SimScale CAE Forum

Area integral exponential results


#1

I’m trying to model a throttle body and find the volume flow rate if it is subjected to a pressure of ~7000 Pa on the outlet. However the results for the Uy for the surface integral are orders of magnitude higher than the expected value from a real life test and they shoot up exponentially at the end of the simulation. [https://www.simscale.com/workbench/?pid=1789804238401889872&mi=spec%3Af40ad3a5-8607-4cb1-9ab0-1533ff716778%2Cservice%3ASIMULATION%2Cstrategy%3A2]


#2

Hi @conord827!

Intuitively I would suggest that you extend the size of the tube and see how the results change. In my opinion the distance between inlet and outlet is too short to really establish a reasonable pressure drop to validate your results.

Best,

Jousef


#3

Thanks for you input. The original test was done on a flow bench with the throttle body just open to the air. Would increasing this distance likely impact the amount of airflow through it?


#4

Hi @conord827

I think that the pressure applied at the outlet is wrong(108292.52 Pa) which is greater than the inlet pressure. So the flow is going in reverse direction. Just put 7000 Pa(which you must have measured through Manifold absolute pressure sensor) on the outlet face. In case of intake manifold, the pressure just downstream of the throttle valve remains almost constant(partial vacuum) with distance so I don’t think that there will be much change in the airflow if you will increase its length.

Thanks
Ani


#5

@conord827

My first comment would be that you should probably try to solve this problem as a steady, incompressible flow. Assuming a 7kPa pressure drop across the system and applying Bernoulli’s equation comes out to about a 106 m/s flow (approximately 0.31Ma).

Given the relatively low Mach number, this flow will probably be very stiff to solve with a compressible solver. This somewhat shows up in your diverging convergence plots. Worst case scenario, back the flow speed down a little bit and get it solved in a fully incompressible region then move up to a compressible flow.


#6

@concord827

I took it upon myself to copy your simulation and run through it. Here is my simulation that you can look at and possibly gain some insights. The mesh around the edges of the butterfly isn’t great, but it is good enough for reasonable results overall. Let me know if you have any questions or would like me to go through the setup I used.

https://www.simscale.com/projects/LWhitson2/whipple_oval_tb_test_-_concord827/


#7

Thanks for your help.

I just ran through an incompressible simulation of my own on a slightly different body with the same settings as your copy of my original. However the Uz graph is having the same type of error. Do you think this would be related to the quality of the mesh or some other error?

[https://www.simscale.com/workbench/?pid=1376799981597094808&mi=spec%3A365bfa85-e109-4423-bc0d-d42af11d4ef6%2Cservice%3AMESHING%2Cstrategy%3A2&sh=1]


#8

@conord827, I believe you have two primary issues. First, you need to extend your domain to a much larger length than what you have in this simulation. Such a small domain will really affect the ability for the solver to work. Second, you have set two Pressure boundary conditions and this is numerically unstable. Typically you need to set a Velocity type inlet and a Pressure type outlet. If you look in my simulation, I specify the inlet as a Total Pressure Inlet which is interpreted as a Velocity Inlet with Dynamic Pressure equal to the Total Pressure. The solver then adjusts the velocity at the inlet until the solution converges.

Another thing I noticed is that you have the higher pressure on the positive-z face of the domain. This is why you are getting a negative velocity as well. Flow will always go from higher pressure to lower pressure. Once you fix the Inlet side of your simulation to be a Total Pressure value (not a Pressure Inlet/Outlet) and set the Outlet side of your simulation to a 0 Pressure Outlet, the simulation should converge rather quickly. Also, I would extend the length of the domain as I did.


#9

The total pressure condition was the problem. Interestingly the length did not seem to affect the solver. The results I got on the shorter domain once I used the total pressure were within 0.3% error of the real world tests i performed.

Thanks again.


#10

Not sure how your results give you conclusive data for showing cfm rate across bore. If I set this up with my own configuration, what am I looking for to get valid results showing cfm rate across bore …??