ANSYS Mechanical – Overcoming Convergence Difficulties with Automatic Remeshing (Nonlinear Adaptive Region)

One of the problems we can encounter in a nonlinear structural analysis in ANSYS Mechanical is that elements become so distorted that the solver cannot continue.  We get messages saying the solver was unable to complete, and the solver output will contain a message like this one:

 *** ERROR ***                           CP =      37.969   TIME= 14:40:06
 Element 2988 (type = 1, SOLID187) (and maybe other elements) has become
 highly distorted.  Excessive distortion of elements is usually a       
 symptom indicating the need for corrective action elsewhere.  Try      
 incrementing the load more slowly (increase the number of substeps or  
 decrease the time step size).  You may need to improve your mesh to    
 obtain elements with better aspect ratios.  Also consider the behavior 
 of materials, contact pairs, and/or constraint equations.  Please rule 
 out other root causes of this failure before attempting rezoning or    
 nonlinear adaptive solutions.  If this message appears in the first    
 iteration of first substep, be sure to perform element shape checking. 

The Solution branch will have the telltale red lightning bolts, indicating the solution was not able to complete due to nonconvergence.

If you are not aware, one technique we can use to get past this problem of excessive element distortion is to have ANSYS automatically remesh the model or a portion of the model while the solution is progressing.  The current state of the model is then mapped onto the new mesh, in the currently deflected state.  In this manner we can automatically continue with the solution after a slight pause for this remeshing to occur.  Minimally all we need to do as users is insert a Nonlinear Adaptive Region under the Static Structural branch, and review and specify a few settings (more on this later).

Let’s take a look at a simple example.  This is a wedge portion of a circular hyperelastic part, subject to a pressure load on the top surface.  Other boundary conditions include a fixed support on the bottom and frictionless supports on the two cut faces of the wedge.

For this case, the nonlinear adaptive region is the entire part. 

The initial mesh was setup as a default mesh, although note that for 3D models the nonlinear adaptive capability requires a tetrahedral mesh up through the current version, 2019 R2.

Prior to solving with the nonlinear adaptive region included, this model fails to converge at about 56% of the total load.  With the addition of the nonlinear adaptive region, the model is automatically remeshed at the point of excessive element distortion, and the solution is able to proceed until the full load is applied.  The force convergence graph has a solid vertical orange line at the point where remeshing occurred.  The method can result in multiple remeshing steps although in the sample model shown here, only one remeshing was needed.

The image on the left, below, shows the original mesh at the last converged substep before remeshing occurred.  The image on the right is the first result set after remeshing was completed.

The tabular view of a result item will show in the last column if remeshing has occurred during the solution.

Here is the final deformation, for the full amount of pressure load applied on the top surface.

Next, let’s take a look at the nonlinear adaptive region capability in more detail.

First, multiple substeps must be used for the solution.  If we are performing a nonlinear analysis, this will be the case anyway.  Second, Large Deflection needs to be turned on in the Analysis Settings branch.  Also, results must be stored at all time points (note that time is a tracking parameter in a static analysis, but all static as well as transient results in ANSYS Mechanical are associated with a value of ‘time’).

There are several restrictions on features that CAN’T be in the model, such as cyclic symmetry (hence the frictionless support BC’s on the simple model shown above), Auto Asymmetric Contact, Joints, Springs, Remote Forces and Displacements, etc.  Also certain material properties are excluded, such as Cast Iron plasticity and Shape Memory Alloy.  Also, as mentioned above, for 3D models, the mesh must be tetrahedral.  For a full listing of these restrictions, refer to the ANSYS Mechanical User’s Guide.  A search on ‘nonlinear adaptive’ will take you to the right location in the Help.

Nonlinear Adaptive Regions can be scoped to 3D solid and 2D bodies, or to elements via a Named Selection. 

In the Details view for the Nonlinear Adaptive Region, the main option to be defined is the Criterion by which remeshing will be initiated.  There are three options available in Mechanical:  Energy, Box, and Mesh.

The Energy criterion checks the strain energy of each element within the Nonlinear Adaptive Region.  If the strain energy is above a criterion, remeshing is triggered.  The input is an energy coefficient between zero and one, and is a multiplier on the ratio of total strain energy of the component divided by the number of elements of the component.  Recommended values are 0.85-0.9.  A lower coefficient will tend to cause remeshing to be more likely.

The Box criterion defines a geometry region based on a coordinate system and bounds relative to that coordinate system.  Elements in the Nonlinear Adaptive Region whose nodes have all moved within the box will be remeshed.  The idea is that if it’s known that elements will be highly distorted as they move into a certain region, we can ensure that remeshing will occur there.

The Mesh criterion allows us to specify that remeshing will occur if mesh quality measures drop below certain levels as the mesh distorts.  For 3D models, the available measures are Jacobian Ratio and Skewness.  These are described in the Mechanical User’s Guide in the section on Nonlinear Adaptive Region.

In the example shown above, the Energy criterion was used with an energy coefficient of 0.85.

There are some things to be aware of when you are trying to implement a Nonlinear Adaptive Region to help overcome convergence difficulties.  First, if any of the restricted features mentioned above are included in the model, such as remote displacements, it’s not going to work.  Therefore, it’s important to review the list of restrictions in the Help and make sure none of those are applied in your model.  Second, ‘buckling’ or element distortion due to an unstable structure is not a behavior that Nonlinear Adaptive Regions can help with.  The Nonlinear Adaptive Region capability is more suited to problems like hyperelastic seals being compressed or objects that are undergoing a high degree of bending (but not snapping through). 

Also, a coarse mesh that distorts may not produce a usable remesh.  The remeshing step may occur, but the simulation may not be able to proceed beyond that and stops with an error in element formulation error.  More mesh refinement may be needed in this case.

As a further word of caution, self contact problems may not work very well within the context of Nonlinear Adaptive Regions.  If self contact is needed, consider splitting the bodies into multiple parts to avoid self contact. 

