Posted on December 4, 2018, by: Ted HarrisOne 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 stick with the default Cubic option. The other properties to define are:
- Minimum Density (to avoid lattice structures that are too thin. Allowed bounds are 0 and 1)
- Maximum Density (elements are considered full/solid for densities higher than this value, allowed bounds are 0 and 1)
- Lattice Cell Size (used in downstream geometry steps and additive manufacturing)
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. 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
If you would like to learn more, especially how simulation can drive your company's product development, please contact PADT.
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.
Press Release: New Expansion into Texas Grows PADT’s ANSYS Sales & Support Across the Entire Southwest
Posted on February 6, 2018, by: Eric MillerWhen people look at PADT and where we are located, they almost always say "You should open an office in Austin, the tech community there is a perfect fit for your skills and culture." We finally listened and are proud to announce that our newest location is in Austin Texas. This new office will be initially focused on ANSYS Sales and Support across the great state of Texas. We have had customers for other products and services in the state for decades and are pleased to have a permanent local presence now. As an Elite ANSYS Channel partner, we provide sales of the complete ANSYS product suite to any and all entities that can benefit from the application of numerical simulation. Across industries, we bring a unique technical approach to both sales and support that is focused on identifying need and then selecting the right toolset, training, and support to deliver a return on the customer's investment as soon as possible. And the initial product purchase is just the start. Our ANSYS customers are our partners that we grow with, always ready to help them be better at whatever it is what they do. Customers in Southern California, Nevada, Arizona, Utah, New Mexico, and Colorado already know this, and it is time for the engineering community in Texas to benefit from the experience. Because we will be there for the long term, we are taking our time to look around the area. Our new salesperson, Ian Scott, is an Austin native and who has worked in the engineering software space for some time. He will be working with existing customers and partners in the area to find the right location for us long-term. But we are already putting plans in place to deliver outstanding training, hold meetings, and maybe even a celebration or two while we settle in. Over time we will add local engineers and additional sales staff to meet the needs of the state, which as you know is big. And we have big plans for PADT and Texas starting with this ANSYS Sales and Support role, it is just the beginning. Make sure you watch this blog, social media, or our newsletter for announcements on a celebration for our new office as well as technical events we will start holding very soon. We look forward to reconnecting with old friends and making new ones. If you are in Texas, please reach out to us and send us any suggestions or recommendations you may have. We are really looking forward to growing in Austin and across the Lone Star State. Please find the official press release on this expansion below as well as versions in PDF and HTML.
Posted on January 25, 2018, by: Joe WoodwardAs it so often does, another blog article idea came from a tech support question that I received the other day. “How do you view edge directions in ANSYS SpaceClaim?” You can do it in Mechanical, on the Edge Graphics Options Toolbar: This will turn on arrows so that you can see the edge directions. The directions of the edges or curves affects things like mesh biasing factors and mass flow rate boundary conditions. You need to make sure that all your pipes in a thermal analysis, for instance, are flowing in the same direction. (I have also had three tech support calls about weird spikes showing up in customers’ geometry. The Display Edge Direction is also how you turn those off.) In ANSYS SpaceClaim, there is no way to just display the edge directions. The directions are controlled by which point you pick first while sketching, so if you are careful, you can make sure they are all consistent. But that doesn’t help when you read in CAD files. So I thought I would share with you what I found, after a little bit of digging and playing. I discovered that the Move Tool behaves in a very specific way, a way that we can use for our need. When you pick on the edge of a surface or solid, or even a straight sketched line, the red arrow of the Move Tool will point in the direction of the curve. These directions match what gets shown in Mechanical. For splines, it’s a little bit different. If you just pick a spline with the Move Tool, the triad will align with the global coordinate system. To see the spline direction, you first have to hover over the spline, to show the vertices of the spline. Then you can pick an interior vertex, and the Blue arrow of the Move Tool will follow the spline direction. This only works at the interior vertices, and not at the ends. At the ends, the Blue tool arrow will always point outward from the spline endpoints, so you won’t really know which is the correct spline direction. I have also found that this technique does not work on sketched circles or arc because the tool always anchors to the center of the curve, and not to the curve itself. You can, however, use the Repair>Fit Curves tool to convert arcs to splines, using only the Spline option. Then the Move tool will show those directions as described above. For circles, you have to make one more step, and first, use the Split tool to split the circle into two arcs. All that though is, in my opinion, more work than it’s worth. I hope this helps make your lives just a little easier. Have a great day.
