Problem with GBI file when using "heat sink" material

[Anonymous]

Dear Forumers and Supporters,

I am having the following problem regarding the heat sink material.

Purpose of simulations: I am trying to simulate scale and optimise a custom heat sink to specific power transistor. Thus, I have the following componenets:

1. Simplified block for power transistor;

2. Simplified block for heat sink

3. Simplified fan;

4. CFD generated air volume;

I did the following steps to set up the simulations:

1. Adding materials:

a. Power transistor - Solid - Copper

b. Heat sink material and customised parameters of the heat sink, as shown in the Autodesk CFD Help menu

c. Internal fan material with certain characteristics

d. Fluid Air and environment "variable" to the generated air volume

2. Boundary Conditions:

a. Volume boundary condition with total heat generation: 300W

b. No boundary conditions to the heat sink

c. No boundary conditions for the fan

d. Pressure Pa=0 to all external surfaces of the air volume

3. Initial Conditions:

a. Volume t=30C  to the air volume

4. Meshed Automatically and then reduces mesh element by 50% for the heat sink.

5. Solver Manager Options:

a. ADV5

b. Steady State Solution Mode

c.300 Iterations to run

d.Flow and Heat Transfer - ON

e. Gravity set to -Z

When i tried to run the simulations i get the following message: GBI File " Check if a problem occured while generating the mesh, and fix geometry as necessary. 

I did try to use Autodesk Help manager to solve the problem but nothing appeared to work....

I tried different scenarios and refinements of the mesh: Also no result

Then i experimented with using not a "heat sink" material but "solid". 

The conclusion was: Whatever i do i can not make the simulation run with heat sink material. But the moment i remove/change it from the simulations - it starts generating results. 

I am pretty sure there is a way to run, because there is such option and it is recommended. Unfortunately, I am unlucky so far....

I am eager to read your replies and your assistance!

Best regards,

Bozhidar

P.S. I am adding the cfz file, hope you can make it run !

[David.Short.]

Good morning @Anonymous,

Please can you send a .cfz file as you have sent a .cfdst file by mistake.

Then I will take a look!

All the best,

David

[David.Short.]

Hello again,

To add to my previous post a colleague of mine has forwarded me this article which seems to be describing your issue.

Let me know if it proves useful.

Thanks,

David

[Anonymous]

Hello David,

Sorry for the missing file. Here it is ! 

To your 2nd statement  - i did use this help guide in order to achieve a result but could not come up with a solutions.

Best regards,

[matt.bemis]

Hi @Anonymous,

I think you are getting this error due to the heat sink material. I bet if you made this volume copper instead, it would solve. There are a lot of specific constraints while using the heat sink material. The approach surface needs to be in the same parallel plane as the exit plane. In your model your approach surface and exit surface are perpendicular. In your simulation, the "exit" surface is the surface which has the copper chip and heat load on it. 2 issues here. 1. the cross sectional area of approach and exit surface are not the same. 2. There's an obstruction on the exit surface- the copper chip.

Here's an image of how the heat sink material is supposed to be used. 

But instead you are trying to model something like the heat sink of this Nvidia board:

The only way to do this would be to actually CAD the real heat sink and assign the material as copper or aluminum (whatever the real solid is made of). This is not a good application for the heat sink material. Check out this and this link to some help documentation on heat sink materials. 

I hope this helps. Please let me know your thoughts.

Thanks, 

[Anonymous]

Thank you very much for the detailed overview ! You are right ! When I enter the CAD model and assign material Copper  and solver manager to  "transient", then the simulation goes on. I thought there might be a simplified way to simulate the real heat sink but as i understand, in my specific application, this is not possible. 

Regarding your advice, I are 2 concerns I have:

1. The processing part is long - i wanted the simulation to run for 20min to see how the heat sink will react . However, for 14h i have reached only 119 iterations. 

Question 1: Is there a way to optimise the simulation in order to obtain results faster?

