Loads, Boundary Conditions, & Solving
Loads and boundary conditions represent the environment acting on the finite element model.
The environment can include those portions of the real-world structure that we chose not to explicitly represent with finite elements.
In this video we will:
Define the different types of loads and introduce the associated APDL commands
Review how to verify and delete loads and boundary conditions
Touch upon some special types of boundary conditions
Review the solve process for a linear static (steady state) model
In the Solid Modeling & Meshing lesson, we learned that the element type defines the physics of the analysis in terms of the variables, or degree-of-freedoms, that will be solved for.
Temperature in a thermal analysis is the DOF.
Boundary Conditions are assigning known values to these degrees of freedom.
With respect to excitations, there are several different types.
Concentrated loads are point-like forces that act on nodes.
Surface loads are distributed over an area like pressure or convection.
A Body load is a volumetric load, such as temperature in a structural analysis that causes thermal expansion.
Or internal heat generation in a thermal analysis.
Lastly there are inertia loads, which involve the mass of the structure, like gravity or an applied rotational velocity.
To be consistent with the MAPDL documentation, going forward, we will use the term load to mean excitations or boundary conditions.
Loads can be applied to either the solid model or the finite element mesh.
Solid model loads have several advantages, as they are applied directly to the geometry, and there are most often fewer geometry entities than there are finite element entities.
The solid model loads will be automatically transferred to the finite element mesh as part of the solve command; until the solve command is issued, please note that the mesh will not show the solid model loads.
By applying loads to the solid model geometry, the mesh can be refined or even remeshed completely without needing to reapply loads.
Finite element loads are typically used if we don t have the solid model geometry.
For example, when importing a mesh from another preprocessor like Ansys Mechanical, only the finite element information is included, so applying the loads directly to the nodes and elements is necessary.
MAPDL Components, which were introduced in the Solid Modeling & Meshing lesson and discussed further in the Select Logic lesson, are very useful when working with FE-based loads as the 'item [node or element ID] that the load is applied to can often be a component name.
Note that commands associated with MAPDL loads can be issued in both the preprocessing and solution processors.
Loads can be defined, listed, plotted, deleted, and some even scaled.
If the load command is X then the list command is XLIST.
Similarly, the command to delete the load would be XDELE.
Note that X may be several characters, and in the case of nodal loads, the N is implied and not present in the commands.
The typical form of a load command is:
Command Name, Entity to which apply the load, label of the load, value 1, value 2,
The entity could be the specific numeric ID of that entity.
Or often we can pre-select a group of the same type of entities and use All to indicate to apply the load to all selected entities.
Most load commands also allow a component name.
Multiple Value fields are shown, as some loads require more than one value for its definition.
For example, in defining a thermal convection load, both a film coefficient value and a bulk temperature of the fluid are needed.
The commands to define loads are: FK and F for concentrated forces on keypoints and nodes respectively.
SFL, SFA, SF and SFE for surface loads.
BFK, BFL, BFA, BFV, BF, BFE for body loads.
DK, DL, DA, and D for boundary conditions.
DSYM is a special boundary condition that we will review in more depth.
There are many inertia load commands, two of which are ACEL that defines a linear acceleration of the entire structure and CMACEL which defines the same for an element component.
Many objects have some kind of symmetry such as mirror, also called reflective, symmetry.
A bottle with a handle often has mirror symmetry if we were to cut the bottle down the axis and through the handle.
A bottle without a handle often shows axisymmetry, or a constant cross section revolved around some axis.
If the geometry, loading, boundary conditions, material orientation, and expected response are symmetric, then the FEM size can be reduced by modeling a portion and enforcing the symmetry, often via boundary conditions.
Compared to the full model with the same element sizing, the FEM will be reduced in terms of the number of nodes and elements which will decrease the solve time and resulting file sizes.
The DSYM command can be used to define the symmetry boundary condition in structural analyses to enforce the symmetry on the model.
A symmetry boundary condition for a structural analysis constrains the out-of-plane (the symmetry plane) displacements and the in plane rotations.
In a thermal analysis, however, surfaces with no applied loads or boundary conditions defined are treated as adiabatic, or perfectly insulating.
The adiabatic condition happens to be the same as a symmetry condition, so in heat transfer or acoustic analyses, no extra step is needed for nodes lying on symmetry planes.
We will exploit this later in the workshop example.
Loads can be verified prior to solving by listing and plotting them.
Only the loads associated with the currently selected set of entities will be listed or plotted.
As we noted before, solid model loads are not transferred to the FEM until solution.
However, we can manually transfer them all at once with the SBCTRAN command.
Individual loads can also be transferred; for example FKTRAN to transfer concentrated loads defined at keypoints to the corresponding nodes.
There are several commands to turn on symbols for entity plots to show the loads.
/PBC controls showing the boundary condition symbols while /PSF and /PBF control the same for surface and body loads.
The /PBC command does extra duty by also controlling the symbols for applied forces, moments, and accelerations.
Once the symbols are turned on, one can plot the entities with the xPLOT command to update the display and show the symbols.
Note that some symbols are turned on by default like the boundary condition and force symbols.
