In case you missed it, Doug Oatis wrote a Focus blog entry on general use of element birth and death in ANSYS Workbench back in November, 2011, which you can access here: 
http://www.padtinc.com/blog/post/2011/11/29/Sifting-through-the-wreckage-Element-Birth-and-Death-in-Workbench.aspx

This new article narrows the focus to contact elements specifically.  We recently had a tech support question about how to utilize element birth and death for contact elements in ANSYS Workbench.  So, a simple example was put together and is explained below. 

The main idea is that we need multiple load steps (labeled Steps in Workbench) in order for elements to change status from alive to dead or vice versa.  We also need a way to select the elements so that we can identify which ones will be killed or made alive.

Keep in mind that ANSYS Workbench Mechanical is a newer pre- and post-processor for good old ANSYS Mechanical APDL.  That means we can insert ANSYS commands into the object tree in Workbench Mechanical and those commands will be executed when the solver reads the batch input file that is created when we click the solve button.

So, we need at least one set of Mechanical APDL commands to identify which contact/target pairs or contact regions we need to kill or make alive.  In our example we’ll focus on killing elements but the same principal applies to making killed elements come alive.  Note that killing elements does not remove them from the model.  Rather, it reduces their stiffness by a default value of six orders of magnitude so that effectively they do not participate.  The Mechanical APDL commands needed are for the contact/target pair identification are scalar parameter commands. 

ANSYS Workbench employs some ‘magic’ parameter names that automatically plug in the integer pointers used behind the scenes for identification of element types and material properties.  In the case of contact and target elements, these parameter names are 'cid’ for the contact elements and ‘tid’ for the target elements.  Thus, for each contact region we want to be able to kill, we need to create unique scalar parameter names, such as:

mycont=cid
mytarg=tid

If we had more than one pair, we might use

mycont1=cid
mytarg1=tid

and increment the ‘1’ in the parameter names on the left side for each contact pair so that we end up with mycont1, mycont2, etc.

These commands need to be inserted directly under each desired contact region so that they will be located in the appropriate place in the solver batch input file at solution time.

The next command snippet needed is the one that selects the desired contact and target elements and then employs the ANSYS Mechanical APDL command to kill them.  Finally we need to re-select all the elements in the model so that they are all active when the solution takes place.  An example of this command object is:

esel,s,type,,mycont
esel,a,type,,mytarg

!kill selected elements (contact and target)
ekill,all

!select everything
allsel

Note that anything that occurs to the left of a “!” is considered a comment.  This second command object needs to be inserted under the analysis type branch.

Next, we need to tell ANSYS to perform at least 2 steps (load steps).  This is accomplished in the Details view for Analysis Settings.  For Step Controls, number of steps needs to be 2 (or more than 2).  Once 2 load steps are specified, we can tell ANSYS to only activate the EKILL command snippet for load step 2.  This is done in the Details view for the command snippet.  Step Selection Mode can be set to By Number and the Step Number set to 2, meaning that the command object will only be active for load step 2.  This will result in the contact elements that have been selected by the above commands being killed in load step 2.

In our example, we have two semicircular rings, connected by contact elements where they touch.  One side of the interface uses bonded contact, active for both loads steps.  The other side of the interface uses frictionless contact, active in load step 1 and killed in load step 2.  We would expect that under a compressive load, the frictionless contacts will prevent penetration in load step 1 but allow penetration in load step 2 since they have been killed.

That is exactly what the results show.  The contact status for the frictionless contact region goes from 2 (sliding) at the end of load step 1 to zero (far or not touching) at the end of load step 2.

Deformation plots indicate that penetration is prevented in load step 1.

In load step 2, penetration is allowed because the contact elements at this location have been killed.

So, here is a fairly simple Workbench Mechanical example of utilizing command objects to select contact and target elements, and to kill those elements using the Mechanical APDL EKILL command.  You can read up on element birth and death in the Mechanical APDL Help for more details on element birth and death.  We hope this is useful information to you.

Anyone who has had to mesh shell assemblies has probably run into trouble with edges that don’t quite line up, edges that meet in the middle of faces and other problems that make the meshing process difficult.  Often geometry operations were required to reconcile those problems and many times significant effort was required to get a continuous mesh.

Another historically used tool to connect shell assemblies was the use of constraint equations to connect edge nodes to surface nodes on the finite element level.  More recently, advances in contact technology have allowed for the use of nonlinear contact elements to connect shell assembly meshes.  Both of those techniques, while useful, have some drawbacks.  For example, constraint equations do not support large rotations of the geometry as the direction of application does not change as nodes rotate.  Also, contact elements increase the computational expense if they can otherwise be eliminated.

