selection is created of through-hole surfaces in the Lid as well as a similar Named Selection of through holes’ surfaces in the Box, see below.

The next step is to open the Object Generator dialog box in the Automation tab.

The first step in the Mechanical Application Wizard (the dialog box) is to identify the object to be used as a template, i.e. what is desired to be patterned, see the image below.

Once the beam which was created earlier is selected in the model tree, the Object Generator dialog box is opened.

Here the two named selections are selected from pull-down menus for Reference and Mobile scoping. The following task is to enter an approximate range for beams length. The software will create beams of the same length as the reference beam, but it is a good idea to still give a small range in case of slight differences in geometry of scoped bodies in all locations.

A default choice for geometry to be scoped to is Adjacent Entities but there are options to choose Each Entity or All Entities by Part if so desired. Here the beams need only be created between the generated named selections, so the default selection is left unchanged. The next is to select whether to Ignore the original or create an object in its place as well. Again, as no additional beams are needed in the place of the initially created beam, the default selection is kept. If no custom names are needed, click on Generate to create desired beams in all holes between the Lid and the Box as shown below.

As can be seen below, beams between the Lid and the Box are created between all scoped geometries, and the job is done!

This example was to show how the job of a fastener creation can be done in a more efficient manner while using the Object Generator to automate and expedite the creation of loads, boundary conditions, beam connections, and other features in Mechanical Applications. I hope this was helpful!

Christmas Ornament Safety with Ansys Explicit Dynamics

By Spencer Crandall

Around this time each year, families around the world gather to decorate their Christmas trees. Unfortunately, we’ve all lost an ornament to a clumsy family member, a domestic pet, or a sagging tree. In the spirit of protecting the sentimental ornaments in our lives, we’re going to use Ansys to discuss the topic of safely decorating with glass ornaments. We’ll do this by using the Ansys drop test wizard ACT extension to look at a representative glass ornament falling from varying heights. We’ll go over some simple considerations during setup, material models available, and ultimately what height you can safely drop a glass ornament and expect it to survive.

Jumping right into the tools that we’ll need to run this drop test analysis; we can go into our ACT manager and make sure that the Mechanical Drop Test Wizard ACT extension is loaded.

Figure 1: Drop Test Wizard ACT Extension

Figure 2: Ornament Geometry

Next up will be finding the proper materials for our model. Thankfully, Ansys includes a library of explicit material models, which we can use in lieu of hunting down the complex, rate-dependent, brittle response, material properties that we will need. We will be using the Floatglass material, which uses the Johnson-Holmquist Strength model. This material model will allow us to show plasticity and damage along with material fracture.

Moving into the explicit module inside of Ansys Workbench, we’ll launch the Drop Test Wizard, which will expedite the setup process. This can be found in the Environment context menu when you have the Explicit Dynamics object selected in the outline.

Figure 3: Context Menu Drop Test Wizard

1. Using the Drop Test Wizard we can complete the following steps:
2. Orientation of the target surface and imported geometry
3. Creation of the target surface
4. Meshing
5. Set initial velocity based on drop height
6. Set analysis end time and analysis preference to Drop Test
7. Establish body interaction contact behavior (frictionless or frictional)

Figure 4: Completed Model Setup

With the setup described, we can iterate on our drop height until our glass ornament experiences a failure as shown in the following GIFs (click on each to play).

Figure 5: 40 Inch Drop Height

Figure 6: 41 Inch Drop Height

Figure 7: 96 Inch Drop Height (Just for fun)

Our analyses indicate that you can safely hang your glass ornaments no higher than 40 inches. Keeping that height restriction in mind will help you and yours keep safety at the forefront of all your Christmas tree decorating parties.

This post focuses primarily on the basic application of the explicit dynamics drop test wizard ACT extension. If you’re interested in a more in-depth overview of explicit dynamics in Ansys then I would recommend reviewing our previous two-part blog post or YouTube video:

Blog Post: https://blogs.rand.com/randsim/2020/11/explicit-dynamics-and-ansys-part-i.html

YouTube Video: https://www.youtube.com/watch?v=J1FJGENPf1k

Performing a Creep Deformation Analysis in Ansys Mechanical

If you’ve ever hung a heavy item on a plastic clothes hanger and come back a while later to see that the hanger has permanently deformed, then you’ve seen a phenomenon known as “Creep” occurring firsthand. When materials are subjected to sustained mechanical loads over long periods of time, they tend to slowly deform, and eventually rupture.  While this failure mode is usually not a concern at room temperature for most engineering materials, the process is accelerated at high temperatures.