There are some other considerations for the method as discussed in the Help, but hopefully the guidelines and recommendations presented here will allow you to filter potential applications appropriately and setup models that can take advantage of the Nonlinear Adaptive Region capability.  We have a short animation which shows the remeshing step in the sample model. 

If you have nonlinear static structural models with convergence difficulties due to excessive element distortion, please consider using this method to help you get a fully converged solution.

Here is a video to help everyone visualize:

Press Release: PADT Awarded U.S. Army Phase I SBIR Grant for Combustor Geometry Research Using 3D Printing, Simulation, and Product Development

We are pleased to announce that the US Army has awarded PADT a Phase I SBIR Grant to explore novel geometries for combustor cooling holes. This is our 15th SBIR/STTR win.

We are excited about this win because it is a project that combines Additive Manufacturing, CFD and Thermal Simulation, and Design in one project. And to make it even better, the work is being done in conjunction with our largest customer, Honeywell Aerospace.

We look forward to getting started on this first phase where we will explore options and then applying for a larger Phase II grant to conduct more thorough simulation then build and test the options we uncover in this phase.

Read more below. The official press release is here for HTML and here for PDF.

If you have any needs to explore new solutions or new geometries using Additive Manufacturing or applying advanced simulation to drive new and unique designs, please contact us at 480.813.4884 or info@padtinc.com.


PADT Awarded U.S. Army Phase I SBIR Grant for Combustor Geometry Research Using 3D Printing, Simulation, and Product Development

The Project Involves the Development of Sand-Plugging Resistant Metallic Combustor Liners

TEMPE, Ariz., August 15, 2019 ─ In recognition of its continued excellence and expertise in 3D printing, simulation, and product development, PADT announced today it has been awarded a $107,750 U.S. Army Phase I Small Business Innovation Research (SBIR) grant. With the support of Honeywell Aerospace, PADT’s research will focus on the development of gas turbine engine combustor liners that are resistant to being clogged with sand.  The purpose of this research is to reduce downtime and improve the readiness of the U.S. Army’s critical helicopters operating in remote locations where dirt and sand can enter their engines.  

“PADT has supported advanced research in a wide variety of fields which have centered around various applications of our services,” said Eric Miller, co-founder and principal, PADT. “We’re especially proud of this award because it requires the use of our three main areas of expertise, 3D printing, simulation and product development. Our team is uniquely capable of combining these three disciplines to develop a novel solution to a problem that impacts the readiness of our armed forces.”

The challenge PADT will be solving is when helicopters are exposed to environments with high concentrations of dust, they can accumulate micro-particles in the engine that clog the metal liner of the engine’s combustor. Combustors are where fuel is burned to produce heat that powers the gas turbine engine. To cool the combustor, thousands of small holes are drilled in the wall, or liner, and cooling air is forced through them. If these holes become blocked, the combustor overheats and can be damaged.  Blockage can only be remedied by taking the engine apart to replace the combustor. These repairs cause long-term downtime and significantly reduce readiness of the Army’s fleets.

PADT will design various cooling hole geometries and simulate how susceptible they are to clogging using advanced computational fluid dynamics (CFD) simulation tools. Once the most-promising designs have been identified through simulation, sample coupons will be metal 3D printed and sent to a test facility to verify their effectiveness.  Additionally, PADT will experiment with ceramic coating processes on the test coupons to determine the best way to thermally protect the 3D printed geometries.

“When we developed new shapes for holes in the past, we had no way to make them using traditional manufacturing,” said Sina Ghods, principal investigator, PADT. “The application of metal additive manufacturing gives PADT an opportunity to create shapes we could never consider to solve a complex challenge for the U.S. Army. It also gives us a chance to demonstrate the innovation and growth of the 3D printing industry and its applications for harsh, real-world environments.”

Honeywell joined PADT to support this research because it is well aligned with the company’s Gas Turbine Engine products. The outcome of this research has the potential to significantly improve the performance of the company’s engines operating in regions with high dust concentrations.

This will be PADT’s 15th SBIR/Small Business Technology Transfer (STTR) award since the company was founded in 1994. In August 2018, the company, in partnership with Arizona State University, was awarded a $127,000 STTR Phase I Grant from NASA to accelerate biomimicry research, the study of 3D printing objects that resemble strong and light structures found in nature such as honeycombs or bamboo.

To learn more about PADT and its advanced capabilities, please visit www.padtinc.com.

About Phoenix Analysis and Design Technologies

Phoenix Analysis and Design Technologies, Inc. (PADT) is an engineering product and services company that focuses on helping customers who develop physical products by providing Numerical Simulation, Product Development, and 3D Printing solutions. PADT’s worldwide reputation for technical excellence and experienced staff is based on its proven record of building long-term win-win partnerships with vendors and customers. Since its establishment in 1994, companies have relied on PADT because “We Make Innovation Work.” With over 80 employees, PADT services customers from its headquarters at the Arizona State University Research Park in Tempe, Arizona, and from offices in Torrance, California, Littleton, Colorado, Albuquerque, New Mexico, Austin, Texas, and Murray, Utah, as well as through staff members located around the country. More information on PADT can be found at www.PADTINC.com.

# # #

Five Takeaways from the New User Interface in ANSYS Mechanical 2019 R2

Ten years is a long time in the life of a software product.  While ANSYS itself has been around since the early 1970’s and what is now known as ANSYS Mechanical is approaching 20 years old, the user interface for ANSYS Mechanical maintained the same look and feel from version 12.0 in 2009 through version 2019 R1 in 2019.  That’s 10 years.  Certainly, there were many, many enhancements over that 10 year period, but the look and feel of the Mechanical window remained the same.

