Discussion Groups

Simulation CFD

Reply
Distinguished Contributor
jrm_1971
Posts: 112
Registered: ‎03-31-2011

Re: Before you hit 'solve' but within the first thumbnail (co...

11-25-2012 10:42 AM in reply to: wildej

Jon,

 

OK, I am not sure that I have a great solid model for analysis, but it appears to be better. I had an issue with the conduit spiraling around and intersecting itself. Fixed that. Also, the conduit and fluid are now one piece and not cut in halves as shown in the previous diagram. The reason this was done in the past is so the top halves could be hidden and the flow could be visualize all the way through (a disadvantage of using planes is only one section of the spiral can be visualized at a time. Impossible to visualize for a 3D spiral with just planes). The mesh has been refined, edges, etc. corrected through the geometry dialog box.

 

1. I am still getting issues with the traces not propagating through the whole conduit. However, sectioning a plane through the discharge end of the conduit, and probing ("shift" with cursuor over plane), I am seeing the expected discharge velocity. Is there some reason the traces do not propagate through the whole conduit? The mesh is 25% (fine) of the automatic mesh.

 

I did to the Advection 4 which the help describes as best for small closed conduits.

 

Incompressible model selected. The max velocity is about 164 ft/s (at the center of the conduit and zero at the walls as expected ), approaching sub-sonic but not near enough for compressible analysis according to the help.

 

2. In the pre-processor, when solve is set to steady state, a number of intervals are selected to save with respect to iterations. How can I extract time in the post processor with respect to those intervals? For example, if temperature is set to the inlet surface with respect to volumetric flow rate (both are set as BCs at the inlet surface), how can I see how long it is taking for that temperature to propagate through the system? Similarly for transient?

 

3. Heat transfer: I want to see the heat transfer and the time it takes for that heat to transfer once the fluid enters the conduit at a set temperature. I have the temperature at the inlet surface of the fluid inside the conduit set as an initial condition. I have a film coefficient set to the volume of the fluid outside the conduit (as a BC). I have a temperature assigned to the surfaces of the "shell" for the fluid outside the conduit (as a BC). Also, I have tried with just the temperature set to the outside of the shell and starting temperature of the fluid inside the shell without the film/heat generation. Those would be a wild guess anyway. The conduit would be exothermic and the fluid in the shell endothermic and the heat transfer between those is what is trying to be determine. I have tried both steady state and transient. Heat transfer is set in "solve" I am not seeing anything close to the anticipated BTUs/hr of heat exchange from the conduit to the fluid outside the tube. In fact it is close to zero. Where and what kind(s) of heat sink should be set to a tube/shell heat exchanger?

Please use plain text.
Product Support
wildej
Posts: 731
Registered: ‎08-25-2011

Re: Before you hit 'solve' but within the first thumbnail (co...

11-25-2012 09:50 PM in reply to: jrm_1971

1. This sounds like an issue with the traces now, if the results are good and you can verify this via a cut-plane. Have you tried using an ISO surface to show the uniformity of the flow through the cente of the tube? You can also make this show vectors, rather than just a surface.

 

2. The save intervals for a Steady State analysis are meaninless, as this is just a single point in tmie we are converging on. There would only be a time option to select if you ran a transient study.

You would need to use Initial Conditions on the volume (be sure to swich from surfaces) of the fluid to do this.

 

3.Same issue here I think, do not use the surface, assign the initial condition to the entire volume. If you have a fixed temp outside the shell, this would overconstrain the model and prevent it heating up, is this to model an ambient condition? You could use a film coefficient here (I typically use 5 W/m2/K) at the ambient temp.

 

Does that answer all your questions and help at all?



Jon Wilde
Please use plain text.
Distinguished Contributor
jrm_1971
Posts: 112
Registered: ‎03-31-2011

Re: Before you hit 'solve' but within the first thumbnail (co...

12-04-2012 06:36 AM in reply to: wildej

1. This sounds like an issue with the traces now, if the results are good and you can verify this via a cut-plane. Have you tried using an ISO surface to show the uniformity of the flow through the cente of the tube? You can also make this show vectors, rather than just a surface. I have. The ISO and plane probing looks good. It is just a mystery why the traces disipate through the conduit. Maybe Autodesk CFD does not know how to handle traces in a 3D spiraling conduit?

