Hi, I'm student of Mechanical Engineering at University of Chile and I'm working in secondary hood modeling for Pierce-Smith Converter in a cooper smelter. I made the geometry of the problem but is unclear for me the atributes of boundary conditions. The domain fluid is air using ideal gas law and the transportated scalar is SO2. I know a priori the mass flow of SO2 and its volume fraction at the inlet. Phoenics solve this variable like mass fraction?,Can I set the ambient conditions like Outlets with zero relative pressure?, What is the meaning of deduced, in-cell, and user-set velocities and SO2 (or contaminant or scalar) values at outlets?. The inlet temperature is 1250 °C, but in the processing the temperature don't grow up in the whole domain, why is this?, if I set the source like density diference, and the natural convection is evident (the velocity inlet is very low), why don't the temperature grow up?. Is there a document in internet with complete information about bondary conditions and scalar transport? I hope te answer of iluminated person

Yes, you are right, PHOENICS solves for the mass fraction of chemical species, but the conversion from volume fraction to mass fraction should be a matter of simple algebra if your problem is completely specified at the inlet plane.

If the outlets are at ambient pressure then set P1 (the relative pressure) to zero at these boundaries and the reference pressure (PRESS0) to ambient. If buoyancy is present this is always expedient, ie it is expedient to remove the hydrostatic pressure, and solve for a pressure pertubation about the hydrostatic equilibrium condition.

In the event of inflow at an outflow boundary, then PHOENICS will convect into the solution domain the values specified for the "external" velocities, etc. If there is outflow at a particular cell, then these "external" are irrelevant, because fluid is convected out of the domain using the value prevailing at the cell node next to the boundary. The meanings of deduced, in-cell and user-set for the "external" values are defined in the PHOENICS VR Reference Guide TR/326, which can be downloaded in word or html format at the following url:

http://www.cham.co.uk/phoenics/d_pol...r000/tr000.htm

The two most common choices for defining "external" values are in-cell and user-set, the former means the value prevailing at the cell node next to boundary is convected into the solution domain at the outflow boundary. User-set means that the numerical value entered by the user in the dialogue box will be used as the value convected for that variable across the boundary and into the solution domain.

Your questions about temperature are unclear and moreover, there is insufficient information to comment because only the inlet temperature is defined and there is no description of the other thermal conditions or flow process details. What I can say is that if there is an entrainment (fixed pressure boundary) boundary at ambient temperature, say 25degC, then this value must be specified, rather than the use of in-cell. This will then create a temperature difference to produce buoyancy forces that will drive the flow upwards. In such a scenario, you should set the reference density to correspond to that of the ambient fluid.

Hi mike, thanks for your answer. When I ask for temperature I refer to density set at inlet. At inlet I know temperature(1250 °C) and mass flow of chemical species. I've being setting a velocity about z axis (perperdicular to plane of inlet), that I deduced from mass flow, density of mixture at 1250° and inlet area ratio. Which Is correct density to set? at 1250° or at Tambient? this a mass or volume flow?, and if I set a flow inlet, Can the solver generate a outflow at inlet because mass conservation?. In the other hand, I trying to set a blockaje as inlet, with temperature (1250), a negligible volume (Inlet area*0,001 m3) and a fixed mass fraction of chemical species. In this point I doubt, PHOENICS have an option to set a total o volumetric flux in the blockage!!!, What means this? a flux of mass fraction? Have this a phisical sense? Hoped in your full-PHOENICS-knowledge,

Leonardo

Leonardo, I am sorry to say it does not make much sense to me what you have written. It is largely incomprehensible, and so I think the best thing to do is for you to tell me exactly what you want to specify at the inlet boundary, and I will tell you how to do it. Thus far, I only know the temperature is 1250degC.

What is the real inlet area and shape, circular or rectangular? What is the composition of the incoming fluid (air+SO2)? If the ideal gas law is required for the density calculation, what is the operating pressure? Presumably, it is ambient pressure.

Regardless of PHOENICS, I don't really understand your proposed solution domain and boundary conditions. Are there other inlets to the solution domain, and where are they? How many outlets are there from the solution domain, and where are they? Are there any entrainment boundaries (outlets) where fluid may be drawn into or out of the solution domain?

The incoming fluid is air+SO2 and its geometry is rectangular (the surface of smelted metal inside the converter), de temperature of incoming flow is 1250 °C, de volume fraction is 20%(m3SO2/m3air) and the mass of SO2 inflow is 93gr/s. There are 4 opens that present ambient conditions (Tambient, Pambient, 25°C and 0 Pa respectively) and are located at top of domain (ceil,up to primary and secondary hoods, the converter have 2 hoods that absorve the inflow gas, this is the tarjet of study, decide the best geometry of hoods and the power of fan to absorb de contaminant), behind of domain (behind the converter and hoods, front is hood exits). What is de best kind of inlet? a velocity inlet or mass flow inlet?. How do I set the pressure at ambient opens (outlets)?, like diffusive dominant (FIXP, FIXVAL) or like convective dominant (FIXFLU) if I estimate a mass flow?

The first thing you need to do is to solve for C1, which can used to represent the mass fraction of SO2. Use whole-field solution for C1 so as to accelerate convergence of this variable. Since your flow conditions indicate that SO2 cannot be considered as a passive contaminant, you then need to use the "ideal gas, mix gcon" density law, and set R_C1=129.91 J/kgK and R_(1-C1)=287.7 J/kgK. Also under "properties", set the reference pressure should be set to 1.01325e5 Pa and the reference temperature to 273K.

You should use an INLET object for the gas mixture inlet (air+SO2). If the inlet geometry is rectangular and aligned with the cartesian coordinates, then it should not matter whether you use the "velocities" or "volume flow rate" specification. For non-rectangular inlets, use "velocities" because this will produce a more accurate momentum inflow rate on a coarsely-grided inlet geometry. Therefore, use a "volume flow rate" of 0.909 m3/s for your rectangular inlet with a "user-set" inlet density of 0.288 kg/m^2, an inlet temperature of 1250degC, and inlet area ratio of 1.0, and an inlet scalar C1 of 0.355.

At free ambient boundaries use an OUTLET object and fix the pressure to 0.0 Pa with a coefficient of say 1000.0, and an external temperature of 25degC.

From your description, it seems to me that the solution domain must include the hood geometry and a small section of the exhaust ducting that extracts the air-SO2 mixture. At the end of this modelled part of extraction duct you should use an INLET or possibly a USER-DEFINED object (with FIXFLU) so as to extract the gas mixture at an estimated volumetric fan rating. In other words, you specify the volume outflow rate. The NETT SOURCE printout for C1 in the RESULT file of the converged solution will tell you the mass outflow rate of C1 computed by PHOENICS. If the hood capture efficiency is inadequate, you will then need to increase the fan rating, ie the volume outflow rate at the extraction boundary.

Thanks, mike

That density at inlet correspond to 1250 °C true?

yest should be, but you had better check my algebra.

Hi Mike:

Happy Holidays!!

I am trying to reconcile your comments (C1, "volume flow rate," "ideal gas, mix gcon") with the VR-Editor input parameters. Are those directions related to PIL, not the VR-Editor? I see two entries (numbers 30 and 31 in the Menu/Properties/DomainMaterial listbox) which both claim to be the Ideal Gas Law for mixture of 3 Gases, but there don't seem to be other settings, such as in the Inlet/Attributes box.

Are you in fact refering to the 3-gases combustion model?

Hi Patti,

The directions relate to the VR Editor, and they are not concerned with the three-gases combustion model. The case in question concerns a mixture of air and vapour gas from metallurgical ladle.