# How is total pressure calculated?

 Register Blogs Members List Search Today's Posts Mark Forums Read

October 27, 2019, 13:24
How is total pressure calculated?
#1
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
Hi everyone!
I've been studying CFX and have faced with misunderstanding.
How does ansys calculate total pressure?
Can anybody explain me it using my example?
Geometry and BC see on fig. 1.
I've simulated this problem three times:
1) Mesh~93,300 cells (fig.2). Referense pressure = 0, pressure outlet = 1 bar.
2) The same mesh. Ref pressure = 1 bar, pressure outlet = 0.
3) Mesh ~3,500,500 cells (fig.3). Ref pressure = 0, pressure outlet = 1 bar.

The results of these simulations see on fig. 4,5,6 correspondingly (F column for difference between upper and bottom planes)

As I've understood, In Ansys:
pressure+reference pressure = static pressure
pressure+reference pressure + *g*h=absolute pressure.
In Ansys help is written, that total pressure = static pressure + dinamic pressure. So why total pressure is less then static pressure in my simulations?
Moreover, why are results for total pressure difference (6F cell) in (1,2) and (3) simulations so different (In about 2,5 times)? All problems have converged to my precision very fast.
Attached Images
 Geometry.PNG (26.8 KB, 59 views) MESH 1 (~93000).jpg (87.4 KB, 41 views) MESH 2 (~3500000).jpg (115.6 KB, 39 views) RES1.PNG (13.4 KB, 59 views) RES2.PNG (13.3 KB, 32 views)

October 27, 2019, 13:27
#2
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
The 6th figure (results for the 3rd simulation) is it.
Attached Images
 RES3.PNG (13.4 KB, 81 views)

 October 27, 2019, 17:17 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,728 Rep Power: 143 I cannot figure out which image refers to which simulation. As they are just tables of numbers can you put the relevant numbers directly in the post, not as images? __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

October 28, 2019, 02:12
#4
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
Quote:
 Originally Posted by ghorrocks I cannot figure out which image refers to which simulation. As they are just tables of numbers can you put the relevant numbers directly in the post, not as images?
I've united tables. Maybe it'll be more clearly.
I think, that putting the relevant numbers directly in the post will be less clearly for understanding (without table).
Attached Images
 All results.png (42.4 KB, 63 views)

 October 29, 2019, 15:00 #5 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 1,171 Rep Power: 23 Pay attention to reference density and location. These may make a difference. By default, location is automatic, so who knows where that would be. It also may depend on whether you are using full buoyancy model or boussinesq approximation. Easiest thing to do would be to make a test model where you know what the results should be already, then you can figure out how CFX calculates these things. Start with free slip walls, and a very low flow, so you are only figuring out the static head portion of the pressure variables. Remember to set a reference density and location. Or use 1 simple 1D model using symmetry for the walls, so there is no pressure drop whether you have flow or not. Start adding to the test model to figure out how other components contribute. PS. That is a very strange mesh for fluids. It does not look like good boundary layer resolution. (Not suggesting that is making a difference here)

October 29, 2019, 16:09
#6
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
Quote:
 Originally Posted by evcelica Pay attention to reference density and location. These may make a difference. By default, location is automatic, so who knows where that would be. It also may depend on whether you are using full buoyancy model or boussinesq approximation. Easiest thing to do would be to make a test model where you know what the results should be already, then you can figure out how CFX calculates these things.
I didn't pay attention to ref. density and location because I haven't understood yet what they mean. But I'll figure it out now.
For this simulation I already know what results should be (I've made hand calculations). And all values (except total pressure) correspond to these results.

 October 29, 2019, 16:19 #7 Senior Member   Join Date: Jun 2009 Posts: 1,815 Rep Power: 32 For clarification, in ANSYS CFX Absolute Pressure = Static Pressure + Reference Pressure Static Pressure = "solved" Pressure (variable in the momentum equation) + hydrostatic pressure For incompressible flow: Total Relative Pressure = Static Pressure + "dynamic" pressure For compressible flow: Total Relative Pressure = Absolute Total Pressure - Reference Pressure Absolute Pressure = Absolute Pressure if the flow is isentropically slowed down to rest.

October 29, 2019, 17:11
#8
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
Quote:
 Originally Posted by Opaque For clarification, in ANSYS CFX Absolute Pressure = Static Pressure + Reference Pressure Static Pressure = "solved" Pressure (variable in the momentum equation) + hydrostatic pressure For incompressible flow: Total Relative Pressure = Static Pressure + "dynamic" pressure For compressible flow: Total Relative Pressure = Absolute Total Pressure - Reference Pressure Absolute Pressure = Absolute Pressure if the flow is isentropically slowed down to rest.
Thanks!
I've understood what absolute pressure, static pressure, ref. pressure and "solved" pressure means.

But I supposed, that:
Absolute Pressure = Static Pressure + hydrostatic Pressure
Static Pressure = "solved" Pressure (variable in the momentum equation) + reference pressure.