ANSYS, Inc. now provides us with another technique for handling shell assembly meshing, called Mesh Connections.  First available in version 13.0 and enhanced in version 14.0, mesh connections use the mesher itself to connect shell assemblies toward the goal of getting a continuous or conformal mesh across the surface bodies that make up the assembly.

Consider this boat hull example.  It consists of panel surfaces defining the hull as well as some stiffening ribs.  All geometry is composed of surface bodies. 

Some of the ribs line up with edges in the hull surfaces, while others do not as shown in the close up image shown below.

We can now create mesh connections in the Connections branch after loading this geometry into the Mechanical editor in Workbench 14.0.

Upon generating the mesh, the mesher will attempt to create a continuous or conformal mesh even though we have do not have intersecting geometry. 

With the default settings, we can see in this image that it did a fairly good job of creating the mesh for the ribs which do not intersect with the hull surfaces.  Nodes on the hull surface were adjusted so that they connect to the rib geometry. 

In this case with relatively little effort we were able to obtain a continuous mesh between the ribs and the hull, even though the several of the ribs shared no intersections with the hull surfaces.  In fact, the mesh connections were able to overcome small gaps in between the geometry as well.

In 14.0, the mesh connections are generally performed after the initial mesh is created by default.  This means that if changes are made only to mesh connection settings, the remeshing operation is fairly quick since the initial mesh does not need to be regenerated in most cases.

Note that mesh connections exist in the Connections branch, not the Mesh branch. The mesh connection setup works in similar fashion to contact region creation in that searching for edges/faces to connect is based on proximity. The proximity value can be controlled via a slider or by entering an explicit distance, both available in the Mesh Connections details window.

To activate mesh connections, highlight the Connections branch and click on the Connection Group button in the context sensitive menu above the outline tree.  Change the Connection Type to Mesh Connection in the details.

Next right click on the Connections branch and select Create Automatic Connections.  You may need to adjust the auto detection tolerance in the details to make sure the tolerance distance is large enough to detect desired gaps between edges and faces or edges and edges for the mesh connection to work.

If any contact regions have been automatically created that you want to replace with mesh connections, delete or suppress them.  You have the choice of automatically creating mesh connections or manually creating them.  Both options are available by right clicking. 

In the example shown here, mesh connections are edge to face.  Edge to edge mesh connections are also available.

With a couple of mesh settings added, we can obtain a better mesh:

Note that the hull surface nodes have moved a bit in order to allow for the mesh connections with the ribs.  Here is a view of the outer hull surface in the mesh connection region:

There are other considerations as well, such as which geometric entities should be the master or slave.  In general slave geometry is ‘pinched’ into the master geometry.  Also, mesh connections can be setup manually for cases where the auto detection is not appropriate or is not providing the desired level of control.  Note that the mesh can end up as an approximation of the geometry since the mesh will have moved to close gaps.  Here is an example:

In summary, mesh connections are another tool that are available to us in ANSYS meshing capabilities, having value for shell assemblies.  In cases where shell geometry edges do not meet at intersections we can still obtain a continuous mesh without having to perform additional geometry operations.  Mesh connections can be faster than using contact elements at the edges as well.  There are other features and considerations for mesh connections which are explained in the ANSYS 14.0 Help.  We recommend you give them a try if you are tasked with simulating shell type structures.

Editors note: For this weeks Focus posting I’m just taking a PowerPoint that Ted Harris created and putting it on the Blog so the search engines can find it easily.  We share this with our customers to help them quickly install the ANSYS software and hope you find it useful.  You can also download a PDF of the PowerPoint if you wish to keep a copy, share it with your co-workers, or print it out: 

ANSYS 14_Install_Quick_Guide_wCAD.pdf

Twice in the last week we’ve taken tech support calls in which the users questioned why their stress or strain results were being reported differently in Workbench Mechanical vs. the results from the same results file in /POST1 with ANSYS Mechanical APDL.  After answering those questions it was pretty obvious that a Focus blog entry was in order.  All we needed was a good, relevant example to demonstrate the issues and the explanation.

First glimpse of approaching dust storm.   All photos by the author.

In case you missed it, the big story here in the Phoenix area this week was our monster haboob, or dust storm.  If you’re not familiar with the term haboob, Wikipedia explains it here:  http://en.wikipedia.org/wiki/Haboob.  In order to have a humongous dust storm, you’ve got to have wind. 

Stopped in a parking lot to take these pictures – the only camera I had was my phone.

About 3 minutes after this picture was taken the dust storm arrived.

