How to define Boundary Conditions for my complex model (and how to unite the similar geometries)

  • 140 Views
  • Last Post 4 days ago
  • Topic Is Solved
moda9742 posted this 2 weeks ago

Dear Peter,

I was wondering if you could do me a favor, and send me a detailed YouTube file (including your file) and show me the following parts:

  • Can you please simply let me know how to unite the six solids into a single body, in order to get rid of a lot of extra contacts in the model? (Could we do it in Geometry e.x by defining Merge Topology- or it should be done in Meshing?)
  • As far as K (thermal conductivity of insulators), please simply use gypsum (ANSYS Data base).
  • I didn't get the point of "pick all the faces that are exposed to the convective cooling on that end." Can you please explain to me a little bit more?
  • As you said correctly, NO resistance between insulators. Please show me how to have ALL insulators as on part, same as widgets as 1 part.
  • Please show me how to get rid of so many BCs such as  contact regions, internal walls, shadow walls,...

Again, I attached the same geometry file that I already attached in last discussion.

P.S. I was wondering if you could keep working with 19.1, as 19.2 version on my laptop is limited (educational version)!

I really appreciate all your support.

Sincerely,

 

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 2 weeks ago

Note to Community: this is a continuation of a previous discussion.

Dear Moda,

You have the parts in SolidWorks, is that correct? 
In SolidWorks, to add bodies together:

  • Click Combine (Features toolbar) or Insert > Features > Combine.
  • In the PropertyManager, under Operation Type, select Add.
  • For Bodies to Combine, select the bodies to combine. ...
  • Click Show Preview to preview the feature.
  • Click okay

 You can do this for the six Insulators that share common faces.
You can't do this for the five air wedges, as they don't have a common face, only a common edge.

When I said in the previous discussion, "you defined RightConv (and LeftConv), but you didn't pick all the faces that are exposed to the convective cooling on that end." I mean that the five air wedge faces and the six insulator faces are also exposed to the convective cooling, but you didn't pick those 11 faces to include in the Named Selection called RightConv. You should add them.  You could also add the two faces of the glass thickness, even though it is a small area, but you will have the edge of the glass that has a temperature BC on it, so you might get a warning for having two BCs on one edge.

I recommend you uninstall ANSYS Student 19.2 and download ANSYS Student 19.1 on your laptop. That way you won't have any problems moving models between the school computer and laptop.  Click on Download, then in the list is Prior Releases where you can find 19.1.  Discard any models saved in 19.2

Regards,
Peter

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

Dear Peter,

 

First of all, thank you so much for all your support. Yes, I did my geometry in SolidWorks. However, I'm in trouble with that feature (attached)- to combine those bodies together. Any clue please?

Sincerely,

Attached Files

peteroznewman posted this 2 weeks ago

Dear Moda, There are many ways to accomplish the same goal.  Here is one way.

In SolidWorks, File, Save As, Type: Parasolid,  with Options = Flatten Assembly. That will make a single file with no assembly, just all the bodies.

You could either open that file in SolidWorks, then the instructions above might work... OR

In SpaceClaim, File Open and open the Parasolid file.  Now you should be able to use the Combine tool to unite the six isolator bodies into one large body.

Regards,

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

Dear Peter,

Like always, please accept my sincere appreciation. Actually, I tried to follow your instructions (to combine the similar wedges and insulators). However, it did not work for me. 

BTW, I just meshed my geometry (maybe not very accurate, but acceptable enough)! My results are enclosed in the attached file. I was wondering if you could do me a favor and take a look!

Finally, I need to calculate heat  flux through each (front &rear) glass plates. My final values should be around 23 & 56 (w/m2). Can you please show me how to get such values from the results?

I really appreciate all your support.

Sincerely,

Attached Files

peteroznewman posted this 2 weeks ago

Dear Moda,

This post is just to show you the merged insulators.
I opened the file attached above and opened SpaceClaim. 

  • File, Save As and set the type to ACIS
  • File Open, type ACIS, set the Options to Uncheck create Components from ACIS bodies
  • Hide all components except for the insulators
  • Click the Combine tool and click the top insulator
  • Click the Add button and box-select all the other insulators, it's done.

