no-slip condition no obeyed?
 

What I was trying to do, is to simulate a cross shape geometry lumen with with FSI. I have had some stability problem but I troubleshooted it by imposing rigid boundary at the vessel edge.

However, when I look at my streamtraces, I found that the results are not making any sense that, places supposed to have low velocity (no-slip wall) does not have lowest velocity. On the contrary, the pressure map from CFX-post actually kind have the contour map of the velocity profile that I expected. (low pressure at vessel wall)

So I go back and start with a simple cylinder with no FSI but rigid wall. Steady case works fine, and I figured out my entrance length needs to be longer. However, once I switched to transient it seems to me that no-slip condition is not obeyed again. Even I prescribed a parabolic velocity profile with vz = 0 at the wall, the wall velocity of fluid is not zero for a pulsatile condition.

So I wonder is any of the following is wrong:

I imposed a 0 static pressure at outlets as Neumann bounndary condition. So I assumed this will also alter the velocity profile, so I increased the length of the pipe to minimize its effect.

Convergence criteria: I started with MAX residual as 1e-5 as initial start, and am running more cases with less residual 1e-8 to check if that's the problem.

For entrance length I extend a 100mm pipe for each inlets and outlets. But since I imposed parabolic profile at the inlets, I would assume that shouldn't take long for the fluid to develop. Also, when I look at the results, the fluid velocity actually change from no-slip to nonzero near wall velocity as the fluid develop from the inlet along the streamline, which is not making much sense to me.

My time step is 0.02s, cycle time is 1s and I ran for 3s in total.

I wonder if you guys face any similar problem from your experience and what do you suggest causing this problem? What convergence criteria and coupling time steps you usually use for FSI?

Thanks a ton in advance! =)

I see. Thanks for that info!~!!!!!! This problem troubles me for long time, now I know why!!!!

No slip condition in walls,CFX
 

Hi

I have simulated a simple model in CFX , with no slip conditions in the walls.
But I can not see this condition near the wall.
Please help me.
Thanks

Have a look at hybrid and conservative variables in the documentation and post processor.

Thanks for your reply.
I have checked hybrid and conservative forms , but the problem is not about it.
close to the wall there is a considerable velocity as you can see, and it is the same for all of the cases that I simulated, changing to the hybrid or conservative does not make a significant change.
I wonder if it is related to the turbulence model that I used(k-e).
I have studied different BC ,pressure inlet and outlet , mass flow inlet and pressure outlet and vice verse , velocity inlet . all of them have more or less the same problem at the wall boundary like the picture attached.

If you plot conservative values you will find they do not go to zero. This is because they show the velocity at the centroid of the control volume, and these centroids lie off the wall - so they are not zero. There is no control volume on the wall, so no velocity vector is drawn there.

Thank you for your reply ,

As I told you , I have checked hybrid and conservative methods,(attached)
As you can see , even on the hybrid method , there is a sudden change to the velocity on the chart and on the vector there is no zero velocity on the wall.
This is not the case for Boundary Layer and I put the y+ which is small enough to be on the viscous sublayer.
I would appreciate if anybody can help me solve this problem.

Thanks

As we can see from your last post, the velocity at the centroid of the first cell is more than 50% of the maximum velocity. Neither is this cell in the viscous sublayer, nor are the y+ values low enough.
The "sudden change" in velocity with the hybrid values suggests the same conclusion.

Thank you for your reply,
Please make corrections if I am wrong;

dy1= L * y+ * (74)^0.5 * Re^(-13/14)

U bulk = 0.5 m/s
Blood density = 1060 kg/m3
Blood viscosity = .0035 kg/m.s
Duct diameter = .031 m
then;
Re= 4694 ,
y+=1 ----> dy1= 1e-4

but I considered first layer thickness of 5e-5.
Please let me know if there is anything wrong with the formulas , I derived them from the ANSYS CFX manual.

I used k-e for turbulence modeling,no heat transfer, and different BCs for different simulations ,but more or less the same problem.

Thank you in advance.

This equation is for fully developed high Re turbulence flows. You have a low Re flow, it is only just turbulent. So you need a finer mesh as Alex says. And I have already explained twice on this thread why it does not go to zero.

Thanks for your reply,

Is there any furmla for first layer thickness of the mesh generation.
I apreciate if you help me on that issue.

It gets very tricky for low Re and laminar flows. So the easiest way is to just look at the results from an existing model and estimate from that. But if you are asking what boundary layer resolution do you need for accurate simulation - that is best determined by a sensitivity analysis.

I thought that for fully turbulent flow a more condense mesh should be considered to better simulate the eddies and for higher shear stress on the walls there should be higher mesh concentration near wall.
If it is true then the formula that I mentioned for first layer suffices for the first layer.
Please tell me if I am on the wrong track.

