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.

PADT-ANSYS-Fastener_Simulation_Part1

Eigenvalue Buckling and Post-buckling Analysis in ANSYS Mechanical

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

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

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

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

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

 

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

Read the article here.

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

Can ANSYS Mechanical Handle My Required Modeling Precision?

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

PADT-ANSYS-Mechanical-Modeling-Precision

 

10 Great New Features in ANSYS Mechanical 19.0 and 19.1

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

ANSYS Mechanical 19.0

1. 4 Cores HPC Solving with No Additional Licensing

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

2. Topology Optimization Includes Inertial Loads

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

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

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

3. Small Sliding Contact

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

4. Element Birth and Death

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

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

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

5. Clipboard Tool

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

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

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

ANSYS Mechanical 19.1

6. Granta Design Sample Materials

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

7. Materials folder in Mechanical

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

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

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

thtest1=typeids(1)

or

et,typeids(1),solid65

8. Result Tracking During Solution

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

9. Save Animations to .wmv and .mp4 Formats

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

10. Solution Statistics Page

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

Conclusions

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

What is New and Exciting in Mechanical Simulation – Webinar Recording

The 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.

ANSYS Licensing FAQ

Were 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:

  1. Server down or not responsive
  2. Installation/Migration
  3. VPN
  4. TECS and license expiry
  5. Versions compatibility
  1. Overuse of licenses
  2. Include list
  3. HPC
  4. Virtual server
ANSYS LICENSING FAQ

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

support@padtinc.com

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.

Press Release: New Expansion into Texas Grows PADT’s ANSYS Sales & Support Across the Entire Southwest

When 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.

Press Release:

Simulation, Product Development and 3D Printing Services Leader, PADT, Opens New Office in Austin, Texas

PADT Becomes the Only ANSYS Elite Channel Partner to Serve the Entire Southwest Region

TEMPE, Ariz., Austin, Texas, February 6, 2018

Phoenix Analysis and Design Technologies (PADT), the Southwest’s largest provider of simulation, product development, and rapid prototyping services and products, today announced it has opened an office in Austin, Texas. With this move, PADT is expanding its sales and support for ANSYS simulation software, becoming the only ANSYS Elite Channel Partner to cover the entire Southwest region.

“This is a major expansion for PADT with the opportunity to significantly grow our customer base,” said Ward Rand, co-owner and principal, PADT. “We have worked with Texas companies on and off since we founded the company in 1994, our success over the last decade has provided the opportunity to become a full-time resident in the vibrant and growing Austin business and technology community.”

Although the initial focus for the PADT Austin office will be on ANSYS sales and support, the company plans to offer its wide array of other products and services in the future. PADT will host a grand opening celebration for customers, partners and media in March, 2018. Ian Scott an Austin native, will be launching the new office and leading the sales effort in the region.

“PADT’s expertise in simulation-driven product development will be a welcome addition to the Austin community,” said Scott. “Our focus at launch will be on educating the Austin technology scene on how to derive the best value from their engineering simulation software investment and building stronger relationships with our new neighbors.”

In 2017, PADT experienced a very successful year in regards to growing its capabilities, as well as in public recognition. PADT was named an ANSYS Elite Channel Partner for North America, partnered with Desktop Metal and Carbon to upgrade 3D printing capabilities and services and was named to Entrepreneur Magazine’s list of the top small businesses in the nation, the Entrepreneur 360 List. The success of the company has enabled PADT to take this step towards further expansion.

To learn more about PADT, visit www.padtinc.com or call 1-800-293-7238.

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; Murray, Utah, and Austin, Texas, 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

Finding curve directions in ANSYS SpaceClaim   

As 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.

Spectre Side-Channel and Meltdown – How will living in this new reality affect the world of numerical simulation?

Literally, 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.
      • 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.
  • 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.
  1. Spectre flaw:
    1. INTEL, ARM & AMD CPU’s are affected by the Spectre array bounds hardware attacks.
  2. Meltdown flaw:
    1. INTEL CPU’s and some ARM high performance CPU’s are affected by the “easier to exploit” Meltdown vulnerability.

I am also interested to see how continued insertion of code barriers and changed memory mappings affect my gaming performance. Haha! No, I am just kidding my numerical simulation performance benchmarks.

Clarifications & Definitions:

  • 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.

The CUBE machine that I used in this ANSYS Test Case represent a fine balance based on price, performance and ANSYS HPC licenses used.

  • CUBE w32s, INTEL® XEON® Gold 6130 CPU, 128GB’s DDR4-2667MHz (1Rx4) ECC REG DIMM, Windows 10 Professional, ANSYS Release 18.2, INTEL MPI 5.0.1.3, 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 first overall impressions of this configuration is Wow! this workstation is fast, quiet and as you will see number crunches its way right on through to being my fastest documented workstation benchmark in this class. This extremely challenging and I/O intensive ANSYS benchmark is no match for this solver! Thumbs up and cheers to happy solving!