With the release of version 2019 R2, the Mechanical user interface has changed to a more modern ‘ribbon’ window, as shown in the red region here:

After having used the new interface for a while, here are 5 takeaways that are hopefully useful:

  1. It’s easy to use.  Sure, it’s different but the overall process is the same with a simulation tree on the left, details to enter and adjust at lower left, graphics in the middle, message, and graphs at the bottom, and the main menus across the top.
  2. ANSYS, Inc. has helped by providing a 12-slide (some animated) usage tips guide which pops up automatically when you launch ANSYS Mechanical 2019 R2.
  • As in the old menu, the ‘Context’ menu changes based on what you have clicked on in the tree.  For example, if you have clicked on the Mesh branch, the Context menu will display meshing controls across the top of the window.
  • As intuitive as the new ribbon interface is, there are some functionalities that you may have trouble finding.  Not to worry, though, as there is a new Search field at upper right that will likely take you to the right place.  Here I am interested in making a section plane for plotting purposes.  My first thought was that it would appear in the Display menu.  When I didn’t find it there, I simply typed in ‘section’ in the search field and the first hit was the right one.

After clicking “Take me there”:

And the resulting section plot:

  • Some capabilities show up in the File menu other than the expected Save and Save As functionality.  For example, Solve Process Settings is now in the File menu.  However, the main functionality is in the Solution context menu, such as using Distributed solutions and specifying the number of cores.

In short, the 2019 R2 improvements to ANSYS Mechanical allow for easier and faster setup of our simulations.  If you haven’t given it a try, we encourage you to do so.

Automating Subsea Design (or How I Learned to Love Parameters)

In a previous life, I worked in the maritime and offshore energy industries and used ANSYS as part of my daily routine in structural design. I eventually discovered myself in a position where I was designing subsea equipment for use in offshore oil and gas fields. One thing I quickly discovered was that although subsea structures tend to be fairly simplistic looking (think playground equipment…but 10000 feet underwater) there are multiple design factors that can easily cause a domino effect that would require redesign(s). Whether it was a change brought upon by the client, tool manufacturer, or to satisfy the whims of marine warranty companies, there was always a need to evaluate multiple variants of any subsea structure.

Sounds like a very reactive process, right? So how can we bring this process into a more streamlined analysis workflow within ANSYS? Just use parameters with SpaceClaim and ANSYS Mechanical!

So what can parameters do to aid in this process?

  • Remove repetitive tasks
  • Account for geometric changes to CAD models
  • Use a range of values for material properties
  • Create associative connections between CAD models and ANSYS results
  • Allow for automatic goal driven design exploration

Now let’s look at some common use cases for parameters that I’ve run into in the past:

Accelerations for Onboard Equipment and Cargo

Cargo transported on the ocean is subject to the same accelerations that affect the vessel transporting it (surge, sway, heave, pitch, roll, and yaw). These accelerations are then combined into three representative accelerations and applied in multiple loadcases.

Typically, these loadcases are resolved in independent analysis systems but we can remove all that fluff with a simple parameter driven analysis. All one has to do is tag inputs and result items as parameters and then input values for each load case (or Design Point). In this case I have selected the XYZ components of an acceleration input applied to a mass point as well as the total deformation and maximum equivalent stress. With the push of a button ANSYS will then solve all of these design points and will amend the table to show the selected results corresponding with each design point. Results from the Design Points can be uploaded individually but this parametric analysis has made it very easy for us to determine which Design Points / load cases have the greatest influence on the design.

Geometry Influence Study

So one of the questions often asked during the design process is “Will the design work after we change this dimension to compensate for X?” which is often followed by a discussion on robustness (which is then followed by a change order). So let’s skip the discussion middle-man and move to be proactive by using parameters to quantify just how much we can change our geometry before a problem arises.

Here we have an example subsea Pipeline End Termination (PLET) structure and let’s say a client has asked us to verify if this design can work for various pipeline sizes. The PLET has some major parts that can be influenced by this change: The pipeline clamp, cradle, flanges, ball valve, and bulkhead.

Because we can use parameters there’s no need to make a new model. Merely tag items you wish to create parameters for in SpaceClaim:

Then ANSYS Workbench will start to populate its parameter tables accordingly:

We can then make certain parameters dependent on others, or define them via simple expressions. In this way we can enforce clearances and relations between the various bodies in our model.

From here all we have to do is define our variables for our future analyses:

Then tell ANSYS to solve all the design points with a single click. Note that users can create charts and tables before the solve and ANSYS will populate these live during the solution process. Individual design point results and geometries can also be reviewed at any time.

For this particular analysis we provided the same load to each Design Point but a good next step would be to set a goal driven analysis and have a range of loadings on the pipeline end of the PLET to represent various installation conditions.

Parameters are a very powerful tool within the ANSYS toolbox. They can remove repetitive tasks within FEA, easily create loadcases, and address concerns about design robustness by letting ANSYS and SpaceClaim handle CAD model rework.

That’s it for this blog post! I’ll be creating a few offshore industry-specific posts in the future as well so stay tuned!

Four Different Ways to Add Customization to ANSYS Mechanical

ANSYS Mechanical is a very powerful tool right out of the box.  Long gone are the days when an FEA tool was just a solver, and users had to write code to create input files and interpret the results.  Most of the time you never have to write anything to effectively use ANSYS Mechanical. But, users can realize significant gains in productivity and access greater functionality through customization. And it is easy to do.

Before we talk about the four options, we need to remember how the tool, ANSYS Mechanical, is actually structured.  The interface that users interact with is a version of ANSYS Workbench called ANSYS Mechanical. The interface allows users to connect to geometry, build and modify their model, set up their solution, submit a solve, and review results. The solve itself is done in ANSYS Mechanical APDL. This is the original ANSYS Multiphysics program. 

