Helpful New Meshing Feature in ANSYS Mechanical 17.0 – Nonlinear Mechanical Shape Checking

ansys=new-mesh-r17Meshing for Nonlinear Structural Problems

Overcoming convergence difficulties in nonlinear structural problems can be a challenge. I’ve written a couple of times previously about tools that can help us overcome those difficulties:

I’m pleased to announce a new tool in the ANSYS Mechanical tool belt in version 17.0.
With version 17.0 of ANSYS we get a new meshing option for structural simulations: Nonlinear Mechanical Shape Checking. This option has been added to the previously available Standard Mechanical Shape Checking and Aggressive Mechanical Shape Checking. For a nonlinear solution in which elements can become significantly distorted, if we start with better-shaped elements they can undergo larger deformations without encountering errors in element formulation we may encounter fewer difficulties as the nodes deflect and the elements become distorted. The nonlinear mechanical setting is more restrictive on the element shapes than the other two settings.

We’ve been recommending the aggressive mechanical setting for nonlinear solutions for quite a while. The new nonlinear mechanical setting is looking even better. Anecdotally, I have one highly nonlinear customer model that reached 95% of the applied load before a convergence failure in version 16.2. That was with the aggressive mechanical shape checking. With 17.0, it reached 99% simply by remeshing with the same aggressive setting and solving. That tells you that work has been going on under the hood with the ANSYS meshing and nonlinear technology. By switching to the new nonlinear mechanical shape checking and solving again, the solution now converges for the full 100% of the applied load.
Here are some statistics using just one measure of the ‘goodness’ of our mesh, element quality. You can read about the definition of element quality in the ANSYS Help, but in summary better shaped elements have a quality value close to 1.0, while poorly shaped elements have a value closer to zero. The following stats are for tetrahedral meshes of a simple turbomachinery blade/rotor sector model (this is not a real part, just something made up) comparing two of the options for element shape checking. The table shows that the new nonlinear mechanical setting produces significantly fewer elements with a quality value of 0.5 or less. Keep in mind this is just one way to look at element quality – other methods or a different cutoff might put things in a somewhat different perspective. However, we can conclude that the Nonlinear Mechanical setting is giving us fewer ‘lower quality’ elements in this case.

Shape Checking Setting Total Elements Elements w/Quality <0.5 % of elements w/Quality <0.5
Aggressive Mechanical 31683 1831 5.8
Nonlinear Mechanical 31865 1249 3.9

Here are images of a portion of the two meshes mentioned above. This is the mesh with the Aggressive Mechanical Shape Checking option set:ansys-new-meshing-17-01
The eyeball test on these two meshes confirms fewer elements at the lower quality contour levels.

And this is the mesh with the Nonlinear Mechanical Shape Checking option set:

ansys-new-meshing-17-02

So, if you are running nonlinear structural models, we urge you to test out the new Nonlinear Mechanical mesh setting. Since it is more restrictive on element shapes, you may see longer meshing times or encounter some difficulties in meshing complex geometry. You may see a benefit in easier to converge nonlinear solutions, however. Give it a try!

Be a Pinball Wizard with Contact Regions in ANSYS Mechanical

pinball-wizard-pinball-machine-ANSYS-3
A pinball machine based on The Who’s Tommy

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.

pinball_radius_contact_illustration

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.

pinball_radius_bonded_noseparation

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.

pinball_radius_visualization

 

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:

pinball_radius_change

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 ValuesLarge Deflection Off
Flexible-Flexible
Large Deflection On
Flexible-Flexible
Frictionless and Frictional1* Underlying Element Depth2*Underlying Element Depth
Bonded and No Seperation0.25*Underlying Element Depth0.5*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.

To Use Large Deflection or Not, That Is the Question

Hamlet-Large-DeflectionIt 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.

Ted-rod-fishing1

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.

Undeformed_deformed_rod

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.

Force_vs_Deflection

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%).

Large Deflection On:blade_large_defl

Small Deflection:blade_small_defl

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.

Instructions for Installing and Configuring ANSYS MAXWELL and PExprt, Versions 16.X

ANSYS_pexpert_maxwell-1ANSYS PExpert is a fantastic tool for the design, modeling, and analysis of transformers and inductors. Using a combination of classical and finite element analysis (FEA) techniques, ANSYS PExprt determines the core size and shape, air gaps, and winding strategy for a given power converter topology. What we and our customers have found very useful is the ability to then evaluate the magnetic design in ANSYS Maxwell to view such things as flux density in the core and current density distribution in the windings. Powerful stuff.

The first step in implementing ANSYS PExprt with ANSYS Maxwell is installing and configuring them correctly.  We created a step-by-step guild for our ANSYS customers here in the Southwest, and thought others would find it useful.

ansys-maxwell-pexprt-install-image

Download: InstallingMaxwellandPExprt16.pdf

As always, feel free to contact us if you have any questions or need more information. Also, even if you are not in our sales area, please consider using PADT for consulting or training.

 

 

 

 

 

 

 

Have You Ever Dreamed in Color – 3D Color? 3D PDF Is Here with VCollab!

VCollab_Shaded_Logo_FinalIf you have ever dreamed of, or at least had a need for a 3D .pdf file of your simulation results, the dream is now realized thanks to VCollab.  As Eric Miller mentioned in The Focus blog back in February, the latest release of VCollab software enables users to save their results in 3D .pdf format.

We’ve now had a chance to test out the capability here at PADT, and we find it quite useful.  We’ve talked about VCollab before, but it’s a software suite that enables virtual collaboration (hence the name) by reducing what may be huge simulation files to a much smaller size, enabling others in your organization or your customers to dynamically view simulation results as well as CAD data in a light-weight viewer.  The folks at Vcollab have gone one step beyond that now by supporting the 3D .pdf format that is viewable in the standard Adobe reader.

Vcollab works with ANSYS results as well as results from lots of other simulation tools.  The process is:

You can download the sample file used in the images below:

vcollab-3d-pdf-sample-bolted1.pdf.

This is what a typical 3D .pdf file created from an ANSYS Mechanical/MAPDL results file looks like, with using the mouse to rotate and zoom around within Adobe reader.

So, if you recognize value in being able to create 3D .pdf files like this, the Vcollab software suite is worth investigating.  Vcollab does lots of useful things besides writing 3D .pdf files, including the capability to be imbedded within the ANSYS Engineering Knowledge Manager (ANSYS EKM) tool.

The best way to see the power of this tool is to request a demo.  Just fill out this form and we will reach out and set one up, followed by a 30 day trial.  .

Or check out www.vcollab.com.

 

Taking NASTRAN Input Files Into ANSYS Mechanical via External Model in ANSYS 16.0

nastran-ansys-external-model-tnI found another very nice enhancement to version 16.0 of the ANSYS Workbench/ANSYS Mechanical toolset.  If you happen to have a NASTRAN input file (.dat, .nas, and .bdf) that you need to get into ANSYS Mechanical, no longer do you have to use FE Modeler in ANSYS Workbench to perform the translation.  In fact, not only can you move the NASTRAN model into ANSYS Mechanical, but you get the existing mesh as well as newly-created geometry that can be used for boundary condition application, etc.  As with most translations from one FE tool to another, you can’t expect everything will be translated.  However, this new technique can be an incredible time saver in addition to giving us capabilities to continue and augment simulations that were previously performed in NASTRAN, now in ANSYS.