Creep Deformation Analysis vs. Stress Rupture Analysis

A Creep rupture test is performed by applying a sustained mechanical load to a test specimen which is maintained at a specific temperature and the time to rupture is measured often over the course of months or even years. A Creep test is similar to a Creep rupture test, but in a Creep test, the elongation of the test specimen is monitored throughout the test. This gives information on the rate of Creep deformation that a Creep rupture test does not provide.

Before beginning an analysis, it is important to determine if a Creep deformation analysis is necessary. If the only concern is ensuring that a component does not rupture after some time, a stress rupture analysis is all that is required. The key question to ask is if the excessive deformation will interfere with the function of a component. For instance, a turbine blade that experiences excessive Creep deformation would begin to rub against the casing that contains it, causing wear and vibration issues. In this case, a Creep deformation analysis would provide useful information. On the other hand, a reformer tube used in the production of hydrogen does not have tight clearances, and the only concern is making sure that a Creep rupture does not occur before the intended design life. In this case, a Creep rupture analysis using a Larson miller curve may be all that is required.

The Three Phases of Creep

Creep can be broken down into primary Creep, secondary Creep, and tertiary Creep. Primary Creep begins at a fast rate and then slows down as it approaches the secondary phase. Secondary Creep is the longest portion of the Creep curve and occurs at a constant rate. Finally, during tertiary Creep, there is an increase in the rate of deformation and may culminate in rupture. Ansys has the capability to model primary and secondary Creep, but Tertiary Creep is not typically analyzed because rupture is impending.

 

 

The Norton model is commonly used for modeling secondary Creep. It is a power-law relation that expresses the Creep strain rate as a function of the stress and temperature.

 

 

Setting up a Creep Analysis in Mechanical

The actual process of setting up a Creep deformation analysis is relatively straightforward. First, add a Creep material model to the material in the Engineering Data section of Ansys Workbench. In the below, example, the Norton model was chosen to model secondary Creep.

 

 

To turn on Creep deformation effects for a particular load step, click on Analysis Settings, specify the current load step number, and then turn Creep effects on under Creep controls. You may want to use the first load steps to set up the initial conditions for the Creep analysis with Creep effects turned off, and then have a second load step where Creep effects are turned on. Finally, note the Creep limit ratio under Creep controls. To ensure an accurate solution, this setting limits the ratio of the equivalent Creep strain increment to the equivalent elastic strain. Typically recommended values are between one and ten.

These are the basics of implicit Creep analysis in Ansys Mechanical. If you would like a more thorough example of a Creep analysis, see Chapter 35 of the Workbench Technology Showcase.

Creating Solids from a Deformed Mesh in Ansys SpaceClaim

Quite often, engineers need to set up a model not by using ideal or undeformed geometry but by using a geometry that has been deformed as the result of structural loading. Checking for clearance or fit within a larger top-level assembly, using the deformed shape for additional simulation or physics, or using the deformed components in a production model could be a reason why a user would seek to create solid geometry from their deformed mesh. With some of the Python scripts available in Ansys SpaceClaim, this process is quite easy.

To start, open SpaceClaim and import the following objects (making sure that they all share the same coordinate system and origin):

1. The original model geometry (solids)
2. The undeformed mesh, exported from Ansys Mechanical
3. The deformed mesh, exported from Ansys Mechanical

 

 

From the File menu, create a new Script:

 

 

Copy and Paste in the code below (This SpaceClaim 2021R1) (Copying the comment lines beginning with “#”is optional)

# Python Script, API Version = V20 Beta

from SpaceClaim.Api.V20.Scripting.Internal import CustomMethods

m0=GetRootPart().Components[0].Content.Meshes[0]

m1=GetRootPart().Components[1].Content.Meshes[0]

b=GetRootPart().Bodies[0]