Posted on January 24, 2018, by: Ahmed FayedPart of the PADT core Philosophy is to “Provide flexible solutions of higher quality in less time for less money”. This part of the philosophy also applies to how we design and build PADT’s internal structure, tools we use, and processes we adopt. Among the growing pains of most engineering and simulation organizations is the constant growing demand for storage capacity, data management, and protection, and BOATLOADS of computing power. Sadly, PADT engineers have yet to develop a near infinite storage capacity (like DNA for storage) or a working quantum computer that can run ANSYS. So we’re in the same boat with everyone else. We have been exploring what are our major pains and what optimizations can be made to our simulation environment (about 2,000 cores of Cube Simulation Cluster Appliances) as well as a structured, controlled solution for engineering data management. As always we started by looking inwards:
- What skills are available, or learnable within PADT that can help address the need?
- What tools & resources do we have access to?
- What do we need to acquire or buy?
Interactive and batch submission to high-performance computing resourcesFor PADT, a very practical feature of EKM is the ability to easily interface to existing High-Performance Computing (HPC) infrastructure. By communicating through ANSYS Remote Solve Manager (RSM), EKM is able to effortlessly interface to most HPC schedulers and resource managers for both the Windows and Linux worlds. This feature is huge because analysts can seamlessly upload their models into the secure EKM repository, submit the jobs to the HPC cluster/s, monitor their runs, and upload their choice of results directly into EKM for review and post-processing. EKM works hard to keep the interface familiar to flatten the learning curve and keep things simple by making the batch submission menus as close as possible to the local ones. At PADT, whenever we are debugging models or application behavior, we want to have an interactive session to have the most control and visibility of the environment. With EKM, we can utilize the remote visualization & acceleration tool Nice – DCV. DCV is launched from within EKM and provides access to an interactive desktop on a cluster target while also accelerating OpenGL graphics for visually intensive programs.
Storage and archiving of simulation data with built-in version control, data aging, and expiry.ANSYS EKM provides a comprehensive data management toolset that is derived from real-world needs. Features like highly granular access control, file and folder sharing and collaboration, version control, check-out and check-in procedures, and many more are enabled and very powerful out of the box. Other more advanced features such as data aging, auto-archiving, auto unpacking option for zip files are also very useful. The capabilities don’t end here as EKM integrates directly with ANSYS Workbench. Analysts can seamlessly access their EKM repository from Workbench to perform any modifications and directly save back to EKM without the need to switch applications. Check-outs are automatically checked back in and new version numbers can be created automatically as well.
Metadata extractionAn extremely powerful piece of EKM is the metadata extraction engine that is baked into the core. EKM stores files as two entries, original file, and file metadata. EKM goes beyond the basic filename, date, owner metadata and digs deeper. It digs into the CAE meaningful metadata of the model, setup, material properties, element counts, mesh type and so on. It also extracts snapshots of the geometry, contours and in some cases even provides a 3d model that can be directly manipulated by the user. A sample of an ANSYS Fluent case metadata is below. Another feature of metadata extraction is the ability to take a quick look at simulation results, perform cutplanes, pan, tilt, and zoom as well as add comments and even capture and share snapshots without leaving the browser window. Metadata extraction is supported for ANSYS data types and the ability to define new data types is straightforward and easy to do for any other CAE data types or in-house codes.
A rich search capability that goes beyond filename, owner and timestamps.How many times have I kicked myself for not using meaningful file names with versions and useful time stamps and ended up spending hours opening a file for a quick peek to find that it isn’t the file I am looking for? Too many. CAE models have hundreds of variables and parameters that are embedded in them. Wouldn’t it be useful if someone came up with a system to store CAE models where an analyst can simply type a search variable and it would search not only name and timestamps but actually dig into the guts of the model and search those? Well EKM is one such system. Analysts can search using thousands of field combinations that encompass everything from material properties to partitioning methods, boundary conditions to cell counts, you get the idea, it's pretty awesome!
