Community
CFD Forum
Welcome to Autodesk’s CFD Forums. Share your knowledge, ask questions, and explore popular CFD topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Advection schemes

15 REPLIES 15
Reply
Message 1 of 16
OmkarJ
1256 Views, 15 Replies

Advection schemes

I pick this thread from one of my recent experiences. Typically, first order advection schemes (ADV1) and second order accurate advection schemes (ADV5) would produce different results because of artificial viscosity in ADV1. But would these results be very much affected ONLY while simulating distributed resistance, which models a negative pressure gradient zone? Or do these schemes always produce significantly different results for ALL types of physics, viz. incompressible turbulent flow, heat transfer, compressible flow etc.?

 

Regards

OJ

15 REPLIES 15
Message 2 of 16
OmkarJ
in reply to: OmkarJ

Anyone, please?

 

Regards

OJ

Message 3 of 16
OmkarJ
in reply to: OmkarJ

Someone?

Message 4 of 16
Jon.Wilde
in reply to: OmkarJ

We would recommend switching away from ADV1 and to ADV5 for many purposes now. Standard incompressible flow should be OK but ADV5 will be better for compressible and pressure driven flows, those with resistances as you rightly say and also for many heat transfer calculations now too.

Message 5 of 16
ssenbore
in reply to: Jon.Wilde

I was about to open a new forum poost but I guess it can go here.

I am simulating a Venturri nozzle as a flow measuring device, and when I use ADV5, the pressure difference comes out ~5 psi less than if I use ADV1. This difference is significant (~ 25% of the entire pressure drop across the nozzle).

Which one is more accurate than the other? When would it be more advisable to switch to AdV5 vs ADV1? Or would ADV4 be more appropriate?

If this helps, my setup is:

1018 psi absolute at the inlet

9 million lbm/hr of water at the outlet

Mesh adaptation is used to solve to 99% mesh independence in both cases.

Message 6 of 16
srhusain
in reply to: ssenbore

Some points to consider here:

  1. You should be applying a flow rate at the inlet and pressure at the outlet as a a standard setup. Any particular reason why you have it the other way around?
  2. Based on a pressure of 1000 psi, 5 psi is a small discrepancy
  3. Beyond that, I would recommend Adv5 over Adv1as it is more stable
Message 7 of 16
ssenbore
in reply to: srhusain

Some points to consider here:

 
You should be applying a flow rate at the inlet and pressure at the outlet as a a standard setup. Any particular reason why you have it the other way around?
I know the inlet pressure and mass flow rate.  There is a head loss across the venturri nozzle that I dont know.  Hence I thought it was wiser to put the pressure at the inlet.

Based on a pressure of 1000 psi, 5 psi is a small discrepancy
True.  But for the Pressure Drop across the big and small diameter sections of the venturri, the lab data is 16.7 psi, so a variatioin of 5 psi in pressure drop is HUGE.
 
Beyond that, I would recommend Adv5 over Adv1as it is more stable
Thanks.  Would ADV4 be a consideration? I know the help says that its specially tuned for flows in long narrow ducts.  This nozzle is 5 ft long, with a large dia of 1.5 ft and small dia of 1 ft.  Does that translate to 'narrow' in CFD terms?
Message 8 of 16
srhusain
in reply to: ssenbore

You are correct about the pressure drop issue.

Based on the dimensions you mentioned, the model should be amenable to analysis with Adv5

Message 9 of 16
nhahn
in reply to: ssenbore

In this case then, would it make more sense to set the scenario environment to 1018 psi, the inlet to specified mass flow, and the outlet to zero psi gage? Or does this end up the same (I wonder). Make sure your material properties are appropriate for the elevated pressure, too.

The bigger issue here is that based on your scale, and the fact that you are interested in the losses due to the nozzle (not in the pressure distribution in the flowfield), what you really need to be interested in is getting the viscous losses right. So focus on good meshing in the boundary layer, make sure y+ is low (enable y+ adaptation) and choose advection scheme to minimize artificial dissipation -- ADV 1 is out, ADV 5 better. Maybe even ADV3 ?

