CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > FloEFD, FloWorks & FloTHERM

FloEFD: Queries related to model setup

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Search this Thread Display Modes
Old   March 9, 2021, 06:54
Exclamation FloEFD: Queries related to model setup
Sai Krishna
Join Date: May 2018
Posts: 32
Rep Power: 5
Sai Krishna is on a distinguished road
Hi friends, Iam using FloEFD embedded with solidedge and I have few queries related to it. It will be helpful if anyone can assist me in the following queries.
  • How to change the CAD model in a cloned project ? I ran a simulation with all conditions like local meshing, global adjustments, Boundary conditions. Now I have to use the same set of input conditions for a similar model. If I clone the present project, can I replace the CAD in that. If so how ?
  • Can we save a cloned project as separate project entity to make it independent from its parent master project .? So that I can use it for further studies.
  • How to model stagnated air or air entrapped in a leakproof region (I need this for for heat transfer studies) .? Can we do that using sub domain option ?
  • How to patch a zone with given P and T in FloEFD, just like we do in fluent for initialing the solution ...?can this be done with a fluid sub domain
  • how to get inflation layers or refinement near walls to account for boundary layers effects ? I didnt mean fluid refinement or fluid-solid refinement. As in ansys meshing, we define 1st layer of thickness and growth ratio, how we can achieve this in FloEFD meshing

Thanks for the help
Sai Krishna is offline   Reply With Quote

Old   March 17, 2021, 08:51
Senior Member
Boris Marovic
Join Date: Jul 2009
Posts: 610
Rep Power: 21
Boris_M will become famous soon enough
Hi Krishna,

Regarding your questions:

Yes, but you will need to create a geometry variant first. Use the Alternate Assemblies to specify either a switch of two parts or a change in parameters such as diameters or lengths etc. Make sure to not rename the first Alternate Assembly. This one is usually called Master in Solid Edge and if you rename it, the FLOEFD project will not find the geometry variant anymore. The new one you can name whatever you like as it will not have a project yet. Once that is done, you can clone the project and select in the cloning setting the geometry variant you want to clone that project into. You will see that in the FLOEFD tree, there is the first instance the geometry configurations/variants and then into those you have the different projects. So the geometry always comes first before you create projects.

These projects are independent of previous projects. They just create a clone with the same setting but then they are independent of the other project, they only might belong to the same geometry configuration if they are assigned to the same one.

If you have the "Exclude cavities without flow condition" activated in the wizard/general settings, then this will cause all empty cavities to be ignored if there is not some boundary condition (BC) that makes clear that there is some fluid. This can be a regular flow or pressure BC, a fan curve or also a fluid subdomain. Once you specify one of those, FLOEFD knows that the cavity in contact with the BC surface is filled with fluid and will not ignore it. So if there is just still air in it without any opening for pressure equalization or flow, then you can use the fluid subdomain.
If you have only that one cavity and not some small entrapped air pockets in screw boreholes etc., then you can also deactivate that exclude cavities option and then everything that is empty space will be fluid in an internal simulation. For external simulations, this is of course automatically disabled.

Yes, this is however the initial condition of the simulation, it will not stay constant as it is not a fixed BC. If this refers to the previous case, then you don't have to specify that if you deactivate the exclude cavity option as the initial conditions from the wizard will be applied by default to everything. The fluid subdomain allows you to specify a specific volume in which a specific fluid is present and its initial condition.
You can also use the initial condition option to do that, but if you already have a fluid subdomain defined here, it will be just double the definition as the initial conditions will also be defined in the fluid subdomain.

You need to forget about Fluent here. FLOEFD uses a wall function approach, so the boundary layer (BL) does not need to be modelled in detail by the mesh necessarily. Of course, you can do that, but in most cases this is not needed and be like asking to add the spare wheel onto your car in addition of the good wheel.
However, you can use the local mesh and define the offset mesh for the surfaces you want it to apply and define how many offsets, the level and how thick those offsets should be. But try it without such layers, these are mostly needed in some very specific aerodynamics cases such as the surface of the car or the wing to represent the pressure better and resolve the flow of the curvature more accurately. I personally have used it maybe once in over 1000 simulations.
And please don't try to create 50 million cells because you were used to have such cell count from Fluent or so. FLOEFD usually handles the same with an order of magnitude less. The reason for that is the SmartCells with the BL treatment and the way it meshes multiple solids and fluids within one cell, by having multiple control volumes within one cell. Otherwise, you ruin the whole benefit of FLOEFD, which is being easy to use, automatic meshing and a fast solution as you make it more complicated than it needs to be and cause more mesh than it needs to solve which leads to high CPU time for the solver.

Hope this helps,
Boris_M is offline   Reply With Quote


floefd17.0(solidedge), heat and mass transfer

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
NEW turbulence TRANSITIONAL model giammy92 OpenFOAM 3 June 30, 2016 09:47
some confusion about the radiation model of Floefd jason kid FloEFD, FloWorks & FloTHERM 4 March 3, 2016 07:13
manualInjection model in sprayFoam Mentalo OpenFOAM Running, Solving & CFD 1 April 2, 2014 09:29
how to setup a periodic numerical model saleh alsubari Main CFD Forum 0 August 22, 2012 04:45
Advanced Turbulence Modeling in Fluent, Realizable k-epsilon Model Jonas Larsson FLUENT 5 March 13, 2000 03:27

All times are GMT -4. The time now is 13:14.