When Desktop Engineering needed a subject matter expert on Topological Optimization and its use to drive product development, they called on PADT’s Manoj Mahendran. The article “Your Optimization Software Respectfully Suggests a Revision” gives a great overview of how designs can be driven by the use of Topological Optimization. They also mention a few of the more common tools, and with Manoj’s help, discuss the importance of 3D Printing to the process. An important take away is how these tools can be used to suggest design changes to the designer.
As I showed in a prior blog post, Fused Deposition Modeling (FDM) is increasingly being used to make functional plastic parts in the aerospace industry. All functional parts have an expected performance that they must sustain during their lifetime. Ensuring this performance is attained is crucial for aerospace components, but important in all applications. Finite Element Analysis (FEA) is an important predictor of part performance in a wide range of indusrties, but this is not straightforward for the simulation of FDM parts due to difficulties in accurately representing the material behavior in a constitutive model. In part 1 of this article, I list some of the challenges in the development of constitutive models for FDM parts. In part 2, I will discuss possible approaches to addressing these challenges while developing constitutive models that offer some value to the analyst.
It helps to first take a look at the fundamental multi-scale structure of an FDM part. A 2002 paper by Li et. al. details the multi-scale structure of an FDM part as it is built up from individually deposited filaments all the way to a three-dimensional part as shown in the image below.
This multi-scale structure, and the deposition process inherent to FDM, make for 4 challenges that need to be accounted for in any constitutive modeling effort.
- Anisotropy: The first challenge is clear from the above image – FDM parts have different structure depending on which direction you look at the part from. Their layered structure is more akin to composites than traditional plastics from injection molding. For ULTEM-9085, which is one of the high temperature polymers available from Stratasys, the datasheets clearly show a difference in properties depending on the orientation the part was built in, as seen in the table below with some select mechanical properties.
- Toolpath Definition: In addition to the variation in material properties that arise from the layered approach in the FDM process, there is significant variation possible within a layer in terms of how toolpaths are defined: this is essentially the layout of how the filament is deposited. Specifically, there are at least 4 parameters in a layer as shown in the image below (filament width, raster to raster air gap, perimeter to raster air gap and the raster angle). I compiled data from two sources (Stratasys’ data sheet and a 2011 paper by Bagsik et al that show how for ULTEM 9085, the Ultimate Tensile Strength varies as a function of not just build orientation, but also as a function of the parameter settings – the yellow bars show the best condition the authors were able to achieve against the orange and gray bars that represent the default settings in the tool. The blue bar represents the value reported for injection molded ULTEM 9085.
- Layer Thickness: Most FDM tools offer a range of layer thicknesses, typical values ranging from 0.005″ to 0.013″. It is well known that thicker layers have greater strength than thinner ones. Thinner layers are generally used when finer feature detail or smoother surfaces are prioritized over out-of-plane strength of the part. In fact, Stratasys’s values above are specified for the default 0.010″ thickness layer only.
- Defects: Like all manufacturing processes, improper material and machine performance and setup and other conditions may lead to process defects, but those are not ones that constitutive models typically account for. Additionally and somewhat unique to 3D printing technologies, interactions of build sheet and support structures can also influence properties, though there is little understanding of how significant these are. There are additional defects that arise from purely geometric limitations of the FDM process, and may influence properties of parts, particularly relating to crack initiation and propagation. These were classified by Huang in a 2014 Ph.D. thesis as surface and internal defects.
- Surface defects include the staircase error shown below, but can also come from curve-approximation errors in the originating STL file.
- Internal defects include voids just inside the perimeter (at the contour-raster intersection) as well as within rasters. Voids around the perimeter occur either due to normal raster curvature or are attributable to raster discontinuities.
Thus, any constitutive model for FDM that is to accurately predict a part’s response needs to account for its anisotropy, be informed by the specifics of the process parameters that were involved in creating the part and ensure that geometric non-idealities are comprehended or shown to be insignificant. In my next blog post, I will describe a few ways these challenges can be addressed, along with the pros and cons of each approach.
I had a very cool music teacher back in 6th or 7th grade in the 1970’s in upstate New York. Today we’d probably say she was eclectic. In that class we listened to and discussed fairly recent songs in addition to general music studies. Two songs I remember in particular are ‘Hurdy Gurdy Man’ by Donovan and ‘Pinball Wizard’ by The Who. If you’re not familiar with Pinball Wizard, it’s from The Who’s rock opera Tommy, and is about a deaf, mute, blind young man who happens to be adept at the game of pinball. Yes, he is a Pinball Wizard. This sing popped into my head recently when we had some customer questions here at PADT regarding the pinball region concept as it pertains to ANSYS contact regions.