CustomMethods.WarpBodyByMeshNew(b,m0,m1,False,0.00001)

# m0 uses the Original Model in STL (Exported from Mechanical)

# m1 uses the Deformed Model in STL (Exported from Mechanical)

# b uses the Original Model geometry in imported or native to Space Claim

# 0.00001 is the tolerance in meters

Select Version V20 Beta

 

Next, we need to use the select tool to verify the entity ID numbers for m0, m1, and b. Change the select tool from the Script Editor to use the “Index” method:

Then, turn off recording, select the facet body of the original geometry (it should be inside of a component in the tree), then select the Select Tool from the Script Editor to define that selection. Repeat this process for the deformed mesh and the original body geometry. Verify that the IDs for those entities match the corresponding assignments for m0, m1, and b.

If it is helpful, you can simply Copy and Paste the portion of each line starting with “GetRootPart()…” to the definitions for m0, m1, and b. Once all three objects have been defined, comment out the selections by placing a # at the beginning of each line.

Finally, to create your deformed solid, select Run from the Script Editor.

Running the script creates a 4^th entity called “Warp0” seen in the below Structure tree, which is the deformed geometry in solid form.

Now you are ready to use your deformed components in any number of new applications!

Utilizing the Ansys Learning Hub (ALH)

There are several ways to take advantage of your ALH access. The first is to use ALH as a searchable database of tutorials and resources for Ansys setups. To do this, you can simply enter in your search terms into the search bar on the top right of the page, shown below in green. Once searched, ALH will display several articles/lectures related to the search terms. This can be valuable when looking for very specific information, but it can be difficult if you are just trying to get started learning Ansys.

The second, and recommended method of utilizing ALH is to use the associated Campus Building, shown below in orange.

Once you’ve selected your Building, you can then drill down the specifics of what you’d like to see. To do this, scroll down until you see the following selections highlighted in orange (note that these will vary based on the building you choose):

Here you can select the specifics of what you’d like to see. We recommend that if it’s your first time using Ansys products that you select the “Getting Started” module highlighted in green above, otherwise feel free to choose a relevant module.

Navigate from Overview to Content. This will allow you to see all the material within the Fluids – Getting Started learning module in a folder tree layout. At this point, select Course and then finally Current Version – note that this may not be the exact version you have, but if it is within a few releases content should be extremely similar. You can also listen through all the content in lecture form by selecting the Live Instruction folder instead of Current Release.

You can then drill down into very specific content related to what you want to learn. Say you are a new Ansys CFD user and you don’t really know much about using Ansys products, you can get a quick overview and demo by going through the content in M02-CFD Overview and Demo.

At this point you can easily navigate to content files, from which you can view Lectures (titled FLU_GS_20**R*_EN_LE**), which summarize the drilled down content, or Workshops (titled FLU_GS_20**R*_EN_WS**), where you can see exactly what steps need to be taken to set up a problem. We recommend you start with scanning over the Lecture, which typically will just take a few minutes, following which you can either read through the Workshop and apply it directly to your problem or you can download the Workshop .zip file and follow along with the same geometry and setup being showcased in the Workshop.

Following this method, it should be easy to jumpstart your Ansys experience, learn new physical applications, or hone your simulation expertise in a field by navigating to the Campus Building, selecting the desired topic/physics, and then drilling down into specific lectures and workshops to enhance your Ansys experience.

Ansys Mechanical Fatigue Module vs. Ansys Ncode DesignLife

Much of the focus in the world of Finite Element Analysis (FEA) centers on designing a structure to withstand a single application of a static load. Frequently, however, structures are subjected to repeated cyclic loading, which can lead to the initiation and growth of cracks, often culminating in sudden fracture. For many common loading scenarios, the fatigue module of Ansys Mechanical can be used to accurately predict the fatigue life of a part. For more advanced cases, Ansys Ncode Designlife is required. In this blog post, we will discuss three approaches to fatigue, when the Ansys Mechanical fatigue module is adequate, and some situations that require a more advanced analysis in Ansys Ncode Designlife.

There are three main theoretical approaches to fatigue: the crack growth approach, the stress life approach, and the strain-life approach.

