CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Visualization & Post-Processing Software > EnSight

Smooth Surface on Clip plane

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 12, 2014, 07:05
Default Smooth Surface on Clip plane
  #1
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Hi,

I am using ensight 10 for post processing. While Ploting variables on clip plane my surface looks distorted . can any one tell me how to avoid this, so i will get better pics?

Thanks in advance..

Last edited by k1k; November 19, 2014 at 05:11.
k1k is offline   Reply With Quote

Old   November 12, 2014, 12:09
Default
  #2
New Member
 
Join Date: Dec 2012
Posts: 5
Rep Power: 13
sirpinkyo is on a distinguished road

https://support.ceisoftware.com/hc/e...ntal-Variables
sirpinkyo is offline   Reply With Quote

Old   November 13, 2014, 05:54
Default
  #3
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Thanks you for your quick reply.......

I have tried your suggested options but still my problem has not solve..

Last edited by k1k; November 19, 2014 at 05:10.
k1k is offline   Reply With Quote

Old   November 13, 2014, 13:40
Default
  #4
Senior Member
 
kevincolburn's Avatar
 
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17
kevincolburn is on a distinguished road
Your image shows that you are still coloring by the "Fluid_Fraction_Restart" variable. You should be coloring by your new variable called "ElemToNode".

Alternatively, if you want to do this just in graphics, Edit -- > Preferences -- >Color Palettes. Toggle ON the "use continuous palette for per-element variables". This is just a graphics smooth, but if all you are looking for is improved "smooth plots", this can be easy/quick (and effects all variable displays at once).

-Kevin
__________________
Kevin Colburn
Computational Engineering International, Inc.
www.ceisoftware.com
kevin@ensight.com
kevincolburn is offline   Reply With Quote

Old   November 14, 2014, 02:32
Default
  #5
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Hi Kevin....Thanks for your reply

I have tried coloring by new variable called 'ElemToNode_re1' and also tried Edit -- > Preferences -- >Color Palettes. Toggle ON the "use continuous palette for per-element variables" options, but still results is same no change.

Last edited by k1k; November 19, 2014 at 05:10.
k1k is offline   Reply With Quote

Old   November 14, 2014, 19:03
Default
  #6
Senior Member
 
kevincolburn's Avatar
 
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17
kevincolburn is on a distinguished road
What solver are you using? Looks like Flow3D based on the variable naming convention?
If your variables were already nodal, then the previous two options are moot, as they only effect element variables. You can see in the Variable Object List panel where the "Location" of the variable are (at the node, or at the element center).
Is your grid coarse, and the gradients high (so that you are the limit of "smoothness" given those two factors?

You might try forwarding this onto the main support line here at CEI, they might have additional assistance or enlightenment to share. (support@ceisoftware.com).

-Kevin
__________________
Kevin Colburn
Computational Engineering International, Inc.
www.ceisoftware.com
kevin@ensight.com
kevincolburn is offline   Reply With Quote

Old   November 18, 2014, 07:17
Default
  #7
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Hi Kevin,

I am using FLOW 3D solver. You can see in images1 my variables reported at element center. So after I have tired your suggested two options the result is still same(In right corner side image variables reported at element center & in left side image at Node)
I have a another query, I want to report a cells volume which occupied by air up to certain height (image 2). Is it possible in Ensight? if Yes, how can I do this?

Thanks In advance...

Last edited by k1k; November 19, 2014 at 05:08.
k1k is offline   Reply With Quote

Old   November 18, 2014, 11:17
Default
  #8
Senior Member
 
kevincolburn's Avatar
 
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17
kevincolburn is on a distinguished road
First. Contact FlowScience regarding your smooth display problem. You may need to ensure that there special switches turned on for your Flow3D work (alternative smoothing routines based on their work for their method of saving results).
Second.
I have a another query, I want to report a cells volume which occupied by air up to certain height (image 2). Is it possible in Ensight? if Yes, how can I do this?
Yes. Use the "IsoVolume" technique (it is a type of isosurface). You can specify the min and max value of the variable. That will create a new Part. You can then use the "Vol()" Calculator function to calculate the volume of that IsoVolume Part.

Please feel free to use the regular support mechanisms (your local EnSight agent, or support@ensight.com).
-Kevin
__________________
Kevin Colburn
Computational Engineering International, Inc.
www.ceisoftware.com
kevin@ensight.com
kevincolburn is offline   Reply With Quote

Old   November 19, 2014, 06:25
Default
  #9
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Hi Kevin ..Thanks you for help..

I have tried Iso volume option but I did not get exact Iso volume which I was expecting. When I am trying to do Iso volume from particular Block it's show or report us total volume which is the solid volume+flow volume (image3). So I just want to know a flow domain volume for different height.
So my question is how to separate this solid volume from flow domain ?

If it is not possible, then how can I measure flow domain volume for different height?

Thanks in advance..
Attached Images
File Type: jpg image3.jpg (21.0 KB, 38 views)

Last edited by k1k; November 19, 2014 at 09:52.
k1k is offline   Reply With Quote

Old   November 19, 2014, 12:41
Default
  #10
Senior Member
 
kevincolburn's Avatar
 
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17
kevincolburn is on a distinguished road
You may first need to create an isovolume of Cell_Volume_Fraction and/or Fluid_Volume_Fraction. But your local Flow3D support person should be able to assist you more directly as well. Are you using FlowSight?