Here is an example of this new procedure.  (Note that we don’t have NASTRAN here at PADT, so I couldn’t create a generic sample of a NASTRAN model in NASTRAN.  Instead, I created a model in ANSYS, then converted it into NASTRAN using ANSYS FE Modeler to get a NASTRAN input file for the purpose of this exercise.)

Once I have the NASTRAN input file that I need to convert into ANSYS Mechanical, I launch ANSYS Workbench 16.0 and insert an External Model branch.  I then click the … button to browse to the NASTRAN input file.  In this case, the file is NASTRAN.nas.

nastran-ansys-external-model-f1

Next, I drag and drop a new analysis type block into the Project Schematic.  In this case, it was a modal analysis.  Note that you can’t drop this onto the Setup cell in the External Model block as you might expect.  You set it up as a separate block and establish the link in the next step.

nastran-ansys-external-model-f2

Next, we drag and drop the Setup cell from the External Model block onto the Model cell of the Modal analysis block.  This establishes the link from the NASTRAN model to the new Modal analysis.

nastran-ansys-external-model-f3

We also need to right click on the Setup cell in the External Model block and select Update to get a green checkmark in that cell:

nastran-ansys-external-model-f4

Notice that there is no Geometry cell in the resulting Modal analysis block.  If all goes well, there will be geometry within the Mechanical model that can be used for selection purposes (in addition to the mesh that comes in from NASTRAN). 

Next we open the Mechanical editor by double clicking on one of the cells in the Modal analysis blocks (other than the Engineering Data cell).  It may take several minutes to bring in the NASTRAN model depending on the size of the NASTRAN model.  The Mechanical window doesn’t really let you know that it’s working, but if it’s sitting there with nothing being displayed, it’s probably churning away at bringing in the NASTRAN mesh and creating surface geometry on it.

Here is what the Mechanical window looks like after the mesh is read in and geometry is automatically created.  This is the mesh from the NASTRAN file, but in this case both solid and surface geometry is also present.  It’s not guaranteed that everything will come across.  I’ve seen contact elements come through for certain types of contact but not for other types of contact for example.

nastran-ansys-external-model-f5

The next image shows that geometry was created that can be used for the purposes of inserting fixed supports, just as if the geometry had come in from a CAD system.  Note that the NASTRAN input file had NO geometry, just finite element entities.  ANSYS is creating the geometry for use in Mechanical from the information in the NASTRAN input file.

nastran-ansys-external-model-f6

Finally, after manually creating a needed contact region, I was able to solve the modal analysis, demonstrating that further simulation can be performed in ANSYS Mechanical from this model which originally came from NASTRAN.

nastran-ansys-external-model-f7

So, the main take away here is that with version 16.0 of ANSYS, we can take a NASTRAN input file and through the use of the External Model block, go directly into ANSYS Mechanical.  Not only do we get the nodes and elements as well as other finite element entities from the NASTRAN model, but if all goes well we get geometry that facilitates further processing within ANSYS Mechanical.

We certainly hope this new capability makes it easier for you to perform additional simulations in ANSYS when the starting point is a NASTRAN model.  The other formats documented for version 16.0 are ABAQUS, Fluent input files, and ICEM CFD input files.

ANSYS 16.0 License Manager – New Look and Feel, New Capabilities

ansys-license-manager-160-tnIf your role includes administering ANSYS licenses, you should be aware that the look and feel of the ANSYS license manager has changed somewhat at version 16.0.  The tasks that used to all be performed within the Server ANSLIC_ADMIN Utility have now been split pretty much between that tool and a new tool that runs within your browser called the ANSYS License Management Center.

The ANSYS License Management Center looks like this:

ansys-license-manager-160-f1

This new License Management Center window is opened on Windows via Start > All Programs > ANSYS, Inc. License Manager > ANSYS License Management Center, and on Linux via /ansys_inc/shared_files/licensing/start_lmcenter.

This utility is where you now install license files, start and start the license manager, and also gather diagnostic information if something goes wrong.  You can also view the license .log files here as well as ANSYS licensing documentation.

The ‘old’ Server ANSLIC_ADMIN Utility is now smaller and does less than it did in prior versions.  This is what it looks like at version 16.0:

ansys-license-manager-160-f2

This window is still useful in that you can click on View Status/Diagnostic Options to get information you can’t get in the new License Management Center, primarily Display the License Status to see what licenses are in use and are available.  This information is also available to clients via the Client ANSLIC_ADMIN Utility.  You can start the ANSYS License Management Center from here too.

One capability you won’t find in either utility is the ability to Reread the License Manager settings.  When you load a new license file, the License Management Center now automatically stops and starts the license manager so you shouldn’t have to do a reread after installing a new file, but just in case, it can still be done via the command line using these instructions:

On Windows, open a command prompt and move to:

C:\Program Files\ANSYS Inc\Shared Files\Licensing\winx64

Then issue the command:

ansysli_server –k reread

The same command works on Linux from the /ansys_inc/shared_files/licensing/linx64 directory.

Another important change is the location of the license files after they have been installed.  The new location is (on Windows):

C:\Program Files\Ansys Inc\Shared Files\Licensing\license_files

This means there is a new sub-folder named license_files that contains the license file(s).  File(s) is now plural since you can have both an ANSYS license file and an Ansoft license file in that folder, both running using the ANSYS License Management Center.  There is a new license file naming convention as well:

ANSYS License file name:  ansyslmd.lic

ANSOFT License file name:  ansoftd.lic

The path on Linux is:

 /ansys_inc/shared_files/licensing/license_files

When you install an ANSOFT license file, the license manager now does some edits to change the daemon to the ANSYS daemon in addition to renaming the file and placing it in the new location. 

One additional piece of information:  The license manager reads any .lic files that are located in the license_files folder, so it’s probably a good idea to ensure that only ‘good’ versions of ansyslmd.lic and ansoftd.lic reside in that folder. 

A major conclusion that can be drawn from all of this is that ANSYS license manager and Ansoft license manager license files can now be managed using a single licensing tool and single set of licensing software.  We’ve been waiting for this for some time and it’s nice to see it’s here and working successfully.

 

10 Useful New Features in ANSYS Mechanical 16.0

ansys-mechanical-16-heade2r

PADT is excited about the plethora of new features in release 16.0 of ANSYS products.  After sorting through the list of new features in Mechanical, here are 10 enhancements that we found to be particularly useful for general applications.


