thermal analysis and load

[mirred]

A question:

i have a force over a  copper beam and i change the temperatur of beam:

To change the temperature of beam I use the "reference temperature without stress"

1. F=500 N; T=100 °C ->   deformation = 0.05050415 mm

2. F=500 N; T=150 °C ->   deformation = 0.05050415 mm

3. F=500 N; T=300 °C ->   deformation = 0.05050415 mm

3. F=500 N; T=600 °C ->   deformation = 0.05050415 mm

...

hmmm ... there is a problem ... if I increase the temperature I want to see a increase deformation with a definite load; is it correct?

thank's

mir

[bjorn_fallqvist]

Hi,

Did you choose a material from the Algor material library? I recall that some of the materials do not have a defined expansion coefficient, so that may be the problem.

Björn

[John_Holtz]

Hi Mir,

Can you provide a little more detail, such as

1. What type of analysis are you doing? (Linear? MES?)
2. How is the beam constrained?
3. What direction is the force? (perpendicular to the beam? parallel to the beam?)
4. What direction is the deformation? (Magnitude? perpendicular to the beam?)

In Linear stress, these items are required for thermal effects on beam elements:

• material properties include the coefficient of thermal expansion.
• a temperature is applied to the beam which is not equal to the stress free reference temperature. This can be accomplished by applying a temperature load to the nodes, or by entering the default nodal temperature (somewhere) in the Analysis Parameters.
• assigning a nonzero Thermal multiplier in the Analysis Parameters.
• optionally, assign a stress free reference temperature in the Element Defintion.

(see the page in the Help "Autodesk Algor Simulation > Setting Up and Performing the Analysis > Setting Up Part 1 > Linear > Loads and Constraints > Temperature".)

You may also need to be aware that in linear stress, one load has no affect on other loads. So if you have a beam with pinned with a distributed load and temperature, the distributed load causes a maximum vertical displacement at the center of the beam. In real life, the thermal expansion of the beam will increase the displacement. In linear stress, the thermal expansion only causes an axial force; it does not create any vertical displacement. This is the definition of linear stress! (Another way to think of it is the method of superposition. Deflection due to force and temperature = displacement due to temperature + displacement due to force.)

MES or nonlinear stress has similar setup (except I believe the material model needs to be set to a value that includes thermal effects.) The difference with nonlinear is that the displacement changes the geometry on each step, which changes the stiffness, and so on. Once the force causes a little bit of vertical displacement, the thermal expansion will cause the bending to increase. The result is not simply the addition of the displacement due to the force + displacement due to the temperature. Hence, the solution is nonlinear!

Hope this helps.

[mirred]

I'm using Oxigen free coper with termic coefficient = 0,000017 1/°C ... 

[bjorn_fallqvist]

I see. As John asked, what kind of analysis are you running, and how is the beam constrained?

[mirred]

1. What type of analysis are you doing? (Linear? MES?)

LINEAR

2. How is the beam constrained?

join in extreme

|-------

3. What direction is the force? (perpendicular to the beam? parallel to the beam?)

perpendicolar to beam (in extreme)

          |

         v

|-------

[bjorn_fallqvist]

I'm not 100% sure what you mean with "join in extreme", but from your images it looks like the beam is fixed to a wall, and the force is perpendicular to it? Then the vertical displacement due to the temperature should be zero. The only influencing factor in this case is the vertical force. If you apply it parallell to the beam instead, I'm sure you will see a change in displacement.

[Joey.X]

 "Reference temperature" in stress analysis is used for "thermal stress", i.e., thermal expansion due to the temperature distribution in simulation domain.  Note that the local thermal expansion is proportional to the difference of local temperature and reference temperature".

 If user does not apply thermal loading (such as temperature result from another thermal analysis), changing reference temperature only will result no thermal loading, and user will see zero deformation change.

[John_Holtz]

Just to clarify for everyone's benefit, Jianhui's sentence from the previous post "changing reference temperature only will result in no thermal loading, and user will see zero deformation change" is not entirely true.

The nodes of a linear stress model always have a temperature. If the user does not apply any temperatures, the default temperature is 0 F. (The default is set under the Analysis Parameters, Thermal tab.) So changing the stress free reference temperature to a nonzero value will create a temperature difference 0 - Tref, thus creating thermal expansion.