When you press the solve button ANSYS Mechanical writes out commands in the languages used by ANSYS Mechanical APDL, called the ANSYS Parametric Design Language, or APDL.  Yes, that is where ANSYS Mechanical APDL got its name. We like to call it MAPDL for short. (Side note: years ago we started a campaign to call it map-dul. It didn’t work.) Once the file is written, MAPDL is started, the file is read in, the solve happens, and all of the requested output files are written. Then ANSYS Mechanical reads those files and shows results to the user.

Customization Tool 1: Command Snippets for Controlling the Solver

Not every capability that is found in ANSYS Mechanical APDL is exposed in the interface for ANSYS Mechanical.  That is not a problem because users can use the APDL language in ANSYS Mechanical to access the full capability of the solver.  These small pieces of code are called Snippets and they are added to the tree for your ANSYS Mechanical model.  When the solver file is written, ANSYS Mechanical inserts your snippets into the command stream.  Simple and elegant.

PADT has a seminar from back in 2011 that lays it all out.  You can find the PowerPoint Presentation here. We do have plans to update this webinar soon.

This approach is used when you want to access capabilities in the solver that are not supported in the interface but you want to get to those features and keep track of them from inside your ANSYS Mechanical Model.

If you are not familiar with APDL, find a more “seasoned” user to help you. Or you can teach yourself APDL programming with PADT’s Guide to APDL .

Customization Tool 2: ANSYS Customization Toolkit (ACT) for Controlling the User Interface and Accessing the Model

As mentioned above, ANSYS Mechanical is used to define the model and review results.  The ANSYS Customization Toolkit (ACT) is how users customize the user interface, automate tasks in the interface, add tools to the interface, and access the model database. This type of customization can be as simple as a new feature, presented as an app, or it can be used to create a focused tool to streamline a certain type of simulation – what we call a vertical application.

image
A Vertical Application Written in ANSYS ACT by PADT for Automating the Design of Turbine Disks

Unlike APDL, ACT does is not have its own language. It uses Python and is a collection of Application Programmer Interface (API) calls from Python. This is a very powerful toolset that increases in capability at every release.  PADT has written stand alone applications using ACT to reduce simulation time significantly. We have also written features and apps for ourselves and users that make everyday use of ANSYS Mechanical better. 

Do note that ACT is supported in most of the major ANSYS products and more capability is being added across the available programs over time, not just in ANSYS Mechanical. You can also use ACT to connect ANSYS Mechanical to in-house or 3rd party software.

Because this is a standard environment, you can share your ACT applications on the ANSYS App Store found here. Take a look and you can see what users have done with ACT across the ANSYS Product suite, including ANSYS Mechanical.   PADT has two in the library, one for adding a PID controller to your model and the other is a tool for saving your ANSYS Mechanical APDL database.

Another great aspect of ACT is that it is fully documented.  If you go to the Customization Suite documentation in the ANSYS help library you can find everything you need.

Customization Tool 3: APDL for Automating the Solve  

With Code Snippets we talked about using APDL to access solver functions from ANSYS Mechanical that were not supported in ANSYS Mechanical.  You can also use APDL to automate what is going on during the solve.  Every capability in the ANSYS solver is accessible through APDL.

The most common usage of APDL is to create a tool that solves in batch mode. APDL programs are used to carry out tasks without going back to ANSYS Mechanical.  As an example, maybe you want to solve a load step, save some information from the solve, export it, read it in to a 3rd party program, modify it, modify some property in your model, then solve the next load step. You can do all of that with APDL in batch mode.

This is not for the faint of heart, you are getting into complex programming with a custom language. But if you take the time, it can be very powerful.  All of the commands are documented in the ANSYS Mechanical APDL help and details on the language are in the ANSYS Parametric Design Language Guide.  The PADT Blog is full of articles going back over a decade on using APDL in this way.

Customization Tool 4: User Programable Features in the Solver

One of the most powerful capabilities in the ANSYS Mechanical ADPL solver is the ability for end-users to add their own subroutines.  These User Programable Features, or UPF’s, allow you to create your own elements, make custom material models, customize loads, or customize contact behavior.

There are other general purpose FEA tools on the market that heavily publicize their user elements and user materials and they try to use it to differentiate themselves from ANSYS. However, ANSYS Mechanical APDL has always had this capability.  Many universities and companies add new capability to ANSYS using this method.

To learn more about how to do create your own custom version of ANSYS, consult the Programer’s Reference in the ANSYS Help. PADT also has a webinar sharing how to make a custom material here.

Next Steps

The key to successful customization ANSYS is to know your options, understand what you really want to do, and to use the wide range of tools you have available. Everything is documented in the help and this blog has some great examples.  Start small with a simple project and work your way up.

Or, you can leverage PADT’s expertise and contract with PADT to do your customization. This is what a half-dozen companies large and small have done over the years.  We understand ANSYS, we get engineering, and we know how to program. A perfect combination.

Regardless of how you customize ANSYS Mechanical, you will find it a rewording experience.  Greater functionality and more efficient usage are only a few lines of custom code away.

Using Command Snippets in Solution (And a cool new ACT Extension to make life easier)

So you have results for a job that took several hours to run, or several days, and now you realize that you need to use a post-processing command snippet. In the past, prior to version 14.5, this would be a huge problem, because just adding the command snippet in the Solution branch would trigger a resolve. So, in those cases, we would usually just jump over to MAPDL to do the post-processing.  In version 14.5, however, ANSYS allowed you to add the snippet to the Solution branch without triggering a resolve.

When you hit “Evaluate All Results”, Mechanical will copy the files to a scratch directory and start a separate MAPDL session. This leads to a secondary problem. Often you need to select nodes or elements to use during your snippet. This is usually done with a Named Selection, or a material ID that you saved to a parameter in a Geometry command snippet.  The problem is that the Named Selections, or components in MAPDL, are not saved in the RST file, neither are parameters. They are stored in the DB file. If you thought ahead, then in the Analysis Settings, you set the ‘Save DB file’ option to ‘Yes’ before you solved. In your post-processing command snippet you could then use the RESUME command to bring the database back to the state that it was just before the solve – having all your Named Selections and parameters. But since the default is to not save the DB file, odds are that you don’t have it.  It’s okay, though. There are still some options.

