uncoupled heat transfer analysis 1

[Goleon]

Hello,

i want to create a model for a presshardening simulation in Abaqus CAE. I planed to make the Die as a rigid shell and the sheet as a deformable solid. The sheet has a tempeature of around 900°C and the die has 20°C. I want to see, how the temperature behaves while the sheet is being deformed.

So first i wanted to know if it is somehow possible to solve the mechanical problem with an explicit solver and the thermal problem with an implicit solver? Or is abaqus maybe not the best program for this simulation?

I want to use surface to surface interaction but i'm not sure about the interaction propertys. Is it even possible to calculate the heat flux in the rigid shells?

Thank you
Konrad

 

[FEA way]

In this case it seems that it would be better to perform fully coupled thermal stress analysis. It’s possible with Explicit too.

Rigid bodies in fully coupled thermal stress simulations have temperature degrees of freedom (at their reference nodes).

 

[Goleon]

Thank you for your replie. I think i use the implicit coupled analysis then. but i'm still not shure how the interaction propertys should look like.
I've got tangential behavior (penalty) for friction and heat generation with default settings for the first test. How about thermal conductance?

 

[FEA way]

If you want to allow for conductive heat transfer between contacting surfaces, you just need the Thermal Conductance interaction property. Specify large value to simulate heat flow with no resistance (like with tie constraint).

 

[Goleon]

Hey again,

i have a problem with my simulation, so that i get zero heat flux all the time.
I'm not sure what the problem is, i use kg,mm,sec,N and the conductivity of my deformable sheet material is set like

0.0307 20
0.0300 200
0.0217 400
0.0236 600
0.0255 800
0.0264 900

The conductivity of all the rigid parts is 0.02 but i'm not sure how to set up the thermal conductance in the interaction property? Can i set it like

1 0
0.7 0.2
0 1

or do i have to type in like above? but is it then dependent on temperature and the gap?
I'm sorry, i haven't done a heat transfer analysis before.

 

[FEA way]

When you define Thermal Conductance contact property you have to specify the value of thermal conductance at 0 clearance (when surfaces are not separated) and the value of clearance at which thermal conductance is zero (no heat flow between the surfaces). You can also define more pairs of conductance-clearance data. Temperature dependence can be added as well.

 

[Goleon]

Okay, i understand that and like above i did set a value for 0 clearance and two other values (just for testing). But do i have to write the value at a clearance of 0 like "1" oder do i have to type the Value in W/(mm*K)?
And i saw, that i can set a temperature dependance in the contact property as well, but i wonder what will happen with the conductivity Data (temperature dependent) in the material property?

 

[FEA way]

Thermal Conductance defined for contact interaction and Thermal Conductivity defined as material property are two different things. When using SI(m) unit system, the former is specified in W/(m^2*K) while the latter is specified in W/(m*K). Thermal Conductance determines conductive heat transfer in the interface between contacting parts. Thermal Conductivity determines conductive heat transfer within the part.

 

[Goleon]

aaah, thank you. That was confusing me all the time. Now everything is clear, i hope i can eliminate my "zero heat flux" error now.