1: Mesh Display Style

This new option in the details view for the mesh branch makes it easy to visualize mesh quality items such as aspect ratio, skewness, element quality, etc.  The default style is body color, but it can be changed in the details to element quality, for example, as shown here:

ansys-mechanical-16-f1a

Figure 1. A. – Mesh Display Style Set to Element Quality

figure1b

Figure 1. B. – Element Quality Plot After Additional Mesh Settings

ansys-mechanical-16-f1c

Figure 1. C. – Accessing Display Style in the Mesh Details


2: Image to Clipboard

How many times have you either done a print screen > paste into editing tool > crop or done an image to file to get the plots you need into tools such as Word and PowerPoint?  The new Image to Clipboard menu pick streamlines this process.  Now, just get the image the way you want it in the geometry view, right click, and select Image to Clipboard.  Or just use Ctrl + C.  When you paste, you’ll be pasting the contents of that view window directly.  Here’s what it looks like:

ansys-mechanical-16-f2

Figure 2 – Right Click, Image to Clip Board


3: Beam Contact Formulation

This was a beta feature at 15.0, but if you didn’t get a chance to try it out, it’s now fully supported at 16.0.  The idea here is that instead of the ‘traditional’ bonded contact methods (using the augmented Lagrange or pure penalty formulation) or the Multi-Point Constraint (MPC) bonded option, we now have a new choice of beam contact.  This option utilizes internally-created massless linear beam elements to connect the two sides of a contact interface together.  This can be more efficient than the traditional formulations and can avoid the over constraints that can happen if multiple contact regions utilizing the MPC option end up generating constraint equations that tend to conflict with each other.

ansys-mechanical-16-f3

Figure 3 – Beam Formulation for Bonded Contact


4: Nonlinear Adaptive Region

If you have ever been frustrated by the error message in the Solution Information window that says, “Element xyz … has become highly distorted…”, version 16.0 adds a new tool to our toolbox with the Nonlinear Adaptive Region capability.  This capability is in its infancy stage at 16.0, but in the right circumstances it allows the solution to recover from highly distorted elements by pausing, remeshing, and then continuing.  We plan on publishing more details on this capability soon, but for now please know that it exists and more can learned in the 16.0 Mechanical Help.  There are a lot of restrictions on when it can work, but a big one is that it only works for elements that become overly deformed due to large and nonuniform deformation, meaning not due to unstable materials, numerical instabilities, or structures that are unstable due to buckling effects.

As shown in figure 4. A., a Nonlinear Adaptive Region can be inserted under the Solution branch.  It is scoped to bodies.  Options and controls are set in the details view.

ansys-mechanical-16-f4a

Figure 4. A. – Nonlinear Adaptive Region

If the solver encounters a ‘qualifying event’ that triggers a remesh, the solver output will inform us like this:

 

**** REGENERATE MESH AT SUBSTEP     5 OF LOAD STEP      1 BECAUSE OF
      NONLINEAR ADAPTIVE CRITERIA

 

 

 

 

AmsMesher(ANSYS Mechanical Solver Mesher),Graph based ANSYS Meshing EXtension,v0.96.03b
(c)ANSYS,Inc. v160-20141009
  Platform           :  Windows 7 6.1.7601
  Arguments          :  F:\Program Files\ANSYS Inc\v160\ANSYS\bin\winx64\AnsMechSolverMesh.exe
                     :  -m
                     :  G:\Testing\16.0\_ProjectScratch\Scr692\file_inpRzn_0001.cdb
                     :  –slayers=2
                     :  –silent=0
                     :  –aconcave=15.0000
                     :  –aconvex=15.0000
                     :  –gszratio=1.0000
  Seed elements      :  _RZNDISTEL block

– 17:6:17 2015-2-11

  ===================================================================
  == Mesh quality metrics comparison                                
  ===================================================================
  Element Average    :  ——–Source——–+——–Target——–
  ..Skewness(Volume) :    4.0450e-001             4.1063e-001        
  ..Aspect Ratio     :    2.3411e+000             2.4331e+000        
  Domain Volume      :    8.6109e-003             8.6345e-003        

  Worst Element      :  ——–Source——–+——–Target——–
  ..Skewness(Volume) :    0.8564  (e552     )      0.7487  (e2217    )   
  ..Aspect Ratio     :    4.9731  (e434     )      6.8070  (e2236    )   

  ===================================================================
  == Remeshing result statistics                                    
  ===================================================================
  Domain(s)          :   1      
  Region(s)          :   1      
  Patche(s)          :   7      
  nNode[New]         :   39      
  nElem[New/Eff/Src] :   79 / 92 / 2076      

  Peak memory        :   10 MB

– 17:6:17 2015-2-11
– AmsMesher run completed in 0.225 seconds

  ========================= End Run =================================
  ===================================================================

 **** NEW MESH HAS BEEN CREATED SUCCESSFULLY. CONTINUE TO SOLVE. 

Results item tabular listings will show that a remesh has occurred, as shown in figure 4. B.

ansys-mechanical-16-f4b

Figure 4. B. – Results Table Indicating a Remesh Occurred in the Nonlinear Adaptive Region

ansys-mechanical-16-f4c

Figure 4. C. – Before and After Remesh Due to Nonlinear Adaptive Region


5: Thermal Fluid Flow via Thermal ‘Pipes’

This has also been a beta option in prior releases, but nicely, at 16.0 it becomes a production feature.  The idea here is that we can use the ANSYS Mechanical APDL FLUID116 elements in Mechanical, without needing a command object.  These fluid elements have temperature as their degree of freedom in this case, and enable the effects of one dimensional fluid flow.  This means we have a reduced order model for capturing heat transfer due to a fluid moving through some kind of cavity without having to explicitly model that cavity.  The pipe ‘path’ is specified using a line body.

The line body gets defined with a cross section in CAD, and is tagged as a named selection in Mechanical.  This thermal pipe can then interact on appropriate surfaces in your model via a convection load.  Once the convection load is applied on appropriate surfaces in your model, the Fluid Flow option can then be set to Yes, and the line body is specified as the appropriate named selection.  Appropriate BC’s need to be applied to the line body, such as temperature constraints and mass flow rate, as shown in figure 5.

ansys-mechanical-16-f5

Figure 5 – Thermal “Pipe” Line Body at Top, Showing Applied Boundary Conditions


6: Solver Pivot Checking Control

This new option under Analysis Settings > Solver Controls allows you to potentially continue an analysis that has stopped due to pivoting issues, meaning a model that’s not fully constrained or one that is having trouble due to contact pairs not being fully in contact. 

