Jump to content
Sign in to follow this  
Sankarsan

AcuProbe. Sign convection error in Mass flux

Recommended Posts

Hello Experts,

I am simulating fluidflow through 2 outlet one inlet manifold. 

My inlet BC is 8.88 Kg/s with Bc type Inflow and other two as outflow.

 

After running simulation, I plotted graph of mass flux at inlet using acu probe, surface output.

 

Surprisingly, It was showing -8.88 Kg/s throughout the time.

 

But the outlet mass flow rate was  4.44 kg/s. Which is expected.

 

My Q,

Why is the sign convection is negative at inlet. From my understanding It should be Positive , ad I have given it as inflow with 8.88 Kg/s. 

Kindly, give me your views.

 

Thank you in advance.

Share this post


Link to post
Share on other sites

The definition for the integrated mass flux (flow rate) includes the surface normal direction.  At the inlet, the surface normal is pointing outwards, while the velocity is going inwards - thus the negative value.  At the outlet, both the surface normal and velocity are pointing outwards - thus the positive value.  You can review the definitions in the Programs Reference Manual > Post Processing Programs > AcuTrans section (towards the end of that section in the 2019.0 Help).

Share this post


Link to post
Share on other sites

Ok, Thanks for the info.

 

1. So, If this is to be true, is My way of giving BC wrong?

 

and If wrong, How to correct it.

 

2. Can we give mass flow rate at both inlet and  outlet as Bc?

3. Similarly Can we give Pressure as Inlet and outlet Bc?

 

 

Share this post


Link to post
Share on other sites

1.  The BC definition in the input file is likely correct - use a positive value for entering flow with Simple BC type = inflow and inflow_type = mass_flux.  The Surface Integrated Output (what you would see on that surface in AcuProbe) will be negative due to how the postprocessing is calculating the value using the surface normal.

2.  You 'can' add a mass-flux type condition along with the outflow Simple BC, but it's not exactly physical, as it will also attempt to create a certain profile for the flow.  You would add an Integrated Boundary Condition of type = mass flux, and use your desired value.  (In AcuConsole, use BC* to expand to Advanced Options to then see Integrated Boundary Condition.  This would be SURFACE_INTEGRATED_CONDITION in the input file itself.)  In this type of boundary condition, you would use a positive value for flow leaving the domain and a negative value for flow entering the domain - again, due to the use of the surface normal in the definition.

3.  Again, possible.  It is better to use 'Stagnation Pressure' (or total pressure) at the inlet and 'Pressure' at the outlet.  These would also be under Advanced Options - then Element Boundary Condition.  But pressure for both will also normally work.  The 'Outflow' type of Simple BC is just a pressure boundary condition.

 

Share this post


Link to post
Share on other sites

So, For my problem,

Which set of BC will be best from the given known values? 

 

-Flow rate from each 3 side and Pressure at 2 Outlets.

 

**Objective is to determine, pressure loss through the Manifold.

Share this post


Link to post
Share on other sites

I would probably first try mass-flux (or velocity, flow rate) at inlet, and Outflow Simple BC with the known pressure values for the two outlets.  That leaves the pressure unknown at the inlet.

Share this post


Link to post
Share on other sites

Ok, The pressure value in Outlet will be a stagnation pressure or Normal..

 

As Acusolve gives 2 options for pressure BC. I am bit confused. 

 

Can you explain a bit about these 2 different types  and in which applications we should use them?! 

Share this post


Link to post
Share on other sites

'pressure' is static pressure (P), where 'stagnation pressure' is total pressure (P + 1/2*Rho*V^2).  The most stable for inflow is stagnation pressure, pressure is fine for outflow.  But pressure at inflow also works for most cases.

Share this post


Link to post
Share on other sites

Hello acupro,

 

I performed  the simulation according to your suggestion. At inlet I gave 8.88 kg/s and at both the outlet I gave 16kp of pressure.

 

After solving..

My Pressure  at outlet  is also changing. Which itself is a BC. 

 

May I know, what is this mean? 

Share this post


Link to post
Share on other sites

The pressure is an 'Element Boundary Condition', so there will be some variation in the result, depending on the mesh resolution and the level of convergence.  (Nodal boundary condition would be a fixed value at the nodes, but it is not recommended.)

 

You could also try with surface integrated condition at one of the outlets, and leave the other with outflow/pressure condition.

Share this post


Link to post
Share on other sites

I would recommend leaving Simple BC type = outflow, but then add the surface integrated condition to specify the mass flux.  In AcuConsole, that would be under Advanced Options > Integrated Boundary Conditions (with BC* or ALL selected in the tree filter).  For exiting flow, the mass flux value will be positive.  Achieving the values will also depend on the mesh density and the level of convergence.

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

Sign in to follow this  

×
×
  • Create New...