John Doyle – ANSYS

There is a complex contact relationship between the roots of a turbine blade and the corresponding rotor. For applications that involve tight radial tolerances and accumulated layers of multiple contact surfaces, the traditional penalty-based methods of enforced contact compatibility can … Continue reading →

The post Normal Lagrange Contact Formulation and When to Use It appeared first on ANSYS Blog.

Consider the impact of structural relaxation Many engineering structures must be designed to operate successfully in hostile thermal environments. Pipe hangers supporting hot and heavy steam lines, aircraft engine blades, and injection molding machine components are just a few examples. … Continue reading →

The post Structural Relaxation Due to Creep Impacts Performance appeared first on ANSYS Blog.

My nonlinear model will not converge. Where do I begin? There are many different reasons for convergence failure of a nonlinear solution. While the causes and fixes may vary widely from one model to the next, the tools and procedures for … Continue reading →

The post Convergence Failure of a Nonlinear Solution appeared first on ANSYS Blog.

The post What Causes Element Formulation Errors in Nonlinear Structural Runs? appeared first on ANSYS Blog.

Is an element formulation error ruining your day? Add in a command object with ‘NLDIAG,eflg,on’ in the Structural Environment branch to execute as part of a restart after convergence failure. From the Project Page, drag and drop a Mechanical APDL … Continue reading →

The post Tips and Tricks for Dealing with Element Formulation Errors in WB-Mechanical appeared first on ANSYS Blog.

The post How to Keep a Balanced Life…and a Balanced FEA Model appeared first on ANSYS Blog.

There are three methods available for extracting the reaction forces across a contact region in WB-Mechanical: Contact(Underlying Element) Contact (Contact Element) Target (Underlying Element) When you choose ‘Contact(Underlying Element)’, the code is selecting the contact elements associated with that region, … Continue reading →

The post Understanding Contact Reaction Probes in ANSYS Mechanical appeared first on ANSYS Blog.

Contact technology is used extensively throughout ANSYS Mechanical and Mechanical APDL to enforce compatible behavior between different portions within a model. With each Release, ANSYS continues to improve the breadth and robustness of our contact technology. In ANSYS 15.0, we … Continue reading →

The post What’s New with Contact Technology in ANSYS 15.0? appeared first on ANSYS Blog.

Many FEA applications can benefit from the ability to strategically modify a mesh during solution, in order to simulate challenging geometry distortions which otherwise cannot be solved. Unlike manual rezoning, mesh nonlinear adaptivity is completely automatic, requiring no user input during solution.

To activate mesh nonlinear adaptivity within Workbench-Mechanical, insert ‘Nonlinear Adaptive Region’ in the Environment Branch.

Scope the Geometric features to be included in adaptive remeshing

Define the Criterion that triggers mesh modification

Define the checking frequency and range of application

Equally Spaced Points
Specified Recurrence Rate

This same technology is also available in MAPDL via the NLADAPTIVE and NLMESH commands.

To use nonlinear adaptivity most effectively, it is very important to understand the meaning and limitations of the criterion that will trigger a modification of the mesh during the solution.

There are three criterion currently exposed in ANSYS Workbench Mechanical:

Energy: When an element’s strain energy is greater than or equal to the mean strain energy of components to which the element belongs during a time increment (or substep), the element is split and remeshed. The energy based criteria will cause the mesh to be strategically refined in regions where a high concentration of stress exists and elements are too large. It applies to current technology 2D elements and 3-D linear tetrahedral elements (SOLID285).

Box: When nodes of an element are within a user defined region (or “Box”), the element is split and remeshed. This is useful for refining the mesh in regions where it is difficult to predict which elements of the model will be present, or move in to. For example, a small cavity filled by the deformation of a compressed seal. This criteria also applies to current technology 2D elements and 3-D linear tetrahedral elements (SOLID285).

Skewness: A mesh quality check that compares the volume of an element to that of a standard tetrahedral inscribed in the same sphere as the element under consideration. The numerical value of the skewness represents the ratio of volume difference of the two elements to that of the standard element. For an ideally shaped element, the skewness approaches zero as the volume of element under consideration approaches that of the standard element. For a poorly shape element, the skewness approaches 1 as the volume of the element under consideration is approaching zero. Skewness only applies to 3-D linear tetrahedral elements (SOLID285).

