Hi,

I am trying to model the flow field inside an oven, which consists of several zones kept at different temperatures. Each zone employs an array of nozzles controled by a tangential fan and there are outlets between nozzles. My problem is:

1) Those fans in different zones are working at the same angular speed and their structure is exactly the same. However, the flow temperature is different. Then how to calculate the temperature dependence of flow rates for those nozzles in different zones? Is it safe to assume that the impinging speed of them is kept constant?

2) The inner cavity of the whole oven is integral, how to determine or estimate the pressure difference between those nozzles/outlets at different temperature in different zones.

3) If turbulence has to be considered, which turbulent model is the most realistic for the flow field inside the oven. If standard k-epsilon model is selected, which is the best way to evaluate the kinetic energy and its dissipation rate for those nozzles?

Thank you very much for your attention and you will be greatly appreciated for any suggestion.

Hao

(1). Before someone can answer your questions, you need to try a little bit harder to describe this oven device . (2). Is the oven a closed unit (something like the kitchen oven? (3). Where is the heat source in the oven? Is it electric? or gas heated? (4). Is the fan located inside or outside the oven? Is the fan used to circulate the hot air in the oven, or used to deliver the hot air from the outside? (5). Anyway, You have to simulate the effect of the fan, assuming that the fan is moving at the constant speed, the mass flow rate will be a function of the density (thus the temperature). (6)If you are using a code, then the standard k-epsilon model is all right, and the nozzle exit condition can be releted to the diameter of the nozzle, and the % of the jet velocity to be used for the tke. This has been discussed here many times before. (7). But I still don't have any idea about the shape of your oven.

Hi,

Thank you very much for your response, I am sorry that I have not described my oven clearly and I hope that the following description is helpful.

The oven is a reflow oven for electronics production. It is several meters long and closed except two ends of the oven. Electronics production is moved from one end to the other at certain speed by a conveyor, so that it is heated up and cooled sequentially. Hence, the oven is divided into several zones at differents so as to obtain well-defined heating/cooling profile for the electronics production.

In each zone, there are an array of nozzles on the top of the oven, hot gas (its temperature differs for different zone, of course) is impinged from them. The hot gas heats/cools the electronics production, and is drawn out from the oven from outlets between nozzles by a tangential fan. Then the fan send the gas back to the nozzles after its temperature is regulated by heating element or cooling device.

Hence, actually the fan works as a recirculation device and it is located outside the oven. I am now using CFDRC program to model the flow field inside the oven and trying to remove the fan-modeling by defining suitable boundary conditions for those nozzles and outlets seperately. I feel it a hard job for me and your suggestion will be appreciated.

As to the turbulence model, I am not sure how much the value for % of the jet velocity is realistic. I am now using 2%, how do you think about it?

Thank you very much and hope to get your reply soon.

With respects, Hao

(1). Well, it is not a difficult problem. (2). But you have multiple inlets and outlets. Assuming this is not a problem, then all you need to do is to specify the inlet jet conditions. (3). Since the outside return loop contain a fan, heating or cooling devices, it is not easy to determine the exaxt mass flow rate through the external duct. (4). It is probably not easy to simulate the external return loop because of the fan and other added objects in it. So, you will have to do some simple measurement. This is essential. (5). Or you can just vary the condition of each jet and do some parametric study. (6). The inlet jet condition for k and epsilon can be done in the same way. If you have a fan and other devices in the duct, and if the duct is relatively short, then the turbulence level at the jet exit will be high. So, you can try to simulate the real condition by increasing the turbulence kinetic energy level , say from 3% to 5% to 10%. (7). Still, it is a good idea to do some measurement, if possible.

Hi,

Thank you very much for your suggestion. I understand that measurement is necessary and also have tried to do some. However, the structure of the oven makes it very difficult. The only data I obtained is the mass flow rate of nozzles when the fan is working at room temperature, it was done while the heating is shut off. Such measurement at higher temperature seems to be impossible, so I am wondering whether there is any realistic way to estimate the mass flow rate at high temperature.

Another difficulty is that I have multiple outlets and inlets in each zone, as you mentioned. For a recirculation of gas, the total mass flow rate for nozzles and outlets should be equal but this restriction can not be defined in CFDRC program. If there is only one zone in the oven, surely it won't be a problem because the mass conservation can assure it. However, there are several zones and it is difficult to keep mass balance in each zone seperately. I am thinking whether I can define reasonable pressure different between those outlets in different zone. If you have any idea, I will greatly appreciate it.

Thank you very much for your patience.

