CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Domain Reference Pressure and mass flow inlet boundary

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

Like Tree5Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 14, 2018, 09:58
Default
  #61
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20
cfd seeker is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
It is possible to have flow driven by a moving mesh and an inlet. I have done it many times. There is some problem with your simulation.

Your images show some pressure variation and some velocity. So the flow is just starting up, isn't it?
Thta would be really interesting to know that if Total pressure B.C is used in such a simulation (one inlet, no outlet and moving wall) then from the solver will get the information about the velocities?
cfd seeker is offline   Reply With Quote

Old   August 14, 2018, 10:19
Default
  #62
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22
Lance is on a distinguished road
I dont get it. What is your question/problem?
You have a single inlet, no outlet and a domain that changes in size?
Given an incompressible fluid you must have a flow rate at the inlet, which is determined by the time rate of change of domain volume. If the flow rate is wrong (compared to what?) then your domain volume change (wall motion) is changing too slow or fast.
Lance is offline   Reply With Quote

Old   August 14, 2018, 16:38
Default
  #63
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20
cfd seeker is on a distinguished road
Quote:
You have a single inlet, no outlet and a domain that changes in size?
Yes

Quote:
Given an incompressible fluid you must have a flow rate at the inlet, which is determined by the time rate of change of domain volume. If the flow rate is wrong (compared to what?) then your domain volume change (wall motion) is changing too slow or fast
No, flow rate is not determined by the time rate of change of domain volume. Mass flow rate is dependent on the pump. Actually the flow coming out from the pump at particular mass flow rate and at particular pressure generates the pressure inside actuator which forces the actuator to lift upwards.
cfd seeker is offline   Reply With Quote

Old   August 15, 2018, 06:04
Default
  #64
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22
Lance is on a distinguished road
Quote:
Originally Posted by cfd seeker View Post
No, flow rate is not determined by the time rate of change of domain volume. Mass flow rate is dependent on the pump. Actually the flow coming out from the pump at particular mass flow rate and at particular pressure generates the pressure inside actuator which forces the actuator to lift upwards.
But that is not what you are modeling if you prescribe the wall motion... You can have any pressure at the inlet, but the mass flow rate is going to depend on the volume change of the domain when you prescribe the wall motion.
Lance is offline   Reply With Quote

Old   August 15, 2018, 07:45
Default
  #65
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20
cfd seeker is on a distinguished road
Quote:
Originally Posted by Lance View Post
But that is not what you are modeling if you prescribe the wall motion... You can have any pressure at the inlet, but the mass flow rate is going to depend on the volume change of the domain when you prescribe the wall motion.
Ok. But in reality the flow enters at particular pressure and mass flow rate which generates pressure inside domain and this generated pressures forces the domian walls to move for a particular distance in a particular time. Can this be modelled? If yes how?
cfd seeker is offline   Reply With Quote

Old   August 15, 2018, 07:53
Default
  #66
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22
Lance is on a distinguished road
Yes,

either with a coupling to a solid solver ("2-way" FSI)

or

using the generated pressures and knowledge about how much displacement that would result in, prescribe the displament using a CEL expression.
Lance is offline   Reply With Quote

Old   August 15, 2018, 09:19
Default
  #67
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20
cfd seeker is on a distinguished road
Quote:
Originally Posted by Lance View Post

using the generated pressures and knowledge about how much displacement that would result in, prescribe the displament using a CEL expression.
I am already specifying the displacement on the walls using expression (using d = V*t) but I know only the pressure at the Inlet. Thr purpose of the simulation is to determine the presure loss of flow till it reaches the displaced surfaces/moving walls. So what could be done in this case?
cfd seeker is offline   Reply With Quote

Old   August 16, 2018, 03:39
Default
  #68
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20
cfd seeker is on a distinguished road
Quote:
Originally Posted by Lance View Post
Yes,
using the generated pressures and knowledge about how much displacement that would result in, prescribe the displament using a CEL expression.
I was already modelling this by specifying the dispalcement on the moving walls using expression (d = V*t, "t" being the simulation time). But in your previous comment you said this problem can't be modelled like this. Can you please elaborate further on this?

Purpose is to study the pressure losses till the flow reaches the lifting surface/moving walls.
cfd seeker is offline   Reply With Quote

Old   August 16, 2018, 04:02
Default
  #69
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22
Lance is on a distinguished road
If you prescribe the motion by d = v*t (assuming v is velocity?) then I assume you know the velocity the wall moving with? Then, if the mass flow at the inlet is too low/high, then this velocity is too low/high.

If the goal of your model is to get the pressure drop from inlet to moving wall, then I would run a bunch of simulations with different prescribed displacement velocities and check the mass flow rate and pressure drop.

You can prescribe the motion of a surface as a function of almost anything, including pressure, force, etc. Use CEL expressions (e.g. areaAve(pressure)@surface). Of course this would require knowledge about mass, external forces, etc. In earlier versions of CFX (v11 maybe?) there used to be a good example of how this was solved on a ball check valve, but it has now been replaced by the rigid body solver.