Simulation process and workflow managementIn EKM, administrators can create simulation workflows and lifecycles that manage all of the different steps that go into creating, running and concluding a simulation while ensuring that proper reviews and approvals handled. In addition, documenting and automating the workflows, some of the underlying work can be automated as well. As we will see later, batch submission is baked right into the EKM capabilities and workflows can automatically launch batch submission scripts to a cluster and get the simulation going as soon as the proper files are loaded and that stage in the process is released. Workflow processes are defined in a simple XML format or created using a dedicated mini-tool and uploaded into EKM ready to roll. Email notifications are preset and will shoot out whenever progress is made on a step in the workflow or an approval is needed. A nifty process chart is also built into the EKM processes interface that shows the workflow structure and current progress.
ConclusionIn conclusion, ANSYS EKM is awesome! (Serious now), PADT invested a lot of time and resources in implementing EKM and in the coming months, we will be transitioning all of our engineering knowledge into it. It is already integrated with our HPC cluster and will be our central repository for engineering data. In this article, I tried to really skim the surface of what EKM can do and what it currently does for us here at PADT. If you are interested in checking out ANSYS EKM or have any questions or thoughts please reach out to us with a comment, email or just give us a call.
Spectre Side-Channel and Meltdown – How will living in this new reality affect the world of numerical simulation?
Posted on January 17, 2018, by: David MastelLiterally, while I was sorting and running benchmarks and prepping the new benchmarks data originally titled. ANSYS Release 18.2 Ball Grid Array Benchmark information using two sixteen core INTEL® XEON® Gold 6130 CPU's. I noticed that my news feeds had started to blow up with late breaking HPC news. The news as you may have guessed is the Spectre and Meltdown flaws that were recently published. I thought to myself “Well this is just great the benchmarks that I just ran are no longer relevant. My next thought was wait now I can show a real world example of exactly a percentage change. I have waited this long to run the ANSYS numerical simulation benchmarks on this new CPU architecture. I can wait a little longer to post my findings.” What now? Oh my more Late Breaking News! Research findings, Execution orders no barriers! Side channels used to get access to private address areas of the hardware! Wow this is a bad day. As I sat reading more news, then I drifted off daydreaming, then back to my screen then the clock on the wall, great it is 2am already!, just go home..." Then thoughts immediate shifted and I was back thinking about indeed, how these hardware flaws impact the missing middle market? HPC numerical simulation!!! I dug in deep and pressed forward content with starting over on the benchmarks knowing after the patches released around Jan 9th will be a whole new world. I decided to spare the ugly details related to the Spectre array bounds/brand prediction attack flaws. The out of order meltdown vulnerabilities! UGH! I seriously believe that someone has AI writing news articles written five or six different ways with each somehow saying the same thing. I also provide the links to the information and legal statements directly from a who's who list of accountable parties: Executive Summary:
- * Remember every case is different so please do your run your own tests to verify how this new reality affects your hardware and software environment.*
- Due to costs this machine has a single NVMe M.2 for the primary drive with a single 2TB SATA drive for its Mid-Term Storage area.
- What was the impact for my benchmark?
- Positive takeaway:
- In all of the years of running the sp5 benchmark. I recorded the fastest benchmark time using this CUBE w32s, dual INTEL® XEON® Gold 6130 CPU workstation.
- Using all thirty two cores 125.7 seconds for Solution Time (Time Spent Computing Solution).
- Next, Coming in at 135.7 seconds the Solution Time metric after running the OS patches is my second fastest data point for the ANSYS sp5 benchmark.
- ANSYS sp5 benchmark data - PADT, Inc. Currently from 2005 until this time.
- Next, Coming in at 135.7 seconds the Solution Time metric after running the OS patches is my second fastest data point for the ANSYS sp5 benchmark.
- The Solution Times continued to solve faster with each bump in cores.
- Performance per dollar was maximized in this configuration.
- Depending on number of cores used that I used for the ANSYS sp5 benchmark. I give the actual data below showing the percentage differences before and after:
- Largest percentage difference:
- Solution Time: -9.81% using four CPU cores.
- Total Time: -7.87% using two CPU cores.
- Largest percentage difference:
- Positive takeaway:
- The need to turn the security screws down within your corporate enterprise network is now.
