[k1k]

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..

[sirpinkyo]

https://support.ceisoftware.com/hc/e...ntal-Variables

[k1k]

Thanks you for your quick reply.......

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

[kevincolburn]

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

[k1k]

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.

[kevincolburn]

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

[k1k]

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...

[kevincolburn]

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

[k1k]

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..

[kevincolburn]

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

[k1k]

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?

[kevincolburn]

You can use the SpaMean calculator function for calculate the area average of your inlet.

[k1k]

Thank you very much for help.....

[k1k]

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 .....

[Marina G]

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

[k1k]

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]

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....

[Marina G]

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.

[k1k]

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...

[kevincolburn]

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