When the defined criteria are met, mesh modification occurs either by a combination of splitting followed by morphing or by general remeshing. During splitting, the current elements are divided into elements having a half-edge length. Splitting applies to Energy and box criterion. General remeshing only applies to Skewness criterion on 3-D linear tetrahedral elements (SOLID285). During remeshing, the selected region is completely remeshed to obtain a high quality mesh. For each mesh modification, mesh quality matrics stats are recorded in the Solver output comparing previous mesh with new mesh

Post processing procedure is same as for any conventional Structural Analysis with multiple results sets. All results are automatically saved to one jobname.rst file in working directory.

It is important to note that mesh nonlinear adaptivity via splitting or refinement, in general, cannot repair an already distorted mesh. In some cases, it can exacerbate mesh distortion by creating smaller elements. Most nonlinear material models, especially those employing hyperelastic materials, have their own applicable ranges. When a deformation is too large or a stress state exceeds the applicable range, the material may become unstable. The instability can manifest itself as a mesh distortion, but nonlinear adaptive region cannot help in such cases.

The post What is Mesh Nonlinear Adaptivity? appeared first on ANSYS Blog.

When choosing a formulation to be used in a contact region, you basically decide the mathematical method that the code will use to enforce the contact compatibility condition (for example, no penetration allowed, no separation, no sliding, or sliding with some resistance).

There are four basic formulations:

Penalty method
Augmented Lagrange
Pure Lagrange
Multipoint constraint (or MPC)

This post focuses on the first two formulations.

The penalty method introduces a force at the contact detection point(s) that has penetrated across the target surface with the express purpose of eliminating the penetration. This method uses very simple formulas:

F_c = k_c*D_p

for contact detection points that penetrate across the target, and

F_c = zero

for open contact detection points. k_cis the contact stiffness (also called penalty stiffness); it is a predetermined property of the contact element. D_p is the penetration at the contact element. Hence, the larger the penetration, the greater the calculated force. The challenge here is that the magnitude of the force necessary to prevent penetration is completely unknown beforehand. Obviously, the force needs to be large enough to push the contact surface back to the target surface and, thereby, eliminate unwanted penetration — but not so large that it pushes the contact completely off the target surface, causing error and instability. A positive aspect of the penalty method is that it is elegantly simple. The negative is that you end up with a finite amount of penetration at the end of the load step. Of course, this penetration is necessary for a contact force to be generated. It is important, therefore, that the contact stiffness be large enough so that the resulting penetration is negligibly small; but the contact stiffness cannot be so large as to cause instability and nonconvergence. This same strategy is used both in the opposite direction to prevent separation (with bonded or no-separation behaviors) and in the tangential direction to enforce frictional resistance and no-sliding behavior.

The augmented Lagrange method is very similar to the penalty method. The calculated force at the contact detection point(s) is

F_c=k_c*D_p+ l

in which l is an internally calculated term that augments the penalty-based force calculation. The purpose of the augmentation is to reduce sensitivity to contact stiffness. All things being equal, the augmented Lagrange method should produce less penetration than the pure penalty method, but it might take more iterations to converge. The program-controlled default formulation for contact between flexible bodies is augmented Lagrange.

The optimal value for contact stiffness in these methods is one that generates a converged result in a reasonable number of iterations with a resulting penetration (or elastic slip in the tangential direction) that is inside acceptable tolerance. Often, such an optimal value will vary as you progress through the load path. To enhance convergence, the program automatically adjusts the stiffness based on the current mean stress of the underlying elements and allowable penetration. You can influence the code-calculated stiffness value by manually defining a multiply factor on the stiffness.

To read more about these formulations, refer to the documentation for the CONTA174 element as well as // Contact Technology Guide // 3. Surface-to-Surface Contact // 3.9.3 Selecting an Algorithm.

My next post will discuss the normal Lagrange and MPC algorithms. Stay tuned!

The post What Are the Differences Between the Contact Formulations? appeared first on ANSYS Blog.

Unlike the traditional penalty formulation, the normal Lagrange formulation does not require any penetration to develop forces at the contact interface. This is because the normal Lagrange formulation simply adds internal force DOFs directly to the contact nodes and directly solves for the forces to simulate effectively zero penetration. It is referred to as normal because these forces apply only to the direction normal to the contacting surfaces to prevent penetration. The penalty method is still used in the tangential direction when friction is also being simulated.Certainly the normal Lagrange method sounds like an attractive alternative to the traditional penalty method for applications in which any amount of penetration at the contact interface is undesirable. However, it should be noted that the advantage of simulating zero penetration comes at a cost. Normal Lagrange formulation can be more costly in terms of run time, and it can be less forgiving in terms of convergence when compared to the penalty method. Normal Lagrange forces are applied like a step function: They are fully on when the contact status is closed, and they are off when the status is open. By contrast, penalty-based forces are ramped in proportion to the amount of penetration, leading to easier convergence in general.

