Home  CFD-ACE+ User Tips Understanding the Mass Flow Summary Output
|
|
Understanding the Mass Flow Summary Output |
|
|
| Some of the modules have
the capability to
produce a summary report of computed data. These summaries are usually
integrations of some parameter over each valid boundary patch, as
well as a
summation of all of the data for the whole model. To print these
summaries in
the output file, you have to select them in CFD-ACE-GUI under the Out-->Print
tab. The most commonly selected summary is that of Mass Flow,
which
will be
discussed in this tip. |
A sample microfluidic problem
setup is shown in the figure above. The Inlet, Outlet and two
interfaces have been highlighted. The flow enters through the
Inlet,
divides into two channels (Straight and Curved) and then recombines
ahead of the Outlet. The solution was run for 5 time steps.
The
Mass Flow Summary (including Interfaces) after the last step is shown
below.
|
|
Name:
User assigned Boundary Name
Key: Unique
identifier
for each boundary (automatically assigned by the
grid generator)
Type: User assigned
Boundary Condition Type
Inflow: Computed
rate of
mass flow entering the system through the
boundary (positive by convention)
Outflow: Computed
rate of
mass flow exiting the system through the
boundary (negative by convention)
Sum: Sum of Inflow
and
Outflow
Mass Accumulation:
This
appears only for transient runs. It is the mass
that has entered the system in the current time step but has not left
the system yet. This is not an error term!
Total volume source:
This
reports the data pertaining to a mass source
in the system, if present. Such a mass source can be introduced in the
system through the problem set up in CFD-ACE-GUI under VC-->VC
Setting Mode:Flow.
Total Mass Flow Summary:
Sum of all the data rows (excluding
interfaces) – this is the overall mass flow summary of the
system. The
three numbers in this row denote total inflow, total outflow and the
total sum. This total sum (or Flow Imbalance) is a measure of the
error
in the flow computation.
|
FREQUENTLY
ASKED QUESTIONS:
Why
select Include Interfaces?
By checking the Include
Interfaces box in the Out-->Print
tab in
CFD-ACE-GUI, mass flow data through the fluid-fluid interfaces in the
system is included in the Mass Flow Summary. This is especially
helpful in cases, like the sample problem, where the flow branches off
into two (or more) streams. Then, the mass flow through any
branched
channel can be located in the Mass Flow Summary. For example, in
the
sample problem, mass flow through the Curved and Straight channels are
given by the mass flow numbers for the CURVED_CHANNEL_INT and
STRAIGHT_CHANNEL_INT interfaces respectively. Please note that
because
flow merely passes through the interfaces, their Inflow and Outflow
have the same magnitude, but opposite sign. Thus, these numbers
are not
included in the Total Mass Flow Summary row.
How
to tell if the solution has converged?
The Residual Plot is usually a good indicator of the convergence of a
solution, but it is recommended that the user confirm the same by
checking the available Summaries. For example, in the Mass
Flow Summary above, the Flow Imbalance
(-1.59428E-21) is 10 orders of magnitude smaller than the Inflow or
Outflow (~±8.37142E-11). This is a well converged solution
–
typically an imbalance 3-4 orders of magnitude smaller than the
Inflow/Outflow indicates good convergence.
Convergence
problems? Is there any inflow through the Outlet?
In certain cases, if the Outlet is not drawn out far enough, flow
disturbances close to it may cause the fluid to come back into the
system through it. This may give rise to convergence
problems. The Inflow column
in the
Mass Flow Summary is the quickest way to find out
if there is any inflow through an Outlet (0.00 for OUTLET_FACE in the
sample problem).
If you have any questions about this feature or would like us to
discuss some other topic in the future, please let us know.
Santosh Kini
Applications Engineer
ESI Group
|
|
|
Restarting a Fine Grid Case from a Coarse Grid Solution Many users have asked for a
method to obtain a solution on a coarse grid and then use it as the
initial guess for a finer grid. This option can be done using the
Map utility in
CFD-Toolkit.
Using Arbitrary Interfaces for Sliding Meshes in CFD-ACE+ When using the Grid Deformation module in CFD-ACE+
with systems containing rotating parts, the system
may require the grid to rotate 360 degrees. However,
this is not possible since the grid will become
highly skewed/stretched.
Using Cyclic Boundaries in CFD-ACE+ There are many applications that involve rotating
mechanical components that result in rotational or circumferential
symmetric flows. One can model an entire 3D rotating system, but
the computational resources to do so can be quite large.
The “Constrained Displacement” Grid Deformation Feature When running Fluid Structure
Interaction (FSI) problems with CFD-ACE+ you may run into problems with
severe grid skewness in the fluid regions. While the CFD-ACE+
Stress module solves for the deformation of the grid for the solid
part, the CFD-ACE+ Grid Deformation module must determine how the grid
for the fluid regions is deformed.
|
|