I’m not sure if the developers at ANSYS, Inc. had this song in mind when they came up with the nomenclature for the 17X (latest and greatest) series of contact elements in ANSYS, but regardless, you too can be a pinball wizard when it comes to understanding contact elements in ANSYS Mechanical and MAPDL.
Fans of this blog may remember one of my prior posts on contact regions in ANSYS that also had a musical theme (bringing to mind Peter Gabriel’s song “I Have the Touch”):
In this current entry we will go more in depth on the pinball region, also known as the pinball radius. The pinball region is involved with the distance from contact element to target element in a given contact region. Outside the pinball region, ANSYS doesn’t bother to check to see if the elements on opposite sides of the contact region are touching or not. The program assumes they are far away from each other and doesn’t worry about any additional calculations for the most part.
Here is an illustration. The gray elements on the left represent the contact body and the red elements on the right represent the target body (assuming asymmetric contact). Target elements outside the pinball radius will not be checked for contact. The contact and target elements actually ‘coat’ the underlying solid elements so they are shown as dashed lines slightly offset from the solid elements for the sake of visibility. Here the pinball radius is displayed as a dashed blue circle, centered on the contact elements, with a radius of 2X the depth of the underlying solid elements.
So, outside the pinball region, we know ANSYS doesn’t check to see if the contact and target are actually in contact. It just assumes they are far away and not in contact. What about what happens if the contact and target are inside the pinball region? The answer to that question depends on which contact type we have selected.
For frictionless contact (aka standard contact in MAPDL) and frictional contact, the program will then check to see if the contact and target are truly touching. If they are touching, the program will check to see if they are sliding or possibly separating. If they are touching and penetrating, the program will check to see if the penetration exceeds the allowable amount and will make adjustments, etc. In other words, for frictionless and frictional contact, if the contact and target elements are close enough to be inside the pinball region, the program will make all sorts of checks and adjustments to make sure the contact behavior is adequately captured.
The other scenario is for bonded and no separation contact. With these contact types, the program’s behavior when the contact and target elements are within the pinball region is different. For these types, as long as the contact and target are close enough to be within the pinball region, the program considers the contact region to be closed. So, for bonded and no separation, your contact and target elements do not need to be line on line touching in order for contact to be recognized. The contact and target pairs just need to be inside the pinball region. This can be good, in that it allows for some ‘slop’ in the geometry to be automatically ignored, but it also can have a downside if we have a curved surface touching a flat surface for example. In that case, more of the curved surface may be considered in contact than would be the case if the pinball region was smaller. This effect is shown in the image below. Reducing the pinball radius to an appropriate smaller amount would be the fix for eliminating this ‘overconstraint’ if desired.
There is a default value for the pinball region/radius. It can be changed if needed. We’ll add more details in a moment. First, why is it called the “pinball” region? I like to think it’s because when it’s visualized in the Mechanical window, it looks like a blue pinball from an actual pinball arcade game, but I’ll admit that the ANSYS terminology may predate the Mechanical interface. The image below shows what I mean. The blue balls are the different pinball radii for different contact regions.
Note that you don’t see the pinball region displayed as shown in the above image unless you have manually changed the pinball size in Mechanical. The pinball region can be changed in the Mechanical window in the details view for each contact region by changing Pinball Region from Program Controlled to Radius, like this:
In MAPDL, the pinball radius value can be changed by defining or editing the real constant labeled PINB.
By now you’re probably wondering what is the default value for the pinball radius? The good news is that it is intelligently decided by the program for each contact region. The default is always a scale factor on the depth of the underlying elements of each contact region. In the first pinball region image shown near the beginning of this article, the example plot shows the pinball region/radius as two times the depth of the underlying elements.
The table below summarizes the default pinball radius values for most circumstances for 2D and 3D solid element models. More detailed information is available in the ANSYS Help.
|Default Pinball Radius Values||Large Deflection Off|
|Large Deflection On
|Frictionless and Frictional||1* Underlying Element Depth||2*Underlying Element Depth|
|Bonded and No Seperation||0.25*Underlying Element Depth||0.5*Underlying Element Depth|
|Rigid-Flexible Contact: Typically the Default Values are Doubled|
Summing it all up: we have seen how the default values are calculated and also how to change them. We have seen what they look like as blue balls in a plot of contact regions in Mechanical if the pinball radius has been explicitly defined. We also discussed what the pinball radius does and how it’s different for frictionless/frictional contact and bonded/no separation contact.
You should be well on your way to becoming a pinball wizard at this point.