Attached is the SpaceClaim 19.1 document.
I will look at the heat flux question later today.

Regards,
Peter

 P.S. I later found an error in the length of the insulators, they extend past the glass and air. You should fix that.

After I fixed the above error, there are remaining geometry errors that cause meshing problems.
The AG extends too far and the Insulator doesn't touch the Air.

Please fix these errors and attach a new Archive.

Attached Files

  • Liked by
  • moda9742
peteroznewman posted this 2 weeks ago

Dear Moda,

In my previous post, I showed changing Air to an Ideal Gas. The reason is you want the density to be a function of temperature so that gravity will create natural convection by pulling down the heavier, colder air, while the lighter hotter air rises. 

In your Fluent model, the Air has a constant density. I will change that to Ideal Gas using the pull down on the Density line that currently says constant.

Another difference which may or may not be important. I changed to the Density-Based Solver, while your model had the Pressure-Based solver. I don't know which one is better.

More later.

Regards,
Peter

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

 Dear Peter,

Thanks for all your clarifications. I think I'm really close to the results! Actually I fixed my model in SolidWorks, and then merged my insulators as well. Also, I followed your instructions for setup. However, my results do not look like correct. Would you please take a look at the attached file? Also, I was wondering if you could give me a hint on heat flux!

Thank you so much,

Sincerely, 

Attached Files

peteroznewman posted this 2 weeks ago

Dear Moda,

I will look at your model today. I just opened the Geometry, and see you haven't used Shared Topology, probably because the geometry is not yet perfect.

When the geometry is perfect, Shared Topology will allow all the bodies to be meshed and no contacts will be needed between the bodies.

On the frontt Wall BC, where you apply a Temperature, did you type in the Wall Thickness value of 0.02 m or was that automatically populated?

If you typed that in, why do you think that is correct? What does the ANSYS Help say about that? The reason I ask is that you are modeling the glass as a solid, so the thickness is already represented in the meshed geometry.

I clicked the Check Case button and got some warnings that you should heed.

I notice on the Fluent Launcher, that you are now using Parallel with 4 cores. You should also check the Double Precision checkbox.

How many iterations did you run? The file only shows 100 iterations, but after 500 iterations, the solution is not yet near to meeting the convergence criteria of < 1e-3.

I will be checking this page for the next 9 hours, so I will see your reply or if you are online.  More later...

Regards,
Peter

  • Liked by
  • moda9742
peteroznewman posted this 2 weeks ago

Dear Moda,

I ran the model until it converged with all residuals < 1e-3. I had two changes: Double Precision and Zero Operating Density.

I created a plane at X=40mm to plot velocity.  There is a 20 cm/s downward draft on the back glass. The mesh is way too coarse for the AirGap wedges.

Heat Flux

In Fluent, in Post Processing, Surface Integrals...

Here is the frontt BC Area-Weighted Average Heat Flux

Here is the reart BC

Here is the leftconv

Here is the rightconv

There is zero heat flux on the top and bottom adiabatic surfaces.

For a Steady-State Thermal solution, I was expecting the sum of all faces to be zero heat flux, but the sum is not even close to zero. I wonder if it will get closer to zero with a finer mesh and a smaller convergence criterion on the Energy residual, like 1e-6.

Regards,
Peter

  • Liked by
  • moda9742
peteroznewman posted this 2 weeks ago

I edited the last paragraph of the post above after you looked at it. 

Shouldn't the net heat flux through the six faces be zero (within some small tolerance)?

moda9742 posted this 2 weeks ago

Dear Peter,

Thank you so much for all your support. You know, the story is this I already did this test (for different angels varying between zero to 90); and now I'm trying to verify my results with ANSYS. For example, for the angle of 60, my measurement resulted 23.6 and 56.7 (w/m2) for front and rear plates, respectively while this parameter matters just for these two plates. Now, I'm a little disappointed why this CFD job is not able to verify my lab measurements. Do you have any idea?

 

As far as density, are you sure I should pick bussinesq for air density (attached)? 

Thank you so much!