The first thing I recommend is that you save the solved project, and then do a ‘Save As’ to make a copy from which to work, just in case something goes wrong.

Method 1:

When you hit the Solve button in Mechanical, it writes out a ‘ds.dat’ file that then gets run in a batch MAPDL run.

If you have all of your needed Named Selections setup prior to the Solve, then you can open an MAPDL session and use the File>Read Input From… command to read in the ds.dat file.  In interactive mode, the file stops just before the Solve command, so you can then save the database file at that point.  You then need to right-click on the Solution branch in Mechanical and hit “Open Solution Directory”, in to which you need to copy the new “file.db” file.  Then you can resume the file.db in your post-processing command snippet. 

If you need to add a new Named  Selection, you can add a new one, even in 14.5, without triggering a resolve, but then you will have to write out a new input file. To do this, highlight the Solution branch in the tree, go to Tools>Write Input File…, and then follow the procedure above.  

Method 2:

If you are using version 17.1 or later, you have another option. You can Right-click on a Name Selection and choose “Create a Nodal Named Selection”. Then right-click that new nodal named selection and hit “Export Selections to CDB File”.  You can select several Nodal Named Selections to export, and the export will all go to one file. Include that text in your snippet.

Method 3:

In R19.2, the Named Selections are now stored in the RST file. If you don’t need to add a new Named Selection, then can you access the Named Selections that were created prior to the solution run.  After a SET command in your snippet, you can just use the name in the NSEL command, as I did in the picture above, with no need to include the CMBLOCK from the CDB file.  If you need a new Named Selection, however, then you have to use Methods 1 or 2 above.

Pitfalls:

Now that all sounds somewhat difficult, and it actually gets worse. With Method 1, you have to know at least enough MAPDL to open it and read in the input file, and then save the database file.

With Method 2 and 3, the parameters are still not saved in the RST file. So if you need parameters that were created in earlier command snippets, then you have to go back to Method 1.

But there’s hope!!

Method 4:  Oh, Joy!!!

There is one other thing that you can do, and this is my favorite method. (Probably because I wrote it. J)  There is now a new free ACT extension in the ANSYS App store. It is called SAVE_DB, and was written because yours truly got tired of dealing with the other three methods above.  SAVE_DB allows you to save the MAPDL database file without having to solve the Mechanical model, or cause a resolve. SAVE_DB will automatically change the Analysis Settings > Analysis Data Management > Save MAPDL DB value to “Yes” so that future resolves are also saved. MAPDL will be run in the background on the same version as the Workbench project, and the “file.db” will be saved to the Solver Files Directory.  Now any new Named Selections that you add will be ready at the push of a button. This one:

This is the first of many helpful tools planned for a PADT_Toolkit. I will post another plug, I mean ‘blog’, when I get more tools added and the PADT_Toolkit uploaded to the APP Store.  Until then enjoy SAVE_DB!

Video: Tips and Tricks for ANSYS Mechanical Users

Over time Ziad Melham, one of PADT’s support engineers, has developed a variety of tips and tricks for ANSYS Mechanical that he shares with users when providing them with support. In this video, Ziad shares that same information with all users.

Users of ANSYS mechanical, both new and experienced, will find them helpful in making their simulation pre- and post-processing more efficient. Please enjoy and do not hesitate to share with your co-workers.

Evaluating Stresses and Forces in Threaded Fasteners with ANSYS Mechanical, Part 2

Fasteners are one of the most common and fundamental engineering components we encounter.

Proper design of fasteners is so fundamental, every Mechanical Engineer takes a University course in which the proper design of these components is covered (or at least a course in which the required textbook does so).

With recent increases in computational power and ease in creating and solving finite element models, engineers are increasingly tempted to simulate their fasteners or fastened joints in order to gain better insights into such concerns as thread stresses

In what follows, PADT’s Alex Grishin digs deeper into how to leverage ANSYS Mechanical to better model fasteners and obtain accurate results. If you did not review Part 1, do so here.

PADT-ANSYS-fastener_simulation_part2

How to Use Lattice Optimization in ANSYS Mechanical and ANSYS SpaceClaim 19.2

One of the great new features in ANSYS Mechanical 19.2 is the ability to perform a lattice optimization.  Accomplished as an option within Topology Optimization, lattice optimization allows us to generate a lattice structure within our region of interest.  It includes varying thickness of the lattice members as part of the optimization.

Lattice structures can be very beneficial because weight can be substantially reduced compared to solid parts made using traditional manufacturing methods.  Further, recent advances in additive manufacturing enable the creation of lattice structures in ways that weren’t possible with traditional manufacturing.

Here I’ll explain how to perform a lattice optimization in ANSYS 19.2 step by step.

The procedure starts the same as a normal topology optimization in ANSYS Mechanical, with an initial static structural analysis on our original part or assembly.  If you’re not familiar with the process, this earlier PADT Focus blog should be helpful:  http://www.padtinc.com/blog/the-focus/topological-optimization-in-ansys-18-1-motorcycle-component-example

For the lattice optimization, I’m starting with a part I created that acts as a corner brace:

At this early point in the simulation, the Project Schematic looks like this:

I used the Multizone mesh method to get a hex mesh on the part:

Simple loads and constraints are recommended especially if you’ll be doing a downstream validation study.  That is because the downstream simulation on the resulting lattice geometry will most likely need to operate on the FE entities rather than geometric entities for load and constraint application. The boundary conditions in this simple model consisted of a fixed support on one side of the brace and a force load on the other side:

After solving, I reviewed the displacement as well as the stress results:

Satisfied with the results, the next step is to add a Topology Optimization block in the Project Schematic. The easiest way to do this is to right click on the Solution cell, then select Transfer Data to New > Topology Optimization:

You may need to re-solve the static structural simulation at this point.  You’ll know if you have yellow thunderbolts in the Project Schematic instead of green checkmarks for the Static Structural analysis. 