- A rogue malicious agent needs to be on the inside of your corporate network to execute any sort of crafted attack. Much of these details are outlined in the Project Zero abstract.
- Pay extra attention to just who you let on your internal network.
- I reiterate the recommendations of many security professionals that you should already be restricting your internal company network and workstations to employee use. If you are not sure ask again.
- Spectre flaw:
- INTEL, ARM & AMD CPU’s are affected by the Spectre array bounds hardware attacks.
- Meltdown flaw:
- INTEL CPU’s and some ARM high performance CPU’s are affected by the “easier to exploit” Meltdown vulnerability.
- Reading privileged memory with a side-channel - Project Zero
- INTEL Responds To Security Research Findings
- INTEL Analysis of Speculative Execution Side Channels
- ARM Vulnerability of Speculative Processors to Cache Timing Side-Channel Mechanism
- AMD Processors: Google Project Zero, Spectre and Meltdown – An Update on AMD Processor Security
- Security Bulletin: NVIDIA Driver Security Updates for CPU Speculative Side Channel Vulnerabilities. NVIDIA DRIVER RESPONSE TO CPU SPECULATIVE SIDE CHANNEL VULNERABILITIES - CVE-2017-5753, CVE-2017-5715, CVE-2017-5754
- Unpatched Benchmark Data – No mitigation patches from Microsoft and NVidia addressing the Spectre and Meltdown flaws have been applied to the Windows 10 Professional OS running on the CUBE w32s that I use in this benchmark.
- Patched Benchmark Data – I installed the batch of patches released by Microsoft as well as the NVDIA graphics card driver update released by NVIDIA addressing. NVIDIA indicates in their advisory that “their hardware their GPU hardware is not affected but they are updating their drivers to help mitigate the CPU security issue.” Huh? Installing now…
- Solution Time – The amount of time in seconds that the CPU’s spent computing the solution. "The Time Spent Computing Solution"
- Total Time – Total time in seconds that the entire process took. How the solve felt to the user also known as wall clock time.
- CUBE w32s, INTEL® XEON® Gold 6130 CPU, 128GB’s DDR4-2667MHz (1Rx4) ECC REG DIMM, Windows 10 Professional, ANSYS Release 18.2, INTEL MPI 22.214.171.124, 32 Total Cores, NVIDIA QUADRO P4000, Samsung EVO 960 Pro NVMe M.2, Toshiba 2TB 7200 RPM SATA 3 Drive.
- Other notables, are you still paying attention?
- My Supermicro X11Dai-N BIOS Settings:
- BIOS Version: 2.0a
- Execute Disable Bit: DISABLE
- Hyper threading: ON
- Intel Virtualization Technology: DISABLE
- Core Enabled: 0
- Power Technology: CUSTOM
- Energy Performance Tuning: DISABLE
- Energy performance BIAS setting: PERFORMANCE
- P-State Coordination: HW_ALL
- Package C-State Limit: C0/C1 State
- CPU C3 Report: DISABLE
- CPU C6 Report: DISABLE
- Enhanced Halt State: DISABLE
- With a read performance of up to 3,200MB/s and write performance of up to 1,900 MB/s using the Samsung NVMe M.2 drive was to tempting to pass up as my solve and temp solve area location. The bandwidth from the little feller was to impressive and continued to impress throughout the numerical simulation benchmarks.
- My Supermicro X11Dai-N BIOS Settings:
- Cube w32s by PADT, Inc. ANSYS Release 18.2 FEA Benchmark
- BGA (V18sp-5)
- Transient nonlinear structural analysis of a electronic ball grid arrary
- Analysis Type: Static Nonlinear Structural
- Number of Degrees of Freedom: 6,000,000
- Matrix: Symmetic
|ANSYS sp5 Benchmark - Unpatched Windows 10 Professinal for Spectre and Meltdown hardware vulnerability - CUBE w32s|
|CPUs||Solution Time||Total Time|
|ANSYS sp5 Benchmark - Patched Windows 10 Professional - CUBE w32s|
|CPUs||Solution Time||Total Time|
|Percentage Difference - Not Patched vs. Patched for Sprectre, Meltdown|
|Solution Time||Total Time|