## Fluids

#### Solar Load Model in Fluent Tutorial

TAGGED:

• Jiezougt
Subscriber

Hello Everyone,

I am learning ANSYS to create a model to apply solar load on it. From what I learned so far, Fluent has the solar load model function build in and all you need to do is to put in the location, date, and time. That was awesome! However, I do have questions/confusions regarding the model set up.

## History

I searched this forum and didn't find any actual solar load model tutorial. (The only answer I found is: "You can find some information in solution ##2042014. The training material is moved to other platform. To get access you may need to contact your account representative. "). So here I create another post hopefully could help other people as well who have similar questions.

## Purpose:

The purpose of this model is to create concrete bridge structure and assign solar load on it. The output will be the temperature distribution on the bridge structure at any given time of a day. (Transient)

## Procedure to Activate Solar Load Model:

1. Setup/Models/Energy: On
3. Click on Solar Calculator button
4. Input Global Position and Starting date and time. Check mesh orientation
• Rob
Ansys Employee
Solar load tells you where the sunlight comes from, and the manual will tell you how it's applied. If you then turn on the radiation models you'll get the effects of reflection etc. nEnclosures around an outside domain are fine, ie where you're modelling the sky. Rooms can get complicated due to the way the model is applied. We sometimes use the calculator to see where the sun is, then apply the result to the boundary conditions of our choosing. nIn your model consider whether you need reflection etc or just the heat load. You also want to review the transient solver and requirements as running a whole day will be very computationally expensive. n
• Jiezougt
Subscriber

Solar load tells you where the sunlight comes from, and the manual will tell you how it's applied. If you then turn on the radiation models you'll get the effects of reflection etc. Enclosures around an "outside" domain are fine, ie where you're modelling the sky. Rooms can get complicated due to the way the model is applied. We sometimes use the calculator to see where the sun is, then apply the result to the boundary conditions of our choosing. In your model consider whether you need reflection etc or just the heat load. You also want to review the transient solver and requirements as running a whole day will be very computationally expensive.https://forum.ansys.com/discussion/comment/104019#Comment_104019

Hey Rob,nThank you so much for your answer. Now it is clear that I do need to turn on the radiation model as I want to apply the reflection from the ground back to the bridge.nI noticed that when I set the solar load calculator (after input the location etc), the console gives the solar load to each face (w/m^2). I wonder when you say 'apply the result to the boundary conditions of our choosing)', do you mean to apply the load to entire surfaces? Or we could apply the result in a ray-tracing manner? In my case, the bridge deck edge is extending outside of bridge girder. During daytime, the sun beam will project heated area at the bottom part of girder web, leaving shade on the top part of girder web. I need to consider this in my model.nThank you again! Brandon
• Jiezougt
Subscriber

Solar load tells you where the sunlight comes from, and the manual will tell you how it's applied. If you then turn on the radiation models you'll get the effects of reflection etc. Enclosures around an "outside" domain are fine, ie where you're modelling the sky. Rooms can get complicated due to the way the model is applied. We sometimes use the calculator to see where the sun is, then apply the result to the boundary conditions of our choosing. In your model consider whether you need reflection etc or just the heat load. You also want to review the transient solver and requirements as running a whole day will be very computationally expensive.https://forum.ansys.com/discussion/comment/104019#Comment_104019