Thanks

I just tried to find the discussion on this in the documentation but could not find it.

Now you have performed the analysis I would look at the y+ it produced and see what you actually got rather than an estimate. So I would forget about it now anyway as you have the true measurement.

I am not so professional on CFX,
Is it possible to have the Y+ on the post p or I have to calculate that and how?
Please feel free to explain as if you are explainig for a beginner to the CFD

Thank you

y+ is a variable available in the post processor. No need to calculate anything.

I checked the y+ on the Post.P , it is about 0.45 along the wall.
I have done some studies about different turbulent models , SSL , kw and ke.
For this range of Re,2500-3500, the ke model does not work and in some cases does not converge .
About the kw and SSL , the problem about no slip conditions solved.(attached) for pressure inlet and mass flow outlet.
Now I have two questions :
1- Please tel me about the y+ range for different range of Re.
2- Please tell me that which turbulence model (SSL , kw) is more suitable for this regime of flow and why, with the SSL the is a sharper velocity profile and more pressure drop maybe because of the higher wall shear stress.

Thank you in advance.

Please post images directly on the forum, don't hide them in word documents. Also a graph comparing one profile directly to another would be useful.

Before going into the details of turbulence modelling, have you shown that both of these simulations are mesh independant, time step independent, fully converged, and any other tunable parameter is OK? If not then you are just comparing random numbers and cannot come to a conclusion about anything.

And this is the point - do not refine a mesh to a y+ value. The recommended y+ value is just a guide as to how fine you will need to be to resolve the boundary layer. The final mesh resolution should be determined by a mesh sensitivity study. This simulation may require a finer or coarser mesh than the recommended - you don't know until you test it and find out.

Dear Glenn,
Thank you for your reply,

After your post I tried to evaluate the time and mesh Independence for this case , and meanwhile some questions arose for me.

- I did the physical time step Independence from the 1/3 to the 10 of the residence time , they have the same trend for the convergence , but the question is ; what is exactly physical time step ? and why it is better to be 1/3 of the residual time? the CFL number can specify the time step and because the CFX uses implicit method then it should not make a problem until very large numbers,
Another question about time step that , in of the post I have read that
the time step should not be smaller than advetcive time step on steady state solution , how can I specify the advective time step?
- On the mesh independency study , I have changed the mesh from y+ 0.5 to 1 , and they have some how the same trend and results but on the y+ lower than 0.3 the solver did not converge ,
on another post I have read that reduction of the mesh size will decrease the numerical dissipation and some cases divergence problem will happen.
The question is , how I can understand that my results are correct and what would be the mesh size ?
another question , if the residuals do not go under 1e-5 , does it mean that it is not converged , and what is the main source of convergence and what does it mean if the residuals stay constant , or in a case that they go to small numbers but fluctuating .

I really appreciate your help in advance

You do not need to do a time step independance check for a steady state simulation. The residuals, imbalances and/or the stability of variables of important to you (eg drag coefficient, pressure loss) are the way to judge convergence.

* Convergence difficulty on refining mesh - you are correct, it is caused by the reduction in dissipation in finer meshes. So that means you might have to use a few tricks to get the finer mesh to converge.

* Not converging beyond 1e-5 - this is an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Thank you Glenn for your reply,

But why should I refine the mesh and get divergence problem with very fine mesh when with y+ .5 to 1 I can get the convergence , I mean what is the criteria for mesh refinement ?

And , I have used some output points to check the convergence like velocity , they get to a constant level and residuals goes to their minimum , but what it means when the residual goes to a number and keep constant or fluctuate ?

And please tell me what the physical time step means , does it define the numerical time step?

The criteria for mesh refinement is until the variables of interest to you have converged sufficiently to an accuracy you are happy to accept. Any convergence issues which come up you just have to figure out a way to resolve.

Your question about the convergence flat line is answered in the FAQ.

Physical time step is the psuedo-time step used to advance the equations. For further details see the software documentation.

Thanks Glenn for your reply,

I would appreciate if you tell me what is "imbalance in the domain" and how I can check it on the CFX ?

have a look at the imbalances under the solver manager. Get the available variables up by right clicking on a graph window and select imbalances.

Thank you for your reply,

I found them , but what is the imbalance in the domain? and I have read that it should be less than 1% , why?

It is the global conservation of that variable. The residual is the accuracy the equations are being solved in that specific control volume.

No, there is not a general rule that 1% is good enough. You need to do a sensitivity study on this to find the conservation tolerance your simulation requires.

I really appreciate your helps and useful comments,

I have some questions that needs the idea of CFD experts ,

I have simulated incompressible flow in a simple duct with different boundary conditions , turbulence and laminar , attached .
The Reynolds number is not so high,Re=3000-3500 then I used SST with y+<1 or laminar .