Wind tends to cause damage, but although our recent dust storm is estimated to have been 100 miles wide and up to 10,000 ft. high, we fortunately did not sustain much significant wind damage.  Things that do tend to get mangled, however, are deployed patio umbrellas and portable expanding sunshades.  These sunshades typically retract into a compact size and fit in a zip up carrying case.  Many of us have collections of damaged sun shades that still work via creative application of duct tape, wire, etc.  These inexpensive shades work great for keeping the sun off of us during birthday parties or other outdoor gatherings, but high winds tend to cause the metal members to bend and break, causing the shades to need some field engineering repair if not just a one way trip to the dumpster.

Here is a solid geometry representation of a typical portion of the frame of a representative shade.  It consists of two rectangular hollow members, pinned to each other at the center, with pins at each end that in the full structure would be attached to additional components.

For simplicity, we fixed the pins on the right side to ground, while those on the left side have an upward bearing load applied to the upper pin and a downward bearing load applied to the lower pin.  These loads tend to cause the members to bend at the central pin.  The bearing loads in our example represent the effect of a strong gust of wind hitting the fabric canopy above the frame, with the load eventually reacting through the frame to stakes that attach the frame to the ground at the bottom.   The main thing to note here is that the applied load is large enough to cause significant plastic deformation, not unlike what one might experience in the real world when one of these structures is subjected to a very strong wind.

Workbench Mechanical, Coarse Mesh, Peak von Mises Stress is 79,219 psi

Same Results File in Mechanical APDL /POST1, Peak von Mises Stress is 83,873 psi

The issue here is that for our initial run with a very coarse mesh, when we view the von Mises stress results in the Mechanical editor and then compare them with the von Mises stress results obtained from the same results file in /POST1 in Mechanical APDL, we notice there is a difference (79.2 ksi vs. 83.9 ksi).  Why is that?  It has to do with how stresses are calculated.  First let’s consider Mechanical APDL and /POST1.  The original graphics display system is known as Full graphics.  Fifteen or twenty years ago ANSYS, Inc. developed a newer graphics display system for MAPDL known as Powergraphics.  There are several differences between these two display systems which affect results quantities. 

ANSYS Mechanical APDL uses PowerGraphics by default, which among other things only looks at results on the exterior surfaces of the model.  Full Graphics, on the other hand, includes interior elements in addition to the exterior surfaces when displaying results plots.  Another difference is that with Powergraphics we can vary the number of element facets displayed per element edge with the /efacet command.  The default is one facet per edge but for midside-noded elements we can increase that to two or four.  With Full Graphics we are stuck with one facet per element edge.  Workbench Mechanical uses an algorithm whose results tend to compare more favorably with full graphics, although it apparently displays with 2 facets per element edge.   Another option in MAPDL is to plot nodal (averaged) vs. element (unaveraged) stresses. 

So, which of all these methods is the correct one?  I would consider them all to be correct, just different.  However, we can use the difference in results as guideline for our mesh density (as well as the presence of singularities). If there is a significant difference between PowerGraphics and Full Graphics results in MAPDL, this usually indicates the mesh is too coarse, at least in our region of interest.  As the mesh is refined, the difference between the two calculations should decrease.  In Workbench Mechanical 13.0, we can plot averaged and unaveraged stress and strain result plots.  The choice is made in the details view for a given plot.  A significant difference between these two quantities also indicates that mesh refinement is needed.  In our shade frame model, we can see that as the mesh is refined, the difference in von Mises stress results decreases, as shown in the table below.

A similar effect is seen with the von Mises plastic strain results:

Regarding the mesh densities used, the coarse mesh had an element size of at least 0.05 in. on the member hole at the high stress/strain location,  while the fine mesh had an element size of 0.025 on the same hole.  Another way to look at the mesh refinement is that the coarse model had 20 elements on the hole of interest while the fine mesh had 104 elements on the same hole.  Clearly the coarse mesh in this example was way too coarse for engineering purposes, but this was selected for this article to ensure the effect of different results calculation methods was significant and observable.

So, the bottom line here is that if you see unacceptable differences in stress or strain results using different results calculation methods, it likely means that your mesh, at least in the area of interest, is too coarse.  Try adding mesh refinement and check the results again.  In Mechanical, you can try adding a Convergence item to a scoped result plot to at least partially automate this process.  Just be careful that you don’t include any singularities in your desired convergence region.

If you were expecting a reference to the Kansas song, “Dust in the Wind,” well, I guess this is it.  Fortunately we don’t seem to have many lingering affects of the big dust storm.  The parking lot here at PADT has a thin layer of dirt that’s gradually disappearing.  Once we get a good rain it will all get washed away.

I’m sure the question comes up for a lot of us from time to time, whether from one of our own offspring, another relative, or an acquaintance.  “Just what is it that you do, anyway?”  Typical answers might be something short and sweet, such as, “I’m an engineer.”  A more detailed response might be, “I use a technique called finite element simulation which is a computer tool we use to simulate the behavior of parts or systems in their real world environment.” 