The options are Program Controlled, Warning, Error, and Off.  The Warning setting is the one to use if you want the solver to continue after any pivoting issues have occurred.  The Error setting means that the solver will stop if pivoting issues occur.  The Off setting results in no pivot checking to occur, while Program Controlled, which is the default, means that the solver will decide.

ansys-mechanical-16-f6

Figure 6 – Solver Pivot Checking Controls Under Analysis Settings


7: Contact Result Trackers

This new feature allows you to more closely track contact status data while the solution is running, or after it has completed.  This capability uses the .cnd file that is created during the solution in the solver directory.  It is useful because it gives you more information on the behavior of your contact regions during solution so you can have more confidence that things are progressing well or potentially stop the solution and take corrective action if they are not.  The tracker objects get inserted under the Solution Information branch, as shown in figure 7. A.

ansys-mechanical-16-f7a

Figure 7. A. – Contact Trackers Inserted Under Solution Information

A large variety of quantities can be selected to track, such as Number Contacting, Number Sticking, Gap, Penetration, etc.

ansys-mechanical-16-f7b

Figure 7. B. – Contact Results Tracker Settings in the Details View

Contact results tracker quantities can be viewed in real time during the solution, as shown in figure 7. C.

ansys-mechanical-16-f7c

Figure 7. C. – Contact Results Tracker Showing Gap Decreasing as the Solution Progresses


8: Tree Filtering

For large assemblies or other complex models, there are useful enhancements in how the tree can be filtered, including the ability to create Groups.  Groups can consist of tree entities that are geometry, coordinate systems, connection features, boundary conditions, or even results.  Grouping is accomplished as easily as selecting the desired items in the tree, then right clicking to specify Group, as shown in Figure 8. A.

ansys-mechanical-16-f8a

Figure 8. A. – Grouping Displacements

A new folder in the tree is then created which can be named something useful.  Figure 8. B. shows the displacement boundary condition group (folder) after it was given a name.

ansys-mechanical-16-f8b

Figure 8. B. – Group of Displacement BC’s, Given a Meaningful Name

It’s easy to right click and Ungroup if needed, and there is also a Group Similar Objects option which allows you to select just one item in the tree and easily group all similar items by right clicking.


9: Results Set Listing Enhancements

In addition to the information on remeshing that we mentioned back in useful new feature number 4, there is a new capability to right click in the tabular listing of results and then right click to create total deformation or equivalent stress results.  This capability can make it faster to create a deformation or stress plot for a particular time point or result set of interest.

The procedure to do this is:

  • Left click on the Solution branch in the tree.
  • Left click on the desired Results set in Tabular Data
  • Right click on that results set and select Create Total Deformation Results or Create Equivalent Stress Results, as shown in figure 9.

The result of these steps will be a new result item in the tree, waiting for you to evaluate so you can see the new results plot.

ansys-mechanical-16-f9

Figure 9 – Right Click in Solution Tabular Data to Create Deformation or Equivalent Stress Result Items


10: Explode View

We’ve saved a fun one for last, the new Explode View capability.  This allows you to incrementally ‘explode’ the view of your assemblies, making it potentially easier to visualize the parts and interaction between parts that make up the assembly.  To use this feature, make sure the Explode View Options toolbar is turned on in your View settings.  There are several options for the ‘explosion center’, such as the assembly center or the global or a user defined coordinate system.

ansys-mechanical-16-f10a 

Figure 10. A. – The Explode View Options Toolbar

As you can see in figure 10. A., there is a slider that allows you to control the ‘level’ of view explosion.  Keep in mind this is just a visual tool and does nothing to the coordinates of the parts in your assemblies.

Figures 10. B. and 10. C. show various slider settings for the exploded view of an assembly.

ansys-mechanical-16-f10b

Figure 10. B. – Explode View Level 3

ansys-mechanical-16-f10c

Figure 10. C. – Explode View Level 4


This concludes our tour of 10 useful new features in ANSYS Mechanical 16.0.  We hope you find this information helps you get your ANSYS Mechanical simulations completed more efficiently.  There are lots and lots of other new features that we didn’t mention here.  The Release Notes in the Help covers a lot of them.  We’ll be writing more about some of the things we mentioned here as well as some of the other new features soon.  

Thermal Submodeling in ANSYS Workbench Mechanical 15.0

thermal-submodeling-18
If you've been following The Focus for a long time, you may recall my prior article about submodeling using ANSYS Mechanical APDL, which was a 'sub' model of a submarine.  The article, from 2006, begins on page 2 at this link:

Also, Eric Miller here at PADT wrote a Focus blog entry on the new-at-14.5 submodeling capability in ANSYS Workbench Mechanical.

Since both of those articles were about structural submodeling, I decided it was time we published a blog entry on how to perform submodeling in ANSYS Mechanical for thermal simulations.

Submodeling is a technique whereby we can obtain more accurate results in a small, detailed portion of a large model without having to build an incredibly refined and detailed finite element model of our complete system.  In short, we map boundary conditions onto a 'chunk' of interest that is a subset of our full model so that we can solve that 'chunk' in more detail.  Typically we mesh the 'chunk' with a much finer mesh than was used in the original model, and sometimes we add more detail such as geometric features that didn't exist in the original model like fillets.

The ANSYS Workbench Project Schematic for a thermal solution involving submodeling looks like this:

thermal-submodeling-1

Figure 1 – Thermal Submodeling Project Schematic

Note that in the project schematic, the links are automatically established when we setup the submodel after completing the analysis on the coarse model as we shall see below.

First, here is the geometry of the coarse model.  It's a simple set of cooling fins.  In this idealized model, no fillets have been modeled between the fins and the block.

thermal-submodeling-2

Figure 2 – Coarse Model Geometry, Idealized without Fillets

The boundary conditions consisted of a heat flux due to a  thermal source on the base face and convection to ambient air on the cooling fin surfaces.  The heat flux was setup to vary over the course of 3 load steps as follows:

Load Step        Heat Flux (BTU/s*in^2)

            1                      0.2

            2                      0.5

            3                      0.005

Thus, the maximum heat going into the system occurs in load step 2, corresponding to 'time' 2.0 in this steady state analysis.

thermal-submodeling-3

Figure 3 – Coarse Model Boundary Conditions – Heat Flux and Convection

The coarse model is meshed with relatively large elements in this case.  The mesh refinement for a production model should be sufficient to adequately capture the fields of interest in the locations of interest.  After solving, the temperature results show a max temperature at the base where the heat flux is applied, transitioning to the minimum temperature on the cooling fins where convection is removing heat.

thermal-submodeling-4

Figure 4 – Coarse Model Mesh and Temperature Results for Load Step 2

Our task now is to calculate the temperature in one of these fins with more accuracy.  We will use a finer mesh and also add fillets between the fin and base.  For this example, I isolated one fin in ANSYS DesignModeler, did some slicing, and added a fillet on either side of the base of the fin of interest.

thermal-submodeling-5

Figure 5 – Fine Model (Submodel) Isolated Fin Geometry and Mesh, Including Fillets at Base

 

ANSYS requires that the submodel lie in the exact geometric position as it would in the coarse model, so it's a good idea to overlay our fine model geometry onto the coarse model to verify the positioning.

thermal-submodeling-6

Figure 6 – Submodel and Coarse Model Overlaid

thermal-submodeling-7

Figure 7 – Submodel and Coarse Model Overlaid, Showing Addition of Fillet

The next step is to insert the submodel geometry as a stand-alone geometry block in the Project Schematic which already contains the coarse model, as shown in figure 8.  A new Steady-State Thermal analysis is then dragged and dropped onto the geometry block containing the submodel geometry.

thermal-submodeling-8

Figure 8 – Submodel Geometry Added to Project Schematic, New Steady-State Thermal System Dragged and Dropped onto Submodel Geometry

 

Next, we drag and drop the Engineering Data cell from the coarse model to the Engineering Data cell in the submodel block.  This will establish a link so that the material properties will be shared.

