Fluid flow through relief valve

[alok]

I am relatively new to Autodesk Multiphisycs as I have been using Fluent for most of my CFD projects. I want to simulate flow through a valve body (attached herewith). The inlet is from the side and the outlet is at the bottom. The fluid entes at the inlet with velocity of 10 in/s and pressure of 1500 Psi. I am trying to give the velocity inlet B.C. at the inlet and the prescribed velocity at the outlet and run the simulation for unsteady fluid flow analysis, but somehow I am getting bizzare results. I am sure I am missing something, but not able to figure out. Do I have to specify the internal section of the valve body as fluid?

Also is there any wall boundary condition to be given for the bounding surfaces?

Any help would be really appreciated.

Thanks in advance!!!

[hupn]

Hi,

As you mentioned that "The fluid enters at the inlet with velocity of 10 in/s and pressure of 1500 Psi. I am trying to give the velocity inlet B.C. at the inlet and the prescribed velocity at the outlet". This is kind of confusing. Please check the Wikihelp for boundary conditions definition: http://wikihelp.autodesk.com/Autodesk_Simulation/enu/2012/Help/0220-Setting_220/0289-Setting_289/043....  You may want to define the velocity and pressure at the side inlet, and define the inlet/outlet boundary condition at the your outlet.

hupn 

[Joey.X]

According to your description, it sounds that you got not-converged result since the 1500psi outlet pressure makes the convergence difficulty. 

It is suggested to offset the outlet pressure from 1500 psi to 0 psi, this is a common simulation setup tip, note that this does not affect result pattern but helps the numerical solution stability. At viewing pressure result, you may notice 1500 psi difference comparing to reality, this is easy to offset back by youself.

[alok]

Thanks Joey and Hupn. I got all by boundary conditions set-up. But every time I run the simulation, I get this error "Non-positive diagonal entry detected in ILU method". So I tried to change it to SSOR, but after doing that I get the error "Divergence detected in iterative solver". So basically my solution is not converging. I have all the solution parameters set to automatic. Any idea what am I doing wrong?

Thanks for the help!!!

[Joey.X]

Suggested check list

- Meshing:

   Is the mesh too coarse in thin part?  This may block the flow numerically

   What kind of mesh type used

   Is boundary layer mesh used? 

  Any errors from mesh log file

- BCs: 

   What kind of BCs in inlet and outlet?

   Is the inlet velocity fully fixed or partially fixed?

You have option to use direct solver which is more stable but slower than iterative solver. However, I strongly suggest you check above items.   Doing CFD from complicated CAD model , it usually needs geometry simplification to suppress or simpify  trial CAD features which has less impact to fluid flow but introduces mesh difficulties. 

[alok]

Joey,

Thanks for the response.

Following are the parameters I'm using:

Mesh: Boundary Layer (Tetra and Wedges) with absolute mesh size of 0.1 (IPS units)

Boundary conditions: Prescribed velocity of 10in/s and total pressure of 1500 Psi at the inlet

                                   Velocity inlet/outlet B.C at the outlet, since I don't know the velocity at the outlet

I tried both standard as well as RNG K-Epsilon turbulence model. I also tried Automatic, iterative and sparse solvers for the solution.

In regards to the geometry and mesh, there isn't any error on the mesh log file. I have also made the geometry as simple as possible by suppressing the external threads which are not required for flow analysis.

All I need to evaluate for this valve body is if there is any pressure drop at the outlet due to the current geometry when the valve is in fully open condition.

Thanks!!!

[Joey.X]

Looks you are close.

But "velocity inlet/outlet B.C" at the outlet sounds strange to me. You can either set zero pressure or inlet/out BC at outlet, but no velocity BC and other BC simultaneously at outlet. 

For inlet BC, do you set velocity specified in single direction or fully constrained in all three directions? The former is less robust numerically.

And, check the solid mesh in postprocessor to see any coarse mesh in thin part, this is not looking for mesh failure but for improper mesh settings, if there are no internal nodes or very coarse internal nodes in fluid part, it  blocks flow in numerical solution, and this unrealistic setup makes difficulty solution. Imaging the scenario of pushing flow in an enclousre, but the flow has no way to reach outlet, no soultion at all.

[alok]

Hi Joey,

Thanks for your response.

I have given the inlet velocity only in x-direction. And the boundary condition at the outlet is "surface inlet/outlet". The mesh looks fine, just can't really figure what exactly the problem is.

[Joey.X]

For your case, it is suggested to specify velocity in x direction, and set zero veolcity in other two directions.

Probally other issue, need to look at the model. 

[alok]

Hi Joey,

I have built the model in SolidWorks and transfered to Multiphysics. Is it possible to encounter such problems while using different softwares?

Is there a way that I can send you the geometry for you to have a look at it? That would really help me in understanding what exactly I'm doing wrong.

Thanks!

Alok

[Joey.X]

Hi, Alok,

It's okay to import SW model to Autodesk simulation multiphysics. For simulation simulation setup and result, it could be different because of different implementations. 

