Flow analysis in a 3" frac valve

[alok]

I am trying to simulate a flow through a 3" frac valve. The valve has a hugh inlet flowrate of 10000 GMP with the pressure of 15000 Psi. The valve body has a cage inside to hold the piston. I have attached the pictures herewith. The cage has 4 small holes 90 deg apart, one of which is concentric with the valve inlet. I want to analyze the behavior of the fluid inside the body and the cage, especially the effects of holes of the cage before passing through the outlet at the bottom. I am not sure about how to specify the internal fluid region for this kind of assembly. Any help would be really appreciated.

Thanks!!!  

[Joey.X]

First is creating fluid part(s) in CAD, I am doing geometry Boolean subtract operation by overlapped objects.
Doing this in CAD is more praticall for complicated CAD geometry or assembly, it may produce multiple fluid parts, this is okay, just make sure the interfaces between fluid parts are well matched(ot you can do your own CAD fluid part assembly). Then you can import the produced fluid part(s) (or assembly with multiple parts) into simulation. 

Here are options up to your preference and model geometry properties
- Solid parts can either deactivated in CAD or in simulation.
- The fluid parts could be produced (Boolean operation) separately and then do assembly in CAD

- Check the produced fluid parts connectivity since some parts may be obsolete with no connection to other parts for some special cases.

One you have fluid parts in simulation, you can move forward for fluid analysis, the parts are connected by bonded (default).
One important step is ensuring surface imprint (check option in CAD import), this makes surface matched between parts and eventually make conforming mesh between parts.

This is my way, probally somebody has better ways. 

[alok]

Hi Joey,

Thanks for the response. I got my geometry done by using the Boolean operators, but I am not able to get a boundary layer mesh due to a very thin section at one of the interfaces in the geometry. Can I use an all Tetra mesh instead of the boundary layered mesh?

Also, as I mentioned, I have to specify pressure as well as velocity (given the flow rate) at the inlet. Is there a way to specify 2 boundary conditions on the same surface?

Thanks!

Alok

[Joey.X]

For fluid flow analysis, boundary layer mesh makes better conditions of solution matrix (better for convergence) and better result accuracy(You can image the velocity gradient close to wall in fluid flow).

If you have difficulty using default boundary layer mesh settings,  try (a) less thickness of the boundary layer (b) using single layer of boundary layer mesh (default =3). If you still have mesh difficulty, yes, you can use pure tetrahedral mesh without boundary layer mesh, one thing be careful is making sure the sufficient interior fluid nodes at boundaries and interior of the fluid domain. 

Velocity BC and pressure BC can't be not simultaneously specified on a surface, that's a typical over-constrained. Think about the all fluid DOF are velocity (3 components for 3D) and pressure (Scalar), all DOFs cannot be fixed at a surface.

[alok]

Hi Joey,

I tried all the possible ways for Boundary Layered mesh, but couldn't get it. So I am moving ahead with the Tetra mesh and see what the results are.

In regards to the boundary conditions, what would be the best way to specify at the inlet, given the maximum flow rate achieved and the total pressure?

Thanks again for your time and help!

Alok

[Joey.X]

Inlet:   Specify flow rate BC or velocity BC (all components)

Outlet: specify inlet/outletBC or zero pressure BC

Validation: Check avarage pressure drop fron inlet to outlet  

[alok]

Hi Joey,

As I mentioned earlier, I tried running the simulation with a pure Tetrahederal mesh (absolute mesh size 0.1). I got the mesh done, but while running the analysis, I got the following warnings in the log file.

Warning: Detected 35960 dead elements.                    

                        and 10484 dead nodes.               

Solid mesh the model using the "Tetrahedra and wedges (boundary layer)" mesh type to avoid this situation.

I am getting this warning no matter how fine I make the mesh.

[Joey.X]

This is typical message from pure Tet meshing in fluid flow analysis, it makes some dead elements (all fixed node in one element), and the dead elements make negative impact of false roughness on the wall and influence the result convergence and accuracy. That's partial reason that boundary layer meshing is preferred as mentioned before.

Sorry I don’t explain why the dead elements form, you can check from online help(I am not sure if it is there). And you can image a box with fully Tet mesh, the corner element will be a dead element.

If you result accuracy is not critical, it usually still be okay to ignore these warning messages.