|
[Sponsors] |
January 8, 2015, 03:45 |
|
#21 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Kevin,
Thanks for your help..... I have a another query. I have X, Y (plot) data, on this data I have to do some operations. I have tried but could not find how to do this 1) I want to create annotation on this X, Y data I want show how mass flow rate is changing with time. I have tried using calculator(Flow function) on clip but Ensight does not understand Flow3D OPEN volume & SOLID volume data. you can see that in attached image file, Flow3D predicting 183.6 & ensight giving me 196. 4 which is not matching with actual value. So can I create annotation on X, Y data? & Summation of those mass flow rate ? Thanks In advance.... |
|
January 8, 2015, 09:17 |
|
#22 |
Senior Member
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17 |
As you are plotting a "Constant Variable" versus time in your graph, you can simply right click on that Constant in the Variable Object List (on the lower left of EnSight), and select "Create Annotation". This will create an annotation with that variable, and it will automatically change as you change timestep. I think that should give you what you are looking for. If not, please feel free to contact our support line too. (support@ceisoftware.com)
__________________
Kevin Colburn Computational Engineering International, Inc. www.ceisoftware.com kevin@ensight.com |
|
January 9, 2015, 07:28 |
|
#23 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Kevin
But how can I create "constant variable" over those X,Y plot? I have attached an images file, there you can see many no. of plots are available. Suppose I want to create a "constant variable" over "Ymax boundary fluid 1 volume flow rate" how can I do that? Right now I can create a "constant variable" over either vector or scalar variables Thanks In advance.... |
|
January 9, 2015, 10:48 |
|
#24 |
Senior Member
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17 |
I thought that you were trying to create an annotation for a constant which you had created. It sounds like you are trying to create an annotation for a query which has been read in directly from the solver (FLOW3D), where there is not already a constant.
In this case, you can turn on the "Display Value" option within the Plotter. This will display the current value as an annotation on the plotter. To do this, create your plotter. In the Edit options of "Marker" for the plotter attributes, there is an option called "Display Value".
__________________
Kevin Colburn Computational Engineering International, Inc. www.ceisoftware.com kevin@ensight.com |
|
January 12, 2015, 03:13 |
|
#25 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Kevin,
Thank you for your help.... The option you have suggested that works very well. But actually I was looking for an option which will help me to convert those plotters/queries into a " constant variables" . I need those parameter values for further post processing like summation, average etc. While doing animation also. So is it possible to convert those plotters/queries into a " constant variables" ? Thanks In advance.... |
|
January 12, 2015, 10:48 |
|
#26 |
Senior Member
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17 |
Unfortunately, we get those straight in from the flsgrf file, and pipe them directly into the query. There isn't a mechanism to take a query and then back out an constant from it. Sorry, unable to get you back into a constant with that data.
-kevin
__________________
Kevin Colburn Computational Engineering International, Inc. www.ceisoftware.com kevin@ensight.com |
|
January 13, 2015, 00:31 |
|
#27 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Thank you for help Kevin......
|
|
May 18, 2015, 10:43 |
|
#28 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Kevin
It's been very long time to see you. I have done DPM particle tracking in FLOW3D tool. I have Import Flow3D results file including particle data. Now I am looking for cells x y z (centroid) data where particles are present I have attached a image file. The particles are in RED color which are present in different x y z co-ordinates not at cell centroid so I am looking cell centroid w.r.t particles ID Is it possible to get data? Thanks in advanced |
|
May 18, 2015, 13:23 |
|
#29 |
Senior Member
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17 |
k1k:
Are you looking to determine which element the particle is currently inside of? Are you trying to map the particleID from the discrete phase over to the continuum domain volume element? Not sure which direction you are heading, or what end-situation you are trying to get to. There might be methods there, depending upon what you are ultimately trying to do. -kevin kevin@ensight.com
__________________
Kevin Colburn Computational Engineering International, Inc. www.ceisoftware.com kevin@ensight.com |
|
May 19, 2015, 02:36 |
|
#30 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Kevin
Thanks for your response Yes, I am looking for those elements where particles are present w.r.t. time. Actually I am interested in the strain rate(Fluid) which is experienced by particles. I have a strain rate excel sheet data(x y z strain rate) and I have a particle excel sheet data ( ParticleID x y z etc.). Now I wanna check the strain rate value of that cell ID & Particle ID, I am doing so by matching both data 's X Y Z coordinate, but the problem is particle x y z are different form strain rate x y z like I have mentioned in attached Image So I am trying to get Particle ID & their cell ID through Ensight which will help me to get particle ID & strain rate value So is it possible to get this data from ensight ? Thanks in Advanced Last edited by k1k; May 20, 2015 at 01:46. |
|
July 9, 2015, 09:49 |
|
#31 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Kevin
I need your help.... I have done a particle tracking periodic simulation in FLOW3D. Now I am using ensight to get particle information (Particle cell Id, x,y,z , strain rate & residence time) through ensight python script. Can you tell me which Ensight module help me to get particle information data? Thanks in advanced |
|
July 9, 2015, 17:31 |
|
#32 |
Member
Marina Galvagni
Join Date: Apr 2014
Location: North Carolina, USA
Posts: 58
Rep Power: 11 |
Hi k1k,
