July 20, 2022 at 6:49 pm1829116Subscriber
I am trying to simulate an air oven that heats a moving solid object. I generated the geometry and made sure the solid part will be in contact with the air part at all times. The mesh was also generated at high quality for the dynamic mesh to work. I set-up FLUENT to use the SST kw model and setup a dynamic mesh with deformation for the air part and a UDF to specify the motion of the walls of the solid part. I specified the motion of the solid part itself through the "moving solid" in the cell zone conditions. The mesh preview showed the dynamic mesh to work perfectly. I set up the boundary conditions for air inlet and run the simulation for 3000 timesteps of a size of 0.005s. After 9 days of simulation and after 1020 timesteps, I get a "float point exception"
Can anyone advice why?
July 21, 2022 at 10:06 amRobAnsys Employee
Have a look at the results a few time steps before it failed (or the last autosave). What are the flow & temperature fields looking like? A screen shot of the TUI output would also help with diagnostics.
July 21, 2022 at 8:25 pm1829116Subscriber
Thanks for your reply
The simulation stopped at timestep 1061 and this is how the velocity and temperature looked like
This is how the velocity and the temperature looked at timestep 1060
At timestep 1040, the velocity and the temperature looked fine as you can see
I was not able to see the TUI since I closed FLUENT after the error showed. I loaded timestep 1060 and ran the simluation again and this is what I received:
In the original simulation, I received similar errors before it failed. Any idea?
July 22, 2022 at 10:38 amRobAnsys Employee
You've still got gas jets at around 100m/s in the stable model. In those regions, how long will it take the flow to cross a cell? How does that compare with the time step size?
July 22, 2022 at 11:14 am1829116Subscriber
My element size (kept as defualt) is 0.13153m and my timestep size is 0.005s. Based on the velocity of around 100 m/s, it will take 0.0013153s.
July 22, 2022 at 12:16 pmRobAnsys Employee
Can you post the velocity contour zoomed in around one of the jets? Divergence means something is not solving well, I tend to start looking around regions with high temperature and/or velocity gradients. For the contour plot with node values off and 20 colour bands.
July 22, 2022 at 1:29 pm1829116Subscriber
How do I set the number of colour bands and se the nodes off in CFD-POST?
Also, do you thing that my timestep size of 0.005s is reasonable?
July 22, 2022 at 2:46 pmRobAnsys Employee
Do the post processing in Fluent. CFD Post is good for making movies but otherwise Fluent is much better.
If the flow crosses a cell in 5-10 time steps the time step size is fine. The image will also show if you're resolving the fluid jets. Mesh quality and cell quality are different: the latter is whether the cell shape is good, the former includes checking you have enough mesh to capture the flow.
July 22, 2022 at 3:12 pm1829116Subscriber
Thanks for your response
In FLUENT, I can turn off the node value but cannot find the option for the for the “colour band”. When I plot the graph, I get a blue field (v=0m/s). Please advice
Regarding my timestep size. As I mentioned, the minimum edge length I have is 0.032175m. If air is moving at 100 – 120 m/s, then I need the timestep size to be 0.00026s approx? Is that correct? I need to run my simulation for 15s so that means that I will have 60000 timesteps?
July 22, 2022 at 4:30 pmRobAnsys Employee
Odd, are you plotting on a wall? If so, don't, use an iso-surface or plane (covered in the tutorials, click on "Help").
Time step will be about right as a starting point. You also want convergence in around 10 iterations per time step. Total duration is dependent on what you want to see, but 60k steps looks about right for 15s.
July 22, 2022 at 4:59 pm1829116Subscriber
Thank you for your prompt responses
I am plotting on a plane already as you can see in the picture. I still cannot see the option to set the colour band Fluent is now loaded at timestep 1061 at which the simulation failed.
If I will run my simulation at a timestep size of 0.00025s for 60000 timesteps with 10 iterations per timestep, then the simulation run on a computer with 40 processors will take around 4 months. This is way too long. Does it sound reasonable?
July 26, 2022 at 3:28 pm1829116Subscriber
Any thoughts regarding the plot to diagnos the problem? I will also be thankful to confirm the timestep size.
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- The solver failed with a non-zero exit code of : 2
- Exporting Data Results
- error in cfd post