Hao

(1). The exhaust air is the mixture of the hot and the cold air. It is part of the flow field solution. (2). Then the jet inlet flow is not fixed at all. Its condition is a function of the exhaust flow entering the external return duct. (3). So, the inlet condition is also unknown. (4). I am not sure that there is a steady state solution. This is because, if you turn on the heater only, the whole system temperature will increase. (5). With the heater and the cooler turned on at the same time, it is possible that there will be a steady state solution. But that depends on the mixing of the hot and the cold flow in the oven. (6). It is a complex control problem. Well, if it is possible to control the inlet jet temperature, then at least the oven temperature field will reach the steady state. (7). The basic problem is that the flow rate for each nozzle is not fixed. So, if you can control the mass flow rate and the jet temperature, then, there is hope to get it solved. (8). Otherwise, you need another global loop to update the inlet jet condition based on the exhaust flow. I mean, assume a inlet jet condition (for each nozzle), then run the flow field to converged state. Once you have the exhaust flow field, you can compute the exhaust mass flow rate for each exhaust. This will become the mass flow rate of the inlet jet. For the jet temperature, you need to specify it based on the heating or cooling. Then start another round of global iteration loop. (9). It is important to do it this way, because the hot jet flow can get hotter, if the returned exhaust air is hot air. On the other hand, the cooling jet can also get cooler for the same reason. This is basically a control problem.

The jet temperature is well-controled in the oven and I think I can keep it constant for each zone. So the flow rate is the major problem. I can understand what you mean about the iteration procedure, probably it is a good suggestion for me, but I still have a doubt on how to define the outlet condition:

We don't know the exact pressure of outlets, as well as it's differences between zones. But the exhaust flow field depends on this value. I mean that, if the pressure of outlet in one zone is becoming much lower than that of outlet in other zones, the outward mass flow in this zone increases while that of other zones decreases. Thus the calculated results becomes quit artificial and depends on how we define the outlet conditions. How could we know that the outlet condition has been set correctly?

You mentioned: "if you can control the mass flow rate and the jet temperature, then, there is hope to get it solved". Could you please explain more about this? Again, I am not clear about how to define the outlet pressure (or other ways defining outlet conditions) for each zone.

Thank you very much, With respects, Hao

(1). The exhaust pressure can be measured inside each exhaust duct. In other words, you can set the exhaust pressure there to get your calculation started. (2). I don't know how your code handle the boundary conditions. But if you need the pressure, just set a pressure. I have no idea whether the code will allow you to set multiple exit conditions. (3). So, the idea is to set the inlet and the exit conditions, and allow the flow field to converge first. Then update your inlet mass flow or conditions. (4). You can update your exhaust pressure based on the external return loop. That is the performance of the fan system will determine the pressure difference before and after the fan. (5). You also need to talk to the support engineer of the code to find out what boundary conditions are allowed in your problem. (6). So, it is a guessing game, you start with a set of conditions to allow you to get the converged solution, then update these conditions to satisfy the external loop conservation law. (the internal loop is solved by the code) And if you have several inlets and outlets, you need to come up with a scheme so that a converged system solution can be obtained.

Normally in CFD-ACE, the exit condition is a fixed pressure condition. This can be independently set for each exit. The inlet condition is a fixed mass flow rate condition which can again be set independently for each inlet. The condition is specified by setting the inlet velocities and the temperature and pressure (T and P are used to set a rho).

It seems that John has a pretty good explanation of what you need to do. Basically, let CFD-ACE calculate the internal domain, and you provide some sort of model for the external plumbing between the outlets and the inlets. You have stated that you have a pretty good idea of the inlet temperature, but don't know the exact mass flow rate which is a function of pressure, temperature and fan performance.

So to close this problem, you need: 1) Fan performance curves that give you the mass flow rate for a given pressure/temperature. 2) Delta pressure through the piping - dpp (including heaters and coolers that connect the outlets to the inlets). 3) Delta pressure through the fan - dpf - should also come from the fan curves.

You could then implement a user boundary condition for ACE where you set the inlet conditions as follows: 1) Inlet T = constant - you know this. 2) Inlet P = OutletP+dpp+dpf 3) Inlet vel = f(mdot_fan_curves,inletT,inletP,inletArea)

Start with an initial guess for all the inlets and the pressures at the outlets, run until the flowfield sets up nicely and mass is reasonably well conserved (i.e. PP equation converged). If the model for the external loop is not satisfied (i.e. calculated inletP not equal to assumed inletP), modify the exit pressure and repeat. This may sound odd to you since you set the inlet pressure, but keep in mind that we are talking about a mass flow rate inlet condition. The pressure you input is used to calculate a density which is held constant during the calculation. The calculated pressure in the cells adjacent to the inlet can (and does) vary from the pressure input.

Since you have multiple inlets/exits this is a multi-point control problem, so you will need a controller so that the entire system converges.

This sounds like a really neat problem. You can contact your CFDRC rep to help you with this, or if you still aren't sure you can handle this on your own, CFDRC offers consulting services. Please contact me directly for details.