thermal-submodeling-9

Figure 9 – Drag and Drop Engineering Data from Coarse Model to Submodel

The final needed link is established by dragging and dropping the Solution cell from the coarse model onto the Setup cell in the submodel.  This step causes ANSYS to recognize that we are performing submodeling, and in fact this will cause a Submodeling branch to appear in the outline tree in the Mechanical window for the submodel.

thermal-submodeling-10

Figure 10 – Solution Cell Dragged and Dropped from Coarse Model to Submodel Setup Cell

After opening the Mechanical editor for the submodel block, we can see that the Submodeling branch has automatically been added to the tree.

thermal-submodeling-11

Figure 11 – Submodeling Branch Automatically Added to Outline Tree

After meshing the submodel I specified that all three load steps should have their temperature data mapped to the submodel from the coarse model.  This was done in the Details view for the Imported Temperature branch, by setting Source Time to All.

thermal-submodeling-12

Figure 12 – Set Imported Temperature Source Time to All to Ensure All Loads Steps Are Mapped

Next I selected the four faces that make up the cut boundaries in the submodel and applied those to the geometry selection for Imported Temperature.

thermal-submodeling-13

Figure 13 – Cut Boundary Faces Selected for Imported Temperature

 

As mentioned above, the Imported Temperature details were set to read in all load steps by setting Source Time to All.  The Imported Temperature branch can now be right-clicked and the resulting imported temperatures viewed.  I also inserted a Validation branch which we will look at after solving.

thermal-submodeling-14

Figure 14 – Setting Source Time to All, Viewing Imported Temperature on Submodel

Any other loads that need to be applied to the submodel are added as well.  For this model, it's convection on the large faces of the fin that are exposed to ambient air.

thermal-submodeling-15

Figure 15 – Submodel Convection Load on Fin Exposed Faces

Since there are three load steps in the coarse model and we told ANSYS to map results from all time points, I set the number of steps to three in Analysis Settings, then solved the submodel.  Results are available for all three load steps.

thermal-submodeling-16

Figure 16 – Submodel Temperature Results for Step 2 (Highest Heat Flux Value in Coarse Model)

Regarding the Validation item under the Imported Temperature branch, this is probably best added after the solution is done.  In my case I had to clear it and recalculate it.  Validation can display either an absolute or relative (percent difference) plot on the nodes at which loads were imported.  Figure 17 shows the relative difference plot, which maxes out at about 6%.  The validation information as well as mapping techniques are described in the ANSYS Help.

thermal-submodeling-17

Figure 17 – Submodel Imported Temperature Validation Plot – Percent Difference on Mapped Nodes

Looking at the coarse model and submodel results side by side, we see good agreement in the calculated temperatures.  The temperature in the fillets shows a nice, smooth gradient.

thermal-submodeling-18

Figure 18 – Coarse and Submodel Temperature Results Showing Good Agreement

Hopefully this explanation will be helpful to you if you have a need to perform submodeling in a thermal simulation in ANSYS.  There is a Thermal Submodeling Workflow section in the ANSYS 15.0 Help in the Mechanical User's Guide that you may find helpful as well.

 

 

 

Configuring Laptop “Switchable” Graphics for ANSYS Applications

IMG_4894

A lot of laptops these days come with “switchable” graphics.  The idea is that you have a lower capability but also lower power consuming ‘basic’ graphics device in addition to a higher performing but higher power demand graphics device.  By only using the higher performance graphics device when it’s needed, you can maximize the use time of a battery charge. 

A lot of the ANSYS graphics-intensive applications may need the higher end graphics device to display and run correctly.  In this article, we’ll focus on the AMD Firepro as the “higher end” graphics, with Intel HD graphics as the “lower end”.  We will show you how to switch to the AMD card to get around problems or errors in displaying ANSYS user interface windows.

The first step is to identify the small red dot graphics icon at the lower right in the task bar:

fix_laptop_graphics_ansys-01

Figure 1 – AMD Catalyst Icon

 

Next, right click on the icon to bring up the AMD Catalyst Control Center, if you don’t see the switchable option as shown two images down.

fix_laptop_graphics_ansys-02

Figure 2 – AMD Catalyst Control Center Right Click Menu Pick

 

Right click on the same icon again, if needed to select “Configure Switchable Graphics,” as shown here:

fix_laptop_graphics_ansys-03

Figure 3 – Select “Configure Switchable Graphics” via Right Click on the Same Icon

 

In the resulting AMD Catalyst Control Center window, click on the Add Application button.

fix_laptop_graphics_ansys-04

Figure 4 – AMD Catalyst Control Center Window

Next browse to the application that needs the higher end graphics capability.  This might take a little trial and error if you don’t know the exact application.  Here we select ANSYS CFD-Post and click Open.

fix_laptop_graphics_ansys-05

Figure 5 – Selecting appropriate executable for switchable graphics

Finally, select the High Performance option from the dropdown for your chosen executable, then click the Apply button.

fix_laptop_graphics_ansys-06

This should get your graphics working properly.  Again, the reason we have the two graphics choices is to allow us to better control power consumption based on the level of graphics that are needed per application.  Hopefully this article helps you to choose the proper graphics settings so that your ANSYS tools behave nicely on your laptop.

ANSYS Workbench Installations and RedHat 6.6 – Error and Workaround

penguin_shWe were recently alerted by a customer that there is apparently a conflict with ANSYS installations if Red Hat Enterprise Linux 6.6 (RHEL 6.6) is installed. We have confirmed this here at PADT. This effects several versions of ANSYS, including 15.0.7, 14.5, and 14.0. The primary problem seems to be with meshing in the Mechanical or Meshing window.

The windows errors encountered can be: “A software execution error occurred inside the mesher. The process suffered an unhandled exception or ran out of usable memory.” or “an inter-process communication error occurred while communicating with the MESHER module.”

The error message popup can look like this:
th1

or
th2

th3
Note that the Platform Support page on the ANSYS website does not list RHEL 6.6 as supported. RHEL is only supported up through 6.5 for ANSYS 15.0. This is the link to that page on the ANSYS website:

http://www.ansys.com/staticassets/ANSYS/staticassets/support/r150-platform-support-by-application.pdf

That all being said, there is a workaround that should allow you to continue using ANSYS Workbench with RHEL 6.6 if you encounter the error. It involves renaming a directory in the installation path:

In this directory:

/ansys_inc/v150/commonfiles/MainWin/linx64/mw/lib-amd64-linux/

Rename the folder ‘X11’ to ‘Old-X11’

After that change, you should be able to successfully complete meshes, etc,. in ANSYS Workbench. Keep in mind that RHEL 6.6 is not officially supported by ANSYS, Inc. and their recommendation is always to stick with supported levels of operating systems. These are always listed in the ANSYS Help for the particular version you are running as well as at the link shown above.

Since the renamed directory is contained within the ANSYS installation files, it is believed that this will not affect anything else other than ANSYS. Use at your own risk, however. Should you encounter one of more of the errors listed above, we hope this article has provided useful information to keep your ANSYS installations up and running.