A phenomenon referred to as chatter can sometimes occur with normal Lagrange that represents the repeated oscillation between open and closed contact status during a substep. Chatter is reported in the solution output when it occurs. Contact element real constants FTOLN and TNOP can be used in combination to help stabilize a chattering normal Lagrange contact when it occurs. Refer to Section 3.9.4.6 of the Contact Technology guide for more details on how to use these parameters.

The post Normal Lagrange Contact Formulation and When to Use It appeared first on ANSYS Blog.

Consider the impact of structural relaxation

Many engineering structures must be designed to operate successfully in hostile thermal environments. Pipe hangers supporting hot and heavy steam lines, aircraft engine blades, and injection molding machine components are just a few examples. When designing such mechanical systems, it is wise to consider the impact that structural relaxation due to creep might have on long-term performance.

Creep is a thermally induced phenomenon that typically occurs in crystalline structures, like metals. Its effects, as observed on a macroscopic level, are caused by the diffusional flow of vacancies and dislocations on a microscopic level within the crystalline structure. These vacancies are point defects, and they tend to favor grain boundaries that are normal, rather than parallel, to the applied stress. Their movement tends to be from regions of high concentration to regions of low concentration. Dislocations in grains are line defects. Their movement tends to be activated by high stresses, although this may also occur at intermediate temperatures. Grain boundary sliding is sometimes considered as a separate mechanism that also contributes to creep deformation.

Creep, like plasticity, is an irreversible (inelastic) strain. But unlike plasticity, creep has no yield surface at which inelastic strains occur. Hence, creep does not require a higher stress value for more creep strain to occur. Creep strains are assumed to develop at all non-zero stress values. While temperature plays a large part in the activation of creep strains, it can also be influenced by stress, strain and time.

Three stages of creep: primary, secondary and tertiary

The primary stage is characteristic of strain rate decrease over time. This tends to occur over a relatively short period at the beginning of the life of the component.

The secondary stage, also referred to as steady-state creep, typically has a constant strain rate associated with it. This stage typically has the longest duration during the life of the component.

The tertiary stage occurs toward the end of the component’s life. The strain rate rapidly increases until failure occurs.

ANSYS Workbench Mechanical and MAPDL offer 13 different mathematical models for simulating creep. These models offer a variety of options for simulating primary or secondary stages, separately or together.

Join us for a free one-hour webinar that discusses in detail the practical setup procedures for performing creep simulation on June 20.

===============================================================

Ask The Expert – Modeling Creep Behavior in ANSYS Mechanical and Mechanical APDL 14.0

Wednesday, June 20, 2012
4:00 p.m. EDT, 8:00 p.m. GMT
REGISTER HERE

Duration: 60 minutes

Creep deformation is irreversible, time-dependent progressive distortion at stress levels less than yield. Its effect is usually only significant at elevated temperatures, but many devices, such as steam turbines, jet engines and heat exchangers, operate at temperatures greater than the minimum temperature required for the onset of creep behavior. Accurate simulation of creep behavior is essential for predicting and preventing in-service failure of critical structural components. ANSYS Mechanical and Mechanical MAPDL have a full library of industry-accepted creep laws as well as the curve fitting tools necessary to generate coefficients required for each law. These capabilities have been enhanced in ANSYS 14.0.

This webinar explains how to model creep behavior in ANSYS Mechanical and Mechanical APDL 14.0. It begins with a short presentation, then a panel of experts from ANSYS development and technical services groups answer questions live via WebEx.

The post Structural Relaxation Due to Creep Impacts Performance appeared first on ANSYS.

Whether you are new to nonlinear analysis or a seasoned veteran, the beginning of any successful diagnostic process starts with a thorough understanding of the information that is recorded in the solver output. If given the choice, I would rather start with a review of the complete solver output file than the model itself when trying to answer the question “What went wrong?”

The solver output is available in the Solution Information branch of an ANSYS Mechanical in ANSYS Workbench session. It contains a wealth of valuable information that the analyst can and should review to determine “Yes that makes perfect sense” or “Wait a minute … that’s not what I wanted or expected.”

