Discussion Closed This discussion was created more than 6 months ago and has been closed. To start a new discussion with a link back to this one, click here.
Pressure changed with respect to temperature in a confined volume.
Posted 22.09.2023, 15:30 GMT-4 Heat Transfer, Materials, Structural Mechanics Version 6.1 1 Reply
Please login with a confirmed email address before reporting spam
Hello
Does anyone know about how to simulate the following case? There is a structure that has hollowed volume with a thin membrane. The membrane can be deforemd.
1) Liquid argon filled in confined volume. 2) The tempetarue changes from 90K to 130K 3) Since, the volume is confined, the pressure will increase in the volume. 4) The pressure is increased, expanding the volume inside, becuase the membrane will deform. 5) there is a piston head that constricts how far the membrane can be extended.
I would like to see the deformation and pressure in the volume.
Thank you
Please login with a confirmed email address before reporting spam
Hello Y Ko, if you are only interested in the effect of the fluid pressure on the enclosing structure, your case may be analyzed in such a way, that the fluid domain does not need to be modeled explicitly. This modeling technique is shown in the Hyperelastic Seal model:
- https://www.comsol.com/model/hyperelastic-seal-206
- https://www.comsol.com/blogs/computing-controlling-volume-cavity/
There are essentially three steps involved:
- Compute the enclosing volume in the undeformed and deformed states.
- Formulate an equation of state for the fluid, p = f(Delta_V, T).
- Apply the computed pressure as a follower load.
The first step involves converting a volume integral into a surface integral using Gauss' theorem (https://en.wikipedia.org/wiki/Divergence_theorem). Assuming that your study is geometrically nonlinear (which is necessary to model the pressure load as a true follower load), you can directly make use of the material and spatial frame coordinates. For 3D, for instance, the undeformed and deformed volumes can be defined as
V_undeformed = -(1/3)*intop1(X*nX + Y*nY + Z*nZ)
V_deformed = -(1/3)*intop2(x*nx + y*ny + z*nz)
where intop1() is an integration operator defined on the enclosing boundaries using the Material frame setting. Similarly, intop2() is an integration operator using the Spatial frame setting. The variables nX, nx etc. are the normal directions in the material and spatial frames, respectively. If the normals point from the solid domain into the fluid domain, there will be a negative sign, otherwise it will be positive. In 2D, the factor 1/3 is replaced by 1/2, and the out-of-plane thickness needs to be taken into account.
Once you have defined the initial and current volumes, you can formulate the pressure law, which in your case will depend on the volume change and the temperature. To do this, you can add a new variable definition for your pressure variable. Depending on the physics interface, add a Boundary Load or Face Load node, and choose the load type Pressure to apply the pressure you defined.
In the upcoming version of COMSOL Multiphysics there will be built-in functionality in the Solid Mechanics interface for this type of simplified fluid-structure analysis.