I lost my comment for some reason... Let me re-write it herenThanks very much for your answer, Rob. Now it is clear that I need to turn on the radiation model because I need the reflection from the ground back to the bridge.nI noticed that you said after we set up the solar load calculator (ie after input location etc), the console shows the magnitude of energy projected to the object in w/m^2). When you say '... then apply the result to the boundary conditions of our choosing', do you mean we read those numbers and apply those to the entire surfaces? In my case, the bridge deck edge is extending outside of bridge girder (deck overhang). During daytime, the sun will heat up the top of deck, bottom part of girder web, leaving shade at the top part of girder web. I do need to consider this ray-tracing manner. Is it possible to apply the load manually and still achieve this ray-tracing effect?nRunning transient for a whole day will ideal. I can reduce it to say 1 hour with 15 minutes as one time step. In this case, hopefully my workstation can handle it. I do want to do parametric study later (with different bridge orientation etc).nThanks again! And hopefully this time my comment didn't get lost Brandon
• Rob
Ansys Employee
They got caught in the spam filters. There's a verify option in account settings, if you can see that please use it. nThe solar load model and solar ray tracing are slightly different. The former adds a heat source into the domain but doesn't automatically turn on radiation modelling. So, you'll see the heat gain but no re-emission etc. nFor CFD we model to the flow time scale, this is typically 1/10 to 1/3 of the time it takes flow to cross one cell, and this gives time steps in the order of (very small) fractions of a second. If you can assume a wall HTC (or calculate from CFD) then Mechanical may be a better option. n
• Jiezougt
Subscriber
Thank you Rob, nI didn't see the verify option under my profile settings but I will dig more.nI am planning to use solar load model to model the bridge structure - add heat source into the domain. Also I would love it to radiate the heat out into the sky/surroundings so I would turn on the S2S. It sounds like if I only turn on the solar load model, the bridge deck will result in a higher temperature due to no re-emission?nDo I understand it correctly: if I set the wind inlet to be 10ft/sec, and a cell is 10ft by 10ft by 10ft (assumed), then it will take 1 sec to have the wind flow to cross one cell. The time step should be 1/10 of a sec to 1/3 of a sec?nLastly, when you say assume a wall HTC (I guess you mean heat transfer coefficient for convection), the mechanical may be a better option. The case is I need to model the sun location and solar load - I believe Mechanical is not capable of doing that... Am I correct? (I tried the mechanical and the solar radiation boundary condition will be assigning a uniform heat flux, meaning no shade effect to my knowledge - bridge deck overhang creates shade on girder webs)nnThanks again, sir,nBrandon
• Rob
Ansys Employee
If you just use the solar load model you won't get any re-emission, this may or may not be important depending on the conditions. nYour calculation is correct, other than using Imperial units: even the British are (mostly) metric now! nI don't know anything about radiation in Mechanical. will know what's possible. Note, if you don't solve the flow equations in Fluent you can speed up the calculation but will lose out on convective losses. n
• Jiezougt
Subscriber

If you just use the solar load model you won't get any re-emission, this may or may not be important depending on the conditions. Your calculation is correct, other than using Imperial units: even the British are (mostly) metric now! ?I don't know anything about radiation in Mechanical. @peteroznewman and @Aniket will know what's possible. Note, if you don't solve the flow equations in Fluent you can speed up the calculation but will lose out on convective losses.https://forum.ansys.com/discussion/comment/104289#Comment_104289

Hi Rob,nHahahaha thanks for your info! The bridge was designed using imperial units, and so as the structural plan set. Actually it is a good point, I might need to consider a unit conversion.nRecently, I watched many tutorial videos from ANSYS. I learned that if I use SpaceClaim to bring a solid and a enclosure into Fluent, then identify the solid region and enclosure region as fluid, a wall/wall shadow pair will be created: The wall can be set as a thin shell with thickness and conduction, and the wall shadow can be coupled with the wall, and interacting with the fluid region next to it for heat transfer (convection). nHowever, I am confused about this issue: Can this wall/wall shadow pair simulate a air-thin steel layer-air situation? Or can one wall/wall shadow pair only simulate air-steel situation? The solid that was created in Space Claim is actually a thin steel box with air inside. I want to simulate this air(outside)-steel(conduction)-air(inside) situation.nnThanks so much!nBrandonn
• Rob
Ansys Employee
Just be careful with units. The common error is mistaking 6'2 with 6.2 feet; it'll depend on how the plans were drawn up. I had the same issue with some furnace ducting from the 60's, not helped that the plans were also A0 and had about 4 amendment sheets.....Thin walls in Fluent can be used between two fluids, as a baffle with the same fluid on both sides, between solids and as baffles in solids. Just read up on coupled walls and remember that the area of the wall is it's geometric area:if you give the wall a thickness (ie for conduction) and it's curved the area is ALWAYS the same. n
• Jiezougt
Subscriber

Just be careful with units. The common error is mistaking 6'2" with 6.2 feet; it'll depend on how the plans were drawn up. I had the same issue with some furnace ducting from the 60's, not helped that the plans were also A0 and had about 4 amendment sheets..... Thin walls in Fluent can be used between two fluids, as a baffle with the same fluid on both sides, between solids and as baffles in solids. Just read up on coupled walls and remember that the area of the wall is it's geometric area: if you give the wall a thickness (ie for conduction) and it's curved the area is ALWAYS the same.https://forum.ansys.com/discussion/comment/105097#Comment_105097

Thank you very much, sir! I really appreciate all your input and helps!!nI am so used to imperial units so it is fine to me (use it every day here in the US, you know how advanced...). But that A0 to A4 amendents.... Sounds like nightmare hahaha. Hopefully it ended up well.nBests,nBrandon Zhoun