[Olds88]

Hi all,

I'm trying to mesh a finned heat sink for a conjugate heat transfer simulation. I'm using Pointwise and Fluent. I want to have good control over the element size between the fins so I've been trying to create blocks between the fins and then combine those with the fluid block. However, I haven't been able to combine the blocks. When exporting to Fluent, it doesn't recognize the fluid between the fins. It just treats the heat sink and fluid between the fins as one entity.

How should I create the blocks so that I can control the element size between the fins and then combine them with the surrounding fluid so that I have small fluid elements between the fins?

Thanks,

Eric

[pdp.aero]

Hi,

After you created your blocks including the fins and the space between them which indicates the fluid volume, go to the CAE, Set Boundary Conditions. Please refer to the connections.jpg in order to following the instruction, attached at this post. I have simplified your problem with 2 blocks, one for solid and one for fluid. Following this further, you will have a domain between a fin and the fluid. In other words, you have a connection between the solid and fluid which is needed to be specify. Therefore, check the select connections in the Set Boundary Conditions panel. Then, select all the connections you are going to specify from the list, below the select connections, both in the opposite and same direction. Click the New. Choose a name for the connection and check the tiny box, left side of the connection name.

Next, you need to specify the volume conditions, so go to the CAE, Set Volume Conditions. Click on New, type your volume name, and specify the type of the volume which means fluid or solid. Please refer to the volume_condition.jpg which illustrates this step.

Finally, in the fluent, you can specify the condition in the Define, Boundary condition for your solid or the fluid.

This is what I understood from your problem. If you meant any other points, please correct me. Besides, a picture from the fins and the surrounding fluid volume would be helpful.

Bests,
PDP

[dgarlisch]

Please be aware there are some issues dealing with solid/fluid heat transfer interfaces when exporting from Pointwise. Depending on the complexity of your grid, there are some workarounds. Take a look at the items below. Ask, if you need more information.

I don't know much about using Fluent, so maybe someone more experienced can give more detailed instructions.

Pointwise has two FLUENT exporters:

ANSYS FLUENT (legacy)

• Ported from Gridgen
• Provides the same functionality as in Gridgen
• Supports porous BC types
• Does not support trex cell combination
• Does not support mirror at export

If you set the BCs for an interblock connection to Porous Jump, Radiator, or Fan, the exporter will ensure that the domain at the interface does not have its points cloned. This allows ANSYS FLUENT to create “shadow patch pairs” on import. This “trick” makes these types of interfaces easier to deal with in ANSYS FLUENT.

In Pointwise, apply a BC to only one side of the internal domain. This BC must be set to one of Porous Jump, Radiator, or Fan.
Export using ANSYS FLUENT (legacy).
In Fluent change this BC to a type "wall". Ansys creates its "shadow" automatically.

ANSYS FLUENT

• Implemented as a plugin
• Supports trex cell combination
• Supports mirror at export
• Does not support porous BC types

Currently, plugin exporters always inflate (clone) grid points on interblock connections that have BCs applied. We already have two feature requests logged (SPRs 15563, 15477) that deal with adding this capability to our plugin SDK.

You must use the plugin exporter if you need the trex cell combination or mirror at export functionality.

In Pointwise, apply the BCs to the solid/fluid connection domains. These regions will be inflated at export.
Export using ANSYS FLUENT.
In Fluent, you must select the appropriate zones and merge them. This should also create the shadow patches you need.

[Olds88]

Hi guys,

Thanks a lot for your help I was able to get the hang of what I needed to do from your input and suggestions.

I'm having another related issue that maybe you can help with. Now I'm trying to model a heat sink with a small heat source attached to the bottom. I'd like them to be separate blocks so that the source generates heat which is dissipated into the heat sink.

I can create the blocks between the fins of the heat sink. But now I would like to create a block that surrounds the heat sink and the heat source at the bottom to represent the rest of the fluid. I have attached a picture of the geometry to help visualize. The small block at the bottom of the sink is the heat source.

Once I make blocks for the heat sink, the heat source, and the fluid between the fins, how do I make a block that encompasses them all to represent the rest of the fluid? I'm trying to use the assemble special: block, feature. I can create a face for the boundaries of the flow (inlet, outlet, etc.) but, I'm having trouble creating a face to go around the contours of the source and sink. I've attached a picture trying to show my problem here too.

I appreciate your help. Sorry if these are dumb questions, I'm relatively new to Pointwise.

Eric

[dgarlisch]

I can't tell from the image. Does the heatsource have a "top" domain that is shared with (part of) the lower domain of the heatsink? If not, it needs to.

For the block that "encompasses the rest of the fluid" (the far field), you need to build a box of domains (or other appropriate shape) around the heatsink/source blocks. There is a glyph script that can build these shapes for you.

