[berkegk]

Hello CFD-online forum,

I am reaching out to seek your assistance regarding a simulation I am conducting in the Floefd program. Specifically, I am attempting to simulate the autoclave and analyze the temperature variations of the air within it over time.
To provide you with a better understanding of my progress, I have attached the relevant images showingcasing the data I have collected thus far. However, I am encountering a challenge due to the absence of heater data. Consequently, when I introduce a heat source into the system, the temperatures tend to escalate to exceedingly high levels.
I kindly request your guidance on how to address this issue as I currently lack any data pertaining to heat sources. Your expertise and support in resolving this matter would be greatly appreciated.
Thank you in advance for your assistance. I eagerly await your response.

[native]

Hi Berke,

Some remarks and questions on your problem:

1. From your first screenshot it seems to me, that you are applying an increasing temperature to the fluid domain. Is this correct? Usually the temperature increase should result from the heat sources in the model.
2. Why do you apply a temperature dependent heat source (second screenshot)? I would rather choose a constant heat source applied to the heater geometry. Are these pipes the heater?
3. 15 000 W is quite high. Is this correct? What's the electric power input to the modeled device?
4. Which boundary conditions did you apply? Is the fluid domain completely isolated to the exterior?
5. Which air temperature does your simulation reach? Which temperature are you expecting?

Best regards
Florian

[berkegk]

Hello Florian,

Thank you for your response.

1- You are right, the temperature increase should occur due to heat sources, but since I don't have any technical data about the heaters, I cannot simulate a fixed heat source.

2- The pipes refer to the heater resistors. Since I don't have any technical data about the heaters, I cannot simulate a fixed heat source. Additionally, I'm planning a real-time analysis that will take 3 hours, so the air temperature will change over the 3-hour period. Let me explain with an example: In the first 20 minutes, the air temperature in the environment reaches 80 degrees Celsius, then it stays constant at 80 degrees Celsius for 1 hour. After that, it will reach 120 degrees Celsius, and it will stay constant for 30 minutes, and then the analysis will end. I'm providing these time frames as examples.

3- I understand that 15000W is quite high, but since I don't have any data, I chose that temperature just to test whether the other components of the system (fan, airflow, etc.) work properly. The main problem is the lack of data for a heat source.

4- As boundary conditions, there is an ideal wall on the inner side. There are no other boundary conditions. Since it is a closed volume, there is a fan inside.

5- As mentioned before, in the simulation, I want to achieve a temperature distribution as explained in point 2. It does reach 9000 degrees Celsius, and this is influenced by the 15000W heat input.

However, as I mentioned, I don't have any data about the heat source. Therefore, I don't know how to proceed.

Best regards,
Berke

[native]

OK, now I understand it a little better.

1. Maybe, I understand your first screenshot wrong (language). But if you assign a certain temperature profile to the fluid domain itself, you definitely don't need this. If you just place any FloEFD heat source inside the fluid domain, this heats the air automatically. Even if you don't know the exact power, this should work.
2. Understand. This I would rather solve by a time dependent heat source. You could then adapt the power of the heat source at certain points in time to reach the desired temperature profile.
3. Maybe, you could estimate the power of the heat source from the electric power input to the complete device. Say, 80 % of the power input are for the power of the heat source.
4. I think this is the reason for the rapid temperature increase. The ideal wall in FloEFD is adiabatic. This means, that no heat is transfered through the ideal wall. Thus, all the power input heats the air and no heat is transferred to the outside. You could either choose an external analysis, remove the ideal wall boundary and let FloEFD calculate the heat transfer on the outside. Or you change the ideal wall to a real wall and estimate the heat transfer coefficient on the outside of the wall, say 5 W/(m^2 K).
5. All right: Change the boundary condition, reduce the power of the heat source, remove the temperature assignment to the fluid domain. As a first step, I would choose a constant heat source and evaluate the final temperature in steady state. By this, you get a rough idea of the needed power.

Hope, this helps.
Florian

[berkegk]

Thank you for the answer. I want to ask something else. I will try what you said. In addition, can we define a sensor in the FLOEFD program since we get the data from a point in real life and the hot air coming out of the heaters in the simulation affects the average air temperature? In this way, maybe I can evaluate the air temperature at the point where we measure the temperature in real life in the simulation and determine the heater power accordingly.

Best Regards
Berke