I am trying to simulate a simple 2D piston, however keep receiving negative cell volume errors, see below.
I have tried to reduce the size of the mesh, and also reduce the time steps but neither of these solve the problem - no matter how small the time step/ mesh is.
Any suggestions as to how I can solve this?
Thanks, John
John, the time step does not have any role in the mesh generation. Negative cells may suggest some wrong initial conditions. Can you please send a file with your settings?
Hi Adrian,
Thanks for responding. I have attached both the file and a screenshot of my settings. The movement of the piston itself, does act how I would like using a UDF, but the surface body mesh of the cylinder just deforms.
I am new to ansys so any help would be appreciated!
You can use dynamic mesh, set smoothing and remesh, generally your moving part should not exceed one cell size at one time step.
This was what others online suggested, but no matter how how small I made the time step, it didn't seem to change anything @M. Gökhan Günay
Hi John Spawton,
I should first tell you the grid and geometry aren't compatible with what you want to do. For using the smoothing and the remeshing method, the grid must be triangular. Also, the grid is very coarse now (in the two regions that have shown in the picture).
After all, in the mesh method setting section, change these parameters:
For smoothing ---> use diffusion method with diffusion parameter = 1
For remeshing ---> size remeshing interval = 1, Minimum length scale = half of the mesh size near the moving surface.
Ashkan Ghafari , thank you - i will try those settings now. These elements are supposed to be inlets and outlets with a crude attempt at valves. Is it the valves you are saying are compatible - or the inlet/outlet pipes? Thanks for your response.
John Spawton, my pleasure. The grid is incompatible. It's better to refine the mesh in inlet/outlet pipes. You are using the remeshing method; this method is applied only to tri cells. So you should change the mesh type to triangular or use the layering method with these quad cells.
Ashkan Ghafari I have simplified the geometry (it is now effectively a box), changed the mesh and used the settings that you have suggested but I still have the same problem. Sorry for the trouble
It seems as if the nodes on the adjacent walls are not disappearing when the piston moves, this has been the problem from the beginning.
John Spawton, the grid is appropriate now. I checked your file, and I have the following suggestions:
Change the name of the side walls to choose them separately in the dynamic mesh section. (Figure a)
Make the changes shown in Figure b. --> turn on the "region face" option and change the parameters based on the mesh info.
Define the side walls as deforming walls, as shown in Figure c.
- Badges
- Science topic