  • 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

It Is All About The Data:

Benchmark data related to Pre and Post Spectre and Meltdown industry software patches on the CUBE w32s.

Table 1 – ANSYS sp5 Benchmark  – UnPatched Windows 10 Professional

ANSYS sp5 Benchmark  – Unpatched Windows 10 Professinal for Spectre and Meltdown hardware vulnerability – CUBE w32s
CPUs Solution Time Total Time
2 631.3 671
4 366.8 422
8 216 259
12 193 235
16 144.3 185
20 143.9 187
24 131.9 175
28 137.4 185
31 142.4 185
32 125.7 171
Apples to Apples, meltdown, spectre, ANSYS numerical simulation benchmark data
ANSYS Release 18.2 – SP5 Benchmark – Unpatched Windows 10 Professional CUBE w32s Solution and Total Time Values

Table 1.1 – ANSYS sp5 Benchmark  – Patched Windows 10 Professional

ANSYS sp5 Benchmark  – Patched Windows 10 Professional – CUBE w32s
CPUs Solution Time Total Time
2 683 726
4 405.5 446
8 235.8 277
12 209.2 251
16 148.8 191
20 145.7 189
24 136.3 182
28 138.7 186
31 134.6 179
32 135.7 179
Apples to Apples, meltdown, spectre, ANSYS numerical simulation benchmark data
ANSYS Release 18.2 – SP5 Benchmark – Patched Windows 10 Professional for the Sprectre and Meltdown hardware flaw – Solution And Total Time Values

Table 2 – ANSYS sp5 Benchmark  – The Before and After In Percentage Difference.

Percentage Difference – Not Patched vs. Patched for Sprectre, Meltdown
Solution Time Total Time
-7.94 -7.87
-9.81 -5.53
-8.34 -6.72
-7.57 -6.58
-2.73 -3.19
-1.09 -1.06
-2.87 -3.92
-0.81 -0.54
4.76 3.30
-6.74 -4.57

Fig 2.a

Percentage of impact for this example. Negative value means in this example. The patched Windows 10 Professional CUBE w32s is taking a performance hit.
Percentage of impact for this example. Negative value means “performance hit” in this example. Notice a very interesting blip of positive percentage at 31 cores. A patched CUBE w32s Windows 10 Professional for Sprectre and Meltdown hardware vulnerability. The data from this Windows 10 Professional CUBE w32s INTEL® XEON® Gold 6130 CPU is showing an impact related to the patches.

FIg 2.b

Percentage of impact for this example. Negative value means in this example. The patched Windows 10 Professional CUBE w32s is taking a performance hit.
Percentage of impact for this example. Negative value means there is some sort of impact. The patched Windows 10 Professional CUBE w32s will feel longer to solve by looking at the clock on the wall.
CUBE w32s in action - January 2018
CUBE w32s in action – January 2018

Please contact your local ANSYS Software Sales Representative for more information on purchasing ANSYS HPC Packs. You too may be able to speed up your solve times by unlocking more compute power!

What the heck is a CUBE? For more information regarding our Numerical Simulation workstations and clusters please contact our CUBE Hardware Sales Representative at SALES@PADTINC.COM

Designed, tested and configured within your budget. We are happy to help and to listen to your specific needs.

CUBE w32s in action - January 2018
CUBE w32s in action – January 2018

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!)

Transitioning to ANSYS

Before joining PADT last July, I have worked on FEA and CFD analyses but my exposure to ANSYS was limited and I was concerned about the transition. To my delight, the software was very easy to learn; most often than not intuitive and self-explanatory (e.g. mechanical wizard), the setup time was minimized after learning couple simple features (e.g. named selection, object generator etc.) and the resources on the ANSYS portal were very instrumental in the learning process. Furthermore, the colleagues at PADT proved to be very knowledgeable and experienced and more importantly responsive and eager to jump for help.

One of the most attractive features that caught my attention was the streamline of the Multiphysics nature that ANSYS has. I have been satisfied with the performance of standalone CFD packages in the past, and same goes for structural ones. But never have I dealt with an extensive software that maintained the quality of a specialized one. The importance of this attribute is showing more and more its powers in recent years given the development of new convoluted products of Multiphysics nature e.g. medical applications.

Using ANSYS to simulate medical applications is one of the most rewarding experience I personally enjoy. Even though, it is definitely satisfying to be able to help accelerate innovation in the aerospace, automotive, and a myriad of other industrial areas…the experience in the medical area has a more refreshing taste, probably due to the clear and direct link to human lives. From intravascular procedures to shoulder implants and microdevices, there is one common factor: ANSYS is decreasing the risks of catastrophic failures, improving the product capabilities and shortening the innovation cycle.

Editors Note: Ziad is part of PADT’s team in Southern California.   He is a graduate of USC and has worked at Boeing, Meggit, and Pacific Consolidated Industries before joining PADT.  He works with the rest of our ANSYS technical staff to make sure our users are getting the most from their ANSYS investment.