Is anybody using CFX (any of the codes) for shock wave calculations and interactions at high Mach numbers.
Re: Shock waves
Yes I have used CFX to successfully model shock waves. I have some info about it on my home page: http://www.eng.uts.edu.au/~glennh/UTS.html
For a introduction to the area, see Reference example 16 in the CFX 4.2 examples. It models a steady state shock.
From memory, (I did the work a while ago), a key factor for stability in the transient case is keeping the maximum CFL number under 0.3. Hope this helps,
the link to your website is dead. could you update the link?
by the way, I hope you can share some info about modeling the shock wave regarding my case (head inside a domain).
I am giving the first domain an intial velocity of 400 m/s and pressure of 125 psi.
The second domain rests at 14.7 psi with zero initial velocity. the object (head) is located in the middle of second (low pressure) domain and I am hoping to see the shock flow around head.
Now I am running the case using subsonic setting. I was wondering if I shoudl change the setting to Total energy and solve it as supersonic as we have a supersonic flow in the first domain?
I would appreciate as much as help possible.
Update the link? No chance. That page is 14 years old and was back in my uni days - you are lucky I am still alive after all that time.
Don't worry, I still remember how to model shock waves. You will have to be careful with the specification of your initial and boundary conditions. Can you explain to me what you are trying to model? Is it a head in a far field condition being hit by a shock wave? What strength shock wave? Is the shock wave source near or far away?
You will definitely need total energy as that uses the compressible flow equations. You do not choose sub or supersonic, the solver does that. The only exception is for boundary conditions, the treatment for sub or super sonic is different so you have to choose in that case.
Yes it is a head in the far field hit by a shock wave.
I am getting some results from Ls-Dyna which simulates the real blast mechanics and I am trying to replicate that study in CFX by simulating blast like situation (as there isn't any option to simulate blast, e.g. by defining detonation mass and stand-off distance like what Ls-Dyna or Autodyne do.)
However, the strength of the shock is such that we expect to see a peak (overpressure) of around 400 KPa at the beginning of the domain in the pressure history and around 400 m/s in velocity time history. Then mild drop of pressure and velocity should be seen through the domain until it hits the head where it has an increase.
The shock in my study is 1 meter away from the head.
I am getting some reasonable results (using the two-domain configurations we already talked) which can be somehow compared with ls-dyna. I am giving the first domain around 400 kPa initial pressure and 450 m/s initial velocity while the second domain is at 14.7 psi and 0 initial velocity.
Hope I could explain good.
CFX can model explosions but LS-DYNA and Autodyne are much more suited to it and it does not surprise me they have built in options to define explosions. In CFX you are going to have to develop the explosion model yourself.
CFX can also model the proximity of the explosion with a circular shock wave coming out. You just need a bigger domain and either a real explosion model or a simple mass source to drive the flow.
For accurate shock wave modelling in CFX I strongly recommend you do some models of shock wave flow in a straight duct, possibly with a wall at one end for a reflection. This has an analytical solution if you use an ideal gas so you have an exact answer to see how accurate your simulation result is. Then you can test the effects of time and space discretisation, time step size, convergence, mesh size and everything else and work out what is the best way to simulate your real blast model. Once you can model shock wave flow to within 1% or so of the analytical solution then you can be sure that you can model shock wave flows accurately.
That was great info.
Actually, I am just confused about how to create the mass source?
do you mean using a sub-domain or a source point?
In any case how should i set up the setting of either one?
let's say I want to detonate 200 gr of TNT at a stand-off distance of 1 meter from head?
I am really confused about doing the setup?
I appreciate your help.
Thanks in advance,
With either a source point or sub-domain you define the mass of material to appear, and its flow properties (temperature, pressure, initial velocity etc). So you would define a gas with a suitable initial temperature and pressure and a mass to make it equivalent to your explosive.
Is there any example of setting a subdomain or a source point for an explosion?
I don't see any pressure to set? (do you mean to solve the problem as a supersonic one and define Total Energy for heat transfer model?) when I turn the total energy on, i can see the mass source pressure coefficient... but don't know how to set?
Could you help me a with setting of either subdomain or source point in my case? (100 gr TNT with the overpressure of 500 KPa and velocity of 400 m/s, all applied on ambient section (or beginning of my media).
It has been a while since I used a mass source point :). You probably do not define the pressure as that comes from the simulation.
So then let's make a few assumptions - that the explosion gas is an ideal gas, and that the explosion takes some defined time (let's guess 1us). Your explosive will generate a certain mass of gas, so the mass source flow rate becomes that mass over 1us to give a flow rate. You are going to have to convert your 500kPa and 400m/s into a temperature for the gas to appear as. If you are too lazy to work it out analytically then have a guess, run a simulation and see what you get - then adjust it until you get the correct shock wave strength.