At this point, the Project Schematic now looks like this:

The Mechanical window now has the Topology Optimization branch added:

The change to make to enable a lattice optimization is accomplished in the details view of the Optimization Region branch:

We then need to specify some settings for the lattice.  The first of these is the Lattice Type.  The various types are documented in the ANSYS 19.2 Help.  In my example I selected the Crossed option.

The other properties to define are:

  • Minimum Density (to avoid lattice structures that are toothin.  Allowed bounds are 0 and 1)
  • Maximum Density (elements are considered full/solid fordensities higher than this value, allowed bounds are 0 and 1)
  • Lattice Cell Size (used in downstream geometry steps andadditive manufacturing)

Values I used in my example are shown here:

Assuming no other options need to be set, we solve the lattice optimization and review the results.  The results are displayed as a contour plot with values between zero and one, with values corresponding to the density settings as specified above.

Note that at this stage we don’t actually visualize the lattice structure – just a contour plot of where the lattice can be in the structure.  Where density values are higher than the maximum density specified, the geometry will end up being solid.  The lattice structure can exist where the results are between the minimum and maximum density values specified, with a varying thickness of lattice members corresponding to higher and lower densities.

The next step is to bring the lattice density information into SpaceClaim and generate actual lattice geometry.  This is done by adding a free standing Geometry block in the Workbench Project Schematic.

The next step is to drag and drop the Results cell from the Topology Optimization block onto the Geometry cell of the new free standing Geometry block:

The Project Schematic will now look like this:

Notice the Results cell in the Topology Optimization branch now has a yellow lightning bolt.  The next step is to right click on that Results cell and Update.  The Project Schematic will now look like this:

Before we can open SpaceClaim, we next need to right click on the Geometry cell in the downstream Geometry block and Update that as well:

After both Updates, the Project Schematic will now look like this:

The next step is to double click or right click on the now-updated Geometry cell to open SpaceClaim.  Note that both the original geometry and a faceted version of the geometry will exist in SpaceClaim:

It may seem counter intuitive, but we actually suppress the faceted geometry and only work with the original, solid geometry for the faceted process.  The faceted geometry should be automatically suppressed, as shown by the null symbol, ø, in the SpaceClaim tree.  At this point it will be helpful to hide the faceted geometry by unchecking its box in the tree:

Next we’ll utilize some capability in the Facets menu in SpaceClaim to create the lattice geometry, using the lattice distribution calculated by the lattice optimization.  Click on the Facets tab, then click on the Shell button:

Set the Infill option to be Basic:

At this point there should be a check box for “Use Density Attributes” below the word Shape.  This check box doesn’t always appear.  If it’s not there, first try clicking on the actual geometry object in the tree:

In one instance I had to go to %appdata%\Ansys and rename the v192 folder to v192.old to reset Workbench preferences and launch Workbench again.  That may have been ‘pilot error’ on my part as I was learning the process.

The next step is to check the Use density attributes box.  The Shape dropdown should be set to Lattices.  Once the Use density attributes box is checked, we can then one of the predefined lattice shapes, which will be used for downstream simulation and 3D printing.  The shape picked needs to match the lattice shape previously picked in the topology optimization.

In my case I selected the Cube Lattice with Side Diagonal Supports, which corresponds to the Crossed selection I made in the upsteam lattice optimization.  Note that a planar preview of this is displayed inside the geometry:

The next step is to click the green checkmark to have SpaceClaim create the lattice geometry based on the lattice distribution calculated by the lattice optimization:

When SpaceClaim is done with the lattice geometry generation, you should be able to see a ghosted image showing the lattice structure in the part’s interior:

Note that if you change views, etc., in SpaceClaim, you may then see the exterior surfaces of the part, but rest assured the lattice structure remains in the interior.

Your next step may need to be a validation.  To do this, we create a standalone Static Structural analysis block on the Project Schematic:

Next we drag and drop the Geometry cell from the faceted geometry block we just created onto the Geometry cell of the newly created Static Structural block:

We can now open Mechanical for the new Static Structural analysis.  Note that the geometry that comes into Mechanical in this manner will have a single face for the exterior, and a single face for the exterior. To verify that the lattice structure is actually in the geometry, I recommend creating a section plane so we can view the interior of the geometry:

To mesh the lattice structure, I’ve found that inserting a Mesh Method and setting it to the Tetrahedrons/Patch Independent option has worked for getting a reasonable mesh.  Care must be taken with element sizes or a very large mesh will be created.  My example mesh has about 500,000 nodes.  This is a section view, showing the mesh of the interior lattice structure (relatively coarse for the example).

For boundary condition application, I used Direct FE loads.  I used a lasso pick after aligned the view properly to select the nodes needed for the displacement and then the force loads, and created Named Selections for each of those nodal selections for easy load application.

Here are a couple of results plots showing a section view with the lattice in the interior (deflection followed by max principal stress):

Here is a variant on the lattice specifications, in which the variance in the thickness of the lattice members (a result of the optimization) is more evident:

Clearly, a lot more could be done with the geometry in SpaceClaim before a validation step or 3D printing.  However, hopefully this step by step guide is helpful with the basic process for performing a lattice optimization in ANSYS Mechanical and SpaceClaim 19.2.

Evaluating Stresses and Forces in Threaded Fasteners with ANSYS Mechanical

Fasteners are one of the most common and fundamental engineering components we encounter.
Proper design of fasteners is so fundamental, every Mechanical Engineer takes a University course in which the proper design of these components is covered (or at least a course in which the required textbook does so).

