hi, all

I am a new user of CFX5.5, I am trying to perform a fully developed laminar pipe flow simulation in CFX5.5. The pipe is 30mm in diameter and the length is 20 times of the diameter. Fluid is oil, density 0.83x10^3kg/m^-3 and viscosity is 0.08kg/m/s. Boundary conditions, set normal speed at 1.5m/s with inlet, 0 relative pressure static pressure at outlet. I set mesh inflation with 5 or 10 layers. The result I got is not like I expected. The volecity profile, Vmax in the center of pipe only reach to 2.5m/s but not 3.0m/s supposed to be. I appretiate if anyone can help me to figure this problem

Dear Wendy,

Firstly, I would like to know what longitudal velocity at different axial positions.

I think you may set a irreasonable pressure boundary at outlet.

Best regards

Wendy,

You probably won't get the right answer doing it this way. Depending on the Reynolds number you need enough length to resolve the entrance region until a fully developed laminar profile evolves.

The right way to do it is to use a translational periodic boundary condition for your inlet and outlet and then specify a momentum source which sets the pressure drop. This way there is no need to resolve the entry length.

Neale.

Dear Wendy, You put a laminar profile equation(parabolic equation) at the inlet itself, using the expression editor, if you are interested in the fully developed flow only. Put average static pressure(rel) as zero Pa at outlet. Ensure mesh is fine near the walls and the domain. Try higher order discretisation scheme. with regards, Retheesh

Not-so-good advice: why one needs higher order scheme for a fully developed pipe flow since there is no velocity in the cross-section, and there is no change of velocity in the streamwise direction? In this case the UD is as good as any scheme since the flow is perfectly alligned with the mesh.

I use of CFX 4.2 and I can tell you how I resolved this problem. You must set on inlet and outlet mass flow boundary e.g.
:>MASS FLOW BOUNDARIES

>>FLUXES

FLUXES -2.989000E-06 2.989000E-06

MASS FLOW SPECIFIED and you have fully developed flow. In direction flow you can set two nodes grids only. If you want fully developed profile temperature too, you write me, becouse this is more complex problem. Best regards

Thanks! But how to 'specify a momentum source which sets the pressure drop' please?

Regards,

Wendy

Wendy,

You need to make your entire cylinder a "sub-domain". You can do this on the domains form. Simply select Create->Fluid Subdomain I think. Then you can specify a momentum source term on your subdomain (which happens to be the entire domain) that will set the pressure drop you want. You should be able to back out a rough value for this using Hagen-Pousille (sp?) relationships.

The other thing you will likely have to do is use full second order discretisation. You can do this by specifying a fixed blend factor of 1.0 in the solver controls form.

Dan.

Sure, if you are using a hex mesh. What about a tet grid?

Retheesh

Thanks for your response. I tried this way before but didn't get the ideal result. I think probably because of the mesh. Could you give me an advice how to make a fine mesh near the wall and domain?

Regards,

Wendy

Dear Mr.Wendy,

how much is max velocity you are getting now?(I think you are expecting 3m/s) One reason for the offset as you rightly imagine is the mesh. Before putting finer mesh with tet mesh, you try with hexahedral mesh. In mesh only mode, you create a hex-mesh, having finer mesh in the radial direction, import it and see if the result obtained from this hex mesh is OK.(you need not put fine mesh in the flow direction) If it is OK, then we can conclude that it is due to the coarseness in tetmesh. You can then make the tet mesh finer in the central portion of the pipe. Please try this..

with regards, Retheesh

Dear Mr Zhang

I set static pressure, relative pressure at 0 with outlet boundary.

Regards,

Wendy