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

Transient, Prescribed Mesh Displacement at a Boundary-Wall

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 28, 2010, 20:15
Exclamation Transient, Prescribed Mesh Displacement at a Boundary-Wall
  #1
New Member
 
Majed
Join Date: Jul 2010
Location: Ottawa
Posts: 6
Rep Power: 7
Majed_A is on a distinguished road
I am trying to setup a transient simulation where a Complex 3D-wall boundary is moving in time. The locations of the nodes on the wall are known for every timestep prior to running the solver. A file for each timestep has been generated which contains the displacements of all the FEA nodes at the boundary of interest in the format X,Y,Z,Xdisp,Ydisp,Zdisp. Using ICEM CFX, I generate a fluid domain with the exact geometry as the wall boundary in the FEA simulation and now I would like to move the CFX nodes at the boundary of interest in a similar manner. I am attempting to implement this by using the profile boundary data method to specify the displacement for the nodes, different for each time step. So far i have only been able to implement this method successfully for the first time step. I would like to know how to use the profile boundary data method to implement a 3d-boundary wall displacement, different for each time step, using ANSYS CFX 12.1. If there is another method that will allow this simulation to work please indicate so.
Majed_A is offline   Reply With Quote

Old   October 29, 2010, 07:05
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This would probably be best implemented in fortran. There used to be an example of using fortran to do moving mesh but it got removed in CFX V12 I think. Have a look at the ball valve tutorial in CFX V11 or ask support for an example fortran to do moving mesh.
ghorrocks is offline   Reply With Quote

Old   November 1, 2010, 18:19
Default
  #3
New Member
 
Majed
Join Date: Jul 2010
Location: Ottawa
Posts: 6
Rep Power: 7
Majed_A is on a distinguished road
Thanks for your reply. So far i have implemented a junction box routine(JBR) that is executed after each time step which replaces the content of the profile boundary data file with that corresponding to the current time step. For example, i set ‘readmyfile’ as the boundary profile data file for the wall boundary of interest. At the start of each timestep the JBR is executed and takes file content from ‘readmyfile_t1’, ‘readmyfile_t2’.... ‘readmyfile_tn’, which corresponds to the current timesteps and re-writes it in ‘readmyfile’. In effect, ‘readmyfile’ is updated everytime step with the corresponding timestep file. After running several simulations, I noticed that the boundary profile data is read only once at the start of the run. Is there any way to enforce the boundary profile data to be read at every timestep in CFX which would be an ideal solution to my problem.
Majed_A is offline   Reply With Quote

Old   November 1, 2010, 21:39
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You will want to keep the mesh topology the same and the boundry definitions the same as much as possible. To update the mesh topology or boundary condition definitions you will need to do an interpolation step - CFX V12 I think has some new stuff for this but I am not too familiar with it.
ghorrocks is offline   Reply With Quote

Old   November 2, 2010, 08:10
Default
  #5
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
Hello,

Perhaps you could use the same technique as i did in this tutorial for a transient boundary profile. I haven't tried it but i cant see why it wouldn't work.

http://www.edr.no/blogg/ansys_blogge...nsient_profile



Klas Johansson, Ph.D.
Technical Consultant at EDR
mailto:klas.johansson@edr.se




EDR blog
http://www.edr.se/blogg
Newsletter
http://www.edr.se/nyhetsbrev
adeban is offline   Reply With Quote

Old   November 3, 2010, 15:27
Default
  #6
New Member
 
Majed
Join Date: Jul 2010
Location: Ottawa
Posts: 6
Rep Power: 7
Majed_A is on a distinguished road
Hi,

Thanks for the reply. The profile boundary data is read only for the initial boundary profile. I need this file to be re-read every timestep becuase the deformation is different every timestep. I have a fortran junction box routine executed at the start of each timestep that replaces the boundary profile data file in the current directory. But the problem is that this file is only read once that start of the run. Your method does work, but only works for the initial timestep, and i am not sure if you force cfx to read the profile data file every timestep.

Majed
Majed_A is offline   Reply With Quote

Old   November 4, 2010, 03:36
Default
  #7
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
Aha,

So the deformation you prescribe is actually changing with the solution then. That makes it more complicated. This method will only work if the displacement is know before the simulation actually starts.

/klas
adeban is offline   Reply With Quote

Old   November 4, 2010, 09:10
Default
  #8
New Member
 
Majed
Join Date: Jul 2010
Location: Ottawa
Posts: 6
Rep Power: 7
Majed_A is on a distinguished road
Aklan,

Yes the deformaiton is different at every timestep, but it has been solved already with FEM using LSDYNA. I have simply taken the transient solution from the FEA solver and generated about 200 .csv files for each timestep. Each file follows the format for the initialized boundary profile data. The problem that i am trying to solve is having cfx-solver read each file at the corresponding timestep. So far it seems that the only way to solve this is to use a fortran routing. I have implemented this already but i am unsure of how to return the data to the RET variable.
Thanks, Majed
Majed_A is offline   Reply With Quote

Old   November 4, 2010, 10:49
Default
  #9
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
Ok.

Since the motion is fixed you can actually use the method i described. You just merge the csv files and add another column for the time (X,Y,Z,time,Xdisp,Ydisp,Zdisp). The read it in and use as normal. The setup of this file should be like this:

http://www.edr.no/var/edr/storage/im...profile_02.png

WOuldnt that work to merge them? Then the displacements for the entire simulation is read in at the start and used later on during the solution. Havent done anything like it so im a bit unsure.

