Learning Forum

[solani]

Hello,

I am interested in the internal heat generation (or in my case: a heat sink). Since the internal heat generation is (as far as I know) not able to calculate the magnitude as a function of temperature I want to calculate the heat sink magnitude outside of this "internal heat generation method" (maybe with an APDL command) and then give this method the specific, freshly for each iteration / load step calculated value.

Thanks in advance.

Regards,

Ani

[dlooman]

Heat generation can be defined as a function of temperature using table input as shown below. It is possible to do it "by hand" by running the solution with many load steps and querying the temperature with a commands object at the end of each solve, but this is easier.
/prep7
et,1,70
mp,kxx,1,1
mp,dens,1,100
mp,c,1,1
block,,1,,1,,1
esize,.25
vmesh,1
fini

/solu
antyp,trans
*dim,hgenval,table,2,,,temp
hgenval(1,0)=0,100
hgenval(1,1)=100,200
bf,all,hgen,%hgenval%
time,10
nsub,10
outres,nsol,1
solve
fini

/post26
nsol,2,1,temp
prva,2

[solani]

this is very very helpful. Thank you very much!!
I am a beginner with APDL so I struggled to set up such a code. But I am more confident now! However, I have a question: Do I need all of the commands in a command tab in the Mechanical GUI? Because I already have a mesh created and other boundary conditions which I want to be taken into account simultaneously.
Another question is, if (e.g.) the hgenval(1,1)=100,200 command passes the heat generation rate by 100 and the temperature bythe value 200 to the table.
Also maybe another question: Do you know if this method will lead to the same results as the heat generation rate with the MASS71 method with tabular input? Or do you know where the difference is?
Best regards and many thanks!
Ani

[solani]

I managed to get your code to work and adapt it. Also I noticed that I only need the \solu-part (without some commands, e.g. without the solu, solve and finite and time command). Thank you very very much! This totally made my day - no even more, it made my week ;-)
I have one more question: Is it possible to plot / to retrieve the "used" heat generation value (hgenval) over time? E.g. to plot how high the heat generation rate / internal heat generation was at a specific time step for a specific element? If there exists such a possibility, it would be awesome.
Another, not so important question: Do you know if this method will lead to the same results as the heat generation rate with the MASS71 method with tabular input? Or do you know where the difference is?
Ani
P.S. For anyone looking at the code and getting confused by the table: The following website helped me a lot: https://www.ozeninc.com/apdl-arrays-tables-quickreference/
Also this website (https://www.mm.bme.hu/~gyebro/files/ans_help_v182/ans_cmd/Hlp_C_BF.html)
helped me a lot for looking up commands in a fast way.

[peteroznewman]

The "Also" website is just a page from an old version of the ANSYS Help system. If you open ANSYS Help on your computer from the Start Menu or from within Workbench, you can navigate alphabetically to Mechanical APDL, then to the Command Reference, then the letter B and find the BL command.
https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v212/en/ans_cmd/Hlp_C_BF.html

[sf]

Hello,

Thanks Dave for sharing this code, is really helpful!

Do you have a proposal for the case when I would like to set the heat generation in function of T_max - T_min of a specific body within the simulation domain?

Thank you, Feri