Determining the Interior Wall Direction in ANSYS Fluent

Boundaries in ANSYS Fluent can be broken into two groups: external boundaries and internal boundaries.  External boundaries appear on the outer boundary of meshed regions (inlets, outlets, interfaces, etc.), while internal boundaries exist within a conformal mesh (interiors, porous-jumps, fans, etc.).  Internal boundaries are not limited to only residing inside a cell zone (for example they can separate two different cell zones); instead their restriction is simply that the mesh be continuous across them.  There is one boundary type that can be used as either an external or internal boundary: walls.

While external walls are fairly self-explanatory, internal walls are called coupled walls (or two-sided walls) because they are actually formed by a pair of wall boundaries that are by default coupled together.  You most often see coupled walls separating Fluid and Solid cell zones, but they can also be used with as infinitely thin baffles with fluid on both sides.  Each coupled wall pair shows up in the boundary list as a zone and its shadow: one for each side of the wall.  Sometimes it is necessary to set different boundary conditions on either side of the coupled wall.

Continue reading


Boundary Condition Setup of Zero Thickness Baffles in ANSYS CFD

Last week we discussed the different ways to create and mesh infinitely thin baffles using the tools in ANSYS Workbench.  In this blog, we’ll discuss how to create and modify baffles using the two flagship ANSYS CFD programs: CFX and Fluent.


In CFX, the method you use to specify your baffles depends on your modeling intent, but the way the baffles were meshed will affect some of our choices. The two methods are as a ‘baffle boundary condition’ or defining a ‘baffle interface’.

Baffle Boundary Condition

Baffle walls can be created by inserting a boundary condition into the surrounding domain and selecting the appropriate faces.


Baffles created this way are for directing flow only!  Boundaries in CFX are always treated as leading to the exterior of the solved domain, which mean information cannot be passed from one side to the other (e.g. no heat transfer across the faces).

Baffle Interface

Alternatively, you can connect one side of a baffle face to the one facing the opposite direction by creating an Interface.

Face selection will depend on whether you made a conformal baffle (Default Method, Option 1, or Option 2 in Part 1 of this blog) or a nonconformal baffle (Option 3).  For nonconformal baffles, you can create Named Selections for each side of the baffle and then pick those from a list.  For conformal baffles, technically only 1 face exists for both sides in the Mesher, so the Named Selection can’t be used to specify side dependent locations.  That being said, conformal baffles will create 2 identical face IDs with different body IDs representing each side, and if you pick them for Side 1, CFX will automatically populate Side 2 with the appropriate pair.


The interface will then need to be set as a wall, and additional interface models can be specified for the different equations.  For example, for Heat Transfer you can specify that the baffle provides a thermal resistance of a certain thickness of some defined material.



Heat transfer in this case is purely through-thickness.  In other words, heat can flow through the thickness of a metal baffle, but a high temperature would not conduct along the length of the baffle; instead the heat would spread through the adjacent fluid (and then interact with the wall at that the next location).


In Fluent, the method you use to specify your baffles is controlled by how the baffles were meshed, but modelling intent will still affect some choices therein. These methods we will separate between Conformal and Non-Conformal.

Conformal Baffles

Baffles formed by conformal meshes within a Part (Default Method, described last week in this blog) will come into Fluent as a coupled wall, consisting of a boundary zone and its shadow.  These zones represent the two opposite-facing sides of the baffle.


For the equations other than momentum, each side of the coupled wall can be treated individually or jointly.  For example, the default thermal behavior is to couple each side of the wall together using either a direct mapping of temperature (0 Wall Thickness) or using a specified thermal resistance (nonzero Wall Thickness), but you could instead set one side to have 0 Heat Flux and the other side to be a specific temperature.


Much like CFX, entering a Wall Thickness will provide a thermal resistance in the through-thickness direction.  However, Fluent additionally has a model called Shell Conduction that allows for heat transfer along the baffle in addition to through it.

Non-Conformal Baffles

Baffles defined by non-conformally meshed faces (i.e. Option 3 in last week’s blog) require different actions depending on whether you are using them to direct flow only or to additionally pass information.