ANSYS SpaceClaim and Mechanical, Plus 3D Printing to the Rescue!

p0One of the great things about working at a company like PADT is that we have the ability to solve problems from start to finish.  By start to finish, I mean: 

  1. Recognize a need
  2. Design a solution
  3. Verify the solution
  4. Manufacture the solution
  5. Deploy the solution

There are other steps that could be added such as optimization and field verification, but in simple terms those steps outline the product development process.  We do this very often at PADT, helping a wide variety of customers develop products to meet needs in the marketplace.  Most of the time, we can’t share the work we do publicly, for obvious reasons involving customer confidentiality. 

So, when we can share, it’s a good opportunity to show what our tools can do, as well as how we can utilize these tools to help our customers with the steps listed above.  We’ll look at a simple example, knowing that the same tools can help with much more complex problems.

In my case, I was faced with a problem.  We recently had our back yard pool deck resurfaced.  The problem at hand was the contractors accidently lost a plastic lid that covered a 5.5 in. hold on the deck of the pool.  This hole was for something like a basketball hoop that could be dropped into this trumpet shaped hole.  Figure 1 shows the work in progress, when the original lid was still in place.

p1Figure 1 – Original lid circled in red.

After the cleanup was done, that lid was nowhere to be found.  You would think it would be simple to find a replacement, especially in metro Phoenix where pool supply stores are abundant.  However, after visiting several supply stores as well as scouring the internet, we could not find a replacement 5.5 in. lid.  All the available lids were too big and would not work in covering this hole.  The hole without a lid is a safety concern.  In fact, our 4 year old niece managed drop a foot into the hole and ended up with a scrape.  Fortunately it wasn’t any worse than that.

Unable to find a suitable lid for purchase, I decided to pursue a 3D printed solution here at PADT.  As I’m sure you are aware, 3D printing has been portrayed all over the media in the last couple of years.  For us here at PADT, though, it has been a significant component of our business since the company’s founding in 1994.  Knowing that I could have this part printed in plastic here at PADT, I decided to go through the product development process as listed above.

So, let’s look at the various steps I followed in our product development process:

  1. Recognize a need.

In this case, it was simple.  We had a hole in the pool deck that was a safety issue.  No replacement part could be found.  A new lid was needed, one that would fit properly but also could support the weight of someone walking over it.  I decided to design a replacement part that could be 3D printed by one of the rapid prototyping technologies we have available here at PADT.

  1. Design a solution

Besides providing 3D printing services and selling 3D printers, we at PADT are a Channel Partner for ANSYS engineering simulation tools here in the Southwest.  I leveraged ANSYS, Inc.’s latest acquisition, the SpaceClaim Direct Modeler as my design tool.  SpaceClaim has been available as part of the ANSYS software suite for several years, but now SpaceClaim is officially part of the ANSYS corporate umbrella.  SpaceClaim runs within the ANSYS Workbench platform, like the ‘older’ ANSYS geometry tool, DesignModeler.  A main different between the two geometry toolsets is that DesignModeler is a history-based modeler, meaning it has a history tree that is followed to create and modify the geometry as we go along.  This works well in many circumstances but it lacks the ability to quickly and easily modify existing geometry.  SpaceClaim, on the other hand, is a direct modeler in the sense that we work on the geometry interactively, allowing us to rapidly modify geometry by ‘pulling’ on surfaces to grow, shrink, fillet, etc.  SpaceClaim is incredibly fast once we get familiar with it.

Knowing that the diameter of the hole was 5.5 inches as measured by a ruler, along with a memory of what the prior cover looked like, I turned to ANSYS SpaceClaim to come up with the geometry model.  I sketched a 2D axisymmetric cross section and swept that 360 degrees about an axis to come up with the solid model.  I very easily moved the 5.5 in diameter face inward by a small amount to allow for some clearance between the plastic part and the hole into which it needs to fit.  The geometry definition literally took just a few minutes, even though I am not yet an expert in SpaceClaim.

p2Image 2 – ANSYS SpaceClaim solid model

p3Image 3 – Cross section shown in SpaceClaim

  1. Verify the solution

I mentioned optimization as a step that could be followed.  In this simple case, I didn’t do any optimization but did perform verification that my design would meet an acceptability requirement.  I wanted to make sure that my plastic lid could support the weight of an adult standing on it.  The tool I used to perform this verification was the ANSYS Mechanical software tool.  Like SpaceClaim can, ANSYS Mechanical runs within the ANSYS Workbench environment, meaning that the geometry and subsequent stress and deflection analyses are linked.  This allows any needed changes to the geometry to quickly and easily pass from the geometry tool to the stress/deflection model, often with as little as one click of the mouse.

Getting the geometry into the Mechanical model for a finite element simulation was therefore quite simple.  Defining loads and constraints on my system was also quite simple.  What remained was to define material properties to characterize the plastic being used.  PADT’s Rapid Prototyping team informed me that the material to be used is one called Veroclear.  This material is used in one of PADT’s 3D printers, called an Objet from Statasys. 

Basic material properties for Veroclear are available on the internet, including Young’s Modulus and Yield Strength.  Poisson’s Ratio was not available so it was assumed to be 0.3.  These properties were entered into ANSYS Workbench.  For those not familiar, Young’s Modulus is a quantification of the stiffness of a material.  The Yield Strength is a measure of the how much stress a material can experience before permanent deformation occurs.  Stress, simply put, is the amount of force being carried per area in a structure.  Poisson’s Ratio relates how much a material squishes in one direction when it’s pulled in another dimension.

The loading consisted of a 210 lb. downward load on a portion of the upper surface, representing someone standing on the middle of the lid.  The constraints were frictionless supports on the outer cylindrical face as well as the bottom lip.  These constraints simulate where these two surfaces touch the hard surface of the pool deck.

p4Figure 4 – Applied Loads and Constraints

Once the model was fully setup in ANSYS Mechanical, the solution was obtained.  Lots of matrix algebra behind the scenes takes care of solving the equations needed to obtain the solution.  The resulting deflections and stresses looked to be acceptable.  I also calculated a factor of safety, relating the calculated stress in the model to the Yield Strength as described above.  A factor of safety of 2, for example, means that the predicted stress in the model is half of the Yield Strength.  The calculated factor of safety for the plastic lid is 3.17. 

p5Figure 5 – Calculated Deflections, showing maximum of 0.044 in. in center of lid.

p6Figure 6 – Equivalent Stress Distribution

p7Figure 7 – Factor of Safety Distribution

From these results we can conclude that, for the loading condition we considered:

  1. The deflections are fairly minimal
  2. The stresses are below the Yield Stress
  3. The minimum factor of safety value of 3.17 gives us confidence that under reasonable loadings, the part will not fail.

Note that this is a simplistic look at the feasibility of our design.  We didn’t consider what happens to the plastic in the hot sun, what happens if something heavy falls on the lid, etc.  Many other factors could be considered, but in this case I chose to keep it simple.