The Crack Growth Approach

The crack growth approach directly considers crack size and the rate of crack growth to predict the number of cycles required for the crack to grow to a critical size (usually determined by linear elastic fracture mechanics). This approach can be handled with Ansys’ “Separating Morphing and Adaptive Remeshing Technology (SMART) and is a topic for another blog post. We will focus here on the stress-life and strain-life approaches which can be utilized with the Ansys fatigue module.

The Stress Life Approach

The stress-life approach, developed by August Wöhler in the late 1800s to assess the fatigue life of railroad components, was the first method of fatigue calculation and is still commonly used today. It involves testing smooth material specimens under constant amplitude stress. By testing many specimens at different stress levels, a stress-life (SN) diagram can be developed that shows the number of cycles to failure (N) for a given stress amplitude. An example S-N curve for aluminum is shown in Figure 1. This empirical curve can also be represented in the form of an equation called Basquin’s rule. The stress-life approach is mainly applicable to high cycle fatigue.

Figure 1: An example of an SN curve for Aluminum with an Ultimate Tensile Strength of 320 MPa

The Strain Life Approach

In the 1960’s, the strain-life method was developed to better predict the fatigue life for components which experience plastic deformation. Even in components that remain nominally elastic, localized plastic deformation can often occur near notches. In the strain-life method, specimens are tested under strain control. In contrast to the stress-controlled method discussed in the previous paragraph, during strain-controlled testing, the force applied to the specimen during testing is adjusted to maintain a constant strain amplitude throughout the test. Because the total strain life approach effectively combines the stress life curve (in the form of Basquin’s rule) with the Coffin Manson expression, it can be used for both high cycle and low cycle fatigue.

So why use the stress-life approach for high cycle fatigue when the total strain life approach can handle both low cycle and high cycle fatigue? One answer is that stress-life fatigue data is widely available. Using the strain-life approach may require costly material testing if test data is not available. Another consideration is that the strain life approach requires the use of an equation fit to the test data, which has the potential to introduce some error into the fatigue life calculation.

Figure 2: Plot of Strain Amplitude vs Reversals to Failure used in Strain-Life Analysis

 

 

Ansys Mechanical Fatigue Module vs. Ansys Ncode DesignLife

So, when should you use Ansys Ncode Designlife instead of the fatigue module in Ansys Mechanical? See below for some guidance.

When Ansys Mechanical Fatigue Module can be used:

• Constant amplitude, proportional loading scenarios
• Non-constant amplitude proportional loading scenarios using rainflow cycle counting
• When it is acceptable to use Neuber’s plasticity correction to convert strains calculated in an elastic analysis into a plastic strain for use in a strain-life analysis
• When stress gradient notch corrections are not needed in a stress-life analysis

When to Ansys Ncode DesignLife is required:

• For multiaxial nonproportional loading, requiring a more advanced approach such as the critical plane method
• When it is desired to use a plasticity correction other than Neuber’s correction, such as Hoffman Seeger
• When it is desired to use the actual plastic strain calculated in an elastic-plastic simulation
• When it is desired to use the actual time history of the stress/strain
• When stress gradient notch corrections are necessary in a stress-life analysis

Acoustic Analysis in Ansys Mechanical

In the minds of many engineers, Ansys Mechanical can be used solely to address the behavior of solids. However, there is another class of problems that Mechanical can be used for: acoustics, which is exposed with Ansys Mechanical Enterprise licensing.

What is Acoustics?

Acoustics is the study of sound. Sound is created by pressure waves travelling in an elastic medium, typically air or water. Applications of acoustics include the design of concert halls, noise minimization in manufacturing environments, sonar, and speaker design. Typical results of interest are pressure distributions and gradients in the fluid, sound pressure levels, and scattering, diffraction and transmission of acoustic waves. Acoustic analyses can either be coupled, which accounts for the effect of the fluid on the solid bodies, or uncoupled, which models the fluid only.

Fluid Analysis in Mechanical? Why not CFD?

While the behavior of fluids is generally left to CFD solvers, there is a key difference between typical CFD analyses and acoustics problems—in acoustics analysis, the fluid isn’t flowing. Sound waves transport energy through a medium, but not mass. As with all waves, particles travel back and forth without any net movement. This property allows the mathematics and Lagrangian meshing of the Mechanical solver to be leveraged, with some additional governing equations.