Loads can be plotted with the symbols and with or without values.
For example, here we have a block with a single valued pressure defined on a face;
and now a meshed block with a pressure gradient applied to the top set of element faces;
and lastly applied structural temperatures to the chips on a circuit board.
Boundary conditions can be shown with symbols with and without values, too.
The traditional symbol is a triangle in the direction of the positive global axis direction.
Here, we can see that displacements are blue; applied rotations are double orange triangles;
temperatures applied in a thermal analysis are orange triangles that point in the negative X global direction while temperatures applied to a structural model are body loads.
Loads can be listed with the xLIST command where x is the type of load that we saw previously;
for example, the DLIST command lists the displacements and/or rotations on nodes.
Loads can be deleted with the xDELE command BFEDELE can be used to delete the body forces applied to a set of elements.
Deleting loads from a solid model automatically deletes the load from the FEM if the load has been transferred.
But the opposite is not true.
All loads can be deleted at once with the LSCLEAR,All command.
Once the model is ready to be solved, we can enter the /SOLU processor to initiate the solution.
For linear static models, there are usually only a few steps needed to solve.
Enter the solution processor; select everything just in case the active selection set only contains a subset of nodes or elements;
possibly save the MAPDL database; and initiate the solve with the SOLVE command.
More information on solves can be found in the following help location.
Some of the often-used solution commands include ANTYPE which defines the type of solution.
Static, or steady state thermal, is the default.
Other choices include time transient, modal, and spectrum.
A Load Case is a set of loads defined for a specific time.
The time is defined by the TIME command with time in a static analysis acting as a counter.
One way to perform a multi load case model is to issue the SOLVE command multiple times with the TIME and appropriate loading commands necessary to define the loading environments.
For example, in a static structural model, we may wish to consider only the effects of gravity at first.
Then, in a second analysis, we may want to add working loads in addition to gravity in this way, we can study the structural response under different conditions.
To accomplish this, we can issue the commands like so:
Enter the solution processor, issue a time, define the boundary conditions, the acceleration and solve.
Update the time, define the boundary conditions, acceleration, working loads and solve again.
During the solution, result items like stress, strain, displacements and the like are saved to the result file.
The OUTRES command can be used to define the frequency at which user-specified results are written to the result file.
This concludes the lesson on loads and boundary conditions, so let's move onto a workshop example.
For this we will revisit the Ball Grid array model from the Solid Modeling and Meshing workshop.
Recall that the BGA model is a 3x3 grid; in this workshop we will take advantage of symmetry to solve for a 9x9 BGA.
Lastly, as we often need to perform both thermal and thermal-structural analyses on BGAs we will review one method that can be used to transition from thermal to a structural analysis in MAPDL.
Let's get started.
A MAPDL archive file in CDB format has been provided of the BGA meshed solid model.
The CDREAD command can be used to read in this file and it is a pre-processing command.
So first, we need to issue the /PREP7 command.
The model was meshed so that the blocks and solder balls had differing material ID numbers, but the actual materials have not yet been defined.
So let's do that now.
The property values shown are generic silicon for the blocks and a lead-based solder for the solder balls.
We can define both the thermal and structural properties at the same time.
KXX is the thermal conductivity; EX is Young's Modulus; ALPX is the thermal expansion value; DENS is mass density; and NUXY is the Poisson's ratio.
We end with a FINISH command.
We now enter the Solution processor and define a heat generation on all the elements in the lower block.
Recall that a thermal symmetry boundary condition is one where there is no boundary condition defined.
To define this condition in this model, let s first select all the exterior nodes of the whole model and define an appropriate convection.
Next we select the solid model areas on the symmetry planes, then select all the nodes on the areas.
We then issue a surface load delete command for all the selected nodes.
Now we can verify the loads by turning on the symbols and plotting the elements for the applied convection.
Let s rotate the model around to verify the symmetry condition.
Next turn on the body force symbol and plot the volumes to show the applied heat generation.
We are now ready to solve so let's issue the TIME,1 command to set the end time and solve the analysis.
To complete the FEA work flow let's finish out of the solution processor; enter the /POST1 processor; and plot the resulting temperature contours.
One neat feature of MAPDL is the ability to change the physics of a model with the ETCHG command; element type change.
We will use this to automatically change the one element type defined in the model from a ten node thermal tetrahedral to the corresponding ten node structural tetrahedral element type.
We will first Finish out of the post processor; enter the /Prep7 preprocessor; and as good practice we first delete all the loads in the model to start with a clean slate.
After the element type has been changed, the temperatures stored on the thermal analysis result file can then be easily read with the LDREAD command into the structural model as applied loads.
Next the structural symmetry boundary conditions are applied in the X and Z directions by selecting the appropriate areas, and then issuing the DA command to restrict the out of plane deformations.
For a static analysis, we need to now constrain the model in the Y direction to be complete.
Here let s simply constrain the bottom keypoint, where the two symmetry planes meet, in the Y direction.
The model is ready to solve so to be complete let s issue the TIME,1 command, then solve.
As before we finish out of the solution processor; enter the post processor; and plot a typical result for the analysis in this case the equivalent stress of the whole model.