  1. Manufacture the solution

The part was printed over a weekend in an Objet printer here at PADT.  The geometry was saved as a Parasolid file in ANSYS SpaceClaim, and the Parasolid file was then provided to PADT’s Rapid Prototyping team, via the rp@padtinc.com email.  While the cost of making this particular plastic part using 3D printing is likely too high for a production run, the technology is perfect for making test articles, prototypes, molds, etc. 

p8Figure 8 – The part as printed by the Objet 3D printer (with a few water spots)

  1. Deploy the solution

In this case I only needed one lid, so I took care to make sure that the geometry was accurate before the CAD definition was sent to the 3D printer.  The proof is always in the pudding, so to speak, so it was a great comfort to see that the new plastic lid fit perfectly in the hole in the pool deck.  If this were a production part, we would probably need a vendor to mold the plastic lids in large batches to make them cost effective.

p9Figure 9 – Plastic lid in place

So, we ended up with a part the met the need, each step done very quickly using the appropriate tools in conjunction with the knowledge of how to use them.  We hope you have enjoyed this tour of the product design process, for this simple example.  Please keep PADT in mind for your product development needs.

Default Contact Stiffness Behavior for Bonded Contact

p7It recently came to my attention that the default contact stiffness factor for bonded contact can change based on other contact regions in a model. This applies both to Mechanical as well as Mechanical APDL. If all contacts are bonded, the default contact stiffness factor is 10.0. This means that in our bonded region, the stiffness tending to hold the two sides of contact together is 10 times the underlying stiffness of the underlying solid or shell elements.

However, if there is at least one other contact region that has a type set to anything other than bonded, then the default contact stiffness for ALL contact pairs becomes 1.0. This is the default behavior as documented in the ANSYS Mechanical APDL Help, in section 3.9 of the Contact Technology Guide in the notes for Table 3.1:

“FKN = 10 for bonded. For all other, FKN = 1.0, but if bonded and other contact behavior exists, FKN = 1 for all.”

So, why should we care about this? It’s possible that if you are relying on bonded contact to simulate a connection between one part and another, the resulting stress in those parts could be different in a run with all bonded contact vs. a run with all bonded and one or more contact pairs set to a type other than bonded. The default contact stiffness is now less than it would be if all the contact regions were set to bonded.

This can occur even if the non-bonded contact is in a region of the model that is in no way connected to the bonded region of interest. Simply the presence of any non-bonded contact region results in the contact stiffness factor for all contact pairs to have a default value of 1.0 rather than the 10.0 value you might expect.

Here is an example, consisting of a simple static structural model. In this model, we have an inner column with a disk on top. There are also two blocks supporting a ring. The inner column and disk are completely separate from the blocks and ring, sharing no load path or other interaction. Initially all contact pairs are set to bonded for the contact type. All default settings are used for contact.
p1

Loading consists of a uniform temperature differential as well as a bearing load on the disk at the top. Both blocks as well as the column have their bases constrained in all degrees of freedom.
p2

After solving, this is the calculated maximum principal stress distribution in the ring. The max value is 41,382.
p3

Next, to demonstrate the behavior described above, we changed the contact type for the connection between the column and the disk from bonded to rough, all else remaining the same.
p4

After solving, we check the stresses in the ring again. The max stress in the ring has dropped from 41,283 to 15,277 as you can see in the figure below. Again, the only change that was made was in a part of the model that was in no way connected to the ring for which we are checking stresses. The change in stress is due solely to a change in contact type setting in a different part of the model. The reason the stress has decreased is that the stiffness of the bonded connection is less by a factor of 10, so the bonded region is a softer connection than it was in the original run.

p5

So, what do we as analysts need to do in light of this information? A good practice would be to manually specify the contact stiffness factor for all contact pairs. This behavior only crops up when the default values for contact stiffness factor are utilized. We can define these stiffness factors easily in ANSYS Mechanical in the details view for each contact region. Further, we need to always remember that ANSYS as well as other analytical tools are just that – tools. It’s up to us to ensure that the results of interest we are getting are not sensitive to factors we can adjust, such as mesh density, contact stiffness, weak spring stiffness, stabilization factors, etc.

Using Probes to Obtain Contact Forces in ANSYS Mechanical

Recently we have had a few questions on obtaining contact results in ANSYS Mechanical. A lot of contact results can be accessed using the Contact Tool, but to obtain contact forces we use Probes. Since not everyone is familiar with how it’s done, we’ll explain the basics here.

Below is a screen shot of a Mechanical model involving two parts. One part has a load that causes it to be deflected into the other part.

p1

We are interested in obtaining the total force that is being transmitted across the contact elements as the analysis progresses. Fortunately this is easy to do using Probes in Mechanical.

The first thing we do is click on the Solution branch in the tree so we can see the Probes button in the context toolbar. We then click on the Probe drop down button and select Force Reaction, as shown here:

p2

Next, we click on the resulting Force Reaction result item under the Solution branch to continue with the configuration. We first change the Location Method from Boundary Condition to Contact Region:

p3

We then specify the desired contact region for the force calculation from the Contact Region dropdown:

p4

Note that the coordinate system for force calculation can either be Cartesian or Cylindrical. You can setup a coordinate system wherever you need it, selectable via the Orientation dropdown.

There is also an Extraction dropdown with various options for using the contact elements themselves, the elements underlying the contact elements, or the elements underlying the target elements (target elements themselves have no reaction forces or other results calculated). Care must be taken when using underlying elements to make sure we’re not also calculating forces from other contact regions that are part of the same elements, or from applied loads or constraints. In most cases you will want to use either Contact (Underlying Element) or Target (Underlying Element). If contact is non-symmetric, only one of these will have non zero values.

In this case, the setting Contact (Contact Element) was a choice that gave us appropriate results, based on our contact behavior method of Asymmetric:

p5

Here are the details including the contact force results:

p6

This is a close up of the force vs. ‘time’ graphs and table (this was a static structural analysis with a varying pressure load):

p7
p8


***** SUMMATION OF TOTAL FORCES AND MOMENTS IN THE GLOBAL COORDINATE SYSTEM *****

FX = -0.4640219E-04
FY = -251.1265
FZ = -0.1995618E-06
MX = 62.78195
MY = -0.1096794E-04
MZ = -688.9742
SUMMATION POINT= 0.0000 0.0000 0.0000

We hope this information is useful to you in being able to quickly and easily obtain your contact forces.

Slide Rules, Logarithms, and Compute Servers

If any of you have been to PADT’s headquarters in Tempe, Arizona, you probably noticed the giant slide rule in the middle of our building.  You can see a portion of it in the picture below, at the top of our Training, Mentoring, and Support group picture.

PADT-TechSupport-Team-Prop

This thing is huge, over 6 feet (2 m) from side to side, in its un-extended position hanging on the wall.

In theory a gigantic slide rule could provide more accuracy, but our trophy, a Kueffel & Esser model 68 1929 copyrighted 1947 and 1961, was intended for teaching purposes in classrooms.  Most engineers had essentially pocket size or belt holder sized slide rules, also known as slip sticks. 

For the real thing, here is a picture of a slide rule used by Eric Miller’s father Col. BT Miller while at West Point from 1955 to 1958 as well as during his Master’s program in 1964.