 

Sincerely,

Attached Files

peteroznewman posted this 2 weeks ago

Dear Moda,

All simulation models have errors in them, you just keep working on them until the error becomes acceptably small. Similarly, all experimental measurements have errors in them, and those errors can be reduced by more elaborate measurements. Then there is the issue of correlation between simulation and measurement. That combines the errors from both sides!

How did you measure the 23.6 and 56.7 W/m^2 heat flux values for the front and rear glass plates?
What about the convection BC on the left and right sides? Should the difference between the front and rear plates be accounted for by the convection out the sides? The simulation showed an almost zero heat flux there.  You should increase the convective heat transfer coefficient.  I also suggested smaller elements and a smaller Energy convergence criterion. Plus I had the question about assigning a thickness to the glass. That may be an error in the model.

My experience is in Structures.  I am learning CFD and am in no way an expert, though there are CFD experts on this forum. I hope one of them takes an interest in this discussion and chimes in. 

Regards,
Peter

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

Thank you so much for your quick reply. Actually, I didn't measure heat flux on sides, as it was not important to me. I had 2 thermopcouples, installed them on each front and rear plate, that showed me temperature and heat flux.

Can you please verify that I should use bussinesq assumption for air density? Also, as you said correctly, maybe I should pick a different h coefficient value?! I simply followed your value of 0.001!

Sincerely,

Attached Files

peteroznewman posted this 2 weeks ago

As far as density, are you sure I should pick bussinesq for air density (attached)?

I didn't say to pick bussinesq.  rwoolhou suggested incompressible ideal gas, but that was without a complete understanding of the problem. It's a fixed volume, so I suggested ideal gas.

maybe I should pick a different h coefficient value?! I simply followed your value of 0.001!

I just made up a number. h coefficients are experimentally determined, so you will have to measure that.

If you have some documentation on how heat flux is calculated from your thermocouples, I would like to read that.

Please start a new discussion for the next phase of your simulation.

Kind regards,
Peter

 

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

That would be fantastic.

moda9742 posted this 2 weeks ago

peteroznewman posted this 2 weeks ago

Dear Moda,

Attached is the perfected geometry version of your model. You can tell the shared geometry is working when you get the purple and yellow colors for common edges. Show your SolidWorks friend that it is possible to have perfect geometry. Zoom into that top right corner as much as you like. They all meet at a point.

I managed to mesh it with smaller elements and kept the mesh below the Student license limit of 512 K nodes/cells.

Because Shared Topology is working, there is No Contact, so the list of Walls is a lot shorter in Fluent now.

Enjoy!

Warm regards,
Peter

Attached Files

  • Liked by
  • moda9742
peteroznewman posted this 2 weeks ago

Dear Moda,

You said in your experiment that you have one thermocouple on the front glass and a second thermocouple on the rear glass. But you also said the instrumentation outputs a heat flux. I think I know how it does that. In addition to the thermocouple on the glass, there is a companion thermocouple on the same side of the wall measuring the air temperature. So there must be at least four thermocouples. The instrumentation is using a convective heat transfer coefficient, h, and calculates the difference between the temperature of the air and the glass as dT and the equation is

  • heat flux, q = h dT.

I can imagine that the temperature could vary over the extent of the glass, especially the glass with the insulator touching it and capturing the air wedge, which could be much hotter than the glass at the bottom that has free moving air inside the wall.

What is it that is actually creating the hot temperature on one side of the wall and the cold temperature on the other side of the wall?  It is air temperature on each side of the wall, right?

In that case, it would be better to have a convection boundary condition on each side of the wall with the known ambient air temperature and a good estimate for the convective heat transfer coefficient. Hint: use the same value that the instrumentation is using. That way, the glass that has internally circulating air next to it can be a different temperature than the glass that has the air wedge next to it.  This would be a more realistic set of boundary conditions than an applied constant temperature, especially since you only measured the glass temperature at one location on the glass surface.  That will be a much more realistic set of boundary conditions for your model.

Kind regards,
Peter

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

Dear Peter,

I really appreciate all your support. I really enjoyed discussing with you today.

Enclosed, I've attached a manual for the thermocouple. As I know (and sure), there was just two sensors (not 4). Please take a look and let me know if you have any idea.

