Hi,all.I got two fatal error in solve,could someone who meet the same errors do me a favor? Thanks Notice Wall Heat Transfer Coefficient written to the results file uses "Wall Adjacent Temperature" for the bulk temperature. If you want to override the bulk temperature then set the expert parameter "tbulk for heat tran coef =' <value>"

ERROR #002100004 has occurred in subroutine Out_Scales_Flu. Message: The Reynolds number is outside of the range expected based on the Option selected for the TURBULENCE MODEL. Check this setting, the values of the properties, mesh scale, consistency of units and solution values in the input file. Execution willproceed.

Hi,

Both are warnings only, not errors. The first says that the heat transfer coefficients in the simulation are based on a local "wall adjacent temperature" rather than a specific temeprature. For some applications it is more meaningful to calculate heat transfer coefficients based on a fixed number and the warning describes how to do this.

The second warning just indicates you are using laminar flow when it is guessing the flow is turbulent. CFX estimates this by global estimates of length, fluid properties and fluid velocity and is therefore sometimes not physically valid. You should have a look at the flow yourself and decide whether it is laminar or turbulent and choose a model to suit.

Glenn Horrocks

Hi,Glenn Horrocks Thanks for your help.In my settings,I set Heat Transfer as heat Transfer Coefficient,700[W m^-2 K^-1],outside temperature as 300[K],The first warning exist all the same . the expert parameter "tbulk for heat tran coef = <value>" means what?

The turbulence model I select is K-epsilon rather laminar,but it doesn't work either.Maybe I shohld try others turbulence model? James

Hi,

Heat transfer coefficient: q=h(t-tbulk) - therefore the vaule of h depends on the tbulk you base it on. By default CFX calculates tbulk from local conditions and so it varies across the field but most h cofficients found in the literature are based on free stream temperature or some other known temperature. This option allows to choose between these options.

Turbulence warning: Or is your simulation laminar and you are using a turbulence model? In that case consider using laminar flow. If you are confident you are OK here then ignore the message.

Glenn Horrocks

Hi,Glenn Horrocks .thank you for your suggestion. About the second error,I changed the multiple model from the Homogeneous model to Inhomogeneous model,and set the turbulet model as Homogeneous ,then the error disappeared.Maybe it is not a good way to solve the problem. By the way,as two phase ,free surface model,such as water fill into a tank with air,which model I should select,Homogeneous model or Inhomogeneous model? James

Hi James,

It is not necessarily a "problem" so that is why you can ignore it if appropriate. Regarding homogenous and inhomogenous models, this is described in the documentation. Generally for free surface models where the water and air stay well defined (that is no bubbly bits) the homogenous model is adequate and considerably simpler. Have a look at the documentation for why this is so.

Glenn Horrocks