Shear Strain Rate in non-circular conduit
 

Hi!

I'm trying to simulate flow through a non-circular conduit (see images), my velocity distribution looks ok (I hope) but the shear strain rate is strange.

The pipe is 380 µm long, the radius of the circle is 3,5 µm.

At the Inlet I defined Total Pressure = 0,003 bar
At the Outlet Static Pressure = 0 bar
Reference Pressure = 1 bar
No turbulence, no heat transfer, no buoyancy.
Initialization --> Static Pressure = 0,0015 bar

The circle section has a wall boundary condition and the vertical/horizontal sections are Symmetry.

The pictures were taken from a front view.

Like I said, the shear strain rate is odd...imo it should be much higher on the extremities...

Does someone know why i get this distribution? I would be very thankfull for any advices. I'm nearly losing my mind here.

Thank you in advance and sorry for my english.

Mesh resolution too coarse? Are you sure you are capturing the gradients sufficiently in that region?

If the two straight walls are symmetry planes, both the velocity and the strain rate contours seem to be reasonable.

I suggest Edmund is on the right track - you need to do a sensitivity analysis on the variables of interest to you. In this case that is shear strain rate. This is a difficult variable to get to converge so you will find it requires a much finer and high quality mesh than velocity.

Thank you for the answers. My mesh is only 1 element thick on the pointy edges...this might be the problem. I will try to refine my mesh and see if I can get better results.

Thank you again

So I refined my mesh and simulated it again. It's another geometry, but the pressure values, initialization, etc. are the same.

I get a better shear rate and velocity distribution but it's still not what I was expecting. Is it possible that these distributions are right?

If this is wrong, where can I have made a mistake?

I've posted the images of the mesh on one extremity, the shear rate and velocity distribution.

Again, thanks in advance for your patience and answers.

You have no inflation layer on your surface. You are totally at the mercy of the wall function of whatever turbulence model you are using. This mesh will not capture the near wall gradient that you need to resolve shear.

So I should use inflation layers on the circular section (wall) or on other location?

They go on your walls.

Read up in CFX help on Near Wall Modeling.

Again, the velocity and shear strain rate contours are qualitatively correct.
Why would you expect something else?

Thank you for the advices Edmund.

Alex: The circular section is a wall. The shear rate should be much higher (color red), and not almost equal to the value on the Symmetrys...

How would you explain the low shear rates on the walls?

In the narrow sections of the geometry, the velocity must be low because of the viscous forces.
Accordingly, the shear strain rate will be lower near the edges.
Maybe the problem with understanding the flow pattern arises from the low Reynolds number of the flow where viscous forces are dominant.
I agree that the contours would look qualitatively different at high Reynolds numbers.

But if the velocity is low because of the viscous forces it means that they are high --> high shear stress. My viscosity is constant, so the shear rate must be high to...please correct me if I'm wrong.

I don't get the physics in your explanation

On the CFX Guides they say you need at least 10 layers for the type of flow I'm trying to simulate (laminar flow). I also read that there is a turbulence model for low Reynolds numbers that is very precise for resolving the boundary layer, but I don't have turbulence in the simulation.

I've inserted 25 inflation layers on the wall, but the results are the same as before. I've posted a foto of the new mesh.

What am I doing wrong? All my results this far are similar to what I've posted...perhaps the flow is like this?

Sorry if the questions anoying, but I need results for monday and I got nothing similar to what I was expecting...

Thanks for the help!

In laminar flow the boundary layer is much thicker. In fact if the flow is fully developed there might not be a boundary layer as such, but a gradient of flow across the entire cross section (eg lamianr flow in a pipe develops to a parabolic profile - no boundary layer). Looking at your flow you do not have a boundary layer - so near wall mesh refinement is not going to help.

So in laminar flows the rules of thumb for turbulent flow does not apply. You do not need anywhere near as much near-wall resolution. But how much do you need? As I said previously, you do a sensitivity analysis. Comparing the flows you show in post #6 and 13, you have a maximum shear strain rate of 3.178 and 3.008, so you are already only talking about a 6% change between these two meshes. This is a small amount for shear strain rate - how accurate do you want to be? This would be adequate for most engineering purposes.

If you want to be more sophistcated than a simple sensitivity analysis then have a look at the grid convergence index and Richardson extrapolation in the link from here: http://www.cfd-online.com/Wiki/Ansys...publishable.3F

I also note you chopped the thin cusps off at the ends of the domain. This will make meshing easier, but will alter the result a little. How much will it alter the result? Do a sensitivity analysis and find out!

Thank you for the detailed answer Glenn.

This is only another geometry I have to simulate. I took this one because i thought it would be easier to mesh, but I still have to simulate the other.

The shear rate values (where the distribution is ok) are not a problem. They are pretty close to what I was expecting. My only problem is at the ends, where I expected much higher shear rates and a completely different distribution. Doing a sensitivity analysis will help me get better shear rate distributions at the ends (after adapating my mesh)?

Yes, do a sensitivity analysis - refine the mesh in that region and see if it makes a difference. Keep refining until you have the results as accurate as required.

And if the result continues to be unexpected then the question shifts from being a simulation accuracy question to a flow physics understnding question.

Thank you!!

I alreadx think it's physic related, but I wanted to be sure I was simulating it right...anyway, thanks to all of you for the help!