Hi guys,

I am running a wing (basically flat plate at 0deg alpha) in free air. The doman is a cube, with a symmetry plane on the one side. My inlet B.C. in Pressure inlet, outlet B.C is Pressure Oulet and my "free air" condition is Pressure Far field.

The material is set to Ideal gas to use the Pressure Far field assumption.

I am running at 50m/s, so my farfield pressure is specified with Ma=0.144001 (gamma=1.4,R=287.05,T=300K) and my inlet Total pressure is defined as 1487.412Pa (based on static density at the inlet).

My case converges to 10e-4 in continuity (everything else 10e-6), but when I look at the dynamic pressure on the inlet - it is not constant as I expect it to be?!

Thanks, Riaan

Update:

I am going to try putting Pressure Far-field conditions on ALL my walls ie. inlet, outlet, far-field. That way I only need to define a single Mach number everywhere.

Comments if this valid?

The only B.C.s that should be touching a pressure far field condition is a symmetry or periodic condition. When a pressure far field contacts any other type of boundary condition (especially wall, but including pressure inlet/outlet, velocity inlet, mass flow inlet, etc...) there tends to be a discontinuity at the intersection. You can use other B.C.s that touch the P-far field, but the best way to use a pressure far-field condition is to use it for the entire "ambient" condition. This minimizes error, and improves convergence of solution. If you look at the Fluent tutorial for a 2D airfoil, they use P-far field all around, even at the outlet. Just make sure that the P-far field is far enough from the body impacting the flowfield that the constant mach and pressure assumptions are valid.

Hope this helps, and goodluck Jason

Tried setting all my B.C to Pressure Far Field (PFF), but I am having issues with convergence.

I am running Laminar,Steady, 1st Order Segregated. I tried switching to PISO Pressure Velocity coupling, and also lowered some of the under-relaxation factors...everything except massflow converges ;-(

Riaan, you didn't specify the size of your wing, so we don't know what the Reynolds number is, but I suspect that it is far too high for laminar flow, in which case you might expect pretty serious convergence problems.

Hi Riaan, I had a case like yours and I used the P-far field all around except the simmetry condition on the surface of the root of the wing. I had no problem at all. I used the inviscid model and the laminar flow. The only thing I would suggest is to put the Far field surfaces quite far form your wing (at least 5 time your aerodynamic reference chord, i used 10 times). Then lower the under-relax factors. I got no problem at all. Luca

Also, you have to be careful that the Pressure far field is far enough from your wing that there is no gradient on the BC (they recommend 5 chord lengths in every dimension, but I recommend 7-10 just to be sure). If any pressure or velocity variation intersects your BC it causes big problems, especially with the continuity residuals (and therefore your massflow). This goes back to the BC's assumptions of constant Static Pressure and constant Mach Number.

Charles is also right that you might be out of the laminar region.

Just things to consider.

Hope this helps, and gooluck Jason

Thanks for all the help. I have been spending time building a journal file that would allow me to vary the domain dimensions in order to see if my B.C were too close to my wing.

Currently, my Pres-Far Field walls are : 2 chord lenghts upstream, 5 chord lenghts downstream, 10 chord lengths high and 5 chord lenghts wide (H-topology) - but I will change these values and see if this helps.

As for the Laminar flow - Reynolds number based on chord is approximately 2.1E+06, so I am expecting that the flow would become turbulent - but the strategy I was following was to get the solution to converge somewhat and then switch over to a turbulent model.

If that's the case, then just turn off the turbulence model under Solve->Controls for about 100-200 iterations, and then turn it back on. Don't go for complete convergence, you just want a better defenition of the flow field before turning the turbulence model back on. The laminar model is just another turbulent model and is going to cause problems at this high of a Reynolds number.

Hope this helps, and goodluck Jason

Nope, still no convergence. I tried refining my mesh and setting a turbulence model (S-A), after about 1000 iterations, everything converges to 10e-8 except continuity....

I will see about posting my Gambit journal file here a bit later, if anyone would be so kind as to have a look at it and maybe give some pointers.

What are you using for convergence criteria? The residuals you are looking at are normalized based on the residuals in the first iteration. What else are you using for convergence criteria (are you monitoring forces, mass flux, etc...)? Your model might be converged.

