noslip 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 (noslip wall) does not have lowest velocity. On the contrary, the pressure map from CFXpost 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 noslip 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 1e5 as initial start, and am running more cases with less residual 1e8 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 noslip 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
1 Attachment(s)
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(ke). 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.

2 Attachment(s)
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= 1e4 but I considered first layer thickness of 5e5. Please let me know if there is anything wrong with the formulas , I derived them from the ANSYS CFX manual. I used ke 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.

4 Attachment(s)
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,25003500, 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 1e5 , 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 
All times are GMT 4. The time now is 17:29. 