Does performing simulation in ANSYS make you think of certain songs, or are there songs you like to listen to while working away on your simulations an addition to The Who’s “Pinball Wizard” and Peter Gabriel’s “I Have the Touch”? If so, we’d love to hear about your song preferences in the comments below.
This video shows a really quick and easy way to extract a fluid domain from a structural model without having to do any Boolean subtract operations.
We have been talking a lot about ANSYS AIM lately. Mostly because we really like ANSYS AIM and we think a large number of engineers out there need to know more about it and understand it’s advantages. And the way we do that is through blog posts, emails, seminars, and training sessions. A new tool that we have started using are “Resource and Productivity Kits,” collections of information that users can download.
Earlier in the year we introduced several kits, including ANSYS Structural, ANSYS Fluids, and ANSYS ElectroMechanical. Now we are pleased to offer up a collection of useful information on ANSYS AIM. This kit includes:
- “Getting to know ANSYS AIM,” a video by PADT application engineer Manoj Mahendran
- “What I like about ANSYS AIM,” a video featuring insights on the tool
- Six ANSYS AIM demonstration videos, including simulations and a custom template demonstration
- Five slide decks that provide an overview of ANSYS AIM and describe its new features
- An exclusive whitepaper on effectively training product development engineers in simulation.
You can download the kit here.
Watch this blog for more useful content on AIM in the future.
It seems like I’ve been explaining large deflection effects a lot recently. Between co-teaching an engineering class at nearby Arizona State University and also having a couple of customer issues regarding the concept, large deflection in structural analyses has been on my mind.
Before I explain any further, the thing you should note if you are an ANSYS Mechanical simulation user is this: If you don’t know if you need large deflection or not, you should turn it on. There is really no way to know for certain if it’s needed or not unless you perform a comparison study with and without it.
So, what are large deflection effects? In simple terms the inclusion of large deflection means that ANSYS accounts for changes in stiffness due to changes in shape of the parts you are simulating. The classic case to consider is the loaded fishing rod.
In its undeflected state, the fishing rod is very flexible at the tip. With a heavy fish on the end of the line, the rod deflects downward and it is then easy to observe that the stiffness of the rod has increased. In other words, when the rod is lightly loaded, a small amount of force will cause a certain downward deflection at the top. When the rod is heavily loaded however, a much larger amount of force will be needed to cause the tip to deflect downward by the same amount.
This change in the force amount required to achieve the same change in displacement implies that we do not have a linear relationship between force and displacement.
Consider Hooke’s law, also known as the spring equation:
F = Kx
Where F is the force applied, K is the stiffness of the structure, and x is the deflection. In a linear system, doubling the force results in double the displacement. In our fishing rod case, though, we have a nonlinear system. We might need to triple the force to double the displacement, depending on how much the rod is loaded relative to its size and other properties, and then to double the displacement again we might need to apply four times that force, just using numbers out of my head as examples.
So, in the case of the fishing rod, Hooke’s law in a linear form does not apply. In order to capture the nonlinear effect we need a way for the stiffness to change as the shape of the rod changes. In our finite element solution in ANSYS, it means that we want to recalculate the stiffness as the structure deflects.
This recalculation of the stiffness as the structure deflects is activated by turning on large deflection effects. Without large deflection turned on, we are constrained to using the linear equation, and no matter how much the structure deflects we are still using the original stiffness.
So, why not just have large deflection on by default and use it all the time? My understanding is that since large deflection adds computation expense to have it on, it’s off by default. It’s the same as for a lot of advanced usage, such as frictionless or frictional contact vs. the default bonded (simpler) behavior. In other words, turning on large deflection will trigger a nonlinear solution, meaning multiple passes through the solver using the Newton Raphson method instead of the single pass needed for a linear problem.
Here is an example of a simplified fishing rod. The image shows the undeflected rod (top), which is held fixed on the left side and has a downward force load applied on the right end. The bottom image shows the final deflected shape, with large deflection effects included. The deflection at the tip in this case is 34 inches.
In comparison running the same load with large deflection turned off resulted in a tip deflection of 40 inches. Thus, the calculated tip deflection is 15% less with large deflection turned on, since we are now accounting for change in stiffness with change in shape as the rod deflects.
Below we have a force (horizontal axis) vs. deflection (vertical axis) plot for a nonlinear simulation of a fishing rod with large deflection turned on. The fact that the curve is not a straight line confirms that this is a nonlinear problem, with the stiffness (slope of the curve) not constant. We can also see that as the force gets higher, the slope of the curve is more horizontal, meaning that more force is needed for each incremental amount of displacement. This matches our observations of the fishing rod behavior.