Example: Speaker and Plate

To demonstrate, a simplified speaker model was created with a flat plate 2 inches in front of it, partially blocking the pressure waves. We’ll use Ansys Acoustics to evaluate the sound pressure levels behind the plate, as well as the overall sound pressure distribution.

Figure 1: Solid model of speaker and plate

Using the Enclosure tool in Ansys SpaceClaim, we can easily create a fluid domain in the negative space around these solids. In this case, we’ll create two layers of enclosures. The outer enclosure will be defined to allow us to calculate results outside of our meshed fluid domain (otherwise known as “far-field” results). This is a useful way to keep the overall node count reasonable. For numerical accuracy, the outer layer should be at least three elements thick, and be thicker than 1/10th of the longest wavelength being analyzed.

Figure 2: Fluid domain

For this analysis, we’re assuming that the solid components are perfectly rigid, so we’ll suppress them from the final model. We’ll use the surfaces that form the face of the speaker to create a mass source excitation—essentially defining the amplitude of our sound wave. We’ll then use the analysis settings in our Harmonic Acoustics analysis to specify a range of frequencies that we’d like to examine.

Within the meshed domain (the “near-field”), we can generate a variety of contour plots showing distributions within the fluid, such as the section view of sound pressure level below.

Figure 3: Sound pressure level at 3000 Hz, in dB

In the far-field, sound pressure levels can be queried by specifying a desired location. Polar plots can be created showing sound pressure at a defined circular boundary—Figure 4 shows the sound pressure level 1 meter away from the model origin in a circle on the XZ plane.

Figure 4: Sound pressure level 1m from origin on XZ plane, in dB

Additionally, as in a structural Harmonic Response analysis, we can sweep a frequency range and store each frequency as a result set in our analysis. Using a far-field mic result, we can pick a location in the far-field and output the sound pressure across the frequency range as shown in Figure 5.

Figure 5: Sound pressure level at (0, 0, 1m) across frequency range

Conclusion

Acoustic analysis is a lesser known category in Ansys Mechanical, but it allows for a wide variety of additional studies to be performed in FEA. Users familiar with the Mechanical graphical interface should find the acoustic modules intuitive, with a little study. The Ansys documentation and the Ansys Learning Hub are great resources for engineers looking to add this analysis type to their toolkit.

Explicit Dynamics and Ansys: Part II

Which Explicit Tool is Right for Me?

In my Explicit Dynamics and Ansys: Part I blog post, I discussed the fundamentals of the theory behind the explicit dynamics method for structural simulation, and some of the scenarios in which the method can be useful. However, the question remains: of all the explicit dynamics tools available through Ansys, which is the correct tool for any given application? Luckily, the options available can easily compared by highlighting a few of the key features of each. The four tools or environments I’ll cover are:

1. Explicit Dynamics in Workbench
2. Workbench LS-DYNA
3. LS-DYNA (LS-Prepost and LS-Run)
4. Autodyn

Pictured: Ballistics study performed using Explicit Dynamics (left) and LS-DYNA (right).

Explicit Dynamics

What is it?

Explicit Dynamics is a system component in Workbench that becomes available with the installation of the Ansys Structures package and an Ansys Mechanical Enterprise license. It uses the “Explicit STR” solver, which is essentially a modified version of the Autodyn solver. The pre-processing and post-processing is done using the Ansys Mechanical environment.

Who should use it?

Users that are new to Explicit but are familiar with the ANSYS Mechanical environment especially will benefit from the workflows used in this tool. It leverages the ease-of-use inherent to ANSYS Mechanical, while simultaneously using program-controlled solver settings for several scenarios to take the burden off less-experienced users. This is also the system component used with the “Drop Test” Wizard available in ANSYS Mechanical.

Workbench LS-DYNA

What is it?

Workbench LS-DYNA is very similar to the “Explicit Dynamics” component in that it is a system component available in Workbench. It becomes available with the purchase of an LS-DYNA license as well as the installation of Ansys Mechanical and the loading of the Workbench LS-DYNA ACT extension. Like Explicit Dynamics, this component also uses Ansys Mechanical for the pre/post-processing environment.

