CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Help in Meshing Solid Cylinder in Gambit. (http://www.cfd-online.com/Forums/fluent/34424-help-meshing-solid-cylinder-gambit.html)

 Andy Singh August 16, 2004 16:44

Help in Meshing Solid Cylinder in Gambit.

hi this is Andy Singh here. I am new to Fluent and Gambit. I am doing a thesis on the optimisation of the rocket pod for helicopters, using fluent. i am having problem in doing the 3D meshing of the solid cylinder. can anybody help me in this case.

 SAM August 17, 2004 05:41

Re: Help in Meshing Solid Cylinder in Gambit.

it is very easy

Mesh the any face , inlet or outlet with triangular mesh or pave mesh, then sweep it throughout the domain by usin option : Elements = Hex/Wedge and type cooper

hope this works

i also recomend one thing. do the 4-5 tutorials of gamibt. this will help u a lot

Regards

 Andy Singh August 17, 2004 16:31

Re: Help in Meshing Solid Cylinder in Gambit.

hi thanx for the reply now the problem is if the 3D cylinder is at the center of the enviornment, or a box around it, then. do we need to subtract the cylinder from the enviornment. then if u try to mesh, the error comes that there is a void inside so cannot mesh. or we have to do it with half the cylinder cut along the axis, just like the 5th tute for a sedan.

 Jason August 18, 2004 09:37

Re: Help in Meshing Solid Cylinder in Gambit.

There's a few different things you can do depending on how you want to mesh it. The simplest would be to split the volume in half using a plane.

Another option would be to create a cylinder at each end of the cylinder you want to keep and split the larger volume with these smaller volumes, don't subtract them. You can cooper mesh this setup pretty easily and it would be very easy to check the mesh afterwards.

Good luck, Jason

 Andy Singh August 30, 2004 20:40

Re: Help in Meshing Solid Cylinder in Gambit.

hi jason how are you thanks for your help, i am able to mesh the model. Now the problem i am facing is in the specifying the values or the boundry conditions. i am getting an error in fluent saying, divergence occured; pressure, or sometimes, x-momentum. i am doing the test at 82m/s. any suggestions please thanks Andy Singh

 Jason August 31, 2004 08:31

Re: Help in Meshing Solid Cylinder in Gambit.

That really depends on everything else you're doing.

Did you check in Gambit to make sure there aren't any skewed cells (for quad mesh I would recommend trying to stay in the low 0.8's but some people say you can go to 0.85 and some people say to stay in the 0.7's... I would stay below 0.9 for a tet mesh, but you can have higher values if they are away from the model far enough that there is almost no pressure or velocity gradient across them).

Are you using a turbulence model? If so, which one? Check your cell height. Some turbulence models require a very small y+ value, while other models can deal with larger values. Also, LES and DES turbulence models need a finer mesh in separation regions then other models.

Which solver are you using: Segregated, Coupled Explicit, or Coupled Implicit? With bluff body flow, I've had trouble using only one solver. What seems to work for me is using a Coupled Explicit model with the multigrid set at 3 or 4, and switching to a segregated model once the solution begins oscillating. If you're using a Coupled solver, use a low Courant number to start (like 1) and raise it every so often if the residuals seem to behave and you don't have any errors. If you're using a segregated solver, then lower the relaxation factors by an order of magnitude. Also, make sure to start your simulation using a first-order discretization. If the residuals behave, then you can up that to a second-order discretization.

I recommend checking your mesh quality in Gambit, and if everything looks alright there, try the coupled explicit solver with a multigrid of 4 and a courant number of .2 using first-order discretization for everything. Up the courant number slowly until you get to 1, watching the residuals to make sure they're behaving. Then switch to second-order discretization for the flow, not the turbulence model. If you're doing more of a research oriented simulation, then switch to a second-order turbulence model down the road. I've never seen it make a big difference, and since everything I do is industry focused, they don't care about 1% or 2% for most models. Eventually you should begin oscillating in a small range(it just seems to be a result of the solver, don't worry about it). If you need to narrow the range more, switch to a segregated solver with second-order discretization. You might need to lower the relaxation factors, but you won't know that until it runs for a few iterations.

Also, SAVE THE MODEL EVERYTIME YOU MAKE A CHANGE!!! There's no un-do button in Fluent, and you might want to go back at some point. Keep a log of what changes you make and the name of the files, so you know what model you want to go back to, if you want to go back.

It's a trial-and-error process and takes some practice to cut down the number of trial-and-errors (mostly errors in my case :) ).

Hope this helps, Jason

 All times are GMT -4. The time now is 00:07.