So, getting back to our original point, it’s often the case that we don’t know if we need to include large deflection effects or not. When in doubt, run cases with and without. If you don’t see a change in your key results, you can probably do without large deflection.
Here is an example using an idealized compressor vane. In this case, the deflections and stresses with and without large deflection effects are nearly the same (the stress difference is about 0.2%).
Bottom line: when in doubt, try it out, with and without large deflection. In ANSYS Mechanical, Large Deflection effects are turned on or off in the details of the Analysis Settings branch.
It’s worth noting that turning on large deflection in ANSYS actually activates four different behaviors, known as large deflection which include large rotation, large strain, stress stiffening, and spin softening. All of these involve change in stiffness due to deformation in one way or another.
If you like this kind of info, or find it useful, we cover topics like this in our training classes. For more info, check out our training pages at http://www.padtinc.com/support/software/training.html.
The local SEMI chapter here in Arizona held a breakfast meeting on Monetizing Internet of Things (IoT) and PADT was pleased to be one of the presenters. Always a smart group, this was a chance to sit with people making the sensors, chips, and software that enable the IoT and dig deep in to where things are and where they need to be.
The event was hosted by one of our favorite customers, and neighbor right across the street, Freescale Semiconductor. Speakers included IoT experts from Freescale, Intel, Medtronics, ASU, and SEMICO Research.
Not surprisingly I talked about how Simulation can play a successful role in product development of IoT devices.
You can download a copy of the presentation here: PADT-SEMI-IOT-Simulation-1.pdf
You can also see more details on how people use Simulation for this application on the ANSYS, Inc. website here. We also like this video from ANSYS that shows some great applications and how ANSYS is used with them:
A couple of common themes resonated across the speakers:
- Price and size need to come down on the chips used in IoT (this was a semiconductor group, so this is a big part of their focus)
- Lowering power usage and increasing power density in batteries is a key driver
- The biggest issue in IoT is privacy and security. Keeping your data private and keeping people from hacking in to IoT devices.
- Another big problem is dealing with all the data collected by IoT devices. How to make it useful and how to store it all. One answer is reducing the data on the device, another is only keeping track of what changes.
- It is early, standards are needed but they are still forming.
If you look at this list, the first two problems are addressable with simulation:
PADT has a growing amount of experience with helping customers simulate and design IoT devices as well as the chips, sensors, and antenna that go in to IoT devices. To learn more, shoot us an email at firstname.lastname@example.org or call 480.813.4884.
PADT is hosting a series of free training classes to introduce users to ANSYS AIM. We have pasted the invitation below. You can register here. We are very excited about this new tool from ANSYS, Inc. and are eager to share it with everyone. Look for more AIM information on this blog in the near future.
Palm trees and movie stars. Endless beaches and deserts that fade to the horizon. Aerospace companies, world class universities, med device developers, and toy manufacturers. Oil, freeways, and big construction. Southern California. A place larger and more diverse than most countries in the world. PADT has done work in the area since our first weeks in business. As our business continued to grow, our customers started asking when we were opening up a local office, but the time never seemed right. Until now.
PADT is pleased to announce that we will be loading furniture and computers in a truck and head on the I-10 to Torrance, California where we will open up a new office. ANSYS, Inc. has expanded our sales territory to include small and medium sized new accounts in the Southern California area. The focus of this new office will be building that business.
You can read the official details in the press release below, or the PDF here. As usual, we want to share some more informal information with our blog readers.
The office will be started with an engineer and a salesperson who have been with us for a while, and another pair that we are hiring locally. This combination of company experience and local knowledge should get us going quickly. Over time, the plan is to grow the Torrance office, and add at least two more. Long term we would like to have between 3 and 10 employees per office in Southern California.
Our team will conduct training and seminars from this office and use it as a base to spread the word on simulation driven product development across Southern California. The initial focus for sales will be on small and medium sized businesses that are currently not using ANSYS products, that want to work with a technical sales and support team who can provide more than the software tool – customers who want a partner who can also help them apply the tools effectively. The dense hotbeds of engineering along the coast will be an obvious area of concentration. We also aim to represent the value of ANSYS products in less visited areas of the region, including the high deserts, “in-between” towns, and inland locations beyond LA, Orange County, and San Diego.
The good news is that we are not starting from scratch. This first office is right down the street from the California campus of PADT’s largest and oldest customer. We also have over one hundred customers who have used PADT for simulation services, training, rapid prototyping, and product development, and we will be reaching out to them shortly to start building our local network even further. And then, our new employees who we will hire locally will be contacting their network as well.