2. When i checked how the air was flowing around the heat sink i noticed that the air, generated by the fan, actually goes through the heat sink. It does not goes out form left and right. I think, this might be the reason why i am not getting accurate results. But I could not manage to make it realistic so far...

Question 2: How to set up the simulation in order to get logical and realistic solutions ?

We can ignore my first concern as long as there are accurate results 🙂 

What is your opinion and how would you tackle such challenge ?

I have attached the .cfz file for your assistance. 

Best regards,

Bozhidar

[Anonymous]

Thank you very much for the detailed overview ! You are right ! When I enter the CAD model and assign material Copper  and solver manager to  "transient", then the simulation goes on. I thought there might be a simplified way to simulate the real heat sink but as i understand, in my specific application, this is not possible. 

Regarding your advice, I are 2 concerns I have:

1. The processing part is long - i wanted the simulation to run for 20min to see how the heat sink will react . However, for 14h i have reached only 119 iterations. 

Question 1: Is there a way to optimise the simulation in order to obtain results faster?

2. When i checked how the air was flowing around the heat sink i noticed that the air, generated by the fan, actually goes through the heat sink. It does not goes out form left and right. I think, this might be the reason why i am not getting accurate results. But I could not manage to make it realistic so far...

Question 2: How to set up the simulation in order to get logical and realistic solutions ?

We can ignore my first concern as long as there are accurate results 🙂 

What is your opinion and how would you tackle such challenge ?

I have attached the .cfz file for your assistance. 

Best regards,

Bozhidar

[Anonymous]

Dear @matt.bemis,

I used you advice and tried to make a simulations with heat sink material, according to your suggestions. It is now works fine, but i am getting inadequate results.

You can see the attached file below !

Please, advice me in this situation how can I improve my simulation!

Thank you in advanced ! 🙂

Best regards,

Bozhidar

[David.Short.]

Good afternoon @Anonymous,

So it looks like you have now implemented the heat sink material correctly however this is not modelling the setup which you initially provided us. Can you please expand on why the results are inadequate?

To model your system (fan blowing directly onto top surface of heat sink) Autodesk's heat sink material is probably not suitable. Instead model the sink completely (as you have done in the test 3 model). Then to improve the simulation a few suggestions are:

1. Define an inlet and outlet to your external system as having p=0 everywhere might be confusing for the software. 

2. Assign a temperature value at the inlet.

3. Create CAD volumes to model the channels in the heat sink. Then you can have more control of the meshing. Try to have at least 5 elements across the width of each channel (i.e. between the fins).

4. Model a shrouding around the fan to improve its performance, such that air flow is not escaping out of the sides of the fan. 

5. Apply a uniform mesh to the fan with minimum 4 elements between the fan inlet and fan outlet.

6. Maybe make air fixed (rather than variable), as forced convection is dominating.

Also i would suggest firstly running a steady state flow only analysis than turn off flow and solve heat transfer transiently. This would mean that initial conditions are not required.

I hope this helps a little.

All the best,

David

[Anonymous]

Hello @David.Short.,

If i understand you correctly, you are suggesting the following:

To model volumes in Inventor between the fins, which will represent the air gap between the fins.

2nd, if i want to stick with simulating the air flow as it works on PC mother board, i should model the heat sink in details.

3rd, best way is to use "Solid" as material and define the material properties;

4th. It is better to define one inlet and one outlet with Pa=0 respectively;

5th, i can try air to be with fixed environment.

6th, i can try do both simulations separately - one for flow analysis and one for thermal.  - But in my case the air flowing around the heat sink, should cools it. Isnt using such method would affect the actual results ?

To my statement why i get inadequate results:

When i am trying to simulate my heat sink with the "heat sink" material properties i get temperature exceeding 35000 deg C. 

As you can see from the file below, i am defining one outlet of the external air volume with Pa=0, and one inlet with Pa=0 and Flow = 2000 l/min.

