Posted on May 22, 2019, by: Eric Miller
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.
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.
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.
Posted on March 12, 2019, by: Joe Woodward
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.
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.
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.
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.
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!
Posted on February 5, 2019, by: Ziad Melhem
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.
Posted on January 28, 2019, by: Alex Grishin
Fasteners are one of the most common and fundamental engineering components we encounter
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.
Posted on December 4, 2018, by: Ted Harris
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.
Posted on September 26, 2018, by: Alex GrishinFasteners 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
Posted on September 10, 2018, by: Joe WoodwardAs 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!
Posted on August 3, 2018, by: Ted HarrisTaking 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 8x4 or an additional 32 cores, etc. For more information, see the ANSYS documentation on HPC licensing.
Posted on July 27, 2018, by: Eric MillerWe 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.
Posted on July 16, 2018, by: Alex GrishinSometimes 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
Posted on June 5, 2018, by: Ted HarrisANSYS 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 LicensingPreviously, 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 ContactThe 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 DeathWe 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: https://youtu.be/62rPclA2Ak0
5. Clipboard ToolThis 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 MaterialsVersion 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 MechanicalYou’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 SolutionA 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 FormatsWe 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 PageFinally, 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:
ConclusionsThese 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.
Posted on April 25, 2018, by: Eric MillerThe use of FEA and CFD techniques to simulate the behavior of structures, fluids, and electromagnetic fields has gone from an occasional task done by experts to a standard method for driving product development. The webinar below is a presentation by PADT's Co-Owner and Principal, Eric Miller discussing recent advances in simulation that are pushing the technology towards covering more phenomenon, faster run times, and greater accuracy. From up-front real-time stress and fluid flow to massive combustion models with chemistry, fluid flow, thermals, and turbulence; simulation is how products are designed. The talk covers:
- What is Simulation and How did we Get Where we are
- Five Current Technology Trends in Simulation
- Business Trends to be Aware Of
- What Is Next?
- How to Keep Up
Posted on April 24, 2018, by: Ziad MelhemWere you so excited to jump on your analysis only to have a “server is down or not responsive” message pop out and alienate you from the fun like a prestigiously exclusive club would make their patrons wait at the door? It might have been your manager running a reverse psychology trick on you or maybe not. If it is the latter, you are not alone. As a matter of fact, licensing questions come to us on a regular basis. And even though there are plenty of information on the web, we figured it would be beneficial to have the most frequent answers gathered into one place: an FAQ document (attached on this blog). The Table of Contents includes the following topics:
Download the PDF here. The document was written with the assumption of the reader having no prior experience with ANSYS or licensing in general. It is formatted in an easy step by step format with photos. The table of contents has hyperlinks embedded in it and can be used to easily navigate to the relevant sections. We do hope that this document will bring value in solving your licensing issues, and we are always here to help if it doesn’t:
1-800-293-PADT or 480-813-4884
Posted on April 4, 2018, by: Alex GrishinA 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.