Radiation to Ambient 2

[flash3780]

I'd like to include radiation to ambient in my model. I've already got SURF152 elements on the exterior for convection, and I think that I can apply ambient radiation to those. However, when I try:

[tt]NSEL,s,TYPE... blah blah blah
SF,,RAD,0.15,29[/tt]

ANSYS doesn't like it.

I tried changing KEYOPT 9 to 1 (Use radiation with the form factor as a real constant). I also set the element real constant to 1 (RMODIF,1000,1,1). ANSYS spits back an error requiring me to set KEYOPT 5 to 1 (One extra node). I do that, and it spits back another error requiring input from FLOTRAN.

Now, I could just use the radiosity solver on those surfaces, but I have a feeling RAD will be MUCH faster than RDSF. Anyhow, the ANSYS help is... well, less than helpful in this instance. I sometimes feel like thermal analysis is a second thought to ANSYS. There aren't any examples in the thermal analysis guide or the verification manual.

Anyhow, I'm pretty sure that this is just a syntax problem on my part; I'd be really grateful if anyone out there's able to point out my error. Thanks a ton.

 

[flash3780]

Ok, I think that I've found a good example that will get me straightened out. Sheldon has again come to my rescue, clearing up things that aren't well explained in the Ansys documentation.

Overall, I actually think that the Ansys documentation is quite good. However, I think that their explanations of how to use their thermal analysis tools sometimes leaves something to be desired. It's a shame, because the program is quite powerful in that area.

I think that what I'm missing is an [tt]ESURF, NODE(X,Y,Z)[/tt] to define the extra node (rather than [tt]ESURF[/tt] alone). After that, I can define an ambient temperature with [tt]D,NODE(X,Y,Z),TEMP,29[/tt].

Anyhow, I'm building a quick test model. Hopefully that will get me back on track.

 

[flash3780]

Ok, well I got it worked out and I thought I'd post my test case (in case anyone else needs an example). Here's how you do it:

1. Define the emissivity of the underlying elements
2. Set the proper SURF152 keyopts (5 & 9 for extra node & radiation)
3. Set the proper SURF152 real constants (1 & 2 for form factor & SB const)
4. Create an extra node ([tt]N,,X,Y,Z[/tt])
4. Create surface elements associated with the extra node ([tt]ESURF, NODE(X,Y,Z)[/tt])
5. Set the temperature of the extra node ([tt]D,NODE(X,Y,Z),TEMP,my_TEMP[/tt])

The SF/SFE command is not required for radiation to an ambient space node. However, if you'd like to include convection to the ambient space node as well, [tt]SFE,ALL,1,CONV,1,my_CONVCOEF[/tt]. The convective coefficient can be a function of temperature if defined as a material property. If so, set my_CONVCOEF = -my_MATERIALNUMBER.

As a bonus, the attached test case also has an example of how how to model radiation and convection across small gaps and how to model convection in an enclosure. I hope that this helps someone out there. It took me a minute or two to figure out the correct syntax.

 

[flash3780]

Quick tip:
Regarding step 1: The emissivity is a material property. In the attached example, I defined the emissivity of the underlying elements; ANSYS seems to inherit the emissivity of the underlying elements to the surface effect elements. Apparently you can also define the emissivity of the surface effect elements directly, overriding whatever is specified for the underlying elements.

 

[HVSmith]

Just found your post - it's been incredibly helpful, thank you. I was stuck with a radiation to ambient problem myself, but a lot of what you said makes sense - I'm going to give it a go now and see where I end up!

 

[flash3780]

Since I mentioned free convection, I think that I should elaborate on how ANSYS handles convective coefficients. ANSYS has several options for calculating convective coefficients based on the KEYOPTs that you set. For free convection, the physical equations lend themselves to the following:
HTC = (film coef)*|T1-T2|^n
Note that for turbulent flows, n is generally equal to 1/3; when you're using SURF152 elements, n is set with real constant 13.
A great reference for computing the film coefficient for various situations is the following: Incropera, DeWitt: Fundamentals of Heat and Mass Transfer

The ANSYS developers smartly give you several options for computing HTC; for free convection SURF152 elements, KEYOPT 5 allows you to associate the elements with an extra node (space node). The temperature at the extra node can be defined with [tt]D,NODE(X,Y,Z),TEMP,myTEMP[/tt] for convection to the environment. For convection to an enclosure, the temperature of the node will be calculated by ANSYS and will depend on the temperatures and convective coefficients of the associated surfaces. You'll also want KEYOPT 6 = 0, which tells the elements to use the temperature of the extra node as the bulk temperature. To parameterize the HTC according to the above equation, you'll want to set KEYOPT 7 = 1, which will multiply the "film coefficient" by the "empirical term", |T1-T2|^n. The "film coefficient" may be defined as a material property versus the average of the bulk fluid and the wall temperature ([tt]MPTEMP[/tt]&[tt]MPDATA[/tt]). To tell ANSYS to compute the film coefficient at the average temperature, set KEYOPT 8 = 2.

Once the SURF152 element properties are set, you'll want to create the elements as was mentioned in my earlier post (select nodes, issue ESURF, NODE(X,Y,Z) command, select elements, and use the SFE command). Note the syntax for associating the surface elements with the extra node.

When you issue SFE command, it should look something like this:
[tt]SFE,ALL,1,CONV,1,-my_MATERIAL[/tt]
Where my_MATERIAL is the material number which the convective coefficients are associated with. Notice the negative sign in front of my_MATERIAL, which tells ANSYS you've entered a material number rather than a single value for the film coefficient.

As it turns out, all of these commands are a bit of a pain-in-the-butt to issue in Ansys/Mechanical when compared to Ansys/Mechanical APDL (Classic). Still, once you get the process down, it's not so bad. The tricky part is confirming that everything made it onto the model the way you think it did. I generally flip over to Classic look over my boundary conditions, but you can also output images with some APDL commands if that tickles your fancy.

Hope this helps. I found convection in enclosures to be less than intuitive. My first method of dealing with it involved do-loops and convective link elements. SURF152 elements seem to work better. I'd encourage you to follow the link in the second post and look at Sheldon Imaoka's presentation on surface effect elements. He provides a lot of great information.

 

[biricio]

What do you think of this test? Does it can go?
thanks

 

[flash3780]

Have a gander at this thread:

http://www.eng-tips.com/viewthread.cfm?qid=302121&page=1

We had a great discussion about radiation to ambient in the above thread. I'll try to repost the WBPZ file if I can find it. You should be able to open it in Ansys Workbench (v13) by going to File > Restore Archive.

Good luck.

//signed//
Christopher K. Hubley
Mechanical Engineer
Sunpower Incorporated
Athens, Ohio
--

http://engineeringliberty.wordpress.com