Before the end of the summer we hope to have a grand opening event, as well as several seminars that will continue through the end of the year. If you live in the area and want to be invited, visit here to register as someone who want to be on the California contact list.
This blog and social media will be used to post our progress. The entire sales and technical team is looking forward to meeting everyone in the area in the coming months.
If you have any questions or suggestions for us, please contact us. Our standard number 480.813.4884 works for all of our offices.
Below is a copy of the press release, or you can view the “official” version here.
In the world of simulation there are two facts of life. First, the deadline of “yesterday would be good” is not too uncommon. Funding deadlines, product roll-out dates, as well as unexpected project requirements are all reliable sources for last minute changes. Engineers are required to do quality work and deliver reliable results in limited time and resources. In essence perform sorcery.
Second, the size and complexity of models can vary wildly. Anything from fasteners and gaskets to complete systems or structures can be in the pipeline. Engineers can be looking at any combination of hundreds of variables that impact the resources required for a successful simulation.
Required CPU cores, RAM per core, interconnect speeds, available disk space, operating system and ANSYS version all vary depending on the model files, simulation type, size, run-time and target date for the results.
At PADT, We Can Help
PADT Inc. has been nostrils deep in engineering services and simulation products for over 20 years. We know engineering, we know how to simulate engineering and we know ANSYS very well. To address the challenges our customers are facing, in 2015 PADT introduced CoresOnDemand to the engineering community.
CoresOnDemand offers the combination of our proven CUBE cluster, ANSYS simulation tools and the PADT experience and support as an on demand simulation resource. By focusing on the specific needs of ANSYS users, CoresOnDemand was built to deliver performance and flexibility for the full range of applications. Specifics about the clusters and their configurations can be found at CoresOnDemand.com.
Call Us We’re Nice
CoresOnDemand is a new service in the world of on-demand computing. Prospective customers just need to give us a call or send us an inquiry here to get all of their questions answered. The engineers behind CoresOnDemand have a deep understanding of the ANSYS tools and distributed computing and are able to asses and properly size a compute environment that matches the needed resources.
Two Halves of the Nutshell
The process for executing a lease on a CoresOnDemand cluster is quite straight forward. There are two parts to a lease:
PART 1: How many cores & how long is the lease for?
By working with the PADT engineers – and possibly benchmarking their models – customers can set a realistic estimate on how many cores are required and how long their models need to run on the CoresOnDemand clusters. Normally, leases are in one-week blocks with incentives for longer or regular lease requirements.
Part 2: How will ANSYS be licensed?
An ANSYS license is required in order to run on the CoresOnDemand environment. A license lease can be generated by contacting any ANSYS channel partner. PADT can generate license leases in Arizona, Colorado, New Mexico, Utah & Nevada. Licenses can also be borrowed from the customer’s existing license pool.
Using the Cluster
Once the CoresOnDemand team has completed the cluster setup and user creation (takes a couple of hours for most cases), customers can login and begin using the cluster. The CoresOnDemand clusters allow customers to use the connection method they are comfortable with. All connections to CoresOnDemand are encrypted and are protected by a firewall and an isolated network environment.
Step 1: Transfer files to the cluster:
Files can be transferred to the cluster using Secure Copy Protocol which creates an encrypted tunnel for copying files. A graphical tool is also available for Windows users (& it’s freeJ). Also, larger files can be loaded to the cluster manually by sending a DVD, Blu-ray disk or external storage device to PADT. The CoresOnDemand team will mount the volume and can assist in the copying of data.
Step 2: Connect to the cluster and start jobs
Customers can connect to the cluster through an SSH connection. This is the most basic interface where users can launch interactive or batch processing jobs on the cluster. SSH is secure, fast and very stable. The downside of SSH is that is has limited graphical capabilities.
Another option is to use the Nice Software Desktop Cloud Visualization (DCV) interface. DCV provides enhanced interactive 2D/3D access over a standard network. It enables users to access the cluster from anywhere on virtually any device with a screen and an internet connection. The main advantage of DCV is the ability to start interactive ANSYS jobs and monitor them without the need for a continuous connection. For example, a user can connect from his laptop to launch the job and later use his iPad to monitor the progress.
Figure 1. 12 Million cell model simulated on CoresOnDemand
The CoresOnDemand environment also has the Torque resource manager implemented where customers can submit multiple jobs to a job queue and run them in sequence without any manual intervention.
Once the simulation runs are completed customers usually choose one of two methods to transfer data back. First is to download the results over the internet using SCP (mentioned earlier) or have external media shipped back (External media can be encrypted if needed).