Simple but important details such as using the appropriate license and version for the application can be easily confirmed by just reviewing the top of the solver output. However, the solver output contains much more than basic statistical information. As you scroll from the top of the solver output file to the bottom, you are looking at a complete text record of the nonlinear model setup and execution. All of the solution control specifications are recorded. All of the calculated contact properties and the initial status are displayed. All of the various element types and element technologies are shown. A summary of calculations related to the Newton–Raphson numerical method for adjusting the stiffness matrix throughout the run are also recorded.

The force convergence graph (also available from the Solution Information branch) is a graphical representation of this same information. Any warnings, error messages and bisections executed during the run are recorded in the solver output file and in the context of when they occur. Warnings, in general, can be interpreted as “Be aware this is happening, it may or may not be a problem.”

For example, a warning about a contact status changing from open to closed might be good news and something that is expected. It might, however, be evidence of when the trouble began. On the other hand, an error message can always be interpreted as “This is a problem. The code cannot continue until something is changed.” Sometimes the code will make changes automatically in an attempt to remedy the situation. These changes are also recorded.

The solver output is basically telling the analyst a story about what worked and what did not. Often after a cursory review of the solver output, the analyst can begin to determine why a convergence failure might be occurring and/or what the code was struggling with. He or she may not yet have the complete answer, but this is a very good place to start.

After reviewing the solver output, the next step depends largely on what information he or she is interpreting from this output. In future blogs, we will explore the numerous options and tools at your disposal to deal with the problems recorded in the solver output. Stay tuned.

The post Convergence Failure of a Nonlinear Solution appeared first on ANSYS.

When the ANSYS structural code issues an element formulation error in the solver output, it is basically reporting that there has been a mathematical breakdown in the computation of the deformed element shape or the derived quantities (stresses and strains) at the integration points within the field of the element. The solver calculates displacements at the element nodes from the stiffness and nodal forces. Element shape functions are used to interpolate these DOF results across the field of the element. The software calculates derived quantities at the element integration points located within the field of the elements from the nodal displacements and the strain-displacement B matrix. From these discrete values, results are extrapolated (if linear) or copied (if nonlinear) to the nodes, averaged, and then interpolated across the field of the elements to produce a nice uniform contour of results.

So why does this not always work? There are several possible causes for element formulations errors. The cause might be due to a singularity (highly concentrated constraint or force) that is introducing a very large amount of deviatoric strain energy into one or more elements — so much so that the element shape functions are no longer able to characterize the deformed shape of the element under load. When element formulation errors are caused by such singularities, the error is often preceded by small or large pivot warnings.

Sometimes element formulations are caused by poorly or insufficiently defined contact relationships. For example, a relatively coarse mesh on a contact and/or target together with an inappropriately large contact stiffness associated with flimsy underlying geometry on a curved surface can lead to element formulation errors. In such cases, often the error is preceded by warnings about abrupt contact status changes.

Sometimes element formulation errors are related to a breakdown in the nonlinear material definition. The structural stiffness is defined in part by the material modulus. If the material has gone elastic perfectly plastic, yielding through an entire cross section under a force-based load, there is no stiffness left in the structure to resist the load. The nonconvergence in this case is really just a reflection of a physical instability. If the structure were loaded the same way in the lab, all things being equal, it would fail to support the load. In the case of hyperelastic materials, sometimes the strain energy density function is inadequate to characterize the stress–strain relationship that is developing in the structure, or perhaps the test data used to derive the function coefficients was inadequate to capture all the modes of strain present in the model.

Whatever the cause, proper diagnostics of such errors requires you to study the solver output carefully for warnings leading up to the element formulation and take advantage of nonlinear diagnostics tools to plot where Newton-Raphson residuals (measures of force imbalance) are highest. Also, take advantage of results-tracking tools to try to understand the trends. Together, these tools can help you determine where you need to concentrate your efforts.The remedy to an element formulation error can vary depending on what is triggering it. Sometimes, it might just be a matter of applying the load more gradually over more substeps and across a finer mesh. Sometimes, dropping a contact stiffness value by one or two orders of magnitude in a critical location can relieve the situation. In cases involving nonlinear materials, sometimes removing singularities that are sources of fictitiously high stress and strain can be helpful. You might find that, in more complicated applications, the corrective action involves some combination of all of the above.

The post What Causes Element Formulation Errors in Nonlinear Structural Runs? appeared first on ANSYS.