Also, I just noticed something in your original post... you said you used a pressure-far field condition, and then you said that your total pressure was 1487Pa... In a pressure far field boundary condition you are defining Mach Number, Static Pressure, and Static Temperature, not total... wasn't sure which you were using to define the P-far-field. You probably were using that for the Pressure-Inlet, but I just wanted to make sure.

Jason

After the first couple of runs with Pressure Inlet B.C and Pres-Far-Field, I had switched over to using Pressure Far Field for all my B.C (including inlet and exit).

As for the residuals, the Cl and Cd level off and energy, Nut (from S-A turb.model) and x,y and z velocities are all down in 10e-7 range.

Its only the continuity that won't go below 10E-2. I will check my convergence criteria again and get back to you.

If your Cl and Cd are converged, as well as all of your turbulence criteria, then your model is probably converged. Since the residuals you are plotting are based on the residuals from the first iteration, your continuity might not drop any further. Things that tend to cause large changes in the continuity residuals are separation regions, shocks, and poor initial guesses. If I remember correctly, your modeling an airfoil at low mach number. You're probably initializing your model based on the ambient conditions, which is pretty close to the final solution. If this concerns you, some possibilities include: refining your mesh (sometimes works, sometimes doesn't), or initialize your mesh based on a lower freestream velocity (i've heard this works, but never tried it).

You should do a mesh sensitivity, and as long as your Cl and Cd are leveling off to the same number as they are now, then you have a successful model.

Goodluck, Jason

Ok, I checked my convergence criteria, and the normalization of the residuals is off. Should I turn this on?

I am also thinking that Fluent may have problems with the sharp corners I have in my flowfield....but which is unavoidable in the H-type topology.

I will post my gambit journal file shortly.

Hi, here is the journal file I wrote to generate my Delta wing at 0deg Angle of Attack. It is a H-type mesh using structured elements.

http://www.100megsfree.com/maverick/...tterAspect.txt

I would appreciate it if you guys could give it a run in Gambit and give some suggestions/comments if I made any obvious mistakes?!

Thanks, Riaan

Why are you saying that your model isn't converged? What I was trying to say before is that if all of your residuals level off, and all of your monitors level off, then you model is converged, even if the continuity residual isn't dropping as low as the other residuals. If everything is leveled off, then check your mass flux just to make sure you're not losing/gaining mass. There will be a slight imbalance, but that's just numerical error in your solution, and is to be expected. You should do a mesh sensitivity to show that your results aren't a function of the mesh, just the model, but other then that from the sounds of it you have a converged model.

Jason

Ok, maybe I should ask my question differently. Assuming my model converges (monitors and criteria level off), why is my continuity residual still so high?

The residuals are based on your initial guess. Your velocity residuals are going to drop because your initial guess has the flow going in one direction, so it suddenly has to turn at the nose of the wing (for example). Your energy and turbulence residuals are going to drop because your initial guess has no near-wall turbulent info, so the energy and turbulent residuals (k & epsilon, or nut, or whatever depending on which turbulence model you're using) have a sharp change to deal with the flow along the wall. The continuity residuals however do not suffer the instantaneous shock that the other residuals suffer. It's still an impact, but much less of one, and since the residuals you are plotting are all referenced to the initial residuals, the continuity doesn't under go as much of a change as any of the other residuals and will not drop as much as the other residuals.

A rough estimate is that you want all of your residuals to drop 2 orders of magnitude, but it's not a law, just guidance. If your residuals don't drop a full 2 orders of magnitude (and actually even if they drop more than 2 orders of magnitude), then you have to rely on your monitor data as well as inspecting the results. Does the resultant flow-field make sense? Are your pressure drops occuring where they should, and are your forces reasonable? If you've got a 1' long wing producing 5-tons of lift, then there's obviously something wrong.

Also, doing a mesh sensitivity study should help you feel more comfortable with the results of your analysis.

I hope this helps Jason

The forces (lift and drag) appears to be reasonable and the flowfield looks correct (1st order at least)

From my mesh, you can see that I have several sharp corners, and it could be that there are issues with the continuity equation at these points. I will try and put in radii and have another go at it.

As for mesh sensitivity, as soon as I am sure I got most of my obvious mistakes, I will do one. Since I am using structured grid, this is not too difficult.

When I did a quick 2d simple model of my case, 2ddp converged the continuity, while normal 2d leveled off at 10e-3. Could be because I have very high aspect ratio cells (<900)

I will run my 3D case at dp, and let you guys know the results.