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!

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.

Press Release: On-Demand High Performance Cloud Computing for Today’s Most Demanding Workflows Offered by PADT in Partnership with Nimbix

Sometimes if you look hard enough, you find what you need.  Ever since people started talking about running large simulation models in the “cloud” our engineers here at PADT have been looking for a good solution. We even offered our own service, and although it was fast and easy to use, we could not make it big enough. Then along comes Nimbix. And they nailed it.

First we asked, are they running on real HPC hardware, not souped up web servers with virtual machines on them? Yes. We found bare metal hardware striped down to fighting weight that is optimized for running simulation.

Then we asked, Is it easy to use or do I have to jump through hoops to just get a job running?  Indeed it was easy and powerful. We just wanted to submit jobs and found that the JARVICE™ interface does so much more to configure, setup, submit, and monitor even the most complex parallel solves.

OK, this looked good, but the real test is do we have access to whole machines or is this just a timesharing system with a great interface?  Turns out it is not.  It is true cloud-based high-performance computing.

We think we found what we were looking for, but we have been burned before.  So we did what any simulation engineer would do, we pounded on it with massive ANSYS FLUENT, Mechanical, and HFSS runs.  We knew it was real when we were monitoring a CFD run on a mobile phone from a coffee shop in-between customer visits.

We liked it so much that we asked if we could partner with them to offer it to our customers. And that is where we are today with this press release.

PADT is proud to announce that we are able to provide our customers with on-demand HPC resources that are fast, easy to use, and cost-effective.  If you are a simulation user who needs to run large jobs, access surge capacity, or just solve faster, Nimbix is the answer. And PADT is here to help determine the right configuration and guide you through the process.

Please read the press release below for more details on what we are doing.

This video explains Nimbix well:

You can also learn more about our experience by watching a free webinar we recorded where we shared our experience using this service: www.brighttalk.com/webcast/15747/330189

Please find the official press release on this new partnership below and here in PDF and HTML

If you have any questions about high-performance computing for simulation, either with local hardware or compute resources in the cloud, reach out to info@padtinc.com or call 480.813.4884.

Press Release:

On-Demand High Performance Cloud Computing for Today’s
Most Demanding Workflows Offered by PADT in Partnership with Nimbix

Nimbix Cloud Provides Access to ANSYS Applications Through Cloud Supercomputing, Removing the Requirement of Expensive Infrastructure and Hardware

TEMPE, Ariz., July 26, 2018 ─ Understanding the need for easy, affordable and reliable access to supercomputing capabilities, PADT has partnered with Nimbix to provide High-Performance Computing (HPC) in the cloud. The Nimbix Cloud is the industry’s first true Software-as-a-Service (SaaS) supercomputing cloud and will provide PADT’s customers with on-demand, mobile access to more than 15 ANSYS applications without needing expensive hardware and complex infrastructure to support it. Current ANSYS applications available with Nimbix are listed here.

“As long-time simulation users, PADT has always wanted to leverage the cloud for running ANSYS models, but no one could support it before Nimbix,” said Bob Calvin, manager, Simulation Solutions, PADT. “The Nimbix Cloud gives our customers a flexible way to run large models from anywhere and accommodate surge capacity when it is needed.”

The Nimbix Cloud is powered by the JARVICE™ platform, which Nimbix purpose-built from the ground-up to accommodate the most demanding workflows by providing superior performance, capabilities, and ease of use. PADT customers can manage start-up, execution, completion and notifications on full-featured ANSYS applications in the cloud, and send their data from any device including desktop, tablet and smartphones.

“With its global recognition as a provider of numerical simulation and product development, PADT is the ideal partner to leverage the JARVICE platform internally and as an offering to its customers,” said Chuck Kelly, senior vice president, Sales, Nimbix. “Nimbix high-performance computing in the cloud provides a competitive advantage by allowing users to more easily solve complex design problems and then send the data anywhere to turn results into actionable insights.”

“We use Nimbix frequently at PADT because of its reliability and performance when running ANSYS software in the cloud,” said Manoj Mahendran, lead application engineer, PADT. “The platform has allowed us to easily check and submit simulation test results off-site and on-the-go, providing more flexibility to our simulation teams.”