Is an element formulation error ruining your day?

Add in a command object with ‘NLDIAG,eflg,on’ in the Structural Environment branch to execute as part of a restart after convergence failure.

From the Project Page, drag and drop a Mechanical APDL Component System onto the Setup and Solution of the Mechanical run. With RMB on Mechanical APDL, click on ‘Edit in Mechanical APDL’.

Once MAPDL interface is open, go to General Post Proc=>Data&File Opts and browse for the rst file created during the Mechanical Run. Then read in the “Last Set” of results.

From here, you can select “Nonlinear Diagnostics” and highlight the item(s) that appear in the ‘Nonlinear Diagnostics – Postprocessing’ dialogue box.

The Component Manager can be used to create components of offending element(s) and generate plots for review.

In this particular case, at least one element in the lower right hand corner of the hyperelastic body is going thru excessive distortion at the point of convergence failure.

Upon closer examination of the WB-Mechanical Plot in this location, distortion appears in many elements, but the diagnostics tool is only reporting one element .

This is because when the element distortion is excessive enough to cause such an error, the code will stop. The element reported by the Nonlinear Diagnostics tool was the first one to trigger this error. Had these elements only caused warnings, then the Nonlinear Diagnostics would have continued and recorded all the offending elements.

The remedy in this particular case would be to remove the singularity at such fictitiously sharp corners, by adding radii and perhaps modeling in a rigid body together with nonlinear contact to interface directly with this hyperelastic body at this location as opposed to applying a displacement directly.

It is also worth mentioning that the coefficients for the Mooney Rivlin material model in this case were derived from uniaxial test data only. While these coefficients fit the uniaxial curve very well, notice that the resulting equibiaxial and shear curves (for which no test data was included as part of the curve fitting) are very steep relative to tension behavior. This implies a very stiff response in compression and/or shear loading.

This might be correct, but without a complete set of material test data that includes tension, shear and compression, it is impossible to judge for sure. A complete set of material test data will enable a more robust and more accurate material model and will likely enhance the convergence.

Life is too short to let these types of errors stand between you and a successful FEA run.

The post Tips and Tricks for Dealing with Element Formulation Errors in WB-Mechanical appeared first on ANSYS.

The key to a balanced life is clean living. There are some simple rules to live by. Always tell the truth, even if it makes you look bad. Don’t spend more than 10 dollars for every 10 dollars that you make. Never steal another man’s wife, his horse, ox or his cattle prod. And never try to push on a rope. If you keep to these simple rules, your life will remain in balance.

As it is in life, so it can sometimes be in the FEA world. There are some first principle rules to live by to keep things in balance.

For example, if you apply a torsional load via remote points, don’t expect your reactions to always balance if you run this as small deflection. Remote loads and displacements in Workbench Mechanical are implemented using constraint equations. With small deflection analysis, we do one pass thru the linear code. These constraint equations are only created once. If the resulting rotation is large enough, the CEs might become invalid thru the large rotation. In the end, things will not add up. We do issue a warning in the solver output. If in doubt, always turn large deflection ON before checking anything else.

If you try to apply a torsional displacement to a flimsy open cross section of a structural beam element, don’t expect your moment reaction to match that of an equivalent model represented with shells or solids. The numbers might be way off. The reason is that, by default, the calculations are based on classical Timoshenko beam theory. We do not include any adjustment for cross sectional warping of the element. To get the beam moment reaction to match that of an equivalent solid or shell model, there is an option to include a warping DOF via KEYOPT(1)=1 (for BEAM188/9). You have to know this. The option is documented in the elements manual, but we are not going to give you any warnings or notes about it in the solver output.

Also, when running a truly large deflection nonlinear contact problem, if the model converges, but the reactions do not add up, consider the Newton-Raphson convergence criteria. If the tolerances are too loose, you might be looking at false convergence. The default tolerances are generally designed to be conservative, but sometimes, depending on the application, they might need to be tightened up or you might need to reconsider how you are applying your loads and/or constraints.

Finally, if you ever do try to push on a rope and you end up face planting to the ground, don’t expect to model this scenario in a static structural run. It will not converge.

The post How to Keep a Balanced Life…and a Balanced FEA Model appeared first on ANSYS.

There are three methods available for extracting the reaction forces across a contact region in WB-Mechanical:

Contact(Underlying Element)
Contact (Contact Element)
Target (Underlying Element)

When you choose ‘Contact(Underlying Element)’, the code is selecting the contact elements associated with that region, selecting nodes attached to the selected contact, and then selecting elements attached to the selected nodes before calculating the reaction.

