July 21, 2022 at 1:59 pm2019023289Subscriber
/* EDIT by DrAmine */
Could you please help me?
The DPM model needs to meet two conditions: 1. The particle size must be far smaller than the mesh size, enough to be regarded as a point masses
2. the particle volume fraction should be less than 10vol%-20vol%.
DPM model and vicous model have contradictory requirements on mesh size. Viscous model requires mesh size to be small enough, while DPM model requires mesh size to be larger than particle size.
But for boundary layer grids, the size needs to be very small, even smaller than the particle size, in order to calculate accurately.
Is it ok if the mesh size at the boundary layer is smaller than the particle size? Is the error in this condition acceptable?
July 21, 2022 at 3:40 pmRobAnsys Employee
Both statements are true: and this results in a mesh that's either too fine at the wall for the particles, or too coarse for the flow. The solver will work if particles are too big, but wall collision is only calculated in the near wall cell.
July 22, 2022 at 1:15 am2019023289Subscriber
Sorry,i am not mean using MPM model.I mean is it ok to use DPM model if the mesh size at the boundary layer is smaller than the particle size? And I don't understand 'The solver will work if particles are too big, but wall collision is only calculated in the near wall cell. '
July 22, 2022 at 8:31 amDrAmineAnsys Employee
I need to edit your post by removing the screenshot from the documentation.
July 22, 2022 at 8:33 amDrAmineAnsys Employee
MPM is not like DPM: there you need to resolve the paritcles to capture the forces properly. 10 to 20 cells per particle are required!
July 22, 2022 at 8:55 am2019023289Subscriber
Thank you, Mr,Ali
So, is it ok to use DPM model if the mesh size at the boundary layer is smaller than the particle size? And I don't want use MPM model.
July 22, 2022 at 9:05 amDrAmineAnsys Employee
Are you now trying to use DPM or MPM?
I can write chapters on this... But for now:
For DPM it is recommended to keep particle size smaller than the mesh size: because one can control that in an easy way.
For sure that cannot be always fulfilled espcially when one wants to resolve boundary layers properly. Just do the right mesh for the flow and accept this paradoxon and try to increate particle streams to make statistics better and flow rate per stream / parcel small to get things well distributed.
So start running and then do a sensitivity
July 22, 2022 at 9:32 am2019023289Subscriber
I try to use DPM.
You mean it's OK to use DPM model if the mesh size at the boundary layer is smaller than the particle size if I increate particle streams.
And increating particle streams can decrease this error?
July 22, 2022 at 9:51 amDrAmineAnsys Employee
Yes. Just take all that into consideration when evaluating the results.
July 22, 2022 at 10:35 amRobAnsys Employee
Increasing particle streams will reduce the parcel mass: that tends to give a more stable solution as the DPM source is more spread out.
Particles larger than the near wall cell may cause stability issues (hence more streams) and can mean the particle is closer to the wall than it's radius would permit. Otherwise, it'll work, but you need to be aware of the conflicts when analysing the results.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Time Step Size and Courant Number
- Difference between K-epsilon and K-omega Turbulence Model
- The solver failed with a non-zero exit code of : 2
- Floating point exception
- How to model free convection warming of liquid in a plastic bag