Convergence problem - intake manifold
 

Hi guys,

My first post...just started with CFD about 6 months ago.

My goal is to compare two different intake manifold (car) designs using STAR CCM+. I am applying a pressure of -6968Pa to the open outlet and leaving the Inlet as pressure outlet at 0Pa.

I am running a mesh with 330k cells, 5 prism layers (no idea of the thickness, so I put 1mm??).
Solvers: Steady, Coupled flow, K-Omega with SST, Y+ wall treatment.

I have tried everything on this post: http://www.cfd-online.com/Forums/cd-...ing-wrong.html
but I keep getting the same results no matter what.

My outlet mass flow seems to stabilize (2% range) after 300 interations but the mass flow at inlet after 900 iterations is around half of the outlet, but it is also very stable!!

Can I trust the mass flow values at the outlet? These are the ones needed for comparison purposes.

Do I need to use extrusions?
Do I need to run it for more iterations?
Is this because my mesh is to coarse? I will struggle to make it any better due to limitations in hardware.

Any help will be much appreciated.

Use segregated. I had the same problem some weeks ago.
Don't know why I used coupled, I normally use segregated...

First of all, I think your mesh is coarse, if you can do it finer would be great. Second, as our friend said above, use the segregated flow solver. Just use the coupled formulation if you have high Mach number flows or flows that the bouancy effect is relevant, for example, in natural convection cases.

You can also specify a target mass flow in the outlet, to better represent your case. Extrusions could be a good idea, mainly if you have reversed flows on the outlet.

Check your y+ values, make sure they are not in the undesirable region (7~20). For this case, I think you can use, or initialize the problem, with k-e formulation.

Hi Maddin and Vinicius,

Thanks for the help.

I have run it with segregated and get good results. Why can't I get them with coupled? Bug in STAR or needs a better mesh?

I have checked my y+ values and they are indeed in the region of (5-30). What can I do to reduced them? Does this mean that my boundary layer is not being calculated correctly? What influence will this have on my outlet mass flow?

I would love to run it with a denser mesh but it is impossible at this stage.

Thanks again.

Is not that you can´t use the coupled formulation, but it has some peculiarities. For example, the convergence happens in a determined number of iterations, independently of the mesh size, so, probably in your case you didn´t run iterations enough.
To accelerate the solution you can increase the courant number, but it might cause instabilities. The segregated solver is much faster and in your case that you can´t increase the number of cells, it is the most appropriated one.

The y+ values indicates which wall function will be used to calculate the boundary layer. There are two stables regions, below 3 and between 20-300. To change this values, you have to change the thickness of the first prism layer. To do that, you can specify the value of this first prism or change the number of prisms and their stretching factor.

Let me know if you have more doubts.

Regards

I have tried to reduce the prism layer thickness but it results in a denser mesh and that means I can't run it.

Am I stuck (i.e. need a better computer) or is there a way around it?

How do you measure your Y+ values? Do you average or look for maximum value?


Thanks

Split the region and mesh per region after doing this. Then you should be able to work with less memory.
With corse grid you also should be able to run the simulation when the y+ value is good, but results will not be "correct". But for first look into the flow it should be ok.

Simulate valves
 

Thanks for the help.

I managed to get some decent results following your instructions and I am now in the process of trying to validate them in a flow bench.

I was wondering how I could simulate the valves opening at each port.
I do not want to simulate the movement, just the pressure varying with time.
I have the pressure values for every 2 degrees of the crankshaft. I have put these into a table and managed to get the values into STAR.

My problem is: how can I change the port from a pressure outlet (table iteration) to a wall during the simulation?

Do I need to use the morpher? Is there any tutorial that focus on something similar to this?

To change the boundary conditions automatically (pressure outlet to wall) you have to create a macro. But you can use the pressure in the outlet with the same value as inlet.

Thanks

Vinicius,

Obrigado pela resposta...:D

If I understand you correctly you mean when I want to simulate a wall just use 0 Pa. Is that right?

Thanks

Yes, certify that you don´t have a pressure gradient between the inlet and outlet.

Você é brasileiro ? :)

Ok, I'm going to run it like that and let you knwo how I get on.

Nao, sou Portugues mas estou a trabalhar em Londres.

Oha what you want to do needs a lot of power and memory.
I don't think that you really needs that. Work with a steady sim and a constant pressure, like on a flow bench.