[Persil]

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

[Zaktatir]

look in your material properties and specially the definition of heat capacity i would say regarding the failure message

[Persil]

thx for the reply: I will try that tomorrow and give feedback, what happend

[Persil]

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

[flotus1]

Originally Posted by Persil

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.

[Persil]

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...

[flotus1]

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.

[Persil]

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

[flotus1]

So what about the standard initialization?

[Persil]

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]

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

[kuzma169]

Originally Posted by Persil

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!