enclosure feature in design modeler

- February 6, 2021 at 10:35 am
  
  pmeghana
  Subscriber
  
  Hello. I am trying to simulate airflow around a ceiling fan. and to save the computational time i was suggested to build an enclosure around my object.
  i tried doing it, but it doesn't have the object right at the center. I have used a cylindrical enclosure. im attaching an image of how it looks.
  my fan is a single body and the cylinder in the y-direction.
  Please help me with this. How do i get it closed to the fan blades. i had used 0.01m as cushion dimensions. (for both radius and reference). Why is it occurring like this? and how do i fix it?
- February 6, 2021 at 1:14 pm
  
  peteroznewman
  Subscriber
  
  nDon't use the Enclosure tool.nCreate a new Sketch on the XZ plane. Draw the circle at the center of the fan with a radius slightly larger than the tip of the blades. Extrude (Add Frozen) a cylindrical body. It should extrude above and below the fan body.nYou need another Sketch on the XZ plane to represent the room in which the air is being circulated. Sketch that rectangle. Extrude (Add Frozen) a body for the room air. It will extrude in one direction down to the floor and in the other direction up to the ceiling.nUse Create, Boolean to Subtract, Target: room, Tool: cylinder, Preserve Tools: Yes.nUse Create, Boolean to Subtract, Target: cylinder, Tool: fan, Preserve Tools: No.nNow you will have one cylindrical air domain with a fan-shaped set of faces. This is the rotating domain and you will have a room-shaped air domain with a cylindrical set of faces to implement the sliding mesh method in Fluent.n
- February 22, 2021 at 7:21 am
  
  pmeghana
  Subscriber
  
  nThank you sir! it helped a lot. nI have another question regarding simulating a fan.nI am using the mesh motion for the cylindrical domain which contains the fan geometry. Would moving this mesh at a certain rpm mean that the fan walls are rotating as well?nSo, for the fan walls, I don't have to include the Moving Wall boundary condition? why?Thankyou in advance,nMeghanan
- February 22, 2021 at 6:59 pm
  
  peteroznewman
  Subscriber
  
  nYes, when you mesh a rotating domain, the walls in that mesh are also rotating. That is how you turn the fan at a certain rpm.nI will request a CFD expert to answer your last question. n
- February 23, 2021 at 9:55 am
  
  Rob
  Ansys Employee
  
  The fan walls should be automatically set as moving at zero relative velocity to the adjacent cell zone. However, I always set this manually to confirm the wall rotation axis has been set correctly: the behaviour changed about 10 years ago to make it unnecessary but it's a habit I've not broken. n

Viewing 4 reply threads

You must be logged in to reply to this topic.

Ansys Innovation Space

Boost Ansys Fluent Simulations with AWS

Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.

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.

Ansys Blog

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.

Trending discussions