[tomide]

----------------------------------
Error in subroutine FNDVAR :
Error finding variable DENSAT_FL1
GETVAR originally called by subroutine cal_DIAM

+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

Details of error:-
----------------
Error detected by routine MAKDIR
CDRNAM = cal_IPTC
CRESLT = OLD

Current Directory : /FLOW/SOLUTION/TSTEP5/CLOOP1/ZN1/VERTICES

[Mudassir]

Hi,
I am getting the same error, have you found any solution to this?

Regards

[ghorrocks]

CFX error messages can be a bit cryptic. I think this one is saying you have not defined the saturation properties (maybe density) for a phase.

[Mudassir]

Dear Gorrocks,
Thanks for the reply,
I am using predefined materials, "Liquid Water" and "Water Ideal Gas", density of Water in gas phase cannot be defined manually, as it is compressible and density is computed by CFX according to temp. press. conditions.
I donot see other place where the density should be defined.
I am using "Water Ideal Gas" as continuous fluid, and Water Liquid as Droplets(Phase change) , if i change Dispersed Liquid , the problem goes away.
But i need Phase change here!


Regards

[JuPa]

Originally Posted by Mudassir

Dear Gorrocks,
Thanks for the reply,
I am using predefined materials, "Liquid Water" and "Water Ideal Gas", density of Water in gas phase cannot be defined manually, as it is compressible and density is computed by CFX according to temp. press. conditions.
I donot see other place where the density should be defined.
I am using "Water Ideal Gas" as continuous fluid, and Water Liquid as Droplets(Phase change) , if i change Dispersed Liquid , the problem goes away.
But i need Phase change here!


Regards

Are you sure you want to use the droplet model? Dispersed liquid phase is fine as long as you know what it means.

Phase change simulations are not easy. There is a ton of literature to read before you even think about attempting a "simple" phase change simulation.

The best advice is: read the CFX theory and user guides.

And then read them again.

Complete the Bartolomej boiling test case in CFX to get you started. You can get the files from Ansys.

[tomide]

Originally Posted by Mudassir

Dear Gorrocks,
Thanks for the reply,
I am using predefined materials, "Liquid Water" and "Water Ideal Gas", density of Water in gas phase cannot be defined manually, as it is compressible and density is computed by CFX according to temp. press. conditions.
I donot see other place where the density should be defined.
I am using "Water Ideal Gas" as continuous fluid, and Water Liquid as Droplets(Phase change) , if i change Dispersed Liquid , the problem goes away.
But i need Phase change here!


Regards

i didnt find any solution to the error. i decided to change my area of study. if you find a solution please share it with me. thanks

[Mudassir]

@ tomide,
Dear i think you are not using proper materials for Phase Change, i have switched to H20v,H20l and i have resolved that error (That error DENSAT... means that Saturation Density not found), You need to use a pair of materials which have well defined saturation properties in CFX.
And... This is my interpretation.

[aer]

Originally Posted by Mudassir

@ tomide,
Dear i think you are not using proper materials for Phase Change, i have switched to H20v,H20l and i have resolved that error (That error DENSAT... means that Saturation Density not found), You need to use a pair of materials which have well defined saturation properties in CFX.
And... This is my interpretation.

Dear Mudassir
I have a problem with phase change (droplet), I find H2Ol in CFX material, but cannot find H2Ov! Can I ask you where you find it?
I built this material from new material, but the error that ‘Error finding variable PSAT’ is appeared!
Could you help me please?
Regards

[Mudassir]

Originally Posted by aer

Dear Mudassir
I have a problem with phase change (droplet), I find H2Ol in CFX material, but cannot find H2Ov! Can I ask you where you find it?
I built this material from new material, but the error that ‘Error finding variable PSAT’ is appeared!
Could you help me please?
Regards

Hi Julia,

That is a mistake in my above comment, Sorry for the confusion it created. The Liquid and Gas phase water materials are H2Ol and H20 (Not H2Ov) respectively, and their Homogeneous Binary Mixture is named as H20vl.
You can find these materials in "Water Data" or "Interphase mass transfer" groups.
Please note that, you would have to import all three to your materials list; H2Ol, H2O , H2Ovl.
That error about PSAT means that Saturation Pressure was not found. Importing all the three materials would correct this Inshallah !
Personally i am now using IAPWS-IF97 water and steam data for my simulations , i found it better and it is also available within CFX.

Hope that helps!

Regards,
Mudassir Farooq

[aer]

Dear Mudassir
Thanks for your help, I used materials in IAPWS-IF97 , but this error appear: ‘Independent variables were clipped during table generation’
I don’t understand this message, which item I must change it?
Thanks a lot for your help

[ghorrocks]

In the materials tab you expand out a few levels and there is some options for table generation.

[Mudassir]

Originally Posted by aer

Dear Mudassir
Thanks for your help, I used materials in IAPWS-IF97 , but this error appear: ‘Independent variables were clipped during table generation’
I don’t understand this message, which item I must change it?
Thanks a lot for your help

Hi Julia,

First i would like to explain what does this error mean so that you can have a deeper understanding. When you start a simulation the CFX-Solver generates the tables of the properties (density, viscosity etc) for different temperature and pressure values, Then during the simulation solver will pick the property value from these tables. This process of making tables is called "TABLE GENERATION". CFX by default generates these table from 273K - 500 K (i dont remember exactly values) in steps of 5 degrees or similar. Now your error means that the temperatures and pressure values in your simulation are outside the default table range.
It is always recommended to to provide Table range manually according to the temperature and pressure EXTREMES in the simulation to avoid this error.
Now to input table range:
Double click the your material in Outline -> Tick TABLE GENERATION under Material Properties tab -> Tick Minimum Temp., Max. Temp , Min Pressure, Max Press and Number of points and provide values for all of these.
-- Do Not Check mark the Extrapolation.