With recent increases in computational power and ease in creating and solving finite element models, engineers are increasingly tempted to simulate their fasteners or fastened joints in order to gain better insights into such concerns as thread stresses

In what follows, PADT’s Alex Grishin demonstrates a basic procedure for doing so, assess the cost/benefits of doing so, and to lay the groundwork for some further explorations in Part 2, which can now be found here.

PADT-ANSYS-Fastener_Simulation_Part1

Eigenvalue Buckling and Post-buckling Analysis in ANSYS Mechanical

As often happens, I learned something new from one of my latest tech support cases. I’ll start with the basics and then get to what I learned. The question in this case was, “Can I use the mode shape as a starting position for an Eigenvalue Buckling?” My first thought was, “Sure, why not,” with the idea being that the load factor would be lower if the geometry was already perturbed in that shape. Boy was I wrong.

Let’s start with the basic procedure for Eigenvalue buckling and a post-buckling analysis in ANSYS. You start with a Static Structural analysis, in this case, a simple thin column, fixed at the bottom with a 10 lbf downward force on top. Then you drag an Eigenvalue Buckling system for the toolbox, and place it on the Solution cell of the Static Structural system. After setting the number of buckling modes to search for, ANSYS calculates the Load Multiplier for each mode. If you applied the real load in the Static Structural system, then the Load Multiplier is the factor of safety with that load. If you put a dummy load, like 10lbf, then the total load that will cause buckling is F*Load Factor (l).

For post-buckling analysis, ANSYS 17.0 or later lets you take the mode shape from a linear Eigenvalue Buckling analysis and feed it to another Static Structural analysis Model cell as the initial geometry. We use to have to do this with the UPCOORD command in MAPDL. Now you just drag the Solution cell of the Eigenvalue Buckling analysis on to the Model cell of a stand-alone Static Structural system. Also connect the Engineering Data cells.

The key is to look at the Properties window of the Solution cell of the buckling analysis. In the above picture, that is cell B6. (Right-click and hit Properties if needed.) This lets you choose the mode shape and the scaling factor for the new shape going into the structural analysis. Generally it will be Mode 1.

You can then apply the same BCs in the second structural analysis, but make the force be the buckling load of F*Load Factor (l), where F is your load applied in the buckling analysis. Make sure that Large Deflection is turned on in the second structural analysis. This will give you the deflection caused by the load just as buckling sets in. Increasing the load after that will cause the post-buckling deflections.

 

In this case, F is 10 lb, and load factor for the first mode (l) is 23.871, so the load at load step 1 is 238.71 lb, and load step 2 is 300 lb. You can see how there is very little deflection, even of the perturbed shape, up to the buckling load at load step 1. After that, the deflection takes off.

So what did I learn from this? Well there were two things.

First, doing another Eigen Value Buckling analysis with the perturbed shape, if perturbed in buckling mode shape 1, returns the same answers. Even though the shape is perturbed, as the post-buckling structural analysis shows, nothing really happens until you get to that first buckling load, which is already for mode 1. If the model is perturbed just slightly, then you have guaranteed that it will buckle to one side versus the other, but it will still buckle at the same load, and shape, for mode 1. If you increase the scale factor of the perturbed shape, then eventually the buckling analysis starts to get higher results, because the buckling shape is now finding a different mode than the original.

The second thing that I learned, or that I should have remembered from my structures and dynamics classes, a few <cough>23<cough> years ago, was that buckling mode shapes are different than dynamic mode shapes from a modal analysis with the same boundary conditions. As shown in this GIF, the Modal mode shape is a bit flatter than the buckling mode shape.

After making sure that my perturbed distances were the same, the scale factor on the modal analysis was quite a bit smaller, 2.97e-7 compared to .0001 for the Eigenvalue scale factor. With the top of the column perturbed the same amount, the results of the three Eigenvalue Buckling systems are compiled below.

So, now you know that there is no need to do a second Eigenvalue buckling, and hopefully I have at least shown you that it is much easier to do your post-buckling analysis in ANSYS Workbench than it used to be. Now I just have to get back to writing that procrastination article. Have a great day!

Using ANSYS HPC or ANSYS HPC Pack Licenses in ANSYS Electronics Desktop (Maxwell or HFSS)

Taking advantage of HPC can dramatically speed up solutions for electronics simulations.  Depending on whether you have ANSYS HPC licenses or ANSYS HPC Pack licenses, a different setting needs to be made in the HPC options, as shown here.

In Electronics Desktop, we click Tools > Options > HPC and Analysis Options:

For ANSYS HPC licenses, we set the option to “Pool”.

For ANSYS HPC Pack licenses, we set the option to “Pack”.

With ANSYS HPC licenses, each license task enables an additional core for solving.  At release 19, 4 cores are enabled with standard licensing, so adding 8 ANSYS HPC tasks enables solving on 12 cores.  With HPC Pack licenses, the first task enables an additional 8 cores, while a second task enables 8×4 or an additional 32 cores, etc.  For more information, see the ANSYS documentation on HPC licensing.

World View talks about ANSYS usage on design of their Stratospheric Balloon Vehicles

We were pleased to see that PADT customer and ANSYS power users World View Enterprises were featured in the latest issue of ANSYS Advantage Magazine.

This is such a cool application of technology and a great example of ANSYS usage.  You need to read the article, but to entice you a bit:

They are using high-altitude balloons to launch what they call Stratollites, instead of satellites.  They can lift large payloads up to 95,000 and leave them up for weeks or months. As you can imagine, the loads a vehicle like that sees are extreme, and weight is at a premium.  A perfect application for ANSYS.

Read the article here.

If you have any questions about the application or want to know more about how you can use ANSYS products to get similar schedule, cost, weight, and performance gains for your products, please contact us.

Can ANSYS Mechanical Handle My Required Modeling Precision?