/klas
adeban is offline   Reply With Quote

Old   November 4, 2010, 11:08
Default
  #10
New Member
 
Majed
Join Date: Jul 2010
Location: Ottawa
Posts: 6
Rep Power: 7
Majed_A is on a distinguished road
Thanks for reply. The problem is when calling the function. CFX only allows a maximum of 3 spatial fields. For my situation there is 4 spatial fields, (X,Y,Z,t). So if i merge all my files to one .csv file in the format you have suggested i will not be able to call a function as myMeshDisp(x,y,z,t) because CFX is limited by 3 spatial fields. I am now working on creating a fortran routine to see where it takes me.Again thanks a lot for your interest and replies.
Majed_A is offline   Reply With Quote

Old   November 4, 2010, 11:25
Default
  #11
New Member
 
Klas Johansson
Join Date: Mar 2009
Posts: 16
Rep Power: 8
adeban is on a distinguished road
ok. That gives this a big limitation. I understand that you end up with a problem.

Good luck with the fortran.
adeban is offline   Reply With Quote

Old   November 26, 2010, 09:59
Default
  #12
New Member
 
Nenad Andric
Join Date: Jul 2010
Posts: 11
Rep Power: 7
Nenad is on a distinguished road
Hello,
I have problem similar to this one http://simutechny.blogspot.com/2010/...g-wall-in.html but I can't make any progress. I have splited geometry, so now it's made of two bodies. I should make spliting plane move in Z direction for 0.3mm displacement (as black arrow shows), but somehow I can't define it very well. My simulation brakes immediately.
http://img809.imageshack.us/i/duese08.jpg/
http://img139.imageshack.us/i/duese07.jpg/
Do you have any ideas how to do this?

Thank you

Nenad
Nenad is offline   Reply With Quote

Old   November 27, 2010, 05:42
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
There are tutorial examples which come with CFX which show how to do this sort of modelling.
ghorrocks is offline   Reply With Quote

Old   April 15, 2011, 13:54
Default @ adeban:
  #14
Senior Member
 
Ugly Kid Joe
Join Date: Aug 2010
Posts: 193
Rep Power: 7
vmlxb6 is on a distinguished road
The link that you shared:

http://www.edr.no/blogg/ansys_blogge...nsient_profile

The step where you enter myin.Velocity(x,z,t), gives me an error saying expected units for Normal component is ms^-1.

Is the expression myin.velocity(x,z,t) correct ???????

Is there another way to do it ?????

Thanks
vmlxb6 is offline   Reply With Quote

Old   March 15, 2012, 09:43
Default mesh displacement or total mesh displacement
  #15
Member
 
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 6
Mina_Shahi is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You will want to keep the mesh topology the same and the boundry definitions the same as much as possible. To update the mesh topology or boundary condition definitions you will need to do an interpolation step - CFX V12 I think has some new stuff for this but I am not too familiar with it.

Hi

I am trying to messure the mesh displacement in CFX, so i i set some monitor points in the walls but i am just wondering that which one i should messure total mesh displacement or mesh displacement? i defined both and i saw different results, i am going to compare the result of CFD with data from Experiment so it is very important for me to know which one is the one i should look for?

i would apppreciate if you can help me
Mina_Shahi is offline   Reply With Quote

Old   March 15, 2012, 12:18
Default
  #16
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 522
Rep Power: 11
Lance is on a distinguished road
Quote:
Originally Posted by Mina_Shahi View Post
Hi

I am trying to messure the mesh displacement in CFX, so i i set some monitor points in the walls but i am just wondering that which one i should messure total mesh displacement or mesh displacement? i defined both and i saw different results, i am going to compare the result of CFD with data from Experiment so it is very important for me to know which one is the one i should look for?

i would apppreciate if you can help me
Total mesh displacement is the displacement relative to the initial mesh, while mesh displacement is the displacement relative to the previous mesh location
Lance is offline   Reply With Quote

Old   March 17, 2014, 11:58
Default mesh displacement
  #17
avk
New Member
 
arun
Join Date: Nov 2010
Posts: 3
Rep Power: 6
avk is on a distinguished road
Hi,

Please help me if someone find a way to model mesh displacement with (x,y,z,t) variables?

Thank you,
AVK
avk is offline   Reply With Quote

Old   March 17, 2014, 17:18
Default
  #18
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What do you mean by xyzt variables? Do you have the xyz position of the body as a function of time? Or the xyz position of the nodes as a function of time?
ghorrocks is offline   Reply With Quote

Old   March 18, 2014, 15:14
Default
  #19
avk
New Member
 
arun
Join Date: Nov 2010
Posts: 3
Rep Power: 6
avk is on a distinguished road
Glenn,

I have the x,y,z values of the nodes changing with time. I have 6 different files denoting 6 different positions of the nodes changing in time in sequence. I was wondering if I can apply these as wall displacement boundary condition and call it at particular time steps.

Thanks a lot,
Avk
avk is offline   Reply With Quote

Old   March 18, 2014, 17:51
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you know the location of each node at each time step then you can use a fortran routine to prescribe the mesh motion. Contact ANSYS support for an example of using this approach, I know they have an example.
ghorrocks is offline   Reply With Quote

Reply

Tags
boundary mesh deformation, boundary profile data, transient

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
boundary conditions and mesh exporting vaina74 Open Source Meshers: Gmsh, Netgen, CGNS, ... 2 May 27, 2010 09:38
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
how to use Total Mesh Displacement for making a subject translating and rotating? snailstb CFX 3 September 16, 2009 04:06
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 13:41.