Who should use it?

Like Explicit Dynamics, Workbench LS-DYNA is a great tool for less-experienced users who want to start leveraging the explicit method. It combines the ease-of-use of Mechanical and Workbench with the power and versatility of the LS-DYNA. LS-DYNA should be considered as an alternative to Explicit Dynamics for a couple reasons:

1. For simulations that involve relatively low-rate or low velocity events (longer than 0.100s is sometimes used as a very general guideline), LS-DYNA may improve solve time over the Explicit STR solver.
2. Prestressing the model using an implicit solution is more easily accomplished with Workbench LS-DYNA
3. Users with some LS-DYNA experience may prefer it over Explicit Dynamics

LS-DYNA using LS-DYNA Preppost

What is it?

This option leverages the exact same solver as Workbench LS-DYNA, but it allows the user to use the LS-DYNA Preppost environment to setup and review the results of their simulation. This option becomes available with the purchase of an LS-DYNA license and the installation of the LS-DYNA Preppost environment from the Ansys Structures installer.

Who should use it?

Obviously, experienced LS-DYNA users will prefer this option over the others. However, this version of LS-DYNA (as well as the Workbench version) are particularly useful for relatively low-speed simulation as compared to Autodyn and Explicit STR. It is the automotive industry standard for crash-test simulation, is leveraged for simulating bird-strikes on aircraft, and is often preferred for some ballistics and other impact studies. It also uses an open input solver file format, which allows for customization and scripting that Autodyn and Explicit STR are not capable of.

Autodyn

What is it?

Autodyn includes both a pre/post-processing environment as well as a solver. This tool is available with an Autodyn license and the installation of Autodyn from the Ansys Structures installer.

Who should use it?

Autodyn is an extremely powerful asset when very high rates of change are introduced. It is especially useful for blast/explosive simulations, hypervelocity simulations, and those that involve the use of Euler domains (fluids or extreme deformations) or Smooth Particle Hydrodynamics (SPH) for when something is expected to get blown into pieces. LS-DYNA can also simulate using Euler and SPH domains, but it is a key area of strength for Autodyn. While Explicit Dynamics uses the same solver technology as Autodyn, it does not allow for the use of mesh-free domains or the full breadth of the equations of state used to simulate blasts that Autodyn has.

Explicit Dynamics and Ansys: Part I

What is the Explicit Method?

In the last 15 years, Ansys has gone from offering a single explicit dynamics workflow, using Mechanical APDL with a third-party solver and postprocessor, to offering several unique and versatile solutions. These days Ansys customers can leverage two distinct solvers and multiple pre and post processors in various combinations in order to best meet their needs. However, before a user can determine the right explicit solution for themselves, they must first understand what the term “explicit dynamics” means and what sort of problems that methodology is meant to tackle.

Implicit vs. Explicit Methods in FEA

Traditionally, finite element analysis of a transient structural system is carried out using an implicit solutions method; this approach involves two key principles:

1. The assembly of the mass, stiffness, and damping matrices to describe the inherent factors relating to the motion of the structure.
2. The approximated solution an ordinary differential equation describing that motion:

For those inclined to stare blankly at the first sign of math, this equation of motion essentially shows that any external force acting on an object will result in displacement (u vector), velocity (v vector) and acceleration (a vector) of that object. The magnitude of that motion will be inversely related to the stiffness in the system (K matrix), the amount of damping (C matrix), and the mass of the system (M matrix). You can think of these matrices as how springy or elastic the material in use is, how much kinetic energy loss occurs due to heat or sound, and how much resistance to a change in velocity exists respectively. Things get further complicated by the fact that displacement, velocity, and acceleration are all interrelated in a way that makes these equations very difficult to solve directly.

The other significant concept here is the use of matrices to define behavior of a complex system. Since FEA in general involves a component or assembly of components that are broken down into many nodes with many more connections to adjacent nodes, the equations of motion for each node starts to get complicated very quickly. Matrices are a way to describe these complex systems in an organized way that allows a solver to take advantage of certain operations possible in linear algebra.

