We received one of those tech support calls last week that you hate getting. It was something like “I need to transfer my ANSYS model to this other FEA package, how do I do that?” We of course asked “Why do you need to go to this other package?” The answer was “Because they have elements that solve for stress and thermal degrees of freedom in the same element.” Well, so does ANSYS Mechanical APDL, and it has for years. But as a Workbench user they had only been exposed to Multiphysics that uses Load transfer as the mechanism to solve different domains in the same run
Therefore, a The Focus posting is born.
In this posting we will go over the basics of direct coupled-field elements and simulation to make everyone aware of what is available.
Direct Coupled-Field vs. Load Transfer
When most people talk about Multiphysics they are talking about Fluid-Structural Interaction (FSI) or some other interaction between two different models where the program solves each physics by itself and transfers the resulting values from one physics as a load on the next physics. This is called load transfer Multiphysics and it is very useful and powerful. But it requires a solve for each physics for each step in your solving process, and often more because you have to iterate back and forth between physics till things converge before you can move to the next substep.
There is a whole other way to do Multiphysics if you have the same mesh for each physics: you can modify your finite element equations to cover all the different physics in one set of equations, therefore in one matrix, and therefore in one pass through the solver for each solve. This capability has been in the ANSYS Mechanical APDL solver for a very long time and has been expanded over time to cover some surprising combinations of physics.
So when should you use one over the other? That depends. Here are some thoughts:
- Load Transfer Approach:
- Your meshes need to be or are different
- Fluid flow with something other then heat-transfer
- Direct Approach:
- The interaction between two physics is strongly coupled
- The interaction is non-linear
- Acoustics is involved
- Piezoelectric is involved
- Porous fluid flow is involved
- Diffusion is involved
In general, if you can use Direct Coupling and you know MAPDL well, it is the preferred way to go, it is just a lot easier to do. But if you are not familiar with MAPDL for running and post processing, you may be better off with the Load Transfer approach.
The Coupled-Field Elements
You access the coupled-field capabilities in the solver through the use of the coupled-field elements. Although there are some legacy elements that can be used as well, we will focus on the three standard coupled-field elements. They all have the same capability, and just vary in topology:
- PLANE223: 2D 8 Node Quad
- SOLID226: 3D 20 Node Hex
- SOLID227: 3D 10 Node Tet
All of these support the following physics, DOF’s, forces and reaction loads:
||UX, UY, UZ
||FX, FY, FZ
||Diffusion Flow Rate
You use a combination of KEYOPTS and material properties to enable the various types of coupling. Take a look at the element documentation to see how it all works.
In addition to these, there are some specialty elements worth discussion. The first are FLUID29/FLUID30. These are the Acoustic field elements. These solve for displacement and pressure. They also can share the displacement DOF’s with structural elements where they touch.
Unfortunately the electromagnetic coupled field elements have been put on legacy status, as ANSYS Maxwell is where the development effort is going in this area. But you can still use them for coupled-field simulation that involves the MAG degree of freedom. The elements are: PLANE13, SOLID5, SOLID98. ANSYS MAPDL still has actively supported electromagnetic elements, but they are electromagnetic only and do no support displacement or thermal degrees of freedom.
Flow in a fully saturated porous media can be modeled with the Coupled Pore-Pressure elements. These elements: CPT212/213/215/216/217, solve for pressure and deflection and are used for things like modeling nuclear waste issues, soil subsidence, oil well stability, and bone deformation and healing.
We should also mention that ANSYS supports circuit simulation using the CIRCU124 element. This element can be coupled to other elements that have VOLT, CURR, or EMF capability.
Running Direct Coupled-Field Multiphysics in ANSYS Mechanical APDL
When I wrote this section heading it seemed like a good idea. But this is supposed to be a short blog entry and not a full one day training class. So I will wimp out and share where you can find more information in the help:
There is a whole manual dedicated to coupled-field analysis: Mechanical APDL // Coupled Field Analysis Guide. Within that guide is the Direct Coupled-Field Analysis section, Chapter 2. In it you will not only find discussions about how to do what you need to do, but also a whole bunch of simple examples that are very helpful.
In general, you run like any other simulation. There is really nothing special or unique and you do not have to deal with managing the load transfer like you do with load transfer coupled field simulations.
Running Direct Coupled-Field Multiphysics in ANSYS Mechanical
This is a question that comes up a lot. Unfortunately only one type of direct coupling is supported, Thermal-Electric. What we recommend people do is they build their models in ANSYS mechanical for one of the physics, then use code snippets to change the elements to the proper direct coupled-field type and to also do any post processing. It will run when you solve, but it will come back with an error, and you need to post processes via APDL code or you need to post process in MAPDL interactively.
NEW INFO: Edward points out in the comment below that you can get this to work. I’ll repeat it here:
“We’ve had some success post-processing U-TEMP-VOLT analyses in Mechanical. Mechanical seems to accept a model as solved, so long as it sees a result file of the correct type in the Solver Files directory. The coupled field analysis in this case output a .rst file, so we used a Static Structural object as the base model.
We could access the structural results directly and used User-defined results to access most of the thermal and electric results.
I seem to recall that we also had success using a Thermal analysis as a base and then changing the result file extension from .rst to .rth, but I can’t find my test model to confirm this.”
I can verify that both of these approaches work. I added a /sys, copy file.rst to file.rth to a code segment for the thermal base. But it was simpler to just use the structural as the base. If you do this you can do your post processing for the most part in ANSYS Mechanical. [E. Miller 3/28/2013)
So this was, as promised, a very high level overview. The fact of the matter is that there are a significant number of users, especially in the MEMS industry, that use these direct coupled-field elements all the time. They are powerful and robust with as many uses as you can dream up, truly expanding the reach of what you can model and the accuracy of those models.
Over the years we have found some good tricks for using these elements effectively:
- Pick one of the physics and get a static run of that physics by itself running first. Debugging your model this way is usually faster and clears out any issues before you deal with the direct coupling issues. If you have more than two physics, add them in one at a time.
- Pay attention to units. When you start mixing voltage and distance or what not, it is easy to get confused. If you are doing MEMS devices, you need to make sure you are using the MEMS units and that you are consistent. Unlike ANSYS Mechanical, ANSYS Mechanical APLD is unitless and requires the user to make sure the are consistent across physics.
- Try not to use the legacy elements if you don’t have to. They may not be around in the future.
- If you are doing EMAG, you may want to look at using load coupling with Maxwell or MAPDL instead of using the legacy direct coupled elements. Maxwell and the newer elements in MAPDL have more capabilities and are more efficient.
- Make sure you really understand how your physics interact. Go through the thought experiment of predicting the interaction on as simple of a problem as you can, while keeping it relevant. Think about what loads interact with what structures and what that interaction implies.