After the customer receives the data and confirms that all useful data was recovered from the cluster, CoresOnDemand engineers re-image the cluster to remove all user data, user accounts and logs. This marks the end of the lease engagement and customers can rest assured that CoresOnDemand is available to help…and it’s pretty fast too.
This week ANSYS, Inc. made a fantastic announcement that has been in the works for a while, and that we think will greatly benefit the simulation community: A free ANSYS Student product. This is an introductory product that is focused on students who are learning the fundamentals of simulation who also want to learn the full power and capability of the ANSYS product suite. It includes ANSYS® Multiphysics™ , ANSYS® CFD™ , ANSYS® Autodyn®, ANSYS® Workbench™, ANSYS® DesignModeler™and ANSYS®DesignXplorer™
Yes you read that right, all of the flagship products for free. No features or capabilities are turned off. It is the exact same software as the commercial product, but the size of problems that you can solve is limited. It runs on MS Windows. Perfect for students.
PADT is excited about this because it gives students access to the ability to learn FEA and CFD simulation with the world’s most popular and capable simulation tool, without running in to brick walls. Want to do a flat plate with a hole in it? No Problem. Want to model fluid-solid-interaction on a flexible membrane valve? No Problem. Want to model explosive forming? No Problem. Want to model combustion with complex turbulence? No problem.
All in the same interface as students will use when they enter the work force or do research at University.
This is great news and we can’t wait to see what schools and students do with this access.
How to Get It – The New Academic Web Pages
The previous Student Portal is being replaced with an Academic Web area on the ansys.com site: ansys.com/academic.
Go to the ANSYS Student site to learn more about ANSYS Student and how to download your copy. These same pages will have resources to help you learn and understand the product.
Let me state categorically that PADT was not consulted on the image that ANSYS, Inc. used for the “student” user that was so happy to find out that there is now a free version of the ANSYS software suite. Here is their picture:
Just kidding. We were happy to see this product come out and thought the picture was hilarious. In all seriousness, we will also plug the recent #ilooklikeanengineer twitter hash tag , highlighting the diversity of female engineers. that was awesome and we would love to see more chances for engineers to show their true selves.
It’s not a series of articles until there’s at least 3, so here’s the second article in my series of ‘what not to do’ in ANSYS…
Just in case you’re not familiar with thin sweep meshing, here’s an older article that goes over the basics. Long story short, the thing sweep mesher allows you to use multiple source faces to generate a hex mesh. It does this by essentially ‘destroying’ the backside topology. Here’s a dummy board with imprints on the top and bottom surface:
If I use the automatic thin sweep mesher, I let the mesher pick which topology to use as the source mesh, and which topology to ‘destroy’. A picture might make this easier to understand…
As you can see, the bottom (right picture) topology now lines up with the mesh, but when I look at the top (left picture) the topology does not line up with the mesh. If I want to apply boundary conditions to the top of the board (left picture), I will get some very odd behavior:
I’ve fixed three sides of the board (why 3? because I meant to do 4 but missed one and was too lazy to go back and re-run the analysis to explain for some of future deflection plots…sorry, that’s what you get in a free publication) and then applied a pressure to all of those faces. When I look at the results:
Only one spot on the surface has been loaded. If you go back to the mesh-with-lines picture, you’ll see that there is only a single element face fully contained in the outline of the red lines. That is the face that gets loaded. Looking at the input deck, we can see that the only surface effect element (how pressure loads are applied to the underlying solid) is on the one fully-contained element face:
If I go back and change my thin sweep to use the top surface topology, things make sense:
The top left image shows the thin sweep source definition. Top right shows the new mesh where the top topology is kept. Bottom left shows the same boundary conditions. Bottom right shows the deformation contour.
The same problem occurs if you have contact between the top and bottom of a thin-meshed part. I’ll switch the model above to a modal analysis and include parts on the top and bottom, with contact regions already imprinted.
I’ll leave the thin sweeping meshing control in place and fix three sides of the board (see previous laziness disclosure). I hit solve and nothing happens:
Ah, the dreaded empty contact message. I’ll set the variable to run just to see what’s going on. Pro Tip: If you don’t want to use that variable then you would have to write out the input deck, it will stop writing once it gets to the empty contact set. Then go back and correlate the contact pair ID with the naming convection in the Connections branch.
The model solves and I get a bunch of 0-Hz (or near-0) modes, indicating rigid body motion:
Looking at some of those modes, I can see that the components on one side of my board are not connected:
The missing contacts are on the bottom of the board, where there are three surface mounted components (makes sense…I get 18 rigid body modes, or 6 modes per body). The first ‘correct’ mode is in the bottom right image above, where it’s a flapping motion of a top-mounted component.
