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

URGENT: Creating Slices in Tecplot360

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 24, 2012, 23:38
Default URGENT: Creating Slices in Tecplot360
  #1
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 8
MASOUD is on a distinguished road
Hi folks,

I need to create a few slices in tecplot. When I use Fluent Data Loader, it is easy to create slice. But when I use Export Data option in Fluent and create Tecplot files and then use Tecplot Data loader in Tecplot, the "Slices" is not active.

Any help is highly appreciated.
MASOUD is offline   Reply With Quote

Old   April 25, 2012, 01:58
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 591
Rep Power: 11
LuckyTran is on a distinguished road
Quote:
Originally Posted by MASOUD View Post
Hi folks,

I need to create a few slices in tecplot. When I use Fluent Data Loader, it is easy to create slice. But when I use Export Data option in Fluent and create Tecplot files and then use Tecplot Data loader in Tecplot, the "Slices" is not active.

Any help is highly appreciated.
That is correct. Slices don't work if you do that.

The Export Data option in Fluent (even when you choose Tecplot format) saves a delimited text file of data points that tecplot can then read. It does not save in anything special that tecplot can interpret.

If you want to create slices in Tecplot then I suggest you keep using the Fluent Data importer or to read the case-data file directly into Tecplot.

Alternatively, you can create a plane in Fluent and then export solution data on only that plane (in tecplot format). Then you can read this data with Tecplot and it will only have and hence only plot data on the planes that were imported. You can simultaneously export from as many planes as you like. This is the method I normally use since I can define my planes in Fluent and export small data files rather than reading an entire case & data file each time in tecplot. This should also be similar to creating "slices" in tecplot.

Happy plotting!
LuckyTran is offline   Reply With Quote

Old   April 25, 2012, 04:30
Default
  #3
Senior Member
 
Philipov's Avatar
 
Svetlin Philipov
Join Date: Mar 2009
Location: United Kingdom
Posts: 176
Rep Power: 8
Philipov is on a distinguished road
save case and data files from fluent calculation and then use Tecplot option Fluent data loader..... there define your slice and whatever you want....
Philipov is offline   Reply With Quote

Old   April 25, 2012, 10:37
Default
  #4
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 8
MASOUD is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
That is correct. Slices don't work if you do that.

The Export Data option in Fluent (even when you choose Tecplot format) saves a delimited text file of data points that tecplot can then read. It does not save in anything special that tecplot can interpret.

If you want to create slices in Tecplot then I suggest you keep using the Fluent Data importer or to read the case-data file directly into Tecplot.

Alternatively, you can create a plane in Fluent and then export solution data on only that plane (in tecplot format). Then you can read this data with Tecplot and it will only have and hence only plot data on the planes that were imported. You can simultaneously export from as many planes as you like. This is the method I normally use since I can define my planes in Fluent and export small data files rather than reading an entire case & data file each time in tecplot. This should also be similar to creating "slices" in tecplot.

Happy plotting!
Many thanks for immediate reply.

1. When I use 'Fluent Data Loader' it does not import all variables, Custom Field Functions, etc. Is there any way to handle this issue?

2. In Fluent itself, it is easy to create planes for the whole computational domain, not for sub-domains. It is attached, in Z-direction if create a plane, it will have all 5 subdomains in it but i want just anode. Any help in this?

Thanks again
Attached Images
File Type: jpg domain.jpg (23.3 KB, 3 views)
MASOUD is offline   Reply With Quote

Old   April 25, 2012, 10:38
Default
  #5
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 8
MASOUD is on a distinguished road
Quote:
Originally Posted by Philipov View Post
save case and data files from fluent calculation and then use Tecplot option Fluent data loader..... there define your slice and whatever you want....
Thanks...please see the other reply.
MASOUD is offline   Reply With Quote

Old   April 25, 2012, 10:50
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 591
Rep Power: 11
LuckyTran is on a distinguished road
Quote:
Originally Posted by MASOUD View Post
Many thanks for immediate reply.

1. When I use 'Fluent Data Loader' it does not import all variables, Custom Field Functions, etc. Is there any way to handle this issue?

2. In Fluent itself, it is easy to create planes for the whole computational domain, not for sub-domains. It is attached, in Z-direction if create a plane, it will have all 5 subdomains in it but i want just anode. Any help in this?

Thanks again
1. Tecplot imports all data that is available. If Tecplot does not import it, then it is not there. Fluent saves only the most relevant variables to save storage space. Redundant variables are not stored and must be maually exported. Again, only the most fundamental variables such as velocity, pressure, turbulent kinetic energy, dissipation are saved. In your save options, you can choose which additional variables are saved. After you choose all the variables that you want, save again and import again into Tecplot.

Also, I am not sure if you are aware but you can perform calculations in Tecplot and come up with derived variables. If all the information is present and you simply want to derive a new variable from information that is present then you can write your own new variables in tecplot.

