[Xansys] [WB][CFX]Fluid-Thermal analysis steps need verif

[shailendra.singh]

Dear Li,

The energy equation generally have lower rate of convergence than mass & momentum equation.You should use a time step 100-1000 times the mass equation`s timestep for getting a converged solution for H-energy.
The result could be totally wrong for your 10% criteria.

generally go for a convergence criteria of 10e-5, for a converged solution for all equation, You will find that even after 10e-4 residuals and .x % energy imbalance, the solution changes for 10e-5(generally acceptable for double precision and high resolution marching scheme) or lower values.So better check the flow field after 10e-4 and -5 iterations rather than depending on energy imbalance criteria.

In CFX the energy equation is solved for the solid domain and the result mapped(Grid Grid interface) to fluid domain as source term for energy equation.So you dont need to worry about computing convection film coefficient if the solid domain is included in the CFX.Use a coarser mesh for solid and the mesh shouldnt be continuous with the fluid domain and then generate an interface :)
Maybe you can go through the Conjugate heat transfer tutorial in CFX help file.

happy computing in CFX :)

Shailendra Singh
Basic Research

Areva Energietechnik GmbH
Sachsenwerk Medium Voltage
Rathenaustrasse 2
D - 93055 Regensburg
Phone: + 49 941 4620 483
Fax: + 49 941 4620 438
e-mail: --email address suppressed--

Dear Shailendra Singh,

Thank you so much for your reply and comments.

With regards to the issue of energy imbalances, it has always occurred to me on this particular analysis that the RMS residuals for P-Mass,U-Mom,V-Mom, W-Mom,E-Diss.K,K-TurbKE, and T-Energy easily reaches less than 1e-4, but the RMS residual for H-Energy is difficult.

The Domain Imbalances of U-Mom,V-Mom,W-Mom,P-Mass and T-Energy easily reaches less than 0.1%, but Domain Imbalance of H-Energy never gets lower than 1%, or even very difficult, requiring many more number of runs to accomplish that.

Currently, I'm accepting results when imbalance of H-Energy is <10%, AND when all other imbalances are <1%. What is your comment on my results acceptance criteria here please?

Furthermore, you also mentioned that 'You dont need to go to Ansys for conjugate heat transfer from CFX.'... how else could i model the fluid-thermal coupling please? The cooling channel in the machine housing is complex where using a closed-form equation to compute convection film coefficient won't be realistic.

Thank you for your kind attention, and i really look forward to hear of your comments again.

Kind regards,
Li ZHANG
Beijing Jiaotong University

Post generated using Mail2Forum (http://www.mail2forum.com)

[zhang.li]

Dear Shailendra,

Thanks a lot for your reply. Sorry for my late response here.

i have a few enquiries if i may, and hope you can help me out again.

1) in the Conjugate heat transfer tutorial in CFX, it doesn't mention about using GGI anywhere...... is there another tutorial you can refer me to please?

2) is there a particular feature i should select/deselect in CFX-mesh to impose that the mesh of solid and fluid will not be continuous please?

3) what did you mean by 'better check the flow field after 10e-4 and -5 iterations ' please?

Thank you for your kind attention, and i look forward to hear from you again.

Kind regards,
Li ZHANG
Beijing Jiaotong University

[shailendra.singh]

You can proceed this way

1 & 2)Inside the workbench (design modeler), select all the solids(not liquid) and right click 'make new part'.

when you import this in cfx mesh,this will force the mesher to create discontinuous mesh.

If there is discontinuous mesh, than you can create "interface" between the two domains

3)The flow field is evolving , so when you are solving and your residuals (for convergence) reach 1e-4 check the flow field,
restart the solving and check for flow field again when residuals reach 1e-5.....The heat transfer is sensitive to convergence.

happy computing :)

[fern.thomassy]

shailendra.singh,

Please include a complete signature on every post (see the Rules page at www.xansys.org for more information). We recommend that you automate this process by completing the signature in your Forum and email profiles.

