Cfd-Post timestep selector problem
 

I am trying to do transient moving mesh simulation and sure about my bc's. The problem is after I rotated my model in Spaceclaim, Cfd-Post began to not get all time steps automatically, I realized that this causes solver to apply moving mesh displacement option as initial mesh, instead of previous mesh. The solver stops with negative volume error because of this. Transient results were defined for every timestep in Cfx-Pre as well. I don't want to define my case again it takes too much time. I hope someone could help me.

Maybe it is just me, but it is hard to follow what you're actually doing from your description. Whether you rotate your model in SpaceClaim does not (or, should not) have any influence on the time steps you see in CFD-Post. Also not having all time steps in Post has nothing to do with whether the Mesh displacement is applied relativ to initial or previous mesh.


The solver stopping from negativ volume error is likely caused by either a bad initial mesh or a mesh displacement distorting the elements so badly, that they collapse. Or a combination of both. To me it looks like a cascade of errors originating from a base error. Maybe you rotated your model but did not adjust the mesh displacement vector, or whatever you used to specify displacement?

Also see FAQ: https://www.cfd-online.com/Wiki/Ansy..._went_wrong.3F

I solved the first issue, I had changed cylinder wall's mesh motion option "stationary" instead of "unspecified" by a mistake. Now walls are in the motion that I expected. I don't get any negative volume so far.
----------------------------
I am trying to simulate Variable Displacement Axial Piston Pump. The study has 7 piston. Each piston has unique sinus displacement function which starts from TDC and considers phase angle between other pistons. Inlet and Outlet domains were connected by pistons. Just one interface defined to connect all domains and no intersection is permitted. CGI frame change model was applied as Transient Rotor Stator. Inlet and Outlet BCs are Openings. 5bar inlet total pressure, 0bar outlet static pressure.Turbulance model is RNG k-epsilon. I expect to see pressure difference driven by mesh motion. While pistons moves axially also rotates with 1500rpm. Time necessary to sweep 1deg is 0.111111E-3 s, when I apply this as timestep, it just can solve 8 deg until overflow divergence. I also tried adaptive timestepping. For maximum of 50 CFL, 1E-6 s timestep selected by solver. My mesh elements counted is nearly 1M. It takes too much time to solve, I wonder how much I can raise CFL number for such a complex problem. This is not commercial project by the way, a friend of mine has close deadline for his thesis.

https://i.hizliresim.com/9Zzref.jpg
https://i.hizliresim.com/rZdrxj.jpg
https://i.hizliresim.com/ggaGPI.jpg
https://i.hizliresim.com/wPLlFk.jpg

I tried to send details but someone deleted my post. I should open new post probably.

I am the moderator of this forum and I certainly did not delete your post. Are you sure it was deleted?

To progress this simulation I would recommend:
* Using adaptive time steps, homing in on 3-5 coeff loops per iteration. Make sure the min and max time steps are wide enough that you do not hit them.
* Rerun the simulation and see if that runs successfully.
* Once you have a working simulation, then you think about how to get it to run faster.

Key things to consider to make it run faster:
* Improve mesh quality. If you use adaptive time steps like I recommended, it will automatically find a new and larger time step if you improve mesh quality
* double precision numerics
* Add more computers to your compute cluster
* Get a faster computer
* Think about whether the simulation can be simplified or made smaller