Actually these definitions aren't making a significant difference here.

The values of these quantities (absolute pressure and static pressure) in my simulation are looking sanity (in my definitions they coincide with the hand calculated values).

I also understand that total pressure should be = static pressure + .

But in my simulation total pressure is less then ("solved" Pressure + ref. pressure). It's wrong, isn't it?

October 29, 2019, 17:32
#9
Senior Member

Join Date: Jun 2009
Posts: 1,815
Rep Power: 32
Quote:
 Actually these definitions aren't making a significant difference here.
It may not make a "quantitative difference" for you, but it makes it understandable for others to speak using a common vocabulary for CFX users.

Quote:
 But in my simulation total pressure is less then ("solved" Pressure + ref. pressure). It's wrong, isn't it?
Do not try to compare Total Pressure to Solved Pressure + Ref Pressure. I was clear earlier, they are not defined that way for ANSYS CFX. If you read it that way, it would be great to point us to the documentation section where it says so.

Does it looks off? Yes it does, but as Evcelica mentioned, more information (in CFX speak) is needed.

Hope the above helps

October 29, 2019, 17:58
#10
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
Quote:
 Originally Posted by Opaque For compressible flow: Total Relative Pressure = Absolute Total Pressure - Reference Pressure Absolute Pressure = Absolute Pressure if the flow is isentropically slowed down to rest.
Can you explain what is absolute total pressure?
There is only the "total pressure" in CFX (not total relative pressure or ablosute total pressure).
Attached Images
 pressures.jpg (152.7 KB, 20 views)

October 29, 2019, 18:29
#11
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
Quote:
 Originally Posted by evcelica Pay attention to reference density and location. These may make a difference. By default, location is automatic, so who knows where that would be. It also may depend on whether you are using full buoyancy model or boussinesq approximation.
Analyzing my results I can suppose, that reference location is located in pipe outlet.
I think, that there aren't any problems with reference density too.
So what is wrong?
Attached Images
 More inf1.PNG (47.7 KB, 22 views) more inf2.PNG (10.8 KB, 13 views)

 October 29, 2019, 18:29 #12 Senior Member   Join Date: Jun 2009 Posts: 1,815 Rep Power: 32 Absolute Total Pressure is effectively Total Relative Pressure + Reference Pressure. That variable is not presented by ANSYS CFX anywhere, but if you were to evaluate Total Density, you will use Absolute Total Pressure and the Total Temperature in the equation of state In ANSYS CFX, "Total" prefix is what others call "Stagnation". Total Pressure = Stagnation Pressure Total Enthalpy = Stagnation Enthalpy Total Density = Stagnation Density, ... jaavga1986 likes this.

October 29, 2019, 18:49
#13
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
Quote:
 Originally Posted by Opaque Absolute Total Pressure is effectively Total Relative Pressure + Reference Pressure. That variable is not presented by ANSYS CFX anywhere, but if you were to evaluate Total Density, you will use Absolute Total Pressure and the Total Temperature in the equation of state In ANSYS CFX, "Total" prefix is what others call "Stagnation". ...
Thanks a lot for your respond again!

But what is total relative pressure then?
You said, that Total Relative Pressure = Absolute Total Pressure - Reference Pressure, then I asked you what is Absolute Total Pressure.

You answered that Absolute Total Pressure is effectively Total Relative Pressure + Reference Pressure

I've also just found some proves of your answers (see fig.) - maybe It'll helpful for other people, like me

But I still don't understand how total pressure in my simulations has been calculated
Attached Images
 helpful information.jpg (70.4 KB, 23 views)

 October 29, 2019, 19:00 #14 Senior Member   Join Date: Jun 2009 Posts: 1,815 Rep Power: 32 Absolute Total Pressure is effectively Total Relative Pressure + Reference Pressure. That variable is not presented by ANSYS CFX anywhere, but if you were to evaluate Total Density, you will use Absolute Total Pressure and the Total Temperature in the equation of state

 October 30, 2019, 05:11 #15 Senior Member   M Join Date: Dec 2017 Posts: 645 Rep Power: 12 Honestly, I have no solution and can't see what might be wrong. However, can you extract the static and total pressure values directly at the inlet/outlet boundaries instead of these planes? As the total pressure relates to density and velocity, also check carefully that these values are in the expected range, calculate the value yourself and see if there's a difference.

October 30, 2019, 08:14
#16
New Member

Valera
Join Date: Dec 2018
Posts: 27
Rep Power: 7
Quote:
 Originally Posted by AtoHM Honestly, I have no solution and can't see what might be wrong. However, can you extract the static and total pressure values directly at the inlet/outlet boundaries instead of these planes? As the total pressure relates to density and velocity, also check carefully that these values are in the expected range, calculate the value yourself and see if there's a difference.
Can I send you a link to a cloud?
Except the extracted values for these planes, I've done it also for inlet and outlet directly (see fig. on the 4th message in this theme).

Values of density and velocity are in the expected ranged. I've calculated them manually.