Hopefully that is enough of a start for you.
What I did so far is:
I read that approximately 10 moles of gas is produced for each of explosive mole.
After doing calculation it gave me that 100 gr of TNT produces 255 gr air.
Now based the assumption of taking 1 microseconds for TNT to explode, the mass flow rate should be 255 e6 gr/s. is that what I am supposed to insert as the total Fluid Mass Source in continuity setting in source point setup?
I am using source point for now and later I may check subdomain. But I am totally confused. It requires Turbulence Kinetic Energy and Eddy Dissipation which I don't have any idea what to set??Any idea on these?
By the way, you said I need to get the temperature from the pressure and velocity.
are you talking using ideal gas EOS: pV = nRT???
should V be the volume of gas or the domain that source point is located in?
I really appreciate your help.
Yes, it sounds like you have a flow rate for the source point.
Now you need to specify the other fluid propoerties. If you know the velocity is something like 400 m/s then I would assume a high turbulence level (say 10%) and this defines k (but note k is an energy, so you need to use the kinetic energy of the flow, not the velocity). Eddy dissipation can be determined from assuming a length scale. To start with I would assume a length like 10% of the distance from the explosion point to the object. Once you have it working then you can do a sensitivity study and determine how sensitive these turbulence parameters are. I suspect they are not very important but you need to check that.
The EOS is p= density*R*T. You say the blast wave is 400m/s, so adjusting T changes density and gives different blast velocities.
I made a mass source point to work with say mass flow rate of 10 kg/s, T = 400 K, kinetic energy= 1% and dissipation rate 2%. I am giving a Cartesian velocity component in the x direction as 500 m/s.
However, I can see the flow (or if we can say, shock waves) coming out of the mass source point but they don't seem to be propagating correctly around my body upon interaction. (as I have seen in other software or even in CFX using two domains) Is there any idea on the BC or mass point setting?
I would appreciate the help.
The body should be far enough away from the source point that the details of the source point are not important. So I suspect the problem is elsewhere. Read this FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
And post an image of what you are getting.
blast simulation in CFX
It's again me with the blast wave problem.
I am really stuck and I don't know what to do. I want to simulate the shock wave in Ansys CFX.
Whatever I do, I fail. I have tried a simple geometry as attached. supersonic flow over a step.
please tell me what kind of boundary conditions I should use. I have shown on the picture the BC.
There is an inlet, outlet, symmetry plane, no slip wall defining the step and the free slip wall for other walls (top, bottom, and side). Are these correct?
v = 500 m/s, p = 800 kpa, t = 300 k
*totoal time: 5e-3 s, timesteps 4e-6 s*
When I get the results, the wave seems to impact the step right away without the wave propagation and then after some time the shock is stuck at the front edge of the step and doesn't advance!!! Also, i can't get friedlander style p-t plot in the media!
2- In another case I have also used a quarter of a sphere at a corner and defined that as an inlet and did the required mesh refinement.
It runs for two iterations and then exits with the overflow error
inlet: supersonic (the sphere quarter) with same conditions as before
outlet: the right hand surface (like before)
all other surfaces: free slip walls to allow for open space blast
is there anything wrong with the timestep or mesh or it is the BC that are wrong. please give any suggestions so maybe i can get somewhere.
here's the link for images:
Thank you so much.
You need to provide more informantion on your actual model that you are running. Post your output and CCL.
Supersonic flow in a simple channel!!!
Actually I am really confused. I want to start off with something super simple.
supersonic flow in a channel!!! I want to do 2D simulation.
To do so I created a 10 x 3 cm rectangular domain with a small thickness (0.1 cm).
1- Total energy, shear stress transport with ideal gas air
1- left side: supersonic inlet, 500 m/s , rel. press = 0, with T = 300K
2- right side: supersonic outlet
3- front and back : symmetry
4- top and bottom : free slip
Domain initialized with the same condition as inlet.
I even try the steady state simulation.
I followed the procedure used in CFX example of "supersonic flow over a wing"
I have attached my mesh and geometry too.
However, my run fails before even starting or it goes for some iteartions and diverges awfully.
I am really confused as I don't see anything wrong but....
Export your CCL and your output as text files. Please post.
Everything is as I mentioned before
just I have used 0 m/s velocity for initialization and
the top and bottom are no-slip walls
You are running a steady state analysis. Try setting your initial conditions to U=500m/s.
|All times are GMT -4. The time now is 07:17.|