Inviscid Analysis

[Anonymous]

Does anybody have an idea of how one might approach an inviscid (essentially potential flow) analysis using CFDesign/Simulation CFD?  Is this even possible?  Any advice would be appreciated.  Thanks.

[Royce_adsk · Accepted solution]

Hi Matt,

This is possible!

Procedure for simulating an Euler (inviscid) flow solution with standard solvers:

1. Create a material with a viscosity of 0 (or very close to 0).

2. Assign slip to all the solid walls

This removes viscosity from the solution.

Another option is that you could use the 'Quick Forced' solver (Quick Forced has a potential flow solver).  Solving for potential flow naturally ignores wall constraints and fluid visocity so the above settings do not need to be followed.

Note: a viscosity that is exactly 0 can cause solution instability. If you see this, use a value that is very close to 0 (such as 0.000001 Poise).

(LINK)

[Anonymous]

Royce,

Thanks! I will give this a shot.   I am curious though, why the slip BC at the walls? 

[Royce_adsk]

When you make the assumption of Inviscid flow you also expect that there be slip at the walls, therefore you need to add the slips.  Otherwise you would still get a 0 velocity along the walls.

-Royce

[Anonymous]

This (sort of) worked.  I was not able to get it to run smoothly using viscosities less than 1e-4 poise, and even then I needed the 'Check Velocity Distribution' flag file command to get it to finish.  Ultimately, however, this did not get me to the results I was shooting for.  There is still a large amount of laminar separation, which is what I was trying to avoid, so that I could check the results of a potential flow calculation.  Any thoughts?

[Royce_adsk]

Would is be possible for you to share your support share file?  Would you consider it NDA or have something that you could mock up quickly?  Otherwise we will have to take it offline to a real case.

-Royce

[Anonymous]

Royce,

 It is not proprietary.  The file is supposed to represent an annular NACA 66(2)-015 airfoil.  There are experimental and potential analysis results published in Lewis, 'Vortex Element Methods for Fluid Dynamic Analysis of Engineering Systems' Cambridge University Press, (C) 1991.  He offers a Pascal code in the back which we are trying to use, but his code results do not match what he published.  We are trying to decide if his results are incorrect or if it is his code that is faulty.  The analysis is laminar and axisymmetric in X.  Also, I am using CFDesign 2010 not Simulation CFD if that makes a difference.

That all being said, the website will not let me attach a *.cfz file.  I get the following error:

Please correct the highlighted errors and try again.

• The file does not have a valid extension for an attachment. doc,pdf,dwf,dwg,dxf,dst,gz,gzip,zip,bm,bmp,gif,jfif,jpe,jpeg,jpg,psd,tif,tiff,png,htm,html,xml,xls,lsp,svf,3ds,vcf,png,text,txt,log,env,dcl,rvt,rfa,ipt,iam,ipn,dwfx,idw,csv,nwf,nwc,nwd,sdf are the valid extensions.

[Royce_adsk]

That is odd.

Change the extension to .cfz.txt

-Royce

[Anonymous]

Here ya go!

[Royce_adsk]

Matt,

Do you have access to CFD 2012?

-Royce

[Anonymous]

Royce,

I do.  We have been avoiding using it though because it has been very problematic for us. I can run this in 2012 overnight if you think it will make a difference.

[Royce_adsk]

Just checking so that if I do some test on my end I can give you a share file to try out on yours.

-Royce

[Royce_adsk]

Can you give more detail on what you are looking for in the results?

-Royce

[Anonymous]

Royce,

We are comparing pressure coefficient and velocity ratio distribution.    I have attached the published results for your reference.

[Royce_adsk]

Matt,

Here are my results from last night.  Do they look reasonable to your expectations?

-Royce

[Anonymous]

Royce,

This is basically what I was seeing.  This really isn't very similar to a potential flow solution though.  There would not be low velocity regions on the airfoil surface (indicating separation), rather the flow would be attached and tangent all along the wall.  The problem is probably too basic for this software to handle.  This isn't too bad though.  It will still give us something close, I think.  Thanks for the effort!

[Royce_adsk · Accepted solution]

Matt,

One last thing for you to checkout.  I turned on the quick forced flow solver.  When Quick Forced Convection is enabled, the flow is computed using a potential flow computation that is complete in one iteration.  When there is no heat transfer boundary conditions present, the heat transfer portion of the analysis is skipped.

-Royce

[Anonymous]

Royce,

PERFECT!!!  This is exactly what I was trying to do.  Thanks! 

-Matt

[RitaSchnipke]

You should be able to run a potential flow solution using the "Quick Forced" option on the "Solve-Physics" widget. You don't need to set any thermal conditions. This should give you a potential flow solution to your problem.

[Royce_adsk]

Matt,

Here is my share file.  If you could share your results on how they compare to the published results, that would be excellent!

Thanks,

Royce