Results stored at predefined time points in transient thermal analysis

[ywan459]

Hi there, 

I am working on a coupled simulation of the transient thermal analysis with static mechanical. I want to store the temperatrue results at a set of predefined time points, and then the results can be re-used as body temperature in the static mechancial analysis. 

I found there is no facilities in the GUI to define the export time points. Can someone please give me some hits of how to do this? Thanks. 

 

[dlooman]

OUTRES,,%array% is an APDL way.  In the context of the Mechanical gui there could be complication specifying all the time points to be used in the stress pass.  Also, if there are multiple steps in the thermal transient you need to make sure your command object is issued for every step.  Otherwise Mechanical will overwrite your OUTRES commands at the beginning of step 2. 

[ywan459]

 

Thanks. Blow is APDL code I used, it give an error message. I found only limited number of time points can be defined (may be only 12 points). 

OUTRES,erase
*dim,t_out,, 218 ! RESULTS OUTPUT TIME ARRAY, DEFINE NUM of POINTS TO BE EXPORTED.
t_out(1)= 100,32400,34500,49500,53700,65400,136800,143100,146700,147300,147900,148200,149100,150000,150600,152700,156000,156900,158400,159300,160200,162900,166200,169200,172200,173400,174900,175800,177300,179700,202200,204900,209100,211800,215100,218100,219900,220200,220800,221100,225900,243900,249600,263400,265800,271800,275100,276000,277500,279300,286200,288600,290700,291600,293100,294000,296700,298200,307500,318900,320100,325800,326700,327600,333600,336900,340500,343200,349800,351600,352800,353700,355500,358200,362100,363300,363900,364200,364500,364800,373200,373800,374700,375300,375900,376500,377700,378000,378300,384000,385800,387000,388500,388800,389100,390600,392100,392400,392700,393000,393300,393600,393900,394500,395100,396300,396900,397800,400800,412500,426300,427200,428100,429600,431100,431700,432600,434100,436800,437700,438300,439500,440400,441000,445200,446400,447300,448200,449100,449700,450300,454500,455400,456000,456900,464700,466200,471900,474900,477300,478200,478800,479400,481500,492600,494100,494700,495300,496500,497400,498900,501900,502800,505200,519300,520200,522000,550200,555000,560400,562800,563400,566400,567000,568200,569400,570300,570600,571200,571800,574200,582300,585300,586500,589200,591600,592800,594000,598200,600900,607200,608100,608400,612600,613800,614700,616500,619200,623400,634500,635700,638400,641700,648600,651300,654300,662700,670800,691200,703800,723300,725400,729600,744000,747000,753600,760200,766200,789000,792000,795000,800400,821400,837900,840600,849000,850800,864000
OUTRES,all,%t_out% ! OUTPUT RESULTS AT TIME SPECIFIED BY THE ARRAY

 

 

 

[dlooman]

The limit is 18 values.  You'll have to use multiple commands:

t_out(1)=100,32400,34500,49500,53700,65400,136800,143100,146700,147300,147900,148200,149100,150000,150600,152700,156000,156900

t_out(19)=158400,159300,160200,162900,166200,169200,172200,173400,174900,175800,177300,179700,202200,204900,209100,211800,215100,218100

t_out(37)=219900,220200,220800,221100,...

etc...

[ywan459]

Thanks. One more question. Assuming I have setup a relative large time step, and would Ansys Mechancial enforce to compute the time points within the time step? For example, I have a time step 300 seconds, the solver computes 100, 400, 700 second etc., I also want to export the results at 150 second, would solver compute 100, 150, 400, 700 second?