So…why don’t we get any contact defined on the bottom surface? It’s because of the thin meshing. The faces that were used to define the contact pair were ‘destroyed’ by the meshing:
Great…so what’s the take-away from this? Thin sweep meshing is great, but if you need to apply loads, constraints, define contact…basically interact with ANYTHING on both sides of the part, you may want to use a different meshing technique. You’ve got several different options…
- Use the tet mesher. Hey, 2001 called and wants its model size limits back. The HPC capabilities of ANSYS make it pretty painless to create larger models and use additional cores and GPUs (if you have a solve-capable GPU). I used to be worried if my model size was above 200k nodes when I first started using ANSYS…now I don’t flinch until it’s over 1.5M
Look ma, no 0-Hz modes!
- Use the multi-zone mesher. With each release the mutli-zone mesher has gotten better, but for most practical applications you need to manually specify the source faces and possibly define a smaller mesh size in order to handle all the surface blocking features.
Look pa, no 0-Hz modes!Full disclosure…the multi-zone mesher did an adequate job but didn’t exactly capture all of the details of my contact patches. It did well enough with a body sizing and manual source definition in order to ‘mostly’ bond each component to the board.
- Use the hex-dominant mesher. Wow, that was hard for me to say. I’m a bit of a meshing snob, and the hex dominant mesher was immature when it was released way back when. There were a few instances when it was good, but for the most part, it typically created a good surface mesh and a nightmare volume mesh. People have been telling me to give it another shot, and for the most part…they’re right. It’s much, much better. However, for this model, it has a hard time because of the aspect ratio. I get the following message when I apply a hex dominant control:
- The warning is right…the mesh looks decent on the surface but upon further investigation I get some skewed tets/pyramids. If I reduce the element size I can significantly reduce the amount of poorly formed elements:
- That’s going on the refrigerator door tonight!
And…no 0-Hz modes!
- Lastly…go back to DesignModeler or SpaceClaim and slice/dice the model and use a multi-body part.
3 operations, ~2 minutes of work (I was eating at the same time)
That’s a purdy mesh! (Note: most of the lower-quality elements, .5 and under, are because there are 2-elements through thickness, reducing the element size or using a single element thru-thickness would fix that right up)
Phew…this was a long one. Sorry about that. Get me talking about meshing and look what happens. Again, the take-away from all of this should be that the thin sweeper is a great tool. Just be aware of its limitations and you’ll be able to avoid some of these ‘odd’ behaviors (it’s not all that odd when you understand what happens behind the scenes).
We just recieved a new tech tip bundle from ANSYS, Inc on Electromechanical Simulation. You may remember when we published the Mechanical and Fluids ANSYS tech tips a few weeks ago. This latest kit continues with information for people making devices and systems that have mechanical and electrical systems. The focus of the kit is the application of ANSYS Maxwell and Simplorer – Maxwell to model low frequency electromagnetics and Simplorer to model systems.
Here is a link to “The Electromechanical Simulation Productivity Kit ” here. The kit includes:
- ANSYS Maxwell Automation and Customization Application Brief
- ANSYS Maxwell Magnetic Field Formulation Application Brief
- Electric Machine Design Methodology Whitepaper
- Electromagnetics And Thermal Multiphysics Analysis Webinar
- Rechargeable Lithium Ion Battery Whitepaper
- Robust Electric Machine Design – ANSYS Advantage Article
We also have a collection of videos that are a great introduction to the tool set and how to use it. Check out the overview and the video on the washing machine at a minimum. Even if you have a simple EMAG or do hand calcs, you need to look at Maxwell and Simplorer.
This video will show you how you can optimize a part using Topology Optimization with GENESIS through ANSYS Mechanical with support from ANSYS SpaceClaim
With the introduction of ACT, the ANSYS Workbench editors have gained capabilities and shortcuts at much faster rate than what can be introduced in a development cycle. One of first and most far-reaching extensions is the acoustics. Inevitably I was called on by one of our customers to show them how to do a vibro-acoustics analysis (harmonic with acoustic excitation), which I did. Since the need for this type of analysis is quite broad, I’ll share it here too.
There was an extra level of excitement with this, in that I’m a structures specialist with no prior acoustics experience. So, I did my own self-training on this topic. I have to give tons of credit to Sheldon Imaoka of ANSYS Inc., who took the time to thoroughly answer the questions I had. That being said, this article will be from the standpoint of a structures engineer who’s just recently learned acoustics.