Below is an equivalent APDL command script, where “cid1” is a parameterized contact element type number for the region of interest.

*****************
ESEL,s,type,,cid1
NSLE,s
ESLN,s
NFORCE
*****************

When you choose ‘Contact (Contact Element)’, the code is only selecting the contact elements and executing “NFORCE,cont”

Below is an equivalent APDL command script.

*****************
ESEL,s,type,,cid1
NFORCE,cont
*****************

The ‘Target (Underlying Element)’ option is similar to the first except we select the Target elements (Type=tid1) instead of the contact elements. Below is an equivalent APDL command script.

*****************
ESEL,s,type,,tid1
NSLE,s
ESLN,s
NFORCE
*****************

The availability of these reaction options is governed by the MISC option of the OUTRES command.

(Refer to on-line documentation: // Mechanical User Guide // Using Results // Structural Results // Structural Probes // Reactions: Forces and Moments for more details.)

Often all three methods produce the same calculated reaction.

Sometimes they will not agree because either the contact and/or the target surfaces share nodes with other constraints or other contact regions.

When this happens, one or more of the methods will calculate a force summation that represents the load transmitted across the contact region in question plus other loads from other sources. The overall result of the FEA model is not necessarily wrong, but these probed force calculations are no longer representing only the load across the contact region of interest. The first suggested workaround is to try to employ a strategically tighter trim tolerance to eliminate this unwanted force bleed off. Trim will remove both contact and target elements from respective surfaces that are separated by a distance larger than the user defined tolerance. In some cases, the default tolerance might be too large or perhaps Trim technology is turned off altogether.

Note, for Trim contact set to “Program Controlled”, it will be off for manually created pairs and if large deflection is ON (for models created in R14.5). If Trim options are not successful or not practical, you might need to consider a change to the way the model is constrained or a change in the contact regions definitions.

What happens if there are no shared constraints and the ‘Contact (Contact Element)’ option does not agree with the other two? The question to ask in this circumstance — Is this problem being run as small deflection with linear contact? If so, does the contact pressure profile look reasonable for the given load? If it does not look reasonable or you are not sure, try turning on large deflection and re-running the analysis. It is important to understand that the ‘Contact (Contact Element)’ extraction option is using the contact pressure profile integrate over the contact surface to calculate the overall reaction force. Hence, this calculation is only as accurate as the accuracy of contact pressure profile. If it is not really a large deflection application and you are not interested in running multiple iterations to improve the contact pressure profile, you could switch to MPC formulation. This will block the ‘Contact (Contact Element)’extraction method altogether.

The post Understanding Contact Reaction Probes in ANSYS Mechanical appeared first on ANSYS.

Trim Contact, first introduced in ANSYS 14.5, is a great tool for reducing the number of unnecessary contact and target elements in large assemblies. In ANSYS 15.0, we have changed the default to activate trim contact even for application involving large deflection.

Many of you are probably aware that a Compression Only Support in Mechanical is simulated with a conventional rigid to flexible contact pair under the hood. While this is a logical application for a nonlinear contact pair, it has sometimes introduced unintended convergence challenges for Mechanical users. For relatively flimsy structures, for example, the default penalty stiffness factor of the contact pair associated with a compression only support might be inappropriately large for the application. In ANSYS 15.0, the details window of compression only supports now gives users the ability to control the contact stiffness and the stiffness updating scheme.

Bolt assembly modeling has been enhanced with the new Increment load option. This option enables users to ramp from the previously solved adjustment to a new value for challenging bolted assemblies that will not solve with the conventional load and lock method.

Also, if there is an interest in modeling the presents of Bolt Thread details, a new option has been added to the Contact details window that enables uses to include the bolt thread details without explicitly modeling them.

In the past, some users have expressed an interest in simulating physical wear between sliding frictional surfaces. Now in ANSYS 15.0, you can do just this with the new Archard Wear Model. This algorithm moves the contact nodes to new positions based on calculated material volume loss as a function of pressure, relative velocity and material hardness.

To learn more about these and other contact related enhancements, please tune in to the next ASK THE EXPERTS session scheduled for April 16^that 9:00 am ET and again on April 30^th at 4:00 pm ET.

The post What’s New with Contact Technology in ANSYS 15.0? appeared first on ANSYS.