nonlinear transient heat transfer
Hi friends,
I want to simulate a nonlinear transient thermal analysis which is coupled with mechanical support. To this aim, first I conducted a thermomechanical analysis in which the thermal load was linear and the response was reasonable.
for nonlinear analysis, I added E(T) in MATT1. I also changed the analysis to generic and added nlparm for NLHEAT analysis according to tutorials. But, I got the following error!
*** ERROR # 1461 *** in the input data:
Card 'NLPARM' is not allowed for this subcase type.
the nonlinear analysis file is attached. could you please help me to proceed with the analysis?
Note: for this model, I aimed to apply the boundary condition such that the tube is in an environment that the temperature is changing. So, I considered all the tube nodes as spcd and spc_temp with the room temperature and applied a variant thermal load. ( I hope it would be a correct way to apply the mentioned BC & load, if it is not, please give me some tip )
Thank you so much for your time and attention,
I am looking forward to hearing from you
Answers
-
Could you also share the .fem and .out fie of the run?
0 -
sure, thank you in advance.
0 -
Dear Rahul,
the problem solved and I finally got a simulation run. But I have 3 further questions and would really appreciate if it is possible for you to help me to proceed.
1) For the thermal load, I gave 1 to spcd as I found it works like a coefficient for the temperature load. ( when I gave 10 to spcd, the temperature load would be 10 times higher.) Am I wrong? Also, I gave spcd (1) and spc_temp (20 centigrade) to ALL of the nodes of the tube. Is that correct? The results are not reasonable! since the stress-strain plot will drop by increasing the temperature!
2) In the real condition, the initial temperature for the tube is 20 centigrade and the ambient temperature increases from 20 to 200 and then decreases. I did not define CHBDYE surface elements and I am not sure if convection condition should be defined for this problem or not!
3) In my experimental work, the temperature would increase from 0 to 200 centigrade, then the temperature would be kept constant (200) and the mechanical load will apply. After that, the mechanical load will be kept and the temperature will decrease to the room temp. How can I do these kinds of multiple step analysis? ( I have read the tutorial file for optistruct thermal analysis but didn't find anything regarding this issue)
Thank you for your time to read my questions. It would be great for me if I had your suggestion.
Cna
<?xml version="1.0" encoding="UTF-8"?>
0 -
Dear Cnaaaaa,
In your previous model I found load collector 8 (spcd) & 9 (spc_temp) haven’t any use. Load Collector 11 named as Loadcol1 is also empty.
However u made changes and simulate the behavior.
1) Whatever value u r defining in spcd is nothing but temp. value.
As u said - “Also, I gave spcd (1) and spc_temp (20 centigrade) to ALL of the nodes of the tube”,
U have to provide value only in spcd not in spc. Spc will automatically consider same temp which is given in spcd. If u provide in both there is something wrong (as ur mini temp result is in 10-15 power).
2) Yes u can simulate for variable ambient temperature behavior.
3) Here of course u can go for such transient tube & ambient thermal loading but it will compatible with your transient mechanical loading or not. I don’t know.
As u said - 'in between thermal loading, the mechanical load will be kept and the temperature will decrease to the room temp.” It is clear u have to give time dependent mechanical loading once temp rises to 200.
0 -
I appreciate your kind help. However, I am a little confused!
According to the attached file, SPCD plays the role of 'A' which is a coefficient and not temp.value! on the other hand, according to the explanation below the formula, it is time dependent temperature BC.
My purpose is the simulation of high temp tensile test. could you please let me know how I should consider the thermal BC? Sorry, but I did not understand what you mean when you say 'U have to provide value only in spcd not in spc. Spc will automatically consider same temp which is given in spcd'.
Thank you very much for your time and help,
Cna
<?xml version="1.0" encoding="UTF-8"?>
0 -
Dear Cnaaaaa,
Here A is an constant value which you want to make time dependent. In your problem u want to make Temp as time dependent with the help of Tload & Tabled card. So for that temp has to be define via SPCD card in constraints (that will not consider now constraint, now it is a entity that can be vary).
Plz have a look in image below.<?xml version="1.0" encoding="UTF-8"?>
Altair Forum User said:Sorry, but I did not understand what you mean when you say 'U have to provide value only in spcd not in spc. Spc will automatically consider same temp which is given in spcd'.
When u define SPCD u also define some D value like in below image-
<?xml version="1.0" encoding="UTF-8"?>
This Value is ur temperature value actually. And has to be define in only SPCD field. In SPC u have to make it zero.
Hope now u will able to run simulation- If still problem u r always welcome.
0 -
Dear Gagendra,
Thanks so much for the time and clarification.
So, here SPCD is excited field or amplitude A for the dynamic thermal load which is defined in TLOAD1. Would you please let me know how I can apply this dynamic load to the ambient node? It seems that it applies directly to the structure which is not desired for my simulation. I tried to define a variant ambient temperature by Analysis>Temp>load (load collector = TLOAD). But it did not work.
Could you please help me how I should apply the BC such that the thermal load be applied to the ambient node? ( so after that I can define SPC of 20 on the tube's nodes and CHBDYE4 elements for convection). It would be great if you let me know if I am on the right track.
many thanks for your attention,
Cna
0 -
Dear Cnaaaaa,
As i know u r well aware to load collectors. So im uploading here a load collector flow diagram which u will understand easily. If any doubt u can ask.
- We have two TLOAD collector (One for Ambient temp, another for Pipe temp), but in Loadstep u can define only one, to do that we will make another loadcollector DLOAD and add both collector in it.
- Here S value for DLOAD is scale factor so keep it 1.
- We have two SPC collector (One for Ambient temp, another for Pipe temp), but in Loadstep u can define only one SPC, to do that we will make another loadcollector SPCADD and add both collector in it.
<?xml version="1.0" encoding="UTF-8"?>
Apart from what collector u have to select in Loadstep..below image will help u.
<?xml version="1.0" encoding="UTF-8"?>
Be helpful to everyone
/emoticons/default_smile.png' srcset='/emoticons/smile@2x.png 2x' title=':)' width='20' />
0 -
Dear Gajendra,
Many thanks for your nice reply. It was really helpful and exactly what I wanted
Best,
Cna
0 -
Dear Cna,
Always Welcome.
Plz let me know after run ur simulation. It will also helpful for me if u share experimental data with me if possible. You can contact me at gkn0504@gmail.com
0 -
Dear Gajendra,
I really appreciate your interest but i am afraid to say the work is confidential and I am not able to share the data. It is also on composite material and I found that optisruct does not support transient thermal analysis on composites! However, I hope to share the final result to check the accuracy of the simulation.
Best,
Cna
0 -
Dear Cna,
Its ok. I understand the confidentiality.
I also never try with composite. If something like that u found, share with me.
0