Anyway, it sounds like you need to take a step back and think through what you are interested in and what you are actually modelling.
Lance is offline   Reply With Quote

Old   August 16, 2018, 10:34
Default
  #70
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20
cfd seeker is on a distinguished road
Quote:
If you prescribe the motion by d = v*t (assuming v is velocity?) then I assume you know the velocity the wall moving with? Then, if the mass flow at the inlet is too low/high, then this velocity is too low/high.
Wall velocity is correct as the stroke length of actuator and the time it takes to complete the stroke is exactly know. I also verified the mass flow rate/volume flow rate from the rate of change of domain size (from initial and final volumes of domain obtained from CAD model and time) and it's correct. So the specified velocity is correct. But the mass flow rate in the simulation is very low. I checked the mass flow rate after 0.08 (total simulation time is 2 seconds) seconds and its very low as comapred to actual mass flow rate.

BTW i am using the following expression for the mesh displacement
Code:
0.0125*t
where t being the simulation time. Is "t" in CFX corresponds to simulation time? Sorry for very basic question but I just want to make sure that there is no mistake in expression.

In the domain settings under "Mesh Deformation" i am using "Displacement Rel. To = Previous Mesh" and then for moving walls under "Mesh Motion" i am using the "Specified Displacement" and specifying the displacement using the expression above. Is it correct?

In the modelling guide of CFX i read about "Mesh Motion" and "Specified Displacement" options there its written " If the Use Mesh From option is set to Initial Values, be careful with restarts because the definition of the initial mesh may have changed." Where I can find this option "Use Mesh From"? I made several restarts but didn't change anything but I think mesh is still moving correctly.

Mesh_Motion_Options.jpg

Also what's the difference between "Specified Displacement" and "Specified Location" Mesh Motion options? If I have the displacement equation (mentioned above) I should be using "Specified Displacement" right?

Sorry if i am asking a lot of questions but this is my first experience with moving mesh simulations and i am still in the learning process.

Last edited by cfd seeker; August 16, 2018 at 17:11.
cfd seeker is offline   Reply With Quote

Old   August 16, 2018, 20:55
Default
  #71
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,746
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
As you are new to moving mesh I would suggest you do a simpler model first to get started. As you know the motion of the actuator, that means you know the flow rate it generates. So remove the actuator and the moving mesh and replace it with an outlet with a mass flow rate from the actuator. This is a simple steady state inlet/outlet simulation with no moving mesh and should be quite easy to do. You should also be able to get this quite accurate relatively easily, so will give you a good starting point to work from.

Once you have this simple model working well then try the more ambitious moving mesh version. As you develop the moving mesh you will then be able to compare against the simple model to check the results are reasonable.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 17, 2018, 03:22
Default
  #72
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20
cfd seeker is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
As you are new to moving mesh I would suggest you do a simpler model first to get started. As you know the motion of the actuator, that means you know the flow rate it generates. So remove the actuator and the moving mesh and replace it with an outlet with a mass flow rate from the actuator. This is a simple steady state inlet/outlet simulation with no moving mesh and should be quite easy to do. You should also be able to get this quite accurate relatively easily, so will give you a good starting point to work from.

Once you have this simple model working well then try the more ambitious moving mesh version. As you develop the moving mesh you will then be able to compare against the simple model to check the results are reasonable.
thanks for your reply. Actually i already did so, i created an outlet and using total pressure and mass flow rate B.C i did the simulation and it was quite simple. Convergence was very good and i was able to see the pressure losses and they made sense also. Now i am upto more ambitious moving mesh version

Can you please clarify my confusions from the last post?
cfd seeker is offline   Reply With Quote

Old   August 19, 2018, 06:06
Default
  #73
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,746
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Specified location and Specified displacement: Let's say you have a mesh at x=1m and you want it to move right 0.1m at 1m/s. This can be defined by:

Specified Displacement = 0.1[m]*t

or

Specified Location = 1.0[m] + 0.1[m]*t

So the difference is whether it is the displacement from the initial position or the absolute position.

Check how much your mesh has moved to check it moved the distance you intended.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 20, 2018, 01:16
Default
  #74
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22
Lance is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Specified Location = 1.0[m] + 0.1[m]*t
So the difference is whether it is the displacement from the initial position or the absolute position.
Since the the above expression will resolve into a single value, all points on that surface will collapse to that location. Probably not what you want.


Quote:
Originally Posted by ghorrocks View Post
Specified Displacement = 0.1[m]*t
This also resolves into a single value, but all points on the surface will be displaced by that value. Probably what you want.
Lance is offline   Reply With Quote

Old   August 20, 2018, 03:45
Default
  #75
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20
cfd seeker is on a distinguished road
Thanks Glenn and Lance,

i understood the difference but the units of following expression is confusing me
Code:
Specified Displacement = 0.1[m]*t
You said if we want the mesh to move right by 0.1m. So in the above expresion Displacement = Displacement*time? "t" in above xpression do-not have units of time i.e seconds?

When you say if we want the mesh to move right by 0.1m with 1m/s. Then the expression shouldn't be Displacement = Velocity*Time?
Code:
Specified Displacement = 1[m/s]*t
Can any of you guys please clarify this?
cfd seeker is offline   Reply With Quote

Old   August 20, 2018, 05:37
Default
  #76
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22
Lance is on a distinguished road
Well, since displacement is a length that is obviously a typo.
Lance is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 58 July 3, 2020 01:13
mass flow in is not equal to mass flow out saii CFX 12 March 19, 2018 05:21
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 15:55
New topic on same subject - Flow around race car Tudor Miron CFX 15 April 2, 2004 06:18


All times are GMT -4. The time now is 22:35.