You’ll probably find that people’s eyes glaze over and they start looking for someone else to talk to by the time you get to the end of that second quote above.  In fact, I find that my extended family is much more interested in my brother-in-law’s surgery stories from the operating room than they are in my own triumphs and challenges in the engineering simulation world.  Maybe you’ve had that same sort of reaction.  You have probably noticed that there are a whole lot more medical dramas on TV at any one time than there are engineering dramas.  They’ve got many characters from Marcus Welby on up to Dr. Ross on ER, Jack on Lost, to Dr. Grey on Grey’s Anatomy, with more than I can count in between. 

We’ve got, well, Scotty.  And even then I think Dr. McCoy got more air time.

So when my kids ask me what I do at work, I recall a scene from that late 1980’s to early 1990’s TV show The Wonder Years.  In the episode “My Father’s Office,” Kevin asks his dad what he does for a living.  His father responds in an angry tone, “You know what I do!  I work at NORCOM.”  As if that were a sufficient explanation.  I suppose it was his way of saying, “It’s complicated.  It can be high pressure.  You might find it boring.  It puts food on the table and a roof over our heads, though.”

Rather than reply that way, I’ve tried to come up with what is hopefully a better response.  In fact, this concept constitutes the first portion of our Engineering with FEA training class, written by Keith DiRienz of FEA Technologies with contributions by yours truly. 

I can’t guarantee that your audience’s eyes won’t glaze over by the end, nor that you’ll become the hit of the party, but this is free and you get what you pay for.  This explanation can obviously be adjusted based on the audience, but it goes something like this:

Simple explanation:

–We have equations to solve for stresses and deflections in simply-shaped parts such as cantilevered beams.

–No such equations exist for complex shaped objects subject to arbitrary loads.

–So, using finite elements, we break up a complex part into solvable chunks, leading to a finite set of equations with finite unknowns.

-We solve the equations for the chunks, and that ends up giving us the results for the whole part.

If we want more details, we can use this:  As an example, here is a simple beam, fixed at one end with a tip load P at the other end.  We have an equation to calculate the tip deflection u for simple cases:

In the above equation E is the Young’s Modulus, a property of the material being used and I is the moment of inertia, a property of the shape of the beam cross section. 

For more complex shapes and loading conditions, we don’t have simple equations like that, but we can use the concept by dividing up our complex shape into a bunch of simpler shapes.  Those shapes are called elements.

A useful equation for us is the linear spring equation, F=Kx, where F is the force exerted on the spring, K is the stiffness of the spring, and x is the deflection of one end of the spring relative to the other.  If we extend that concept into 3D, we can have a spring representation in 3D space, meaning the X, Y, and Z directions.  In fact, the tip deflection equation shown above for the beam fixed at one end can be considered a special case of our linear spring equation, solved for deflection with a known applied force.

By assembling our complex structure out of these 3D springs, or elements, we can model the full set of geometry for complex shapes.  The process of making the elements is called meshing, because a picture or plot of the elements looks like a mesh. 

Using linear algebra and some calculus (stay in school kids!) we can setup a big  series of equations that takes into account all the little springs in the structure as well as any fixed (unable to move) locations and any loads on the structure.  The equations are too big to solve by hand by normal people so computers are used to do this.

When the computer is done solving we end up with deflection results in each direction for the corner points (called nodes) in each element.  Some elements have extra nodes too.

From those deflection results, the computer can calculate other quantities of interest, such as stresses and strains.  Further, other types of analyses can be solved in similar fashion, such as temperature calculations and fluid flow.

Here is an example using a familiar object that practically everyone can relate to.  This plot shows the mesh: 

This is fixed in the blue region at the bottom and has an upward force on the left end.  The idea here is that someone is holding it tightly on the blue surface and is pulling up on the red surface.

After solving the simulation, we get deflection results like this:

The picture above shows that the left end of the paper clip has deflected upward, which is what we would expect based on common experience with bending paper clips.  Using our finite element method, we can predict the permanent deflection resulting from bending the paper clip beyond it’s ‘yield’ point, resulting in what we call plastic deformation. 

Clearly there is a lot more to it than these few sentences describe, but hopefully this is enough to get the point across.

In sum, not as exciting as my brother in law’s medical stories involving nail guns or other gruesome injuries, but hopefully this makes the world of engineering simulation a little more accessible to our friends and family.

In the Wonder Years episode, Kevin ends up going to work with his father to see for himself what he does.  I won’t spoil the episode, but hopefully you’ll get the chance to show your family and friends what it is that you do from time to time.