The particles that are exported from Flow3d do not have any ID. Unfortunately, this means that you can't follow their path in time (as you can't know which particle corresponds to which one at different timesteps), and this makes it difficult to do any kind of analysis on them directly in EnSight. You'd have to submit to FlowScience a request for them to export particles with IDs, in order to have a direct way to analyze them in EnSight. As this isn't possible at the moment, you'll need to create a particle trace part in EnSight that follows closely the particles from Flow3D and analyze these traces. The way to do this is the following: go to timestep 0. Select all your fluid domain, and create a pathline with emitter = part corresponding to the particle part in the dataset. You'll see the particle traces start from the particles. You can now extract your information from the pathline part directly - give a look at this FAQ for more details on how to do that: https://support.ceisoftware.com/hc/e...cle-Trace-Data Please note that a particle trace in EnSight is calculated assuming decoupled, massless particles. This means that you could have traces that are different from the path of the particle solved directly into Flow3D - how different, depends on the settings in Flow3D and the nature of the problem. You should look at the evolution of the particles and the shape of the pathlines in EnSight to evaluate if the integration that EnSight does is (or not) a good approximation for your particular problem. Please let us know if you have any question or problem. Best Regards, Marina Galvagni CEI Software Support Engineer |
|
July 10, 2015, 01:49 |
|
#33 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Marina
Thank you for your suggestion...... I will work on your suggestion and I will let you know if there is any issue Thank you |
|
August 26, 2015, 08:59 |
|
#34 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Marina,
I have done particle trace in Ensight. I have attached an image file there You can see that I have released few particles from injection point but It did not reach to the outlet. I have shown pathlines in image file I have transient solution form 0 to 5 sec. I have released particles from 2 sec. But not a single particle escape from outlet between 2 sec to 5 sec. I have checked available options (Min step , max time) but did not work out. How I am suppose to resolve this issue? Thanks In advance Kedar |
|
August 26, 2015, 10:21 |
|
#35 |
Member
Marina Galvagni
Join Date: Apr 2014
Location: North Carolina, USA
Posts: 58
Rep Power: 11 |
Hi,
Give a look at this FAQ on our website: https://support.ceisoftware.com/hc/e...ng-prematurely It explains the conditions in which a particle trace stops, and explains how to make it longer - when it makes sense to do so physically. In addition to the link, color the pathlines by Time and then set the Time palette limits to (0;5). This will show you at which time each segment of the particle trace is. It may be that the traces all end because they have reached the end of the simulation time. In this case, EnSight can not calculate their path any further as it doesn't have the information about the velocity field at the following timesteps. Indeed, in order to calculate a pathline, EnSight does a time integration of the velocity field - but if you have reached the end of the simulation time, there is no velocity field any more to integrate, and therefore the path stops. I hope this helps. Let me know if you have more questions. Best Regards, Marina |
|
August 26, 2015, 11:04 |
|
#36 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Marina
Thank you for your quick response I have calculate each particle residence time. The max residence time is 1.033 sec so it means that within 1.05 (From 2sec to 3.033sec) sec all particles just disappear without reaching outlet. So I do not think so there is any velocity field issue. Kedar |
|
August 27, 2015, 02:08 |
|
#37 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Marina,
Thank you for valuable suggestion. It help me to resolve my pathline issue. Kedar |
|
September 1, 2015, 02:21 |
|
#38 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Marina,
I need your help.. When I want to see the latest time results in Ensight, every time I have to reload the Case (projects). To avoid this, I am looking for a case update option. Is there any way in Ensight which will help me to update my latest time results without reloading case? Thanks In advance Kedar |
|
September 8, 2015, 12:17 |
|
#39 |
Member
Marina Galvagni
Join Date: Apr 2014
Location: North Carolina, USA
Posts: 58
Rep Power: 11 |
Hi Kedar,
We call this feature "coprocessing" and it has been introduces in EnSight version 10.1.4(a). So, you'll need to have this version (or a later version) of EnSight to have it working. Also, this feature at the moment is present only for a few file formats, including the .case gold format. Please give a look at the Help -> How To Manual -> Load transient data -> Advanced, and at the User Manual, ch. 9.1 for all the details. Here is how it works. In the .case file, under the TIME section, you'll need to have an extra line "maximum time steps", that tells EnSight what is the maximum number of timestep you expect to have once the entire simulation is over (EnSight uses this information to do the memory allocations). So, if for example you expect that the simulation at the end will have 20 timesteps, insert the new line: maximum time steps: 20 Now, load your partial data as you'd normally do. When new data files become available, go into the Solution Time window and click on the "Update number of timesteps" button. This will load the new timesteps. Let me know if you have more questions. Best Regards, Marina Galvagni |
|
November 25, 2015, 05:14 |
|
#40 |
Member
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14 |
Hi Marina & Kevin
Need your help to sort out following problem Ensight V10.1.4a & 10.1.6b unable to open FLOW3D V11.1 result file (flsgrf). I have been facing following problem while opening Flow3D V11.1 results file (flsgrf) Error code 39 while initializing data file ~/flsgrf.test_bird Error: Error initializing Geometry file Error occurred while reading the fixed data, Low level error code 39 Error: Error initializing Geometry file ~/flsgrf.test_bird Error occurred while opening word addressable data file, Low level error code 40 Can you please help me to sort out this issue? Thanks In advance Kedar |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Bulk averaged values on a surface plane other than the inlet or outlet planes..How?? | nikesh | FloEFD, FloWorks & FloTHERM | 5 | August 19, 2014 02:42 |
Validation of surface roughness model approaching a hydraulically smooth surface | jola | CFX | 1 | October 20, 2010 11:06 |
Bug: Surface Integral->Sum w/cut plane and x-face-area | agodfrey | FLUENT | 0 | June 9, 2009 14:11 |
smooth DTF surface | N.R. | CFX | 0 | July 25, 2007 14:45 |
solid edge problem....can you help? | cindy | Main CFD Forum | 3 | April 5, 2004 14:43 |