Non-conformal baffles are exterior faces in the mesher, so if you only need them to direct the flow, they will automatically do so without any user intervention (note that if you also have a non-conformal mesh across regions where there are no baffles, you will need to have an interface across those faces).

If you do need to pass information across the baffle (like heat flow), you must create a non-conformal interface using the coupled-wall option.


This will create 4 addition zones: the Boundary Zones (Side 1 & 2) which are used to control the wall information for areas where the two sides do not line up, and the coupled wall Interface Wall Zones (Side 1 & Side 2) which are used to specify the wall behavior when there is overlap between the two sides.  From here, the coupled wall Interface Wall Zones can be set as described in the Conformal Baffles section, other than that Shell Conduction is not supported (through-thickness heat transfer is still allowed).

One important thing to remember here is that Fluent non-conformal interfaces regularly experience trouble with significant overpenetration between the two sides of the interface.  This typically occurs when there are different mesh sizes on either side of a curved interface.  To combat this, you can enable the Mapped Interface Option, which will use an alternative heat transfer calculation across the coupled wall that performs much better with excessive mesh penetration.


Meshing Tips for Zero Thickness Baffles in CFD

nobaffleA common technique in distributing ducted flow involves thin guiding vanes, or baffles.  One of the biggest hurdles to modeling baffles is how thin they are relative to the rest of the model.  If you were to model their true thickness, you typically have a choice between poor quality, skewed elements and an excessively high mesh count.  Instead, thin baffles are often approximated as infinitely thin.  There are several ways to create these zero thickness baffles, and the method you choose will affect your meshing strategy as well as your boundary condition setup.  Today we will focus on meshing challenges, and next week in Part 2 we will cover setup in CFX and Fluent.

Default Baffle Meshing; Non-Manifold Faces

The traditional method for creating baffles involves grouping surface bodies and solid bodies into a Part in DesignModeler (or into a Component using the Merge Topology option in SpaceClaim).  This results in a single solid body in the Mesher with internal faces where the surface bodies intersected it.



These internal faces (with the same body on both sides of the face) are referred to as Non-Manifold Faces, and had to be created using the method above because most geometry editors don’t actually allow non-manifold faces.  In the Mesher, non-manifold faces limit the types of mesh methods that you can use: except in rare cases, you must use tetrahedral elements (which will typically drive up your mesh count and negatively affect the convergence rate)


.Inflation on these non-manifold faces is also problematic.  For a finite thickness wall, inflation would simply wrap around the thin face from one side to the other; but for an infinitely thin baffle there’s no way for it to wrap around without producing a degenerate (i.e. collapsed) element.  Instead, the Mesher will stair-step the inflation down to nonexistence by the time it reaches the end of the baffle.


Not only does this create poor quality pyramid elements where the stair step occurs, it tends to result in high y+ and bad element transition ratios, which can be just as problematic.  It is generally recommended to fix this behavior using one of the options below.

Option 1: Adjacent Nonconformal Interfaces

The problems listed above stem from the fact that the baffles are composed of non-manifold faces.  The fix is then to convert them exterior faces instead!

Rather than having surface bodies that end in the middle of a solid body, we could slice the model in such a way to make each passage between the baffles its own body, and then combine these bodies into a Part.  We can then give a Named Selection to these faces to be treated as walls.baffle5

The bodies adjacent to these passages will need to be nonconformally meshed though (i.e. be a separate Part so they do not share nodes).  If you were to leave everything as a single Part (or Merged Topology Component), The inflation layers would branch out and produce many of the same problems we saw with the tetrahedral inflation layers.

Option 2: Extending Baffle Faces

A drawback of Option 1 is that it typically results in a lack of mesh refinement immediately downstream of the baffles, which is an area where you often need more resolution.

Instead of placing nonconformal interfaces directly adjacent to the baffles, you could offset these and extend the baffle faces up to these offsets (alternatively you could not use any nonconformal interfaces and just extend the baffles to the ends of the model).  The trick would be to only select some of the faces between these bodies to be baffles.  Any face between bodies but within a multibody part that is not explicitly given a Named Selection will be treated as interior and not block the flow.


Option 3: Nonconformal Interfaces as Baffles

The above options use multibody parts to define the baffle locations; if you are using a swept mesh this forces all the passages to use the same number of divisions in the sweep direction.  If each passage were drastically different in size, you might want to use different mesh controls for each passage, while still maintaining hexahedral elements and baffles in between.  This can be done with a noncoformal mesh between the passages.

