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

Hybrid Initialization Error

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

Like Tree1Likes
  • 1 Post By kuzma169

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 5, 2013, 05:13
Default Hybrid Initialization Error
  #1
Member
 
Join Date: Nov 2013
Posts: 43
Rep Power: 12
Persil is on a distinguished road
Hello,

I want to simulate the flow through 2 stages of a gas turbine and therefore built a model like this: mixing plane=mp

vane1 -> mp -> blade1 -> mp -> vane2 -> mp -> blade2

energy equation: on, k-e-model

after setting the boundary conditions, solution methods (SIMPLE, Standard 5x first order) and controls (reduced the under relaxation factors to increase them later on...) I wanted to initialize with hybrid initialization. There I get the error:

Eror: Specific_Heat_by_T_Integral: invalid lower bound, T0 <= 0.
Error Object: #f

I don't know where to look for fixing this error: maybe changing the boundary conditions at the outlet? Thankful for any feedback
Persil is offline   Reply With Quote

Old   December 5, 2013, 11:47
Default
  #2
Senior Member
 
Join Date: Jan 2010
Location: Germany
Posts: 268
Rep Power: 17
Zaktatir is on a distinguished road
look in your material properties and specially the definition of heat capacity i would say regarding the failure message
Zaktatir is offline   Reply With Quote

Old   December 5, 2013, 11:54
Default
  #3
Member
 
Join Date: Nov 2013
Posts: 43
Rep Power: 12
Persil is on a distinguished road
thx for the reply: I will try that tomorrow and give feedback, what happend
Persil is offline   Reply With Quote

Old   December 6, 2013, 05:22
Default
  #4
Member
 
Join Date: Nov 2013
Posts: 43
Rep Power: 12
Persil is on a distinguished road
I took a look at the material settings and changed the given to piecewise-linear with some modifications but that did not solve the problem. The error still occurs...

instead of initializing the 2 stages at once, I will try to initialize the components separetely in another cas-file each... mabye this way I can figure out the right boundray conditions
Persil is offline   Reply With Quote

Old   December 6, 2013, 05:34
Default
  #5
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,406
Rep Power: 47
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
Quote:
Originally Posted by Persil View Post
Eror: Specific_Heat_by_T_Integral: invalid lower bound, T0 <= 0.
Smells like you didnt use SI units (Kelvin temperature scale) to specify a temperature dependency.
Try using constant material properties to see if this is the source of error.
flotus1 is offline   Reply With Quote

Old   December 6, 2013, 06:43
Default
  #6
Member
 
Join Date: Nov 2013
Posts: 43
Rep Power: 12
Persil is on a distinguished road
well I kept the default unit settings, so SI: kelvin for temperature was enabled from the beginning

could I initialize successfully if I adjust the under relaxiation factors? I thought until now, that you would change them between simulations to reach better convergence...
Persil is offline   Reply With Quote

Old   December 6, 2013, 06:59
Default
  #7
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,406
Rep Power: 47
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
The under-relaxation factors have nothing to do with the initialization, so changing these wont help.

I didnt mean that you changed the default setting for the units.
How EXACTLY did you specify the specific heat of the material? And again, try a constant value here to make sure that this causes the error.
flotus1 is offline   Reply With Quote

Old   December 6, 2013, 07:59
Default
  #8
Member
 
Join Date: Nov 2013
Posts: 43
Rep Power: 12
Persil is on a distinguished road
ok, was just making sure

you can see the material settings for the specific heat in the attachment

I also tried initializing with just the specific heat as constant and kept the rest as it was before... but that still generated the error from before
Attached Images
File Type: jpg Specific_Heat.JPG (92.6 KB, 33 views)
Persil is offline   Reply With Quote

Old   December 6, 2013, 08:05
Default
  #9
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,406
Rep Power: 47
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
So what about the standard initialization?
flotus1 is offline   Reply With Quote

Old   December 6, 2013, 08:45
Default
  #10
Member
 
Join Date: Nov 2013
Posts: 43
Rep Power: 12
Persil is on a distinguished road
same error with standard initialization

could you explain me, what this error means? for me it sounds like that due to some wrong boundary conditions or related the temperature falls below 0 K, which is something you don't want to see displayed...
Persil is offline   Reply With Quote

Old   December 6, 2013, 10:51
Default
  #11
Member
 
Join Date: Nov 2013
Posts: 43
Rep Power: 12
Persil is on a distinguished road
I found the problem:

whilst modeling I created periodic boundaries via mesh/modify/mp but did not check the grid afterwards... so I didn't notice that one rotation angle was defined in the wrong direction.

fixing that (grid/repair-improve/repair-periodic) hybrid initialization went smoothly
Persil is offline   Reply With Quote

Old   December 19, 2018, 07:59
Default
  #12
New Member
 
Join Date: Apr 2016
Posts: 14
Rep Power: 10
kuzma169 is on a distinguished road
Quote:
Originally Posted by Persil View Post
Hello,

I want to simulate the flow through 2 stages of a gas turbine and therefore built a model like this: mixing plane=mp

vane1 -> mp -> blade1 -> mp -> vane2 -> mp -> blade2

energy equation: on, k-e-model

after setting the boundary conditions, solution methods (SIMPLE, Standard 5x first order) and controls (reduced the under relaxation factors to increase them later on...) I wanted to initialize with hybrid initialization. There I get the error:

Eror: Specific_Heat_by_T_Integral: invalid lower bound, T0 <= 0.
Error Object: #f

I don't know where to look for fixing this error: maybe changing the boundary conditions at the outlet? Thankful for any feedback
It's result of having warpage element faces. Search for bad elements . You need finding wrong surface orientation, wrapped element face or negative - neglected volume etc. It's my opinion founded to my experiences.

Best regards.

Cheerio!
Dodul likes this.
kuzma169 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
[OpenFOAM] Native ParaView Reader Bugs tj22 ParaView 270 January 4, 2016 11:39
Ansys Fluent 13.0 UDF compilation problem in Window XP (32 bit) Yogini Fluent UDF and Scheme Programming 7 October 3, 2012 07:24
checking the system setup and Qt version vivek070176 OpenFOAM Installation 22 June 1, 2010 12:34
POSDAT problem piotka STAR-CD 4 June 12, 2009 08:43
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 20:50


All times are GMT -4. The time now is 04:22.