Sincerely,

Attached Files

peteroznewman posted this 2 weeks ago

Dear Moda,

Thanks for the manual on the instrumentation; I learned something new!  The sensor you called a thermocouple is actually a heat flux sensor with an integral thermocouple. I didn't know about that before, now I understand how you get heat flux, it is measured directly.

I made the following figure to represent your Thermal Wall. You have a cold side where the bulk temperature of the air is Tbc, you have a heat flux sensor on the glass measuring the glass temperature on the cold side of Tgc and the heat flux qgc.  You have a hot side where the bulk temperature of the air is Tbh, you have a heat flux sensor on the glass measuring the glass temperature on the hot side of Tgh and the heat flux qgh

Outside of the controlled temperature environments on either side of the wall is the lab space where the temperature is Tlab and that is where the voltages are being measured, probably on the FluxTeq DAQ.  Is the correct?

My point on a previous post was that the temperature of the glass on the hot side could be very different near the top where there is a trapped wedge of air next to the glass than it is near the bottom where there is natural convection occurring in the wall cavity.

That is why a better BC for your Thermal Wall model would be Convection on both glass surfaces. I assume you have some idea of the bulk temperature of the air on each side. But the issue is what is an accurate estimate of the convective heat transfer coefficient, h, for use in the CFD model convective BC?

Get two or three more thermocouples and plug them into the DAQ to measure the bulk temperatures directly.  Also, it is more accurate to have a thermocouple measuring the temperature in the lab.  Here is the updated figure.

Given that you have an actual heat flux sensor, you can calculate the convective heat transfer coefficient from the equation

h = q/(T- Tb)

which is the definition of that quantity.

Do this for the hot and the cold side of the wall and use each value of h in your convective BC along with the measured bulk temperature.

Finally, looking at the photograph of the Thermal Wall, I see a wooden frame on the sides and top and bottom of your Thermal Wall, so I would make those four sides Adiabatic.

There is a lot more detail in the heat flux sensor manual you provided above. Are you implementing the temperature correction for the heat flux?  I assume you read the bit about the voltage output from the thermocouple gives you the temperature difference between Tg and Tlab so that if you want the absolute value of the temperature of the glass, Tg, you have to add Tlab to the reading from the thermocouple.  How are you measuring Tlab?  You could do that with an extra thermocouple.

Kind regards,
Peter

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

Dear Peter,

Thank you so much for all your information. I really enjoyed your points. Actually I had another sensor (HOBO) and I measured the lab temperature using that sensor (which was almost constant and around 70F. BTW, for calculating the wall thermal resistance (R), I didn't need to add that temperature- as basically it was defined by deltaT/q. In other words, Tlab should be subtracted from both sides. However, for T constant on BCs (rear and front), I believe that I should update my temperatures with absolute values.

I liked your idea for and got your point that "the temperature of the glass on the hot side could be very different near the top where there is a trapped wedge of air next to the glass than it is near the bottom where there is natural convection occurring in the wall cavity". Also, i believe that constant temperature is not an accurate assumption for this model. However,as I do not have anymore sensors in the lab, I should keep continuing with this assumption (I forgot to say that inside the wooden box, i had a hair drier as a heat source. What I did was not modeling directly that source, and instead assuming a constant temperature on the hot glass- which was just simplifying the problem!).

Also, I read your comments in the other discussion and enjoyed your justifications and explanation. Just as a quick question, I was wondering if you could let me know about "Coupled Pressure Based Solver". I didn't see that option in Solver menu and wondering if you could let me know how to select that option! Hopefully someone reply to us in that discussion forum. In addition, do you think should I consider Boulder's elevation and its local atmospheric pressure? If yes, would you please update me how to do it?

Finally, I was wondering if you could do me another big favor and show me how you corrected my geometry to your perfect geometry (by video or explaining the steps to me please), as I need to redo it for 6 more angles (0,15,30,45,75, and 90 degrees). Did you fix it in SpaceClaim?

Like always, pleas accept my sincere appreciation for all your help and support.