 

2. The save intervals for a Steady State analysis are meaninless, as this is just a single point in tmie we are converging on. There would only be a time option to select if you ran a transient study.

You would need to use Initial Conditions on the volume (be sure to swich from surfaces) of the fluid to do this. OK thanks

 

3.Same issue here I think, do not use the surface, assign the initial condition to the entire volume. If you have a fixed temp outside the shell, this would overconstrain the model and prevent it heating up, is this to model an ambient condition? You could use a film coefficient here (I typically use 5 W/m2/K) at the ambient temp. I have taken away the overconstrained BCs and initial conditions. Here are the BCs as they exist now: volumetric flow rate applied to the inlet surface, pressure applied to the discharge surface, film coefficient applied to the outside surface of the shell. Initial conditions: Temperature applied to the volume of fluid in tube (this fluid has flow for my study). Pressure of 14.7 applied to the top of the shell side fluid (this fluid is designed to be static). I am still getting heat flux near zero (both in steady state and transient). I would expect it to be in the thousands of BTUs/hr. The heat sink just isn't sinking for some reason. Please advise.

 

Does that answer all your questions and help at all?

Please use plain text.
Product Support
wildej
Posts: 731
Registered: ‎08-25-2011

Re: Before you hit 'solve' but within the first thumbnail (co...

12-04-2012 06:45 AM in reply to: jrm_1971

I think we may have to leave (1) for now, I am just not sure what the issue is, without seeing the model it is tough to troubleshoot. It does sound as though the flow results are OK though.

 

I would like to focus on (3) as your setup is not quite correct by the sounds of it. I am not 100% clear on what the 14.7 pressure for, please could you expand on this?



Jon Wilde
Please use plain text.
Distinguished Contributor
jrm_1971
Posts: 112
Registered: ‎03-31-2011

Re: Before you hit 'solve' but within the first thumbnail (co...

12-08-2012 06:36 PM in reply to: wildej

I would like to focus on (3) as your setup is not quite correct by the sounds of it. I am not 100% clear on what the 14.7 pressure for, please could you expand on this? 14.7 is in psi. It is atmospheric pressure (or 1 bar as my friends in the UK use). As mentioned, the fluid on the shell side is static (it does not flow). A good example is a process storage tank with a static fluid in it being heated by a coil with a fluid flowing through the coil. I assigned the atmospheric pressure to the top of the static fluid because I have gravity turned on in Solve. As one might expect, the static fluid moves around in the tank as it is heated. Storage tanks, in some cases and in my case, have an atmospheric vent, hence no pressure other than atmospheric. I am under the assumption, to properly model this phenomena, I have assigned gravity and atmospheric pressure.

Please use plain text.
Product Support
wildej
Posts: 731
Registered: ‎08-25-2011

Re: Before you hit 'solve' but within the first thumbnail (co...

12-10-2012 12:07 AM in reply to: jrm_1971

Ah, I understand. That is something that we cannot model right now, the effect of height of fluid within these models.

 

You can still take into accounf the effect the heat will have on the fluid density, but there is no need to assign a p=0 to the top surface, this just leaves it acting as an opening for flow to enter/exit. Remove the p=0 and it will act more like it would in reality, with fluid unable to escape - maybe apply a film coefficient, just to allow heat to escape?



Jon Wilde
Please use plain text.
Product Support
wildej
Posts: 731
Registered: ‎08-25-2011

Re: Before you hit 'solve' but within the first thumbnail (co...

12-21-2012 01:07 AM in reply to: wildej

I have your file now, thanks.

 

There are a couple of points to make:

 

  1. To properly capture heat transfer through a solid, you need to have at least 2 elements through the thickness, so it would probably be worth splitting the coil into 2 so you essentially have one coild inside another, this will guarantee a mid-node with no additional meshing work needed.
  2. The same applies to the outer solid of the unit.
  3. You need to have a temperature at the fluid inlet
  4. We probably need to refine the mesh generally - run with those suggestions first and then refine the mesh to 0.7 and see if the results change, if they do, by more than 5%, refine again and continue until the results remain stable.


Jon Wilde
Please use plain text.