- is it correct to have the pressure inlet and mass flow outlet instead of mass flow inlet pressure outlet ? the profile of the velocity is different as the mass flow inlet imposes constant velocity profile at inlet ,
- at the Mass flow inlet BC , the profile of the velocity shows that the velocity is not maximum at the center far away from the inlet, is it correct .
- What is the exact procedure for the solving other variables when I set the pressure inlet at the boundary, is it zero gradient , is it more physical ?
- for the laminar condition , the velocity profile at the middle of the pipe is lower than some pints of the corner , is it physical ?

They are converged and mesh independent .

Thank you in advance

Sorry for the low quality picture ,
this might be better,

Thanks

1) Mass flow at inlet or outlet - put it where it best represents the flow you are modelling. You can correct in saying that by default it assumes a constant velocity across the section so that will require additional upstream space for the boundary layers to develop.

Your other questions really focus on what is important for you to model. If you are interested in the fully developed flow then you need to ensure your domain is long enough for the fully developed flow to form. That length will be different for a pressure and mass flow boundary (mass flow will be longer). And as for whether the laminar result is realistic - again, if the real flow is laminar then yes. If the eral flow is turbulent then no. CFD is about reproducing the results of the experiment, so you match the models to what happens in the experiment.

Thanks Glenn for your reply,

I am not really concerned about the fully developed as I am doing this as a pilot study for my final simulation, but as far as I know , the velocity should be maximum at the middle , but I see some results for mass flow inlet SST or Laminar , as I discussed before not conforms with this fact ,
And I have another question , should I get the flat velocity profile at the inlet with laminar flow and pressure inlet BC , or generally is it possible to have the flat profile at the inlet with the pressure inlet BC?

Thank you ,

If you start a flow with plug flow (ie constant velocity across the whole section) and allow it to develop into fully developed flow, have a think about how it progresses through the development. You will find that during the development of the flow you will get regions away from the centre which are the maximum flow.

The pressure inlet should allow a flow closer to fully developed.

Thanks Glenn

I really appreciate your comments as an expert .

My question is , how the flow develop such a way that has not maximum velocity at center? Because of the effect of the zero velocity at the wall and the viscous flow then as we go further from the walls we should have highest velocity , I am a little bit confused
And It seems not to be physical ?? Do we have some condition like this in experiment ?

Thank you

Have a think about it - the flow in the centre needs to go faster than the initial plug flow in the fully developed flow. So how does it "know" it needs to accelerate?

If the thought experiment does not explain it for you, do a simulation and have a look at how the flow evolves from plug flow to fully developed.

As it can be seen from the image ,Velocity in the core of the flow outside the boundary layer increases with increasing distance from entrance. This is due to the fact that through any cross section same amount of fluid flows, and boundary layer is growing.
It is exactly the mass flow inlet with inlet uniform velocity profile , but the way that flow develops by the numerical solution is different from what it is seen from the image.
I can not justify the numerical result that center line velocity is not maximum ,

:) The diagram you show is wrong. The person who drew that diagram does not understand the details of how fully developed flow forms.

You haven't thought about it yet - how does the flow in the middle accelerate? What is required to make it accelerate?

Here the reason that can accelerate the fluid is the effective area reduction because of the BL . And as the fluid outside the BL can be assumed inviscid then it should have a flat profile outside BL.
Then I do not understand the cause of non flat profile outside of the BL with the maximum velocity on the corner. I have seen an experimental result showing this issue.
Please refer me to any article that discusses this issue , I need to know about it.

Thanks

Hi again ,

I have attached the experimental result for flow profile development in a pipe.
Please let me know your idea about my previous post.

Thanks

Hi ,

I would appreciate if you can help me out,
As It can be seen from the experimental result(previous post image) , the velocity profile after the BL is somhow flat and in some points in the center a little higher than the corner outside of the BL.
But as previously discussed , if the mass flow inlet is set as BC then we do not see this profile , but after BL , on the corner is higher than the center .
But if we use Pressure inlet as BC then the profile is something that is expected like explained , before Fully developed length it is flat after BL and we can get to fully developed profile after considerable shorter length compared to mass flow inlet.
Then my question are ,
- is the Mass flow inlet a wrong BC because I do not see the correct velocity profile , or I am wrong in the theory or simulation?please explain for me.

The answer to this question is important for me and I hope you help me out.

Thank you in advance.

Do a simulation of flow in a laminar pipe, at say Re=500 (so well laminar) and have a look at how the flow develops.

In turbulent flows it is hard to see the details as it is lost in the turbulence, so the image you posted is not clear.