Sincerely,

peteroznewman posted this 2 weeks ago

Dear Moda,

Here is another idea for a boundary condition for the air on the hot side of the wall. What was the wattage of the hair dryer?  Say it was a 1000W hair dryer.  What if you set the air (or the air wall) on the hot side to have a 1000W heat generation in the hot air domain. Then you don't specify a glass temperature on the hot side at all, the solution figures out the temperature distribution on the glass. On the cold side, you could keep the measured cold glass temperature or you could go for the convective BC but then you need the heat transfer coefficient and the air temperature.

I don't know what the Coupled Pressure-based Solver is.  I don't know if the local air pressure is relevant.  You can run the model twice, once at sea level and then rerun it at Boulder, CO elevation.

To make the perfect geometry, I exported Parasolids out of SpaceClaim and brought them into my NX 11 CAD software, where I used Move Face, and moved point-to-point to get the perfect corner point. That worked for the top wedge that only had that error. The next four wedges also overlapped the glass and had a gap to the adjacent wedge. Rather that fix them, I deleted them and copied the first wedge down using point-to-point so there was no gaps and no overlaps. Finally, I did one more Move Face, point-to-point to shift the face on the large air cavity to close the tiny gap to the fifth air wedge. I deleted the insulator body, as it didn't match anything anymore. I used the new perfect edges of the five wedges and the air cavity edges to extrude a new insulator.  There may be a way to do all that in SpaceClaim, but I don't have those skills yet.

Warm regards,
Peter

 

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

Dear peter,

I really appreciate all your points. I liked your idea for the hot plate BC. Thanks!

BTW, would you please let me know how to " run the model twice, once at sea level and then rerun it at Boulder, CO elevation". I don't know where could I define my current location/elevation.

Sincerely,

peteroznewman posted this 2 weeks ago

I mean set the operating pressure for sea level and then set the operating pressure for whatever it is in Boulder.

  • Liked by
  • moda9742
moda9742 posted this 2 weeks ago

Thanks. I see. However, I do not know how to change that operating pressure!

Sincerely,

moda9742 posted this 1 weeks ago

Dear peter,

Just as one more quick question: Would you please let me know after I edit my geometry in SpaceClaim, should I reopen the file in ACIS format? I followed all your following steps, however when I open the file in geometry, my changes have not been applied (merged insulators still shows separately!)

  • File, Save As and set the type to ACIS
  • File Open, type ACIS, set the Options to Uncheck create Components from ACIS bodies
  • Hide all components except for the insulators
  • Click the Combine tool and click the top insulator
  • Click the Add button and box-select all the other insulators, it's done.

Sincerely,

peteroznewman posted this 1 weeks ago

Dear Moda,

When I deviate from the standard workflow, I do also wonder if I have to Save As, and how exactly do I get the geometry into Meshing.

One way that seems reliable (and there must be many others) after you have done anything special like you did above is to do a File, Save As to a SpaceClaim file format.  Close SpaceClaim.  In Workbench, open the project you wanted to use this improved geometry in (or start a new project) and on the Geometry cell, RMB and select Import, then point to the file you just saved.

On a separate topic: where did you come up with the density of Glass in your Fluent model?  You are using 8000 kg/m^3 while the Engineering Data for Glass shows a density of 2,500 kg/m^3.   You also use a thermal conductivity at 0.8 W/m k which is quite a bit smaller than the thermal conductivity of 1.4 W/m k that I find in Engineering Data.

Regards,
Peter

P.S. I was looking at where to set the Operating pressure and didn't find it yet. 

 

  • Liked by
  • moda9742
moda9742 posted this 6 days ago

Dear Peter,

I really & warmly appreciate all your support and help.

Sincerely,

peteroznewman posted this 5 days ago

Dear Moda,

Sorry, I don't work for ANSYS so I don't have any licenses to hand out.  Ask your school if there is a way to take home the full license, maybe on a school laptop.

I suggest you find out how to get Windows Remote Desktop access to the computer at school that has ANSYS installed. That way, you can run your model on the school computer from home.

Kind regards,
Peter

  • Liked by
  • moda9742
moda9742 posted this 5 days ago

Thank you so much for your help. It could be really a good idea. Thanks!

Show More Posts
Close