CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Transient: Domain Timescale Factor

Register Blogs Community New Posts Updated Threads Search

Like Tree1Likes
  • 1 Post By Gert-Jan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 13, 2019, 13:08
Default Transient: Domain Timescale Factor
  #1
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,183
Rep Power: 23
evcelica is on a distinguished road
Greetings all,
I'm doing a cool down simulation where It takes many days to cool down a geometry (295K down to 4K)
The fluids equations must be solved on a small time scale (~0.01s) where the solids can be solved on much higher timescales (100+ seconds). What I have been doing is freezing the fluids equations, then solving the energy equations @ 100+second timesteps. Using constant properties for the cool down gas. Unfortunately It seems the fluid balancing (there are 98 parallel routes) changes during the cooldown once temperatures start getting low.

So what I'm wondering is:
Can I use the domain solver control: Timescale Factor = 10000 for the solid domains during a transient simulation. The option is there, so I will test it to see what happens, and report back. Documentation seems to hint at Yes, but it is a bit unclear. CFX Pre Users Guide Section 13.4.10.1.
Would this be roughly the same as reducing the specific heat of the solid materials by a factor of 10000? Would Specific Heat reduction of the solids be an alternative option if the timescale factor does not work?
Approximate solution is fine, It should be better than my frozen fluid equations solution, which I can use for comparison.
evcelica is offline   Reply With Quote

Old   May 13, 2019, 19:48
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,841
Rep Power: 144
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I think your frozen fluids approach is probably the best one.

You cannot use time scale factors in transient simulations (to my knowledge anyway).
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   May 14, 2019, 00:15
Default
  #3
Senior Member
 
Join Date: Jun 2009
Posts: 1,865
Rep Power: 33
Opaque will become famous soon enough
It is effectively changing the thermal capacitance w/o messing around with the material details.
Opaque is offline   Reply With Quote

Old   May 14, 2019, 04:35
Default
  #4
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,903
Rep Power: 28
Gert-Jan will become famous soon enough
Quote:
Originally Posted by evcelica View Post
Greetings all,
I'm doing a cool down simulation where It takes many days to cool down a geometry (295K down to 4K)
The fluids equations must be solved on a small time scale (~0.01s) where the solids can be solved on much higher timescales (100+ seconds). What I have been doing is freezing the fluids equations, then solving the energy equations @ 100+second timesteps. Using constant properties for the cool down gas. Unfortunately It seems the fluid balancing (there are 98 parallel routes) changes during the cooldown once temperatures start getting low.

Do you do this manually? Or do you make use of Fortran?
Gert-Jan is offline   Reply With Quote

Old   May 14, 2019, 07:38
Default
  #5
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,183
Rep Power: 23
evcelica is on a distinguished road
Thanks for the responses all,

So, reporting back, it does seem to work. Yes, the domain timescale factor works for the transient simulations (It is set in each domain). Results track along with with my frozen fluids approach.
It is much less efficient though, after an overnight run on 5 machines, it is only 1.3 equivalent hours into the 130 hour cool down. So It isn't practical in this case, and frozen fluids seems to be the best. (Quickest anyways.)

I do the frozen fluid equations manually: using the expert parameter: solve fluids = f.
What benefit would Fortran offer? I thought about if it would be possible to change this expert parameter every so often to true, to update the fluid field. I would have to change the time steps as well (much shorter) during this time, then increase again when solving only energy equations. I did this a few times on the fly in solver manager manually during the cooldown. Could that be automated?
evcelica is offline   Reply With Quote

Old   May 15, 2019, 04:02
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,903
Rep Power: 28
Gert-Jan will become famous soon enough
In CFX-10.0 I had a fortran code which did this automatically. That can help you overnight.
The code was able to switch off fluids for a certain timestep so only energy and scalar were solved using a large timestep.
It was a buoyancy driven flow where the coupling was quite strong. So the allowable timestep increase when fluids were skipped was only a factor 3. Otherwise the flow would deviate too much.
Maybe in your case the coupling is less strong allowing a larger time step increase. I can share the old Fortran. Alternatively ask ANSYS for a more recent version.
evcelica likes this.
Gert-Jan is offline   Reply With Quote

Old   May 15, 2019, 09:24
Default
  #7
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,183
Rep Power: 23
evcelica is on a distinguished road
That sounds very interesting. My flow won't deviate too much. I would like to take a look at the fortran. I have never used fortran with CFX, so that will be new to me, but could prove very useful. Thank you, I'll PM my email.
evcelica is offline   Reply With Quote

Reply


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
Can CFX model periodic heat transfer problem Ethan_Sparkle CFX 41 June 14, 2017 08:22
Sudden increase the residual of Maxwell's equations hsezsz CFX 2 October 13, 2016 07:58
Setting rotating frame of referece. RPFigueiredo CFX 3 October 28, 2014 05:59
CFX domain comparison Kiat110616 CFX 4 April 3, 2011 23:43
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05


All times are GMT -4. The time now is 18:46.