--
Martin Liddle, XANSYS moderator, Tynemouth Computer Services, Staveley, Chesterfield, Derbyshire, S43 3TW, UK.
Fern Thomassy, XANSYS moderator, Fallbrook Technologies Inc., Cedar Park, Texas, USA.

> -----Original Message-----
> From: --email address suppressed-- [mailto:--email address suppressed--] On
> Behalf Of shailendra.singh
> Sent: Thursday, November 05, 2009 2:57 AM
> To: --email address suppressed--
> Subject: Re: [Xansys] [WB][CFX]Fluid-Thermal analysis steps need verif
>
> You can proceed this way
>
> 1 & 2)Inside the workbench (design modeler), select all the solids(not
> liquid) and right click 'make new part'.
>
> when you import this in cfx mesh,this will force the mesher to create
> discontinuous mesh.
>
> If there is discontinuous mesh, than you can create "interface" between
> the two domains
>
> 3)The flow field is evolving , so when you are solving and your residuals
> (for convergence) reach 1e-4 check the flow field,
> restart the solving and check for flow field again when residuals reach
> 1e-5.....The heat transfer is sensitive to convergence.
>
> happy computing :)
>
>
>
>
>
>
> +-------------------------------------------------------------+
> | XANSYS web - www.xansys.org/forum |
> | XANSYS blog - xansys.blogspot.com |
> | The Online Community for users of ANSYS, Inc. Software |
> | Hosted by PADT - www.padtinc.com |
> | Send administrative requests to --email address suppressed-- |
> +-------------------------------------------------------------+

Post generated using Mail2Forum (http://www.mail2forum.com)
_________________
Regards . . . Fern Thomassy
www.fallbrooktech.com

[zhang.li]

Hello again Shailendra Singh,

Again, i need some advice on modeling a CHT analysis between fluid and solid.

my model consists of a housing with cooling channels in it, and a cylindrical solid that sits inside the housing inner part as well. This cylindrical solid is the main heat source, and using water to flow in the channels to cool the entire model.

Your previous advice is that mesh the fluid finer than the solids. Do i use coarser meshings for both the housing and cylindrical solid please?

the way i'm applying heat on the cylindrical solid is by defining a subdomain in CFX, and specifying the heat in Watts per unit volume of the cylindrical solid.

I look forward to hear from you again. Thank you for your kind attention.

Regards,
Li ZHANG
Beijing Jiaotong, University

[shailendra.singh]

Dear Li,

1)Yes you can have coarser mesh for both housing and cylindrical part.If your housing is sheet metal,then have one element in thickness
2)In the subdomain, you can also apply "total heat" rather than "heat per volume", in the same drop down menu.

Regards
_________________
Shailendra Singh
Areva T&D,Germany

[zhang.li]

Hi Shailendra,

Thanks so much for your quick reply.

I just like to make an additional comment that, i asked about the coarser mesh approach is because i encountered an error saying:

ERROR #001100279 has occurred in subroutine ErrAction.
Message:
SYMASS_ZIFCS_EL: The solver ran out of temporary space while building a linked list for a domain interface. Try setting the expert parameter "topology estimate factor zif" to a value greater than 1.0. Values higher than 1.2 should not be necessary.

I've set the Temporary Directory in the Edit > Options menu to a disk drive which has 400GB of space......

Is it a space or memory problem please? what can i do? i've set the factor to 1.1 and still this error occurs.

Will using less meshing on the solids help do you think?

Thanks for your kind attention, and i look forward to hear from you again.

Regards,
Li ZHANG
Beijing Jiaotong University

[shailendra.singh]

Hello Li,

It looks like this error message is related to mesh

1)Either the number of elements are large or
2)There is problem with meshing and interconnections. Delete the connections inside CFX

Why dont you start with a simplified model with grid points less than
100 000...You can always later complicate your model :)
_________________
Shailendra Singh
Areva T&D,Germany

[zhang.li]

Hi Shailendra,

thanks for your reply.

i'm trying with a coarse meshing on the solids, and simulation is running now.

Regards,
Li ZHANG
Beijing Jiaotong University