It is perfered to send full model rather than CAD geometry to check possible modelling problems, for large file size. You can use dropbox (free) and shate this file to me for email xjohnh@gmail.com. 

Btw, I tried to reply your privite messge, but for some reason, it seems that your multiple screen name blocks the message return.

Let me know if you can try dropbox, and I am open if you have other ways to share. 

[alok]

Hi Joey,

I have sent you the model and the .fem multiphysics file with the mesh and loads through drop box to the email that you provided. Please have a look into it whenever you get a chance and let me know where am I going wrong.

You can reach me at alok.dange@gmail.com.

I really appreciate your time and help.

Thanks!

Alok

[Anonymous]

Alok

I am very interested in the response here as I have a simular issue with the fluid part of a heat exchanger analysis. The multiple inlet stream lines dissipate to just one on the outlet when experience says they should not. Also, the volumetric flow rate is 1/10 of expected theoretical (i.e. If Q=VA where the velocity is 1 ft/s and the area 1 ft, then Q should equal 1 ft^3/s but does not. The post processor throws back 0.1 ft^3/s).

 Using k-epsilon, tets and wedges, etc. Much of the same you're experiencing. I hope Joey.X pays special attention to this as I've been fighting it for months.

BTW, Joey.X,

1. for the characteristic velocity in the k-epsilon turbulence model, what should that be set at? (i.e. if the system velocity is 10 ft/s with no anticipated losses at the entrance, should the characteristic velocity be 10 ft/s too?)

2. Also, how does one refine the mesh such that the turbulence y+ comes out to about 30 as speficied in the Wiki?

3. In Alok's case, he wants a pressure of 1500 psig, and assuming a 10% pressure drop for the discharge (or possibly to 0 psig, 14.7 psia), is there not an option to specify inlet/outlet pressures on their respective 3D faces while simultaneously specifying the prescribed velocity at the inlet? I've tried variations of what Alok is doing and can only respond UGH!

With more than one user with this problem, it may be a good idea to pay special attention to this issue. This may help both Alok and me!

[Anonymous]

Alok

BTW, if you're meshing with tets/wedges, be sure you exclude the inlet/outlet from the mesh

set mesh to tets/wedges>do not mesh yet>select the 3D inlet/outlet faces in the GUI>right click>there's a mesh option there you can exclude the inlet/outlet

[alok]

Hi jrm,

I believe you cannot specify pressure and velocity simultaneously on the same surface. Even I tried doing that, but didn't get the solution. I was using K-Epsilon RNG model before, but my solution was not converging. So I used the LES as suggested by Joey. Here's the suggested changes given by Joey. This might help you in your case as well.

Hi, Alok,

It looks that you already did good job in the modeling.

Below are the changes base on your ach model, it works fine.

(1) Exclude inlet and outlet surface from boundary layer mesh, it's a one of the blocks for convergence. (search my post before for detail)

(2) Change turbulence model to LES (Was k-epsilon), LES is more stable but less accurate. You can turn it back to TKE later on

(3) Change fluid default segregated formulation's pressure to BCSLIB which is direct solver, which is more robust for tough model than default iterative solver, but little slower. You can try to turn this back depending on the convergence performance.

(4) Single step for same value of multiplier in load curves. This saves simulation time, as mentioned before, simulation Multiphysics fluid flow uses it's own inertial relaxation for progressive convergence rather depending on user's inputting load curve changes.

(5) change inertial relaxation factor to 0.3 (default =1)

Note that all my changes are making model solution more stable, you can change back/or tune up at your wish depending on convergence behaviors.

I am now trying to figure out the solution by switching to k-epsilon for better convergence. I will post the results as soona s I am done with this case.

Please have a look at my new post as well. Similar case with an added part in the assembly.

http://forums.autodesk.com/t5/Autodesk-Simulation/Flow-analysis-in-a-3-quot-frac-valve/td-p/3223924

Thanks!

Alok

[Anonymous]

Joey.X,

I see what you and Alok are writing, however, I have had no success with LES turbulence model in my analysis. If k-epsilon is bad, why is it there? I think it can be stable, it just has more parameters. Please pay special attention to this. SEE MY PREVIOUS THREAD REGARDING THE FLOW RATE DISCREPANCIES.

1. for the characteristic velocity in the k-epsilon turbulence model, what should that be set at? (i.e. if the system velocity is 10 ft/s with no anticipated losses at the entrance, should the characteristic velocity be 10 ft/s too?)

2. Also, how does one refine the mesh (TETS & WEDGES) such that the turbulence y+ comes out to about 30 as speficied in the Wiki?

3. In Alok's case, he wants a pressure of 1500 psig, and assuming a 10% pressure drop for the discharge (or possibly to 0 psig, 14.7 psia), is there not an option to specify inlet/outlet pressures on their respective 3D faces while simultaneously specifying the prescribed velocity at the inlet? In the real world fluid mechanics has both pressure and velocity (i.e. pump and piping system where the function Q(v,p)). I've tried variations of what Alok is doing and can only respond UGH!

With more than one user with this problem, it may be a good idea to pay special attention to this issue. This may help both Alok and me!