Burt-Miller-SlideRule-D2

Why do we care about the slide rule today?  Have you ever seen World War II aircraft, submarines, or aircraft carriers?  These were designed using slide rules and/or logarithms.  The early space program?  Slide rules were used then too.  Some phenomenal engineering was accomplished by our predecessors using these devices.  Back then the numerical operations were just a tool to utilize their engineering knowledge.  Now I think we have a tendency to focus on the numerical due to its ease of use and impressive presentation, while perhaps forgetting or at least de-emphasizing the underlying engineering.  That’s not to say that we don’t have great engineers out there; rather it’s a call to energize you all to remember, consider, and utilize your engineering knowledge as you use your simulation tools.

By contrast, here is a picture of PADT’s brand new server room, with cluster machines being put together in the big cabinets.  Hundreds of cores.

servers

What about the giant slide rule?

My father found a thick book at an estate sale a few months ago.  There are a lot of retirees living in Arizona, so estate sales are quite common and popular.  They occur at a life stage when due to death or the need for assisted living, folks are no longer able to live in their home so the contents are sold, clearing out the home and generating some cash for the family.  This particular estate sale was for a retired engineer.  The book caught my father’s eye, first because it was quite thick and second because the title was, Mechanical Engineers’ Handbook.  Figuring it was a bargain for the amazing price of $1.00, he bought it for me.  This book is better known as Marks’ Handbook.  It’s apparently still in publication, at least as late as the 11th Edition in 2006, but the particular edition my father bought for me is the Fifth Edition from 1951.

marks-handbook

Although the slide rule is mostly a curiosity to us today, in 1951 it was state of the art for numerical computation.  While Marks’ has a couple of paragraphs on “Computing Machines”, described as “electrically driven mechanical desk calculators such as the Marchant, Monroe, or Friden”, the slide rule was what I will call the calculator of choice by mechanical engineers at the beginning of the 2nd half of the 20th century. 

As an aside, these mechanical calculators performed multiplication and division, using what I will describe as incredibly complex mechanisms.  Here is a link to a Wikipedia article on the Marchant Calculator:  http://en.wikipedia.org/wiki/Marchant_Calculator

Marks’ Handbook devotes about 3 pages to the operation of the slide rule, starting with simple multiplication and division and then discussing various methods of utilization and various types of slide rules.  It starts off by stating, “The slide rule is an indispensable aid in all problems in multiplication, division, proportion, squares, square roots, etc., in which a limited degree of accuracy is sufficient.” 

The slide rule operates using logarithms.  If you’re not familiar with using logarithms then you are probably younger than me, since I recall learning them in math class in probably junior high in the late 1970’s.  The slide rule uses common logarithms, meaning the log of a number is the exponent needed to raise a base of 10 to get that number.  For example, the common log of 100 is 2.  The common log table in the 1951 edition of Marks shows us that the common log of 4.44 is 0.6474.  For the sake of completeness, the ‘other’ logarithm is the natural log, meaning the base is the irrational number e, approximated as 2.718.

log-table

Getting back to common (base of 10) logs, the math magic is that logarithms allow for shortcuts in fairly complex computations.  For example, log (ab) = log a + log b.  That means if we want to multiple two fairly complicated numbers, we can simply look up the common log of each and add them together.  Similarly, log (a/b) = log a – log b. 

Here is an example, which I will keep simple.  Let’s say we want to multiple 0.0512 by 0.624.  On a calculator this is simple, but what if you are stranded on a remote island and all you have is a log table?  Knowing the equations above, you can look up the log of 0.0512 which is 0.7093-2 and the log of 0.624 which is 0.7952-1.  We now add:
adding_numbers

Writing that sum as a positive decimal minus an integer is important to being able to look up the antilogarithm or number whose log is 0.5045 – 2.

Looking up the number whose log is 0.5045 we get 3.195, using a little bit of linear interpolation.  The “-2” tells us to shift the decimal point to the left twice, meaning our answer is 0.003195.  Thus, using a little addition, some table lookup, a bit of in the head interpolation, and some knowledge on how to shift decimal points, we fairly easily arrive at the product of two three digit fractional numbers.  Now you are free to look for more coconuts on the island.  Or maybe get back to a hatch in the ground where you need to type in the numbers 4, 8, 14, 16, 23, and 42 every 108 minutes.  Oops, I’m really becoming Lost here…

sliderule-book

Getting back to the slide rule, one way to think of it is a graphical representation of the log tables.  In its most basic form, the slide rule consists of two logarithmic scales.  By lining up the scales, the log values can be added or subtracted.  For example, if we want to multiply something simple, like 4 x 6, we simply look from left to right on the scale on the ‘fixed’ portion of the slide rule to get to 4, then slide the moving portion of the slide so that its 1 lines up with the 4 found above on the fixed portion.  We then move left to right on the movable scale to find the 6.  Where the 6 on the movable slide lines up with on the fixed portion is our solution, 24.  What we’ve really done is add the log of 4 to the log of 6 and then find the antilog of that result, which is 24.  Now that we’ve found 24, we’re not Lost

We don’t intend to give detailed instructions on all phases of performing calculations using slide rules here, but hopefully you get the basics of how it is done.  There are plenty of online resources as well as slide rule apps that provide all sorts of details.  Besides multiplication and division, slide rules can be used for squares and square roots.  There are (were) specialty slide rules for other purposes.  Note that with additional knowledge and skill in visually interpolating on a log scale, up to 3 or even 4 significant digits can be determined depending on the size of the slide rule.

ted-slide-ruleThe author, attempting to prove that 4 x 6 is indeed 24

After having studied the Marks’ section on slide rules, experimenting with a slide rule app on an iPad as well as the PADT behemoth on the wall, I conclude that it was a very elegant method for calculating numbers much more quickly than could be done by traditional pencil and paper.  It’s must faster to add and subtract vs. complicated multiplication and long division.  My high school physics teacher actually spent a day or two teaching us how to use slide rules back in the early 1980’s.  By then they had been made functionally obsolete by scientific calculators, so looking back it was perhaps more about nostalgia than the math needed.  It does help me to appreciate the accomplishments made in science and engineering before the advent of numerical computing.

The preparation of this article has made me wonder what the guys and gals who used these tools proficiently back in the 1930’s, 40’s, and 50’s would think if they had access to the kind of compute power we have available today.  It also makes me wonder what people will think of our current tools 50 or 60 years from now.  When I first started in simulation over 25 years ago, it would have seemed quite a stretch to be able to solve simultaneously on hundreds if not thousands of compute cores as can be done today.  Back then we were happy to get time on the one number cruncher we had that was dedicated to ANSYS simulation.

Incidentally, this article was inspired by my colleague David Mastel’s recent blog entry on numerical simulation and how PADT is helping our customers take compute servers and work stations to the next level:

http://www.padtinc.com/blog/the-focus/launch-leave-forget-hpc-and-it-ansys

If you are ever in our PADT headquarters building in Tempe, don’t forget to look for the giant slide rule.  Now you will know its original purpose.