Consider this 1-dimensional system of springs and nodes. Note that we are only considering the elastic (displacement-related) portion of the motion equations and not inertial (acceleration) or damping (velocity):


The total force acting on, and displacement of each node is going to be related to the relative displacement of the adjacent node or nodes and the stiffness of the springs connecting them. Using a stiffness matrix, we can describe the behavior of the entire system mathematically:

This might look somewhat familiar if you look at the first part of that motion-equation we looked at earlier. In this case, we’re looking at the global stiffness matrix of a simple system as opposed to the matrix of a single node or object. The stiffness between nodes in a finite element model can be thought of as being very similar to the springs’ stiffness in our simple system, and the mass of the system and damping properties can be thought of very similarly to the stiffness in terms of matrix assembly.

So, where are we going with all this? Well, FEA software uses a linear algebraic approach to simplify these matrices before attempting to solve the full equations of motion of the system. In fact, much of the CPU time consumed during the solve process is taken up by this matrix “decomposition” as it is known. Additionally, because the full transient equations of motion can’t easily be solved directly from one point in time to the next, a set of values known as Newmark’s Parameters are used to approximate an incremental change of displacement, velocity, and acceleration between time-steps. The most common method of leveraging these parameters is known as the Newton-Raphson iteration, and involves an iterative approach to solving for the force on any node in the system.

It works like this: the starting position, velocity, and acceleration of the system are known, so the matrices at this state act as our starting point. For the first time increment, a set of matrices modified using the Newmark’s Parameters are formulated and a test force is applied at each node. This test force will result in a new set of positions, velocities, and accelerations at each nodal location. This newly calculated equilibrium state will also result in a new set of calculated forces at each node, and this calculated force can then be compared to the test force. Usually the first iteration will not result in values that fall within a range resulting in an acceptable residual value, so the matrices will be further modified from this first attempt and the process will repeat. This same process repeats until the test force and the calculated force are close enough to be considered converged.

That, in a nutshell, is how the implicit transient method works. In contrast, explicit dynamics takes a different approach to solving motion equations altogether. Instead of using a test force value and incrementally adjusting the system matrices until that test force value matches the resultant equilibrium forces, the explicit approach involves simply integrating the acceleration and velocity terms in the equations over a short period. This results in equations that are defined in terms of displacement alone, meaning they can be solved without the need for convergence toward a solution! Not only that, but this approach also bypasses the need for matrix assembly and decomposition as well, meaning no need for the solver to spend all that time building and simplifying a matrix.

By getting rid of these two often onerous steps, the explicit method allows users to tackle highly complex and nonlinear problems that would otherwise be very difficult to converge (and in many cases it can do so much, much faster). In fact, the Explicit method can be used for some very sophisticated analyses, such as simulating breakage (elements being deleted from the simulation) based on a limit strain value, because the solution at a timestep does not need to converge based on the state of the system at a previous step.

You might be thinking, “Great! Clearly the explicit method is superior. Why wouldn’t we use that approach for everything?” Well, here is the rub: explicit study requires that the analysis be both time-dependent (or transient), and that a minimum time step size be used. The explicit dynamic EOMs are probably not worth showing in their entirety, but one particular term is the issue here:

That innocuous-looking little term might look familiar if you know the equation for the natural frequency of an oscillator:

The significance here is that if the timestep of the explicit analysis, identified here as Δt_i, is longer than the shortest period corresponding to the natural frequencies of the system divided by pi, the motion equation becomes unstable and can’t be solved.

The natural frequencies of the system are sensitive to numerous factors, most significant here are that this period for the natural frequency will decrease with:

1. Increasing material stiffness
2. Decreasing material density or decreasing mass
3. Decreasing size of the SMALLEST element in the entire model

Therefore, the stiffer, more massive, and smaller that smallest element in the model is, the shorter our timestep needs to be to get a solution. And these timesteps can be a tiny fraction of a millionth of a second in many cases! Therefore, even though the Explicit method is a more direct way of solving the equations involved, depending on the problem involved, it might still be more efficient to approach with an implicit solver because of the numerous timesteps necessary for an explicit solution.