It’s at the very top, under ‘A’ for “Acoustics”
One thing you’ll notice when you unzip the Acoustics Extension package is that it contains and entire Acoustics training course. Take advantage of this freebie when learning acoustics analysis. I’ll note that, most of the process outlined in this article comes from the Submarine workshop in the acoustics training course.
Once you’ve installed and turned on the Acoustics extension, insert a Harmonic Analysis system into the project schematic, link to the solid geometry file, and specify the material properties for the solid. You’ll specify the properties for the acoustic region in Mechanical under the appropriate Acoustics extension objects.
Rename as you see fit
Assuming you just have the geometry for the solid and not the acoustics domain, create two acoustics regions around the solid. The first region, surrounding the solid, will function as the fluid region itself, through which the acoustic waves travel and interact with the structure. The second region, surrounding the first acoustics region, will function as the Perfectly Matched Layer (PML). The PML essentially acts as the infinite boundary of the system. (If you’re an electromagnetics expert, you already know this and I’m boring you.) You can easily create these domains using the enclosure tool in DesignModeler.
Now we’re ready for the analysis. Open up Mechanical. Look at all those buttons on the Acoustics toolbar! Yikes! Fortunately we just need a few of them.
Here they are
Insert an Acoustic Body and scope it to the acoustic region surrounding the structural solid. In the Details, enter the density and speed of sound for the fluid. Also set the Acoustic-Structural Coupled Body Options to Coupled With Symmetric Algorithm.
Pay attention to the menu picks, Details, and geometry scoping here and in the rest of the image captures
“Coupled” refers to coupled-field behavior, i.e. the mutual interaction between the structure and the fluid. You’re probably familiar with this. You need that, otherwise the acoustic waves are just bouncing off the structure and the structure isn’t doing anything. Regarding the Symmetric Algorithm: The degrees of freedom for the acoustic system consists of both structural displacements and fluid pressures, giving you an asymmetric stiffness matrix. However, ANSYS has incorporated a symmetrization algorithm to convert the asymmetric stiffness matrix to a symmetric matrix, resulting in half as many equations that need to be solved and thus a faster solution time yadda yadda yadda, so go with that.
Now insert another Acoustic Body, this time scoped to the outer acoustic region (body). This is your Perfectly Matched Layer. Specify fluid density and speed of sound as before. This time, leave the Coupled Body Option as Uncoupled. But, set Perfectly Matched Layers to On.
Apply an Acoustic Pressure of zero to the outer faces of the PML body (Boundary Conditions > Acoustic Pressure). As you may have guessed from the menu pick, this is your acoustics boundary condition.
Now we’ll apply some acoustic wave excitation to this thing. From the Excitation menu, select Wave Sources (Harmonic). In the Details, set the Excitation Type to either Pressure or Velocity, set the Source Location and specify the excitation pressure or velocity value. In this example, I went with Pressure since that’s what MIL-STD-810 specifies, but this option will be based on your customer requirements. I also assumed an external acoustic source (hence, Outside the Model), but again, that will be based on your particular project. You also need to specify the vector of the wave source, via rotations about the Z and Y axes (f and q). In this case I chose 30 and 60 degrees, respectfully, to make it interesting. Once again, enter the density and speed of sound for the fluid.
Insert Scattering Controls under the Analysis Settings menu and specify whether the Field Output should be Total or Scattered. Total gives you constant pressure waves that interact with the solid but not each other. Scattered gives you wave that interact and interfere with each other as well as the solid.
Set up the Fluid-Structural Interaction boundary condition where the structural faces are “wetted” by the acoustic domain. The FSI Interface is found under the Boundary Conditions menu.
Apply structural constraints and specify harmonic analysis settings just like you would with a standard harmonic analysis. Make sure you request Stresses under the Output Controls. Solve the model.
Plot your structural results as you would for a typical harmonic analysis. Acoustic Pressure wave results may be found under the Results menu in the Acoustics toolbar. If you used Total field output for the scattering option, you can verify your wave source direction by looking at the Acoustic Pressure Contours. Keep in mind that the contours will be orthogonal to the axis of the sine wave; you may need to put some extra spatial thought into it to fully understand what’s going on.
Acoustic Pressures: Field Output = Total
Acoustic Pressures: Field Output = Scattered
Von-Mises Stresses, Max Over Phase: Field Output = Scattered
As you’ll note in the training course, there are a number of design questions that can be answered with acoustics analysis. In this article, I’ve addressed what I thought would be one of the more popular applications of acoustics simulation. If the demand is there, I’ll research and compose more articles on various acoustics applications in the future. For instance, another area I’ve examined is natural frequencies of a structure that’s submerged in a fluid. If there’s another acoustics topic you’d like us to write about, please let us know in the comments.