Nimbix Cloud is available today, and PADT invites customers to learn more about the challenges, tools, and mindset needed to run simulation in the cloud, and how the Nimbix platform can be an effective solution, in a webinar on August 8, 2018. To register for the webinar, please visit https://www.brighttalk.com/webcast/15747/330189.

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.

# # #

Media Contact
Alec Robertson
TechTHiNQ on behalf of PADT
585-281-6399
alec.robertson@techthinq.com
PADT Contact
Eric Miller
PADT, Inc.
Principal & Co-Owner
480.813.4884
eric.miller@padtinc.com

 

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

 

Updates and Enhancements in ANSYS Mechanical 19.1 – Webinar

Don’t miss this informative presentation – Secure your spot today!
Register Here

If this is your first time registering for one of our Bright Talk webinars, simply click the link and fill out the attached form. We promise that the information you provide will only be shared with those promoting the event (PADT).

You will only have to do this once! For all future webinars, you can simply click the link, add the reminder to your calendar and you’re good to go!

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.

Extracting Relative Displacements in ANSYS Mechanical

A recurring theme in ANSYS Technical Support queries involves the separation of rigid-body from material deformations without performing an additional analysis. Many users simply assume this capability should exist as a simple post-processing query(or that in any case, this shouldn’t be a difficult operation). “Rigid-Body” displacements implies a transient dynamic analysis (as such displacements should not occur in static analyses), but as we’ll see, there are contexts within static structural environments where this concept DOES play an important engineering role. In static structural contexts, such rigid-body motion implies motion transmitted across multiple-bodies. There are two important and loosely related contexts we’ll look at; zero strain rotations of the CG and those rotations combined with strain-based displacement.

The following presentation explains the issues including the math behind it, offers solutions including useful APDL marcros, and then gives examples.

The models and macros used are in this zip file: PADT-ANSYS-Extract-Dsp-Files

PADT-ANSYS-Mechanical-Extracting-Relative-Displacements-20180404

You can also download the PDF here.

Find this interesting? This is just a small sample of PADT deep and practical understand of the entire ANSYS Suite of products.  Please consider us for your training, mentoring, and outsourced simulation services needs.

Save, Save, Save! Setting up a Save after Solution in ANSYS Mechanical

NOOOOOOOOOOOOOOOOOOOOOOOOOOOO!!!!

Is this the reaction you have when you come in on Monday morning, and realize that another Windows update has, once again, rebooted your PC before you had a chance to save the 30-hour run that should have finished over the weekend? There a Workbench setting that can help relieve some of that stress.

The “Save Project After Solution” option will save the entire project as soon as the solution has finished. So when your model runs for 30 hours over the weekend, it gets saved before a Windows update shuts everything down.  These settings are persistent, so once you’ve changed them to ‘Yes’, then you are all set for next time. You just need to make sure that you change them for each ANSYS version if you have more than one installed.

Now on to my next blog… “How to recover a run if you forgot to change the settings above.” (Grumble Grumble!)

Estimating Structural Response to Random Vibration in ANSYS Mechanical: Reaction Forces

One of the key outputs from any random vibration analysis is determining the response of the object you are analyzing in terms of reaction forces.  In the presentation below. Alex Grishin shares the theory behind getting accurate forces and then how to do so in ANSYS Mechanical.

PADT-ANSYS-Random-Vib-Reaction-Forces-2017_11_22-1

As always, please contact PADT for your ANSYS simulation, training, and customization needs.

 

 

Using External Data in ANSYS Mechanical to Tabular Loads with Multiple Variables, Part 2

ANSYS Mechanical is great at applying tabular loads that vary with an independent variable. Say time or Z.  What if you want a tabular load that varies in multiple directions and time. In part one of this series, I covered who you can use the External Data tool to do just that. In this second part, I show how you can alternatively use APDL commands added to your ANSYS Mechanical model to define the tabular loading.

PADT-ANSYS-Tabular-loads-2