Like before, each passage between the baffles is split up into its own body, but also remains as its own Part.  Then, we only need to specify where the interfaces go.  Faces where the baffle doesn’t exist will need to be set as interfaces, but baffle locations will only require interfaces if we need to pass data across them (like heat flow, species diffusion through a membrane, etc.).


In our next blog, we’ll discuss how to handle the setup of infinitely thin baffles in CFX and Fluent.


Restarts in ANSYS Mechanical Can Save Time and Effort!

‘Restarting’ the process in ANSYS Mechanical Products by which a model is solved starting from a previously solved point. The previously solved point contains data for all nodes/elements in the model; there is no results mapping and interpolation when a restart is performed. This is the most accurate method for starting an analysis from a previously solved point.

By default, restarts are not kept when a simulation finishes. The user must modify the Analysis Settings in ANSYS Mechanical to keep the restarts points that will be needed. Those options are shown below:


Restarts do have limitations. For instance, modification of loads in a step before a restart point is to be used invalidates that restart point. Several tables in the ANSYS Help documentation characterize what happens to restart points if objects in the model tree are changed. This section can be found in Mechanical Applications > Understanding Solving > Solution Restarts, as shown.


Here’s one of the tables showing where restarts can be used followed by common questions we related to restarts.


What can solution restarts be used for?
For cases where some subset of the loads does not change and only a few loads change/vary. This is commonly referred to as load case modeling. ANSYS Mechanical FEA can do load case modeling.

Can you give an example of load case modeling?
A model that solves bolt pretension in the first several steps and then locks them in place. Commonly, service loads are applied after the bolt tightening is simulated. The service loads can represent multiple load cases, say one load case is a pressure load, another is a force load.

Another example is a ROPS (Roll Over Protection System) analysis, where loads are sequentially applied on a structure until some criteria is met (usually energy dissipated by the structure). Once the criteria are met for one load case, the load is removed and another load is applied. This process can also be done via restarts.

Why would we do this?
This saves time on solving models. Using the example above, without restarts, the bolt pretension steps would need to be solved every time a load case is added/modified. With restarts, loads can just be activated/deactivated in a step following the bolt pretension and the bolt pretension final step used as the restart point.

Things to know before attempting this method:
All of the load cases that will be solved should be known beforehand. The restart analyses require that ALL loads are defined in the initial model. In ANSYS Mechanical, loads cannot be added to the model tree without invalidating the previous results (ignoring the ability to use restarts).

Newly added loads also will not be applied in a restart analysis as the restart method does not create new elements for these new loads.

If bolt pretension is to be used, any loads defined for a load case should be applied in a step after the final bolt pretension, as usual.

Also, if bolt pretension is used, a step after the final pretension occurs IS REQUIRED. If this is not included, ANSYS assumes the last bolt pretension will be Loaded and not Locked. This means that ANSYS would modify the pretension to maintain whatever preload you have assigned, rather than applying the service loads as a working load on the bolt. Physically, it would be like tightening/loosening the bolt as the service loads are applied.

The general steps to this method are as follows:

  1. Set up a model with all of the loads applied to the structure. This includes bolt pretensions and any loads that need to be simulated for the load cases. Set up the Analysis Settings as required for the analysis (multiple load steps, Large Deflections, etc.).
  2. Modify the Restart Controls to keep all restart points once the model is solved.
  3. Modify the loads for the load case studies to be inactive.
  4. Solve the model.
  5. Duplicate the analysis, sharing the Engineering Data, Geometry and Model cells. This guarantees the model setup remains the same for all models.
  6. In the new system, activate the load for the first load case study.
  7. Use the Tools > Read Results File… and locate the file.rst from the previously run analysis. This imports the results data into the model.
  8. Modify the Restart Analysis options in Analysis Settings to restart from the end of the first simulation (the final bolt pretension loading, for example).
  9. Solve the model.

The example shown here uses an oil field fluid end model with bolt pretensions applied. There are two load cases: 1) a pressure load on the cylinder bore, 2) a force load applied on one side of the fluid end body.