thermal equilibrium between positive and negative heat source
Hi everyone,
I am trying to perform thermal simulation with heat source and sink as boundary condition. I have a positive heat flux(as QVOL acting on solid elements) and a negative heat flux (as QBDY1 acting on conduction interface). However most of the time I could see that the simulation does not converge and the Temperature results are very big.
Attached here I have 2 fem files with exactly the same geometry and boundary condition and element size, but different meshing directions. the 1.fem file yields correct results while 2.fem doesn not converge. I have tried to experiment with changing element normal and changing material direction all to be along heat transfer direction but still 2.fem file does not converge and I cant find what makes the difference in simulation results.
can anybody check to see if you can converge the 2.fem file ? and what makes 2.fem file not converge?
thanks and looking forward to hear from you
Rafezi
Answers
-
As you can see here 1.fem file converges with sensible results while 2.fe file does not converge !
does anybody have any idea?
<?xml version="1.0" encoding="UTF-8"?>
<?xml version="1.0" encoding="UTF-8"?>
0 -
This is strange.I will check this internally and let you know the outcome.
0 -
Altair Forum User said:
This is strange.I will check this internally and let you know the outcome.
Thanks Rahul, few words Regarding the meshing for the model that converges:
I have created 2D elements and dragged them along to create 1 big 3D component, then I have deleted some elements until I have reached the model that you see, therefore the element material directions are on the same orientation. for meshing of the other model, the meshing is done in differenet directions.
Although I have tried to orient all material direction and element normals of the not-converging-model, still this model is not converging. Therefore I assume material direction and element normals dont have influence.
0 -
Do you simply want to study the temperature difference? Please refer attached fem deck.
<?xml version="1.0" encoding="UTF-8"?>
0 -
.
0 -
Altair Forum User said:
Do you simply want to study the temperature difference? Please refer attached fem deck.
<?xml version="1.0" encoding="UTF-8"?>
Thanks Rahul but my problem is not how to do thermal simulation, my problem is that I have a negative and positive heat source with the same magnitude and the simulation isn't converging
0 -
.
0 -
I think you are violating the governing equation of steady state heat transfer in your case by not considering temperature boundary condition. Please refer screenshot from help.
<?xml version="1.0" encoding="UTF-8"?>
0 -
Altair Forum User said:
I think you are violating the governing equation of steady state heat transfer in your case by not considering temperature boundary condition. Please refer screenshot from help.
<?xml version="1.0" encoding="UTF-8"?>
that is correct, the boundary condition that I have defined should only be able to calculate the temperature difference (that is ΔT in Fourier's law q=k.ΔT/L or ∇T in matrix presentation: Q=K∇T) but In order to do that the simulation should first converge. The converging of simulation is highly dependant on mesh orientation while in reality it should not.
It seems like optistruct is not handling a simulation with heat source and heat sink correctly, or independant of mesh orientation.
0 -
I guess you were in touch with local support team for this issue and they suggested two points:
1. hm_volume entity_type mark_id (Related to pre processing)2. When exporting the model, you can achieve greater accuracy with the * Long Format *:
I tried exporting fem file in long format and observed comparable results for the above shared two fem files.
0 -
Altair Forum User said:
I guess you were in touch with local support team for this issue and they suggested two points:
1. hm_volume entity_type mark_id (Related to pre processing)2. When exporting the model, you can achieve greater accuracy with the * Long Format *:
I tried exporting fem file in long format and observed comparable results for the above shared two fem files.
Yes I am in contact with Altair and the solutions that were devised didn't work. I am able to read the volume and enter the flux B.C. with high precision but still the energy equation doesn't hold fully and the simulation wpnt converge.
0 -
Final resolution from my side is the output which you are getting for second model is because of singularity(-4.25e+09 Grid temp of second model). Hence considering temperature boundary condition of 25 degree c in your model yields same output for both the model. PFA screenshot & updated model files for the same.
You can also refer similar thread to your query.
https://community.altair.com/community?id=community_question&sys_id=5746c0b61b2bd0908017dc61ec4bcb9d<?xml version="1.0" encoding="UTF-8"?>
0 -
Altair Forum User said:
Final resolution from my side is the output which you are getting for second model is because of singularity(-4.25e+09 Grid temp of second model). Hence considering temperature boundary condition of 25 degree c in your model yields same output for both the model. PFA screenshot & updated model files for the same.
You can also refer similar thread to your query.
https://community.altair.com/community?id=community_question&sys_id=5746c0b61b2bd0908017dc61ec4bcb9d<?xml version="1.0" encoding="UTF-8"?>
Hi Rahul Thanks for you response but I have to disagree with you. The reason that simulation of GAJENDRA KUMAR NHAICHANIYA on the other thread is not converging is not singularity, He has the wrong boundary condition because he has introduced a heat source without a heat sink, that means you have a closed unit and you only heat it up, of course the temperature will only rise until it reaches the maximal long number that the software can handle. that means the energy balance is not holding now if you introduce a spc temperature and fix some nodes with some temperature, the iteration will not go on and has to stop but the temperature results wont be accurate.
In my model I have been entering the QVOL and QBDY1 which are multiplied with element volume and element area. Now if the element volume has deviated a very small amount from what your CAD model that means discrepency between energy input and output which leads to not converging. QVOLxVolume = QBDY1xArea
I would expect however that the software would be able to handle thisw deviation since they are very small but as you see they magnify with each iteration.
However I found a work around which is to read the volume and area using command consule with 17digits of precision and then enter QVOL and QBDY1 values with 17 digits and run it on cluster and without determining any temperature constraints. In this case all the models would converge and calculate a dT.
furthermore the test that you made by adding the temperature would lead to very bigger deviations once you have a more comlex geometry and more elements.0