Sometimes you need to use ANSYS Mechanical to model a big part as a way to determine a very small deflection.  The most common situation where this happens is optics. A lens that is around a meter in diameter may have nanometer distortions from mechanical or thermal loads that impact the optics. A customer asked if ANSYS Mechanical can handle that.  Please find Alex’s interesting and in-depth response in the attached presentation.   There is theory that explains the situation, then an example of how to determine if you can get the information you need, followed by advice on how to view the results.

PADT-ANSYS-Mechanical-Modeling-Precision

 

10 Great New Features in ANSYS Mechanical 19.0 and 19.1

ANSYS Mechanical version 19.0 has been available since late January 2018, while version 19.1 was released in May. If you haven’t had a chance to check them out, we thought it would be helpful to list what we see as 10 of the top newest features. We’ll start with five new features from version 19.0 and will then round it out with five from version 19.1.

ANSYS Mechanical 19.0

1. 4 Cores HPC Solving with No Additional Licensing

Previously, you were limited to solving on 2 cores at a maximum without having additional ANSYS HPC or HPC Pack licenses. That limit has been raised to 4 cores at 19.0.
To utilize the cores while solving, from the Solution branch in Mechanical click on the Tools menu, then Solve Process Settings. Click the Advanced button. Set the Max number of utilized cores to 4 and click OK.

2. Topology Optimization Includes Inertial Loads

Topology optimization became a native option in ANSYS Mechanical in version 18.0. Topology optimization allows us to perform studies in which we preserve stiffness while reducing weight, for example. Since inertia loads are now supported in a topology optimization, one type of problem we can now solve is starting with geometry that has a mix of an inertial load (gravity in the downward direction) along with additional loading such as forces or pressures.

Solving the topology optimization and moving to the verification step we can see the optimization results (shape and contour results plot) for the combined loading.

The ability to include inertia loads adds quite a few more problems that can be considered for topology optimization.

3. Small Sliding Contact

The idea here is that if we have confidence that the contact and target elements within a contact region will not slide very much, we can turn on the small sliding assumption. This speeds up the computations because less checking is needed for the contact elements during the solution. It’s activated in the Details view for one or more contact regions. We’ve seen some marginal improvements in solution times for a couple of test models. It’s clearly worth trying this if it applies to your simulations.

4. Element Birth and Death

We now no longer have to use APDL command objects to incorporate element birth and death. If you’re not familiar with what this is, it’s the ability to selectively deactivate and/or activate portions of the finite element model to simulate forming operations, assembly, etc. Further, the implementation is fantastic in that unlike with the old MAPDL implementation, we no longer have to manually keep track of which elements have been ‘killed’ or made ‘alive’. The postprocessing in Mechanical 19.0 automatically displays only elements that are alive for a given results set.
Here is how it is implemented in the Mechanical tree, under the analysis type branch:

The entities to be killed or made alive can be selected by geometry or Named Selections. There is a handy table that shows the alive or dead status for each Element Birth and Death object once they are setup:

This animation shows a temperature results plot and demonstrates how the killed elements are made alive and automatically displayed when postprocessing:

5. Clipboard Tool

This new menu pick gives us an improved method for tasks such as selecting multiple faces. Rather than having to carefully pick all of them at once or use a combination of named selections, we can now simply select the faces that are easy to pick, add them to the clipboard, rotate the model, select more faces now that they are in view, etc.

Once all the desired faces are in the Clipboard, we simply use the Select Items in Clipboard dropdown and we can now assign a load or mesh control, etc. to the desired faces.

Note there are convenient hot keys for Adding to, Removing from, and Clearing the clipboard, shown in the screen captures of the menu dropdowns above.

ANSYS Mechanical 19.1

6. Granta Design Sample Materials

Version 19.1 adds a whole new set of sample materials from Granta. To access them, open up Engineering Data, click on the Engineering Data Sources button, and then click on the Granta Design Sample Materials button. This adds a lot more sample materials than have been available in Engineering Data previously.

7. Materials folder in Mechanical

You’ll see a new branch in the tree in Mechanical 19.1: Materials. All materials that are part of your Engineering Data set will show up in this branch. For each material defined, we can click on the Material Assignment button or right click as shown here:

One the new Assignment branch is created for a material, we can then select the bodies for which that material should be assigned. Each material has its own color which can be changed in Engineering Data if so desired.

Important note for Mechanical APDL command users: Assigning material properties using the Materials branch results in all parts with the same material property having the same MAPDL material number. This is different from prior behavior in Mechanical in which each part in the geometry tree had its own material number identified with the ‘magic’ parameter name matid. Parameter matid now no longer is unique for each part if materials area assigned using the Materials branch. There is a new ‘magic’ parameter named typeids which identifies the element type number for each part in the tree. This new parameter is actually a 1x1x1 array parameter rather than a scalar parameter, so to make use of it in a command snippet we need to add the dimension (1) to the parameter name, like this:

thtest1=typeids(1)

or

et,typeids(1),solid65

8. Result Tracking During Solution

A new, useful capability is to be able to view a result item on a body, while the solution is running. You can now insert certain results items under Solution Information and view the status of the results while the solution is progressing. If birth and death is employed it will even display just the elements that are alive as the solution progresses. Here is an example of a temperature plot on a body while a transient solution is in progress:

9. Save Animations to .wmv and .mp4 Formats

We now have two new options besides the old .avi format for exporting animation files. The .mp4 and .wmv formats both tend to produce smaller files than .avi format. When you click on the Export Video File button the new options are available in the dropdown:

10. Solution Statistics Page

Finally, there is a new Solution Statistics page, available under Solution Information when a solution has completed. This is a quick and easy way to view performance information from your solution and helps determine if more cores or more RAM could be beneficial in future solutions of the same model. Here is an example:

Conclusions

These are just a few of the enhancements that have been implemented in versions 19.0 and 19.1. These should help you be more productive with your solutions in ANSYS Mechanical as well as increase your capacity for simulating reality, and creating new geometry when it comes to topology optimization.