 ## General Mechanical

#### What does ‘An unknown error occurred during solution. Check the Solver Output on the Solution’ mean

• phanicmsf
Subscriber

What doe the error messages mean in ansys solution information.?

I am able to solve the problem setup using Structural steel material for both geometries. But when I applied different materials Sic_Pores and Sic_Sic for each geometry I got the fallowing error.

• peteroznewman
Subscriber
It looks like you are simulating the thermal strain created by cooling down a composite material from 1326 C to 20 C.
I assume the two materials have zero thermal strain at the beginning of the simulation, and the thermal strain develops as the materials cool down.
To accomplish that, you need to set the Environment temperature to 1326 C since that is the zero thermal strain temperature for all the bodies.
What you have done by leaving the Environment temperature at 20 C is that is the temperature where there is zero thermal strain, then in step 1, the temperature increases to 1326 C, causing massive amounts of thermal strain, which turns elements inside out.
Under Analysis Settings, turn on Large Deflection.
• phanicmsf
Subscriber  Thank you for your explanation.
Does the 'Zero-Thermal-Strain Reference Temperature' in the Engineering data of the material and the 'Environment Temperature' in the menu detais of static structural should be same ?
Is it correct defining 'Zero-Thermal-Strain Reference Temperature' and'Environment Temperature' as 1326 ?
• phanicmsf
Subscriber

a) SOLVING THE ANALYSIS WITHOUT APPLYING MECHANICAL LOADS. ONLY THERMAL CONDITIONS ARE APPLIED --> Cooling the body from 1326 to 20 C. (After solving for the case a) After simulating the thermal strain created by cooling down a composite material from 1326 C to 20 C. I would like to apply mechanical loads
case :1 ) Compresive unit loads
and want look for the stresses distribution.

b) Shall I need to apply mechanical loads in the same analysis where I specified Cooling Thermal conditions ? Shown in the tree below
Thermal condition---> has cooling curve with time
Displacement--> has symmetry zero displacements in each of respective plane.
Force ---> Unit load acting on each face of the outer cube (Compressive unit loads)

In this case the resulst I got is same like solving the analysis without mechanical loads.  When there are mechanical loads in addition to uniformly cooling two different materials having different CTE(as a function of temperature) the stresses I would expect should be higher then the stresses got in the simulation without mechanical loads.
Can anyone explain why I am getting the same results in both cases? Is there any mistake in model setup ?

• peteroznewman
Subscriber
Is it correct defining 'Zero-Thermal-Strain Reference Temperature' and 'Environment Temperature' as 1326 ? Yes.
Run a model with no change in temperature and apply the mechanical load, what is the stress? Compare that stress with the stress from the temperature change. What is the ratio between the two stresses?
If the stress from mechanical load only is 1000000 times smaller than the thermal stress, and you only show 5 digits in the stress result, it will seem as if you get the same result in both cases.
To apply a mechanical load after the cool down, simply add another step, keep the temperature constant at 20 C and change the load from 0 in step 1 (or more) to the load value you want in the last step.

• phanicmsf
Subscriber
Thank you. 