Finally, make sure you know where/how the lab data was gathered - it can't be an average across the exit plane like you can do in CFD - so if it was a pitot tube try to use a results point the same location, if not on centerline.
Message 10 of 16
srhusain
in reply to: nhahn

Hi:

 

These are good points.

 

One thing about incompressible flow (unless you are concerned or on the lookout for cavitation), is that the pressure is not a thermodynamic quantity and is purely mechanical in nature. So, when density is fixed (frequently a good idealization), the boundary condition for pressure is largely a relative value and the interesting result is the variation of pressure itself (such as a drop or a rise) within the model.

 

In the end, it depends on your judgement and the assumptions you want to make regarding the material properties when setting up the problem.

Message 11 of 16
ssenbore
in reply to: nhahn

Let me try to be more clear.

 

I am not really interested in the head losses in the nozzle.  I am more interested in the change in pressure as the water flows from a larger diameter area (green) to a smaller diameter area (red).  This is water at 440 F and 1018 psi absolute.  The system is a closed system (so the outlet does not dump to the atmosphere) so there is really no place that I can use a P=0 Boundary Condition.

 

Is the Boundary Layer meshing still a concern in this case?

 

Capture1.PNG

Message 12 of 16
srhusain
in reply to: ssenbore

As i mentioned previously, for constant density flow the P=0 boundary condition is purely a relative value- with constant density (which is an excellent assumption for a fluid like water) you will get the same velocity field with P=0 or with P=1000psi as a boundary condition while maintaining the same flow rate.

 

Moreover, with a constant density you should get the same pressure variation regardless of the pressure boundary condition value at the exit as long as you have the same flow rate at the inlet.


So, for example, suppose you put P=0 psi(gauge) at the exit and find that the pressure solution at the inlet is 17 psi (gauge). If then you assign P=1000 psi(gauge) at the exit and re-run the problem with the same flow rate as previously, you should get a pressure of 1017psi (gauge) at the inlet as part of the solution.

 

If, however, you are trying to model density changes due to pressure, you have to run compressible flow, which is entirely different from a constant density assumption. At this stage, you have to decide from apriori knowledge if the flow is sub-sonic or supersonic. Most water based analyses (except for water-hammer) assume that the density is only a function of temperature at best and that the flow is essentially incompressible., so this is likely not your concern, but i may stand corrected.

 

Finally, if you want to let density change with temperature as well because you are running heat transfer, then select as Variable for the water material and be sure to prescribe appropriate reference pressure and temperature for the environment settings.

 

Message 13 of 16
Royce_adsk
in reply to: srhusain

The boundary layer mesh is still very important and critical to achieving a good pressure drop through pipes/valves, orifice plates, etc.

 

Like the earlier post said.  Leverage the mesh adaptation and set your Y+ value to 30-50 for K-e.  If you wanted to try using SST then I would change my strategy since the physics at the wall are modeled differently. Use 2015 since I am finding adaptation works really well in this version.  Consider this rev3 of our mesh adaptation development.

 

If you toss your share file up here you might be surprised what sort of work people on this forum will do/show you with your model.

 

Cheers!

 

 



Royce.Abel
Technical Support Manager

Message 14 of 16
ssenbore
in reply to: Royce_adsk

The Archive file can be downloaded from the link below.  If anyone wants to take a stab at it, I would greatly appreciate it.  Real world and hand calcs put the pressure difference between the green and red sections (screenshot in earlier post) at 16.7 psi, but I am getting 20 psi in the simulation.

 

Thanks!

 

https://www.dropbox.com/s/6fz2lyr46t9xuog/fluent-demo2_help.cfz

Message 15 of 16
ssenbore
in reply to: srhusain

Hi Everyone,

Thanks for your help! I focused on getting the simulation in the Boundary Layer region right, used Mesh Adaptation with Y+ adaptation turned on, and Intelligent Wall Formulation (k-e turbilence model).

I got within 4.9% of hand calculated values, (which is very good in my book.)

Thanks for all your help and suggestions, to everyone that commented on this.
Message 16 of 16
ssenbore
in reply to: Royce_adsk

Thanks Royce. Your suggestion of Y+ adaptation worked well. That helped me get close to thehand calculated value within 4.9%.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report