Unstable pressure contour in dynamic mesh
 

Hi dear all,

I am simulating a gear pump with dynamic mesh. Though my settings seem good, I read very big differences in pressure contour between two following time steps. My time step size is near e-008 level. How can very big differences like this happen by this very little time step? Does it mean that analysis is still in unstable region and then will become stable? How can this be commended?

Note that, I have run the first 200-300 time steps. After reading this different pressures, I have stopped the simulation.

Thx.

Mert.

which software are you using?

Also by dynamic mesh, do you mean mesh motion or remeshing?

Ah sorry my friend,

I use Fluent and i mean remeshing.

Thx for interest.


Sent from my iPhone using CFD Online Forum mobile app

So in case of remeshing it is possible. The same thing would happen if you use starccm too.

Here is a hint: No matter how many iterations you run for that time step the problem won't go away. And if i am right then reducing time step only make problem worse.

Now it is a teaser, so I give you some time to think over it. I will tell you the reason.

PS: I encountered this problem when I joined cd adapco and figured out where this error was coming from so it is not new to me.

Haha ok :)

My time step size has to be very low like this. Because my tip clearance is very very small, so elements here are very small too. This reduces the time step size to avoid negative volume issue.

I got negative volume even e-006 time step size. These time steps also make me very slow.

And i am still thinking about :))

Thank you very much for your interest. I am waiting for your answer :)


Sent from my iPhone using CFD Online Forum mobile app

I will not tease you much.
The main problem by which you are likely suffering is that when the remeshing happens new mesh is generated and along with it new control volumes are generated. Variables are interpolated to these new cell centers.

That means velocity and pressure are also interpolated to these new cell centers. This new velocity and pressure does not follow Navier Stokes (or it has much more error than previous velocity and pressure field).

This velocity appears in time derivative in momentum equation. At the current level of time velocity and pressure are solved and error reduces but previous time level values are untouched. For this reason no matter how many iterations you run on that time level error won't go away (this is your test to confirm whether what i write is the reason).

The solution that reduces this pressure fluctuation is to have one continuity solved once on previous time level pressure and velocity so that at least continuity is followed there. This reduces the problem very much. (I could demonstrate).

Thx. But i have two questions.

1) Frankly, I could not understand the last paragraph well.

2) In general case, should I increase the time step size? But if I do it, I will receive negative volume issue exactly. Then, how will I be able to fix negative volume issue?


Sent from my iPhone using CFD Online Forum mobile app

You actually can not do much about it. What you can do first try to confirm the problem by increasing number of iterations per time step to very large value. (i used 200 iterations)

Second you can create a simple test case demostrate the same. I made a simple pipe and run it without remeshing for a while. Then remeshed and run 1 times step with 200 iterations for that time step. After that i could show the pressure inconsitency.

Once you could demostrate, then aproach Ansys and other people involved and let them know of problem.

PS: Notice that there is density in time derivative in momentum. The problem reduces when density is low. So variation on it is another check.

Thank you very much. I will try and make a report for you. I hope we will discuss the results again.

Best regards.


Sent from my iPhone using CFD Online Forum mobile app

I already worked on this issue, when i was working at cd adapco and a client showed us this gear calculation that you are doing.
I think it would be better to let ansys know so that they could suggest work around.