-kevin
__________________
Kevin Colburn
Computational Engineering International, Inc.
www.ceisoftware.com
kevin@ensight.com
kevincolburn is offline   Reply With Quote

Old   December 12, 2014, 07:27
Default
  #11
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
hi Kevin

I am using FLOW-3D solver for multiphase. Initially I am using Volumetric flow rate BC for inlet. Now I want to know the pressure value at Inlet. So I was looking for Area Weighted Average (pressure) at inlet, but I didn't get this option.

Can you tell me how to get Area Weighted Average (pressure) at inlet?
k1k is offline   Reply With Quote

Old   December 12, 2014, 08:22
Default SpaMean calculator function
  #12
Senior Member
 
kevincolburn's Avatar
 
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17
kevincolburn is on a distinguished road
You can use the SpaMean calculator function for calculate the area average of your inlet.
__________________
Kevin Colburn
Computational Engineering International, Inc.
www.ceisoftware.com
kevin@ensight.com
kevincolburn is offline   Reply With Quote

Old   December 12, 2014, 09:17
Default
  #13
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Thank you very much for help.....
k1k is offline   Reply With Quote

Old   December 12, 2014, 09:40
Default
  #14
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Hi Kevin ,

I just want to confirm that the given SpMean is correct or not

So I want create an expression for area weighted average (pressure)

A(p)= Sum(Ai*Pi) / A

Ai: element area
Pi : element pressure

A: total area of Inlet


How do I create this sum (Ai * Pi) ?

Thanks In Advance .....
k1k is offline   Reply With Quote

Old   December 12, 2014, 16:33
Default
  #15
Member
 
Marina G's Avatar
 
Marina Galvagni
Join Date: Apr 2014
Location: North Carolina, USA
Posts: 58
Rep Power: 11
Marina G is on a distinguished road
The SpaMean function will return what you defined as A(p):

Sum(Ai*Pi) / A

So, one way to get Sum(Ai*Pi) is to multiply SpaMean by A. You can get A with the function Area().

An other way to get Sum(Ai*Pi) is the following. First, define a variable that is the area of the single elements, using the EleSize function. Then, define the new variable (second tab of the calculator):
New_var = EleSize * P
Finally, take the sum over the elements of New_var with the function StatMom -> sum

Marina

__________________
Marina Galvagni
Computational Engineering International, Inc.
www.ceisoftware.com
support@ensight.com
Marina G is offline   Reply With Quote

Old   December 13, 2014, 03:10
Default
  #16
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Hi Marina,

Thank you very much for help....

I will try what you have suggested & I let you know it's working or not

Thanks once again.....
k1k is offline   Reply With Quote

Old   December 13, 2014, 08:24
Default
  #17
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Hi Kevin & Marina,

I have tried your both options for area weighted average (pressure) calculation 1)SpaMean & 2) through expression , which are closely matched.

But...

The ensight results & Flow-3d results are not matched. (Image1 & 2)

As you can see that in image1 which is a Flow-3D post-processing image. It's shows the Pressure value only on open volume cells (Flow region) & there is no pressure value on Solid volume cells. Now I want to calculate the area weighted average (pressure) of only open volume cells.

In image2 which is a ensight post-processing image. It's gives me the pressure value on both Open & Solid volume cells which I don't want.

So Can you tell me, how can I get a pressure value or other results only on open volume(fluid region)

Thanks In advance....
Attached Images
File Type: jpg flow3d1.jpg (28.3 KB, 23 views)
File Type: png ensight2.png (43.7 KB, 20 views)
k1k is offline   Reply With Quote

Old   December 15, 2014, 11:01
Default
  #18
Member
 
Marina G's Avatar
 
Marina Galvagni
Join Date: Apr 2014
Location: North Carolina, USA
Posts: 58
Rep Power: 11
Marina G is on a distinguished road
You will need to first create a part that includes only the open volume cells, and then do the calculation on this part. In this way, only the open volume elements will be taken into account in the calculation.

To create this new part: select the model part, and then create an isovolume - probably you want to create an isovolume of Cell_Volume_Fraction and/or Fluid_Volume_Fraction.
Marina G is offline   Reply With Quote

Old   January 2, 2015, 08:21
Default
  #19
k1k
Member
 
kedar
Join Date: Sep 2011
Posts: 33
Rep Power: 14
k1k is on a distinguished road
Hi Kevin & Marina,

(Happy New Year...2015)

I am doing Two phase (water+air) simulation in FLOW3D. I want to measure how much volume of water is added after certain time (Image 2). So I am using following expression over clip ( Image 3)

Volume of water : sum{delta(Time)*volumetric flow rate}

I have given a try but did not succeed.
Can you tell me how to create "delta(time)" or full expression?

If you have another method which will help me to measure volume of water that also you can suggest me. It will be really helpful


Thanks In advance...
Attached Images
File Type: jpg volumerate.jpg (14.9 KB, 9 views)
k1k is offline   Reply With Quote

Old   January 2, 2015, 10:56
Default
  #20
Senior Member
 
kevincolburn's Avatar
 
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 17
kevincolburn is on a distinguished road
You can get the current timestep's time, and the next timestep's time via EnSight Calls (Interface Manual, Chapter 6). From that, you can determine your delta T.

Alternatively, if you have a volumetric flow rate calculated for a particular timestep, then this is perhaps a method for you:
a. Create a query of that constant.
b. Use the Query Integrate operation to integrate the query over time). (it is a "operation on query" from the pull down menu.

-kevin
__________________
Kevin Colburn
Computational Engineering International, Inc.
www.ceisoftware.com
kevin@ensight.com
kevincolburn 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
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


All times are GMT -4. The time now is 03:07.