Here’s the Bottom Line

The Implicit approach is still a robust and reliable method for solving FEA problems, and usually is the more time and effort-friendly approach for static cases or those that don’t involve much nonlinearity. However, whenever a simulation involves very rapid changes to the state of the model, involves large amounts of deformation or material nonlinearity, or deletion of elements based on material failure, the explicit method excels.

High/Hyper-Velocity Impact and Material FailureFoam and other Highly Non-linear Material

Blast/Explosion/Deflagration

Explicit dynamics can also be very useful for simulating snap-through behavior, metal forming operations, and any number of other events that might otherwise be impossible with the implicit approach. In part 2, we will explore the Ansys Explicit Dynamics portfolio and discuss how each software stacks up against the others in some key areas.

Automation in Ansys Mechanical using Python

Before Ansys Mechanical for Workbench was developed, engineers relied on a scripting language called Ansys Parametric Design Language (APDL) to set up and perform analyses. APDL is a powerful tool, and it is still used behind the scenes whenever a user creates and solves a model in Ansys Mechanical. While the learning curve is steeper than using the modern Ansys Mechanical user-interface, APDL does have some distinct advantages: besides giving the user a fine level of control over the analysis, as a scripting language it also allows for automation of repetitive tasks. Users of Ansys Mechanical still have the option of incorporating APDL code into their model by inserting command snippets into the analysis tree. However, this approach has some drawbacks. Any objects created using a code snippet are created when the model is solved and are not well integrated into the Ansys Mechanical environment. Also, APDL was developed many years ago, and is somewhat cumbersome to use.

With the introduction of scripting into Ansys Mechanical, users can use the modern Python programming language to automate a vast array of tasks. Python scripting is well integrated into the software, and any objects created or analysis settings changed can immediately be seen in the Mechanical GUI. Lines of code can also be quickly saved to a user defined button in the ribbon for tasks that will be performed frequently.

Below, we’ll briefly introduce Python automation in Mechanical and perform a simple automation example to illustrate how powerful this approach can be.

Start by clicking the “Automation” tab in the Mechanical Ribbon. Clicking on the “Scripting” button will open the Mechanical Scripting Editor, where python commands can be entered. Two windows will appear. The top window allows for the user to write a script – multiple lines of code that will be executed sequentially. The bottom window is the Shell, which is useful for issuing single lines of code.

For this example, we will generate point masses given user supplied arrays of masses, coordinates, and mass moments of inertia.  First, a few comments about the python programming language:

• In Python, indentation is used for more than just aiding in readability—it is used to indicate a block of code. For instance, an indented block of code following a for control flow statement indicates all the code that should be executed in that for loop.
• Python is a dynamically typed programming language, meaning that you do not need to declare variables and give them a specific data type.

To create the script, we first define three variables and assign string values representing the units used for length, mass, and mass moment of inertia.

Next, we create list variables to represent the values of the masses and mass moments of inertia for each point mass. The first value in each list corresponds to the first point mass, the second value to the second, and so on. In this example we will create three point-masses.

Now create list variables for the x, y, and z cartesian coordinates.

The command to create a point mass is:

“ExtAPI.DataModel” is used to access the Mechanical datamodel.  Once you type “ExtAPI.DataModel” followed by a period, a list will display showing options. From there, you can drill down through the Mechanical object tree (See below image). Because a point mass in Mechanical is added by right-clicking on “Geometry” in the tree, we need to access “Geometry” via the API in order to add a point mass. The “AddPointMass()” method will create a new point mass. Note the ending parenthesis “()” which are required in python to indicate a method.

Now that we know the command to create a new point mass, we will use a for loop to iterate through the values of the lists defined above and create the point masses. Note the “zip” function allows us to loop through multiple lists simultaneously. Also note that the values are assigned using the “Quantity” type, which allows the value to change based on the unit system selected.

The full code is shown below. Given a list of masses, mass moments of inertia, and cartesian coordinates, it can generate a massive number of point masses in a matter of seconds.

For a thorough introduction to automation in Ansys Mechanical, see “Ansys Mechanical Scripting” and “Introduction to Ansys ACT in Mechanical” located in the Structures Customization Learning Room of the Ansys Learning Hub.