2. Each sub-domain should have it's own "zone" in Fluent. Export solution data individually zone by zone and then import zone by zone. Maybe there is a way to get Tecplot to recognize zones, I haven't looked that deep into it.
LuckyTran is offline   Reply With Quote

Old   April 25, 2012, 11:25
Default
  #7
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 8
MASOUD is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
1. Tecplot imports all data that is available. If Tecplot does not import it, then it is not there. Fluent saves only the most relevant variables to save storage space. Redundant variables are not stored and must be maually exported. Again, only the most fundamental variables such as velocity, pressure, turbulent kinetic energy, dissipation are saved. In your save options, you can choose which additional variables are saved. After you choose all the variables that you want, save again and import again into Tecplot.

Also, I am not sure if you are aware but you can perform calculations in Tecplot and come up with derived variables. If all the information is present and you simply want to derive a new variable from information that is present then you can write your own new variables in tecplot.

2. Each sub-domain should have it's own "zone" in Fluent. Export solution data individually zone by zone and then import zone by zone. Maybe there is a way to get Tecplot to recognize zones, I haven't looked that deep into it.

1. If i am not mistaken, to have additional variables:
File=>Data File Quantities=>select Additional Quantities=>OK and then File=>Write=>Case and Data and then use Fluent Data Loader in Tecplot

With this procedure, again I can't see my defined variables using Custom Field Function (which uses two UDM calculated in a UDF)

2. To have a plane on Z-axis (e.g. z=2), Fluent can create a plane using the Surface=>Plane=>options=>Alligned with surface...
But this gives me a plane which hass all 5 sub-domains in the attached figure. But I just need the anode in this plane. How can I do this?

Thanks a lot.
MASOUD is offline   Reply With Quote

Old   April 25, 2012, 12:02
Default
  #8
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 591
Rep Power: 11
LuckyTran is on a distinguished road
Quote:
Originally Posted by MASOUD View Post
1. If i am not mistaken, to have additional variables:
File=>Data File Quantities=>select Additional Quantities=>OK and then File=>Write=>Case and Data and then use Fluent Data Loader in Tecplot

With this procedure, again I can't see my defined variables using Custom Field Function (which uses two UDM calculated in a UDF)

2. To have a plane on Z-axis (e.g. z=2), Fluent can create a plane using the Surface=>Plane=>options=>Alligned with surface...
But this gives me a plane which hass all 5 sub-domains in the attached figure. But I just need the anode in this plane. How can I do this?

Thanks a lot.
1. That is the correct procedure. Not sure why you can't see the UDF variables, I might edit when I think about this more and find the answer.

2. You can also create a point (or point surface) the same way.
LuckyTran is offline   Reply With Quote

Old   April 25, 2012, 12:25
Default
  #9
Senior Member
 
MASOUD
Join Date: Mar 2009
Posts: 102
Rep Power: 8
MASOUD is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
1. That is the correct procedure. Not sure why you can't see the UDF variables, I might edit when I think about this more and find the answer.

2. You can also create a point (or point surface) the same way.
Thanks. I didn't understand Answer-2. How can a Point give the plane?
MASOUD is offline   Reply With Quote

Old   April 25, 2012, 13:28
Default
  #10
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 591
Rep Power: 11
LuckyTran is on a distinguished road
Quote:
Originally Posted by MASOUD View Post
Thanks. I didn't understand Answer-2. How can a Point give the plane?
Oops. I thought you mean a node, I just realized you meant anode. So that would not work.

Do you have the different regions set up in Fluent as different zones? You should, cause otherwise they are the same logical zone and there is no differentiation between each. You can export data by zone.
LuckyTran is offline   Reply With Quote

Old   April 26, 2012, 18:25
Default
  #11
Senior Member
 
Scott Rumage
Join Date: May 2009
Location: Seattle, WA
Posts: 117
Rep Power: 8
scott_rumage is on a distinguished road
Masoud, the latest release of Tecplot 360 2012 has the ability to do a "constrained slice". This feature may solve your need to create a slice of the anode area only. Here is a link showing to a page with a video showing this feature: http://www.tecplot.com/Solutions/Pro...strainedslices

One can download the latest version or a full-featured demo version from the Tecplot web-site as well.

Scott
scott_rumage is offline   Reply With Quote

Old   April 27, 2012, 01:30
Default
  #12
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 591
Rep Power: 11
LuckyTran is on a distinguished road
Quote:
Originally Posted by scott_rumage View Post
Masoud, the latest release of Tecplot 360 2012 has the ability to do a "constrained slice"
Any luck with this Masoud? Don't forget you can show more than one slice at once.
LuckyTran is offline   Reply With Quote

Reply

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
Problems in creating a wedge type mesh Joscha OpenFOAM Native Meshers: blockMesh 22 May 14, 2015 05:10
Fluent3DMeshToFoam simvun OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 48 May 14, 2012 05:20
Problem in running ICEM grid in Openfoam Tarak OpenFOAM 6 September 9, 2011 17:51
Problems with Meshing: Collapsed Cells Emmanuel Resch CD-adapco 1 July 30, 2007 03:02
Gerris software installation mer Main CFD Forum 2 November 12, 2005 09:50


All times are GMT -4. The time now is 07:22.