What happens is that if I use "steady state simulations", the results goes crazy in respect to the temperature.

If I use "transient"  - then there is no heat transfer from the power resistor to the heat sink - i see that only the transistor is heated up.

If I do not use the heat sink material - i did not get such results.

I will try what you were suggesting and tell you about the results ! 

What are your suggestions for fixing the simulation, using the heat sink properties? How does the simulations work on your machine ? 

Best regards,

Bozhidar

[David.Short.]

Hi @Anonymous,

Thank you for your very clear response. Yes you understood me perfectly.

To answer your question regarding separate simulation:

You are correct the air flow is cooling the heat sink. However because the flow supplied by the fan is constant the effect of the flow should be completely accounted for just using the converged flow results. When HT is turned on the flow is still there but simply not varying thus its effect on the temperature is included.

You only need to calculate flow and HT simultaneously is the heat itself actually drives some parts of the flow (as is the case with natural convection). For your system it is fair to assume that forced convection dominates, thus HT and flow can be solved separately to save on run time.

I will have a look at your model and get back to you shortly regarding using the heat sink material.

All the best,

David

[David.Short.]

Hello @Anonymous,

I think the problem with your simulation using the heat sink material is that the chip has a different cross section to the heat sink cuboid. 

You should instead use a two part model for your heat sink. One cuboid to represent the fins and one to represent the base plate. 

Here is a good example of what I am suggesting. As you do not have a spacer simply give the lower cuboid the same thickness as your heat sink base. Then in the heat sink material editor apply base thickness zero.

Thanks,

David

[David.Short.]

Hi @Anonymous,

Another issue with your heat sink material simulation is the boundary condition implementation at the inlet.

Firstly, you should apply either a flow rate or a pressure BC at a boundary not both as the flow rate will affect the pressure and vise versa! So remove the p=0 at the inlet. 

Secondly at an inlet to a system where heat transfer will be solved a temperature BC must be applied, think of this as the ambient temperature being inducted into the system at the inlet. If there is no temp the solver won't know what to do!

Hope this helps,

David

[Anonymous]

Hi @David.Short.,

I will try what you are suggesting tomorrow! I looked in details the link you gave me but I do not understand one thing - From the example they attached the same heat sink material to both blocks ? 

Should I use two different custom heat sink materials - One representing my fin design with base thickness = 0 and One representing the whole heat sink - base thickness and fin design  ? 

Or I create one heat sink material with specified base thickness = 0 and use it nevertheless one block represent fins and the other represents my base ? In this case, how the system when there is mo base plate defined?

Or should I define the base plate with solid material and only the fins with heat sink material ?

Best regards,

[David.Short.]

Hi @Anonymous,

No need to model two separate heat sinks when your system only has one! I am saying you need to model your heat sink as a two part model (one for the base and one for the fins)! Use a solid material for the base and heat sink material for the fins.

Try and do as in the screenshot attached but as you don*t have a spacer the lower part should just be the thickness of your base. You can assign which ever type of material you would like to the base part and then use the heat sink material for the fins.

I suggest this method as the heat sink material works best when whatever is below it has the same cross sectional area (footprint). 

Also 300W is a lot of heat for such a small chip. Are you sure this is realistic?

Thanks,

David

[Anonymous]

Dear @David.Short.,

In the attached file i did the changes you suggested. However, probably some parameter is missing because during simulation, the heat is not transfered to the simulated heat sink material (see the attached screenshots). 

What might be the reason for that?

About the chip  - yes, there is such power transistors that generates tremendous amount of heat - at the moment to be exact i have calculations that the total heat generation is 683W. If you are interested in such technology, I offer you to look in the RF power transistor amplifiers. This would be a great help menu or video lesson for simulation ! 🙂 

I am waiting for your reply !

Best regards,

Bozhidar 

[Anonymous]

I will finde you