To create the far field unstructured block, select all the domains (ONLY domains) and press the assemble block toolbar button. Use can use the Create/Assemble Special/Block... menu item + Automatic tab if you want to change the settings.

Initialize the block after it is created.

FYI...

After you create the far field domains. You should be able to recreate the all the uns blocks with one command.

1) Create far field domains.
2) Delete any existing blocks.
3) Set grid mode to unstructured.
4) Select all domains in the grid (ONLY domains. Do not select any connectors!).
5) Choose Create/Assemble Special/Blocks... menu item.
6) Choose Automatic tab.
7) Check Create Interior Blocks.
8) Press Assemble Faces button.
9) Press OK button.
All blocks should be created including the blocks between the heat sink vanes.

[Olds88]

No, the top of the heat source, and the bottom of the heat sink each have their own domain. How do I make them share a domain?

[Olds88]

Never mind. I figured out how to make the source and the sink share a domain where they connect.

Now I have the blocks created for the heat sink, the heat source, the fluid between the fins, the fluid around the heat source, and the surrounding fluid (far field?) I have attached a picture.

When I'm defining the connections between the blocks, what should I set the connection type to? I have attached a picture where I'm creating the connection between the fluid blocks between the fins and the surrounding fluid.

[dgarlisch]

I am glad you figured out how to make the shared domain between the heatsink and heatsource!

if the fluid blocks between the fins and the far field fluid block are the same VC, you probably don't want to set BCs on those domains. They are just connections. With respect to the solution calculations, Fluent will treat the far field block and the inter-fin blocks as one big volume when they are connected by domains without BCs.

FYI...

Unless you need to handle the fluid between the fins in a special way (e.g. during solving or post processing), there is no need to have blocks between the fins at all!

Now that you have far field domains, you could:

1. Delete all the the blocks in your grid.
2. Delete the inter-fin block connection domains (the selected white domains in your image).
3. Select all domains (ONLY domains).
4. Auto-assemble the new blocks as described in my previous post (fill voids).
5. Initilize the blocks.

When done, the single, far field "fluid" block will include the space between the fins.

I hope this helps.

[Olds88]

I was trying to use the blocks between the fins to better control the element size in that area. However, it made things a little confusing once I exported to Fluent. Is there a better way to control the element size between the fins?

[dgarlisch]

Now you are getting into an area I am not very strong in. I hope others can give you better advice.

in general...

A proper starting surface grid (domains) is a requirement. The surface cell sizes must be appropriate for the volume cell sizes and resolution you need. I assume that in your case the heatsink surface domains would have smaller cell sizes, the outer far field domains would have relatively larger cell sizes.

There are various controls available in the iso block solver that set the decay rate at which cell sizes grow as they get farther from the surface.

if you need any boundary layer resolution, the tight space between the fins would be best handled by the trex mesher. trex also gives you the ability to use cell combination (tets to prism/pyramids) at export for lower cell counts.

FYI... Pointwise just announced this online tutorial (http://www.pointwise.com/videos/). You may want to participate.

[pdp.aero]

Originally Posted by dgarlisch

Please be aware there are some issues dealing with solid/fluid heat transfer interfaces when exporting from Pointwise. Depending on the complexity of your grid, there are some workarounds. Take a look at the items below. Ask, if you need more information.

Pointwise has two FLUENT exporters:

ANSYS FLUENT (legacy)

• Ported from Gridgen
• Provides the same functionality as in Gridgen
• Supports porous BC types
• Does not support trex cell combination
• Does not support mirror at export

ANSYS FLUENT

• Implemented as a plugin
• Supports trex cell combination
• Supports mirror at export
• Does not support porous BC types

Thank you David for the update. I used the one which supports the TRex. However, fluent shows a very poor performance with TRex, in particular when using it for boundary layer, having trouble with convergence, and also with cross sectional Cp distribution in compressible external flow cases. Although, fluent gives competitive results with structure grid topology and covering moving boundary apart from its speed up and convergence acceleration options. For these reasons without doubt I am converting TRex to Prism before exporting to the Fluent, like what Dr. Sideroff and his colleague did for
airflow over a golf club head.

Thanks again.

[pdp.aero]

Hi Eric,

Sorry for my delayed reply, I was a little bit busy. First, if you were interested in using a state-of-the-art solver instead of charismatic old-fashioned fluent, or even interested in overheating read this. By the way, is this a chipset with its heat sink? sounds very interesting. I had a little problem with my cooling system.

Back to the point, I gave your geometry a try, creating something similar to your heat sink and source. Although, you have a several options, like using complete unstructured grid or even high aspect ratio anisotropic tetrahedral meshing like what TRex is doing for boundary layer, because of the solver that you are using, I choose structured grid for the space between the fins, and part of the outside domain, then unstructured grid for rest of the domain