January 24, 2023 at 7:04 pmreza121Subscriber
Hello. I hope you are doing well.
I am using the K-Omega SST model to simulate airflow through five layers of screens in fluent. The wire diameter in the screens is about 0.05mm and the distance between two consecutive wires is 0.127 mm.
At low velocities (below 1m/s) I get reverse flow at my outlet. I have a 1mm*1mm*113mm channel where the B.C.s are velocity inlet and pressure outlet at the pressure of 0 Pa. Since this is a study on a small opening of the whole screen module, the side B.C.s are symmetry.
I surfed the internet and have tried the following suggested solutions but neither has worked so far:
1- I extended the domain length and put the outlet 100mm away from the last screen layer. (as a comparison, the distance between the layers is 3 mm in my geometry). I am pretty sure that this length is enough because the pressure does not change from the last layer until very close to the outlet.
2- I increased the grid resolution. my cells are poly-hexcore and the initial cell sizes were 1.6e-5m and 3.2e-5m. I studied the case with a mesh of half of this size and the backflow is still here. It is noteworthy that the cell sizes are smaller close to the wires.
3- I decreased the "Pseudo time explicit relaxation factors" through solution>controls down to 0.1 and it didn't solve the problem.
4- I won't get any backflows if I change my outlet BC from pressure outlet to outflow. However, this BC should not be selected for compressible gases based on the manual, so I don't think this is an appropriate solution for my case.
Attached you can see screenshots of pathlines colored by static pressure in the range of -0.01 to 0.01 Pa. Very close to the outlet, the flow is deflected downward and there's a backflow on the top part of the outlet. There is also a vertical pressure gradient which makes no sense. I expect a constant 0 Pa pressure from a little away from the last screen layer all the way to the outlet.
Can you please help me how I can solve this issue?
Thanks in advance
Path line colored by static pressure for vel= 0.005 m/s - 45% back flow
January 25, 2023 at 7:25 amSRPSubscriber
- Can you try standard initialization rather using hybrid initialization if you use earlier hybrid initialization.
- Try to decrease relaxation factor.
- you can use 2nd order or higher order methods
January 25, 2023 at 11:07 amRobAnsys Employee
If you're using compressible flow (ideal gas?) what is the back flow condition that you're using? How does that compare to the bulk flow near the outlet?
January 25, 2023 at 2:39 pmreza121Subscriber
Thanks for your reply Rob,
Yes it's a real gas model. I specified the backflow properties close to the flow properties at the outlet. These properties are the turbulence intensity and hydraulic diameter and temperature.
Right now, the temperature does not change in my simulations as all the heat sources are off and flow remains at 25C temperature similar to inlet.
I was hoping that assigning these real backflow properties may help the convergence and resolve the backflow but it didn't work.
I think that the solver is getting trapped at a wrong answer and needs a little push toward the right answer. One idea that I had was pitching a 0 pressure on the part of the domain between the last layer and the outlet. Then I would first run it under this condition for a few iterations, and then will remove this forced condition and let it naturally converge. But I'm not sure how I can pitch a property to a specific volume in the domain.
What do you think?
January 25, 2023 at 4:25 pmRobAnsys Employee
Why do you need real gas? You can try the "prevent reverse flow" and see if that helps (turn OFF before running to final convergence) but I suspect it'll not be much use.
January 25, 2023 at 7:20 pmreza121Subscriber
Thanks again for your reply. I found the issue and I will say it here, it may help other people in the future:
the vertical pressure gradient was actually ok because gravity is activated in my model. At such low velocity, rho g h becomes important since the inertial terms are weak. the solver was detecting the vertical pressure gradient due to gravity correctly but it was forced to assign a 0 Pa pressure all over the outlet which was causing the backflows. The solution to that is activating the "average pressure specification" option in the pressure outlet panel. This will make sure that the area-weighted average of pressure on the outlet plane is zero, while it gives the solver the flexibility to change the pressure in different cells.
January 26, 2023 at 4:45 pmRobAnsys Employee
First time I've seen that effect on a 1mm boundary. The other approach is to set the operating density to the "outside" conditions, ie 1atm and 25C (or whatever the backflow value is), use Fluent to calculate the value and take ALL decimal places/significant figures.
January 30, 2023 at 7:59 pmreza121Subscriber
Thanks for your reply Rob,
You are right. activating the operating density sounds like a better solution for that. I am using the "real gas redlich-kwong" material model for my airflow and I get the following warning when I changed my operating density to 1.1845 kg/m^3:
Warning: For compressible (ideal and real) gas models with buoyancy,
it is recommended that you use a specified operating density value of zero:
Should I ignore it or will it cause any problems you think?
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.