Computational Aerodynamics Questions & Answers

Question by Student 201327132 Professor, I have a question about design. In problem 3, Should we consider about 3 shocks when I generate grid? I made grid that is consider 3shocks. But I think it is not correct grid. If we should consider about 3 shocks, Would you please some hint for me?	05.27.18

Yes, for problem 3, there should be 3 oblique shocks and the pressure ratio across each shock should be the same. You need to design your inlet so that these 3 shocks appear, have all the same pressure ratio, and meet at one point. I am not sure what you don't understand. Can you explain better the problem?

Question by Student 201327132 Thank you professor. I have a problem with some grid. My strategy is attached pircture. To generate oblique shocks, I set the very small value that is length of between (im 1, jm 1) and (im 2, jm2). Likewise (im 3, jm3) and (ie, js). And plot the my strategy(also i attatched picture). I think it is not correct method, but i didnt find better method. Sorry for my lack of explanation.

Your grid has issues. You should make the grid so that the spacing is more or less uniform everywhere. Don't worry about making the grid parallel to the shocks. The shocks can go through the cells at an angle — this is fine. Simply make sure that your bottom wall has the right shape, that the cells are more or less of the same size everywhere (and are not distorted as in your mesh), and the shocks will appear correctly positioned.

Question by Student 201327103 professor, How can I open the post file? I want to know number of properties, like density : 7, but I can't open the post file.	05.28.18

The instructions are in the CFDWARP HOWTO here: ​ https://bernardparent.ca/viewtopic.php? ... 6568#p6568 ​ You need to read in the data file with the -i flag and output it to a post file with the -op flag. Also, specify a gnuplot datafile with the -pt gnuplot flag.

Question by Student 201427116 Professor, I am doing Design Problem #2, flow over cylinder. After manipulating some code, I printed out drag coefficient but found some weird drag coefficient. The drag coefficient had negative value. Can I ask you some advice for this negative coefficient? $$ $$ Also, I cannot understand what those xstation[] or Area[dim] in Post() module mean. If I need all of xstation[1], xstation[2], and xstation[3]? or can I just erase it? It will be big pleasure of me to learn more about that. Then I may find out some errors in that Post(). Thank you.

Please attach a picture of the pressure contours around your cylinder. Maybe your flow is not yet at steady-state. Because you are doing the cylinder case, you don't need the xstation. Inside the Post() module, delete the part about the x-station and only keep the line Fpressure[dim]=_Fpressure(... Then, add a bit of code to find the drag coefficient using Fpressure[1] (the pressure force acting on the body along $x$).

Question by Student 201327132 Professor, I have a question about design problem No.4. I run a my case. And I tried to find converge point of shock. But I don't know each shock angle at point. Do I need the shock angle? If not so, I think we should know length of between each shock. I have tried a lot. I didn't find converge point. Thank you.

Problem 4 is harder than the others. You need to find $\sigma$ and $\delta$ for each shock using the obliqueshock program. Once this is done, you need to find the bottom surface of the ramp that will make all shocks meet each other at one point (such is only function of $H$, and the 3 $\delta$s and $\sigma$s). Thus, this requires a bit of geometrical calculations on paper. I recommend another problem if this is taking too long.

Question by Student 201327103 professor, i have some problem to run 'warp -r control.wrp -i data.01 -opm'. Terminal say 'could not interpolate at j=0 k=0 for xcut=1.000E-01 m..' what this mean?

Here xcut is the xstation you specified in the Post() module. The program can't find a proper xstation at 0.1 m. If you are solving Problems 1 or 2, you don't need to create xstations, so get rid of the code related to the xstations within Post(). If you are solving Problems 3 or 4, you need only one xstation fixed to the $x$ just slightly before the domain exit.

Question by Student 201327133 Professor, i have a question about ximax. You showed us that ximax being similar as zero when state is steady. I run the code about Question #3, and i've got the result about time,iter,etc... but there is no more less than 1.0E+3 at ximax. but i can't believe that it could be zero... is it correct result? or are there more exact solution?	05.29.18

As I explained today, ximax probably won't go down to zero for your problems if you use the TVD Van Leer limiter or WENO. The residual will thus “hang”. So, you can't rely on ximax to determine convergence. You need to proceed differently as explained in class.

