Velocity Profile in a Pipe - 2D Axisymmetric

[Anonymous]

 Hello!

I am working on modeling the velocity profile of various flows through several different pipe sizes.  I have done this before using a 3D model (http://forums.autodesk.com/t5/cfd-forum/velocity-profile-of-water-in-a-10-quot-pipe-for-various-cfd/...) but was hoping to save a lot of time by doing future studies using a 2D axisymmetric model.

Unfortunately, the results do not seem to match what I expected.  Please see the screenshots below for details.  The inlet is on the right-hand side (BC is v=20 ft/s) and the outlet is 30 diameters downstream, on the left-hand side (BC is p=0psi).

The profile changes as the flow moves downstream--shouldn't it be the same all the way down the length of the pipe?  It also appears much "flatter" than expected, with the only gradients occurring very close to the wall.

Any help would be appreciated!

Thank you,
Eric

[Jon.Wilde]

Hi Eric,

Nice to see you still using CFD 🙂

I would think what you are seeing is the change from non to developed flow, which is why we usually have a ton of diameters upstream before any region of interest.

The further to the left you get here, the more accurate the curve I would think.

I would also say you should refer back to the 3D thread, think about Y+ again etc 🙂

Hope that helps,

Jon

[Anonymous]

Hi Jon,

Thank you for the quick reply!

I added a lot more straight run (120 D) and switched to a manual mesh which seems to have drastically improved my results.

Is there a good way to check y+ values in a 2D model?  When I switch to view them in the Global results it just gives me the scale and then shades everything blue.  I can't identify the high value regions even if I change the scale or zoom in.

Thanks again for the help!
Eric 

[Jon.Wilde]

Hi Eric,

No worries 🙂

The scale should be enough I think? But to look more locally, maybe an ISO surface?

[Anonymous]

Hi Jon,

The ISO surface worked, thank you!  I didn't realize that they were enabled after a 2D analysis.

I have one more question.  I thought I had everything in the bag, but then found that when I run the analysis at 8 ft/s everything falls apart.  The results looked great at 20 ft/s so I cloned the scenario twice and changed one to 8 ft/s and the other to 2 ft/s.  The 2 ft/s analysis came out cleanly, but the 8 ft/s analysis came back covered in spots instead of the nice, curved velocity profile I'm getting on the other runs.

Is this because the mesh is so fine that more iterations are needed?  It didn't seem to be conforming to anything close to a normal flow profile.  Except for the velocity it should have had the same exact settings and number of iterations (4000) as the other scenarios.

Thank you!
Eric

[Jon.Wilde]

OK, agreed - that looks weird 🙂

Try running it out for longer, yes. Maybe turn off the convergence assessment entirely so it doesn't stop until you are ready.

Thanks,

Jon

[Anonymous]

Hi Jon,

Running it out for more iterations seemed to help eliminate the "splotches."

New question:  why is there such a difference between running the same simulation with the KE and K-omega turbulence models?  See the screenshot below for both of their profiles.

 
This was the crux of my issue with the 3D model, and I never feel like I really understood the disparity. This is a 2D model now, so I have a very fine mesh and low y+ values--shouldn't both turbulence models predict the same result?

 
Thank you in advance for your insights!
Eric

[Anonymous]

Update:  It looks like the finer the mesh, the more the KE seems to agree with K-omega.  Each "Copy" run in the screenshot has a progressively finer and finer mesh.  I'm going to try kicking off a few more runs to see if it ever converges on a shape.

[Anonymous]

Jon,

I wanted to post this graph as it summarizes all of my analysis thus far.  I think this issue may require some in-depth assistance, though, so I have opened a support case.  I uploaded my CFZ file there.

Thank you for all of the help,
Eric
 

[Anonymous · Accepted solution]

Hi Eric,

you may have to consider that for kEps the mesh can be too fine near the wall and produce unnatural results. Check the help system for intelligent wall formulation and make sure it is enabled.

Marco

[Anonymous]

Hi Marco,

Thank you for the assistance!   Turning on IWF made the profiles of the KE agree with those of the K-omega:  

I did not have Intelligent Wall Formulation turned on for the K-Eps runs, but did have it turned on for the K-omega runs. 

As the help file you linked to mentions, IWF is turned off by default for K-Eps turbulence models, but I've been using it for K-omega because I believe it was recommended in the "Understanding Turbulence Models" webinar (although I couldn't find it when I just went back to check).  The webinar is here: https://www.youtube.com/watch?v=Yf2iVABc8cg

Is there a reason why IWF is turned off by default?  Should I turn it on all the time, or are there cases when it's detrimental to the analysis?

Also note that I changed the advection scheme from ADV1 to ADV5 per the recommendation in the help file--I'm assuming that won't affect this profile?

Here is the help file I'm referencing: http://help.autodesk.com/view/SCDSE/2015/ENU/?caas=caas/sfdcarticles/sfdcarticles/Intelligent-Wall-F...

Thanks again for the help,

Eric

[Anonymous]

I read up a bit more on IWF and think I have an understanding of it now.  Checking that box allows the program to ignore elements too close to the wall for the KEps model to handle (y+ of about 12).  

I found where Royce mentions it in the Turbulence Model webinar (around the 11:30 mark): https://youtu.be/Yf2iVABc8cg?t=11m24s

Thanks for the assistance, I think my issue is resolved!