Electronical and thermal analysis

  • 999 Views
  • Last Post 15 February 2019
ranked posted this 12 February 2019

Hello everyone,

I have to do the following simulation:

Heating source is a copper conductor path with an aplied voltage. This is "printed" on the surface of a substrate.

I want to know how long it takes, to heat the substrate, which electricity is needed an how long it takes until the substrate is cooled down again.

Boundary conditions are heat transfer in the sustrate, convection and thermal radiation on the surface of the substrate. And the voltage on the conductor path. 

Which tool can I use for this case?

Thanks a lot in advance.

Order By: Standard | Newest | Votes
jj77 posted this 12 February 2019

I suppose thermal-electric in workbench mechanical.

 

Not sure if there is an act for that, oterwise use a transient thermal, and add element

et,1,226,110         ! 20-node thermo-electric brick

then, apply a voltage on a face say called vf, via d,vface,volt,12

and other thermal BC and run.

There is an ansys example called thermo-electric cooler analysis.

 

if you need to look at forced cooling and more complex flow (not only natural convection), then perhaps you might need to dig a bit into other ways (perhaps even CFD, Fluent,CFX,..).

 

ranked posted this 12 February 2019

Thank you for your answer. Can you give me a hint, where I can find the ansys example called thermo-electric cooler analysis? I will try this first. 

jj77 posted this 12 February 2019

It should be in the help manual. just search  thermo-electric cooler analysis:

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v192/ans_cou/Hlp_G_COU3_thermele.html%23couthermelecooler

(copy paste this into the ansys help browser).

 

Also have in mind that if you are using WB and not apdl, then you would need to input some commands snippets, like mentioned in my previous post.

ranked posted this 12 February 2019

Acutally I am working with WB. How and where do I have to input the commands?

jj77 posted this 12 February 2019

There is also a heat generation BC in transient thermal, that might just be easier to use instead of doing this coupled analysis.

For the commands I do not know, where exactly to put them since I never done this either.

Hopefully someone else can help, or if you can find a tutorial on the internet.

peteroznewman posted this 12 February 2019

I agree with jj77 that you should make your first model in Transient Thermal..

Do you know the resistance of the copper trace on the board?  If so, you can calculate the power dissipated P = (V^2)/R. Divide that by the volume of the copper for your Internal Heat Generation.

Then you have to apply convection BCs.  You will have to do some research to estimate a good Convective Heat Transfer Film coefficient. If you can't find a good estimate, do a parametric study to see how much the results change over a range of Film coefficients. You can add radiation BCs. I haven't had to use those. How hot do you expect this substrate to get?

The alternative is to build a CFD model to let the air convect away the heat. That way you don't need a Film coefficient as you are modeling the actual flow of air carrying away the heat on an element-by-element basis. That is a lot more work!

ranked posted this 14 February 2019

I have already done a Model in Transient Thermal. But there I applied a temperature on the copper trace, only to check my BCs. That already worked. 

But i still have problems to include the voltage. With the heat generation BC the Substrate gets much to warm. The trace should have 50°C and the Substrate on the opposite Surface, without the trace, should be 40°C.   

Is there any other possibility to do this Simulation?

jj77 posted this 14 February 2019

It should be OK, not sure why you are not happy with that. Joule heating should be prop. to J^2*rho, where J is the magnitude of the current density and rho is resistivity. 

 

The only way I can think since I am not sure how to add all the commands we discussed in APDL, is to run a thermal - electric in WB, which is steady state (K*T=Thermal load), transfer it in WB to APDL, and change it in APDL to a transient (KT+CT' = Loads). Also do not forget to add heat capacity (mat. prop.) in APDL since that is needed for the Global Heat Capacity Matrix (C).

 

I just tried that on a conducting rod/wire and it works.

 

Not sure if that will give much difference though to just applying the Joule heat as a heat source in thermal transient.

 

 

 

jj77 posted this 15 February 2019

Actually we do not have to go to APDL. just define the thermal-electric analysis in Workbench (all BC,....), and then we can convert it to be a transient analysis using the following command snippet (they should be placed under the Steady State Thermal Electric Conduction in the tree structure, which includes the BC and analysis settings). 

 

/SOLU

!

ANTYPE,4                     !Specify transient analysis

!

TIME,1000                       !Set time at end of load step (you need to change this as needed)

AUTOTS,-1                    !Program chosen automatic time stepping

DELTIM,10,10,10,     !Specify time step sizes (you need to change this as needed)

TIMINT,1 ! Transient effects on

KBC,1                        !Specify stepped loading (voltage is stepped up immediately)

!

 

Also as I said thermal heat capacity needs to be defined for the materials (say under Geometry in the tree structure, and the relevant part/body enter a command and use this: mp,c,1,400,, where 400 is the actual value).

OUTRES,ALL,ALL               !Write to file at every step

Close