Question by Student 201227111 Professor, I don't understand what the value from -opm command mean exactly. At first, I thought it was the average of values at x=x_station and y=(node1 to node 60). So, I extract data at i=2,10,20,30,40,50,60 and j=1 to 60 using "-pr" command. And averaging each value, And compare to value obtained from "-opm command" with varying x_station. (compare density, Temperature, velocity) When i is small, "-opm" value is similar to my average value. But the bigger the i, the bigger the difference. When i=60, "-opm command" value is similar to average value of i=60, j=1 to 20(only 1/3 nodes). So, I'm stuck here, I don't what to do after. Sorry about my poor explanation.

05.30.18

I need more information. Please show a plot of the pressure contours. Also, show your code in the Post() module. Further, how are you invoking warp with -opm? I hope you read in your data file... Otherwise, this will simply post-process the initial conditions..

Question by Student 201227111 Professor! I bring more explain about previous question. I wanted to know the meaning of Post() modules command to compute mass flux average stagnation pressure. I simply gridding like this.(ie=60, je=60, dx is constant) Result is like this. And My post code is same as original, only changing x_station[1] set to L-1e-5 (L is length of inlet)) and for loop range set 1 to 1. And I use "warp -r design3.wrp -i data.1500 -op post60.1 -pt gnuplot -pr 60 1 60 60" this command, I get properties that x is fixed in one line and y is vary.(like above picture) And, use matlab code, I compute average of each properties($\rho$, $T$, $q$). Then, I compare this average value to value that obtained from "warp -r design3.wrp -i data.1500 -opm". (Because properties vary along y axis but using "warp -r design3.wrp -i data.1500 -opm" is give only one value) then my computed average value is $\rho=0.2774$, $T=467.5837$, $q=2403.5$, but value obtained by "-opm command" is $\rho=0.6730$, $T=789.1027$, $q=2297.65$. I think value obtained by Post() module is average of value on fixed x line, but it isn't. It only work when i is very small(only 2 or 3..). So I want to understand about meaning of value that obtained by Post() module. or I think something wrong?

Everything seems fine except your matlab values. Are you doing a simple averaging using matlab? This will of course be wrong. You need to do a mass flux averaging (do $\frac{1}{\dot{m}}\int P d\dot{m}$ in matlab not $\frac{1}{H}\int P dy$).

Question by Student 201327103 professor this is my counter plot for cylinder. I can't get shock wave. I Think my boundary condition is wrong, but i don't know where is wrong. here is my code

The problem may be that you are imposing free stream boundary conditions on all boundary nodes..? You should check your boundary conditions are well imposed using the -on flag.

Question by Student 201327103 Professor, i check the boundary node and it looks like good. but the result still has same problem

This looks fine: your boundary conditions are well imposed. The contours you showed previously seem to have not been iterated at all. After the iteration process, are you reading in the data file (obtained after 1000 iterations or so) before outputting the post file?	05.31.18

Question by Student 201327132 Dear professor, I have a question about order of accuracy P. Assuming P>1, We obtained $GCI_f$. If P<1, Should we change to$\left\vert\frac{\triangle x_c}{\triangle x_f }-1\right\vert$? I obtained P that is smaller than 1 and minus value. Did I do it wrong way? Thank you.	06.11.18

Very good question. We made this assumption only when deriving the GCI. So, within the $\rm GCI_{f}$ equation, you should change the term to $\left\vert\left(\frac{\triangle x_c}{\triangle x_f }\right)^p-1\right\vert$. That is, the GCI should always be positive. However, when determining order of accuracy $p$, we did not use the GCI and we did not assume that $p$ should be greater than 1. So you should not change any of the equations used to determine $p$.

Question by Student 201427116 Professor, I have a question about WENO. We used below terms in WENO: $$ {\bar w_0} = \frac{\gamma_{0}}{{(\epsilon+\beta_0)}^2}, {\bar w_1} = \frac{\gamma_{1}}{{(\epsilon+\beta_1)}^2} $$ There is $\epsilon$ in denominator but what is it for? and how can I decide the value of $\epsilon$ ? $$ $$ Another question is about $\gamma_0$ and $\gamma_1$. With Taylor series expansion, we found $\gamma_0=\frac{1}{3}$ and $\gamma_1=\frac{2}{3}$ for 3rd order accuracy. With 3rd order accuracy, that is, WENO3, does $\gamma_0$ and $\gamma_1$ have fixed value of $\frac{1}{3}$ and $\frac{2}{3}$, respectively? Or are they also variants?

06.13.18

The user-defined constant $\epsilon$ is included to prevent a division by zero. Set it to a very small value. As for $\gamma_0$ and $\gamma_1$, they are fixed constants: don't change them.

Previous   1  ...  4 ,  5 ,  6 ,  7    Next  •  PDF 1✕1 2✕1 2✕2  •  New Question