Sorry for being lengthy, too descriptive!

Hope that helps!

Regards,
Mudassir Farooq

[aer]

Originally Posted by Mudassir

Hi Julia,

First i would like to explain what does this error mean so that you can have a deeper understanding. When you start a simulation the CFX-Solver generates the tables of the properties (density, viscosity etc) for different temperature and pressure values, Then during the simulation solver will pick the property value from these tables. This process of making tables is called "TABLE GENERATION". CFX by default generates these table from 273K - 500 K (i dont remember exactly values) in steps of 5 degrees or similar. Now your error means that the temperatures and pressure values in your simulation are outside the default table range.
It is always recommended to to provide Table range manually according to the temperature and pressure EXTREMES in the simulation to avoid this error.
Now to input table range:
Double click the your material in Outline -> Tick TABLE GENERATION under Material Properties tab -> Tick Minimum Temp., Max. Temp , Min Pressure, Max Press and Number of points and provide values for all of these.
-- Do Not Check mark the Extrapolation.

Sorry for being lengthy, too descriptive!

Hope that helps!

Regards,
Mudassir Farooq

Hi Mudassir
My problem is solved and the error is eliminated, thanks for your help
I wish the best for you!
Best Regards

[aer]

Hi Mudassir
Can I ask you a question?
do you simulate wet steam flow in CFX?
if your answer is positive, can I ask you some question?
Thanks
Julia

[Mudassir]

Hi Julia,
Yes I did simulate wet steam, Actually i vaporized water in my system and the steam you get would be wet steam unless you superheat it.
You may ask the questions, May be i could answer.

Mudassir Farooq

[adilsyyed]

Originally Posted by Mudassir

Hi Julia,

That is a mistake in my above comment, Sorry for the confusion it created. The Liquid and Gas phase water materials are H2Ol and H20 (Not H2Ov) respectively, and their Homogeneous Binary Mixture is named as H20vl.
You can find these materials in "Water Data" or "Interphase mass transfer" groups.
Please note that, you would have to import all three to your materials list; H2Ol, H2O , H2Ovl.
That error about PSAT means that Saturation Pressure was not found. Importing all the three materials would correct this Inshallah !
Personally i am now using IAPWS-IF97 water and steam data for my simulations , i found it better and it is also available within CFX.

Hope that helps!

Regards,
Mudassir Farooq

Sorry for bringing up an old post.
In phase change simulation, say direct contact condensation, do we have to import all the three materials i.e. H2O, H2Ol and H2Ov, as you mentioned.
Shouldn't two materials H2O and H2Ol do?
If I import the third material H2Ov then I have to define it as Continuous/dispersed liquid. It kind of becomes a 3rd phase.

Regards

[Opaque]

Be careful not confuse "materials" with "phases" when using ANSYS CFX.

"Materials" describe the thermodynamic state, properties of a substance.

"Phases" are how you want these substances to be modeled.

For example, you can import MatLiquid, MatVapor, MatBinMixture materials. Then you decide how to model the physics:


1 - Single phase using a homogeneous binary mixture: you assign the MatBinMixture to the unique phase in the model.

2 - Single phase using the vapor state: you assing the MatVapor material to the unique phase in the model. Similar if you decide to model the liquid with MatLiquid

3 - Multiphase modeling using independent phases: you assign MatVapor to a phase (and the appropriate morphology), and you assign MatLiquid to another phase (and its morphology as well).

Summary: you can import as many materials as you want, you then create phases as your modeling needs require.

Hope the above helps,

[adilsyyed]

Originally Posted by Opaque

Be careful not confuse "materials" with "phases" when using ANSYS CFX.

"Materials" describe the thermodynamic state, properties of a substance.

"Phases" are how you want these substances to be modeled.

For example, you can import MatLiquid, MatVapor, MatBinMixture materials. Then you decide how to model the physics:


1 - Single phase using a homogeneous binary mixture: you assign the MatBinMixture to the unique phase in the model.

2 - Single phase using the vapor state: you assing the MatVapor material to the unique phase in the model. Similar if you decide to model the liquid with MatLiquid

3 - Multiphase modeling using independent phases: you assign MatVapor to a phase (and the appropriate morphology), and you assign MatLiquid to another phase (and its morphology as well).

Summary: you can import as many materials as you want, you then create phases as your modeling needs require.

Hope the above helps,

Thank you, it does clarify a few things.

[abubakarizhar]

have someone tried the Bartolomej subcooled boiling test provided by ansys. i want to know wether the wall boiling model can be applied at low pressure of 3 bar or not. moreover how has ansys input bubble diameter expression in this case.can someone guide to provide input at 3 bar.

[soumitra2102]

Originally Posted by JuPa

Are you sure you want to use the droplet model? Dispersed liquid phase is fine as long as you know what it means.

Phase change simulations are not easy. There is a ton of literature to read before you even think about attempting a "simple" phase change simulation.

The best advice is: read the CFX theory and user guides.

And then read them again.

Complete the Bartolomej boiling test case in CFX to get you started. You can get the files from Ansys.

You are right JuPa
I am also finding difficulty in the boiling simulations.