I am completly new to CFD and currently working on a project where I have to do a simulation of an 2D-Airfoil.
The following data is given:
Fluid velocity: 4.5 m/s
Stationary and incompressible flow
Static Pressure: 3 bar
So for structered mesh, you have to consider the diffrent types of farfields, which effect the quality of mesh, but since Simulation CFD only supports unstructered mesh, I have chosen a simple rectangle as my farfield, with two more fields for denser mesh.
Since I am a novice in this field, I would like to ask you some Questions.
1) My first question is about the boundary conditions: I have set the right edge (inlet) to "velocity" (fluidspeed 4.5 m/s) and the outlet to "pressure" (3 bar gage). The other two edges are set to slip/symmetry. Are these BCs chosen correctly?
2) I am amazed but at the same time sceptical about the mesh generation. It seems really easy to generate a unstructured mesh but at the same time I can't estimate its quality. Seeing the results, my generated mesh seems to do a good job. Could one of you take a look at my mesh and results? So far, I have mostly seen hexa-meshs for 2D-simulations, but can a tetra-mesh be that accurat too?
3) How can I make a cp-plot (pressure coefficient along both surfaces (pressure and suction side)). I have an excel-file with points of interest for measuring. Is there a possibilty to import these points? How do I get infos on pressure loss and energy dissipation?
4) My last question for now: Autodesk Simulation CFD chooses the Standard k-ε turbulence model by default. I don't know where I can change this but is this model suitable for my task?
I know these are quite some questions, but I would really appreciate it if you guys could help me here.
Many Thanks and Best Regards
PS: Here is the result file
Solved! Go to Solution.
I can try to help here
- The Boundary Conditions are OK. Although you would be better off settting a P=0 at the outlet and a reference pressure within the environment (right click on materials within the Design Study Bar)
- Simply, yes Try shading the model by mesh (a button at the very top of the screen) or plot Nodal Aspect Ratio with an ISO surface (turn on Stream Function within Solve > Result Quantities to enable this)
- You should be able to make a plot using your points (this is great approach in 2D), if you go to Results > Planes > XY Plot, there you can choose 'read from file'
- Might be better with SST. You can change this within Solve > Physics > Turbulence. You can also look on AKN - Turbulence for any of this. Check out the reference to using 10 boundary layers, although you may wish to check the mesh to ensure they are still within a reasonable distance to the solid surface
Your results look OK although it might need to run longer. Try turning off the automatic convergence assessment and running it longer (Solve > Solution Control > Advanced).
I am not sure why you chose to turn off Intelligent Solution Control, leave it on
Hope that helps
many thanks for your detailed answer. I have made a new (hopeyfull better) mesh. Could you plz have look on this once again and tell me what you think about it? I also have enabeld stream function in the results and added a iso surface too, but I dont get how to see the nodal aspect ratio.
I have turned the automatic convergence assessment off, because the solver seems to end the calculation too early, as the vy-component was not converging completely. Also the general flow of this setup does not seem to be fully developed (see red circles in the screenshot). What settings should I apply so that the automatic convergence assessment does not stop the iterations too early?
For my future calculations, I've set the SST k-omega turbulence model and 10 boundary layers. The problem of adding the coordinates of the measuring points still remains, as the xy-plot only accepts .xyp-files. But the coordinates, I have are given as excel-files. Is there any possibility to convert them to .xyp? Or can I use Sketch or Work points direct vom Autodesk Inventor 2013? Is there any other way to measure values along the suction side for example?
I have set the static pressure in the materials section to 3 bar and for the oulet to 0 bar, but looking at the results it only shows 0 bar in the farfield. Whats wrong with this?
Plz bare with me Jon, I might be asking to many questions but I would like to achieve best results out auf Simulation CFD
Many many thanks in advance
With kind regards
PS: Here is the new simulation. Same profile but with a Gurney-Flap at the trailing edge.
No problem at all.
Good point, I guess there is no Nodal Aspect Ratio in 2D, your mesh quality is fine though. Run a quick mesh sensitivity study if you need to verify it. Refine the mesh to 0.7 and see if the results change significantly (more than 5%).
Looking at your model, the Automatic Convergence Assessment is still on turn it off and CFD will run as long as you want it to.
I think you can just rename an xls to xyp. List all the points down the first column only (#,#,#). That should work I think.
If you look at Absolute Pressure, that should show the correct pressure. Although you will need to right click on the legend and change the scale, or it will just all be red.
It's probably clear to you Usman_s, but looking at your image and the pressure plot above this particular airfoil at this angle of attack has a substantial area of separated flow, with that and the gurney flap causing periodic vortex shedding. It may never converge completely to a single solution. If this is a static model this shedding will not necessarily be physically accurate but will cause the solution to oscillate somewhat, which you may be able to see if you place some monitor points in the wake region.
Do you care about these stalled cases? If not lower the angle of attack & nevermind... But if you care about the separated cases, you may need to find a way to relax the simulation and/or do some averaging. John, is there a way to do this in a static simulation? (the most time/resource consuming but appopriate would be to time-average the results of a transient simulation at a pretty fast capture rate once it has settled into steady oscillation.)
I was thinking the same and the convergence plot suggests you are right. Although I would like to see how it performs when run out futher. Looks like it might stabilise...
If not then really the best solution would be to run a transient, this is 2D so entirely possible.
thank you for ur answers and sry for my late reply. I've applied ur suggestions and have set the 3 bar environtal pressure in the materials scection. I have also slightly changed the mesh and made some calculations with different Angles of Attack. I have the feeling, that the flow in these calculations tends to break-off very early. You can look at the settings & results in the new file I have uploaded. I also asked a person who by profession does cfd- calculation with ansys cfx. He did one simulation with my airfoil for aoa = 0° and his flow does not seem to break off. he. Also after seeing my results in simulation cfd, he told me that my solution (especially for aoa =10°) does not seem to be stationary, as the flow behiind the airfoil looks "wavey" which is unusual for stationary solutions. He gave me these two screenshots. Maybe you can help me here. How can I achieve same results? Btw. he used the same parameters
5 m/s water speed
advection scheme: upwind
and so on...
PS: New result file
Here is my quick results:
Some notes on setup:
More mesh the better along the wall. This my go-to settings for this kind of thing. Depending on what the results look like I adjust from there.
Solution I turn off for external aero problems like this to speed up the simulation. If unstable then turn solution control back on. Leave the sliders in the default position.
Auto Startup could be left On, but Off helps speeds things up again. If unstable then you would turn back to On
This was my first attempt quick results... I would technically like to add a mesh refinement region in the wake, but even though it seem to be captured fairly well.
Many thx for your detailed instructions, Royce . I have applied your suggestions and the result has improved, but it still does not look like yours. Also I could not find the "Enable enhancement blending" option. May be it's named as mesh_boundarylayer_blend under flags? How can the Max and Min values in ur simulation be the same as in Ansys? Have you set them manually? I have uploaded a new result file. Could you plz have a look at it again and upload your .cfz-file from your last calculation? How many iterations did u run?
Many many thx in advance
PS: I am using the student-version of Simulation CFD 2014
Ha! Maybe I jumped the gun a bit. The flag will work for you, the CFD 2015 interface now shows that flag option as part of the UI so we don't need to use the flag moving forward.
Yes, I locked the lengend to new values. Easier to compare.
Take the region all the way to the exit of the domain. You'll notice after the mesh expansion the wake mostly disappears or diffuses away. Not desireable.
I had run for 6663 iterations. Your model hasn't finished solving yet.
Give those changes a shot!