turbulent kinetic energy is not zero at the wall
hi all
i am solving multiphase turbulent flow problem. velocity profile is correct but turbulent kinetic energy and intensity is not zero at the wall, although it should be zero at the wall. turbulent kinetic energy and intensity is showing maximum on the wall. i do not why is it so? i need help thank you 
i am waiting for guidance from experts. it will really help me a lot.

What kind of wall modeling are you using? If you are using a wall function with Y+ around 60 it is normal that the TKE has a maximum value in the first cell away from the wall. If I recall correctly, the maximum for TKE is occurs at around Y+=30 for a flat plate.

Thank for your guidance
In my case fluid is flowing in a circular pipe. i am using komega viscous model. As you told wall model and Y+ value, i am not clear how and where to use wall model and Y+ value. i mean where is the input for Y+ value in gui. probably you are getting my point thank you very much 
Y+ is not an input parameter.
It is the nondimensional wall distance of the first cell. You can evaluate it as a postprocessing variable at solid walls. The only way to influence it (besides the flow conditions) is with the mesh size. If you want to resolve the boundary layer and thus capture the "correct" behavior of the flow variables near the wall, Y+ should be around 1 as a rule of thumb. Additionally, you will have to use the "enhanced wall treatment" in the turbulence modeling section. 
thank you very much Alex S

It may help to use the scalable wall treatment if it is available with the turbulence model you are using. This applies the different wall treatments based on the value of Y+ or Y* as far as i am aware.
I had this problem as well a while ago. Good luck. 
Quote:
I think the question is to ask why turbulent kinetic energy and turbulence intensity are not zero at the wall, but the replies are all related to Yplus! The answer is, FLUENT doesn't implement zero boundary condition for kinetic energy k (k omega based model)! It uses zero gradient boundary condition (the change rate across the wall boundary is zero, instead of fixing a zero value for k), so you will see a finite value of k on the wall. I don't know why FLUENT does this. Among literature, I see some use zero, while some use zero gradient. You probably need a reference discussing boundary condition. The k change very near wall surface may be quite not trustful. One guy from my university shows me the difference from FLUENT and inhouse DNS code. He then implements a UDF turbulence model using zero value boundary condition and also finds difference from FLUENT default turbulence models. Sheng 
All times are GMT 4. The time now is 17:01. 