equivalent mechanical load

[kotawsu]

suppose a bar is subjected to a temperature change. I run a thermal analysis to get the temperature distribution in the bar. Later on i want the equivalent mechanical load tht would stress the bar by the same amount. How could i obtain that load? i know that sigma= alpha*delta T where delta T is the temperature difference. But the thing is I have different temperatures at different points in the bar. Could any one tell me how to go about it? Thanks
Kota

 

[PamCrash]

Idea:

- Fix all degrees of freedom at all nodes (*Boundary,....)

- Apply stress distribution obtained by thermal analysis to your fully fixed model using *InitialConditions,Type=stress and run a static analysis

- Output the reaction forces and moments. These are the mechanical loads which generates the same stress distribution than the thermal analysis. Possibly that's what your looking for.

Pam

 

[kotawsu]

hey pam..thanks a lot for ur suggestion. it sounds like it should work. i shall try it out.but i have one question.how do i write the stress distribution obtained by thermal analysis to a file. if i am right it should be a .fil file right.and should i input those stresses in in the initial step or the step-1 when i am running my static analysis??

 

[kotawsu]

i tried using the *initial condition but i am not able to figure out how to direct the stresses from the thermal analysis to the present static analysis...

 

[kotawsu]

i got this error
***ERROR: THE FILE PARAMETER IS ONLY VALID FOR INITIAL CONDITION TYPES
TEMPERATURE, FIELD, AND PRESSURE
CARD IMAGE: *initialconditions, type=STRESS, file=al_thermalstrain
*Step, name=load
*output, field
*output, history
*Step, name=load
*Step, name=load
*static
*output, field
*contactoutput
*elementoutput
any idea of whats wrong??

 

[PamCrash]

Since youre using beam elements it couldn't be so difficult. I recommend to output the stresses to the dat file, extract them (editor, awk or whatever) and include them into your input file like described below. Try it first with a simple test model to be sure that it will work

Pam

Data lines for TYPE=STRESS if the GEOSTATIC, REBAR, SECTION POINTS, and USER parameters are omitted:

First line:

Element number or element set label.

Value of first (effective) stress component, axial force when used with the *BEAM GENERAL SECTION or *FRAME SECTION options, or direct membrane force per unit width in the local 1-direction when used with the *SHELL GENERAL SECTION option.

Value of second stress component.

Etc., up to six stress components.

Give the stress components as defined for this element type in Part V, “Elements,” of the ABAQUS Analysis User's Manual. Stress values given on data lines are applied uniformly over the element. In any element for which an *ORIENTATION option applies, the stresses must be given in the local system (“Orientations,” Section 2.2.5 of the ABAQUS Analysis User's Manual).

Repeat this data line as often as necessary to define initial stresses in various elements or element sets.

 

[kotawsu]

pam, actually i am using solid elements. and if i define an element set and then would want to give the stress values i would not be able to because each of the element has a different stress value. like its not uniform. so in this case how do i input the stress value?

 

[PamCrash]

Try this: Use a dense mesh and output stress at the centroid of the element. So you have only one stress tensor per element. Should work if mesh is dense enough in areas with high stress gradients.

Pam

 

[MattSmith]

kotawsu,

Following on from Pams idea, simply add another step to your analysis. Fix the displacements from your first thermal analysis step using '*boundary,fixed' and fix the degrees of freedom as pam suggests. This should hopefully give you the loads you're after as reactions.

Matt

 

[kotawsu]

Hy matt..thnx for ur suggestion.will try that out. i couldnt try what pam said as i have lot of temperature gradient through out the structure so i cant use one stress value to represent the whole structure and hence i couldnt use the intial condtions, type=stress. But i guess what you said is much simpler.thanks

 

[kotawsu]

just one question...should i just give the *boundary fixed card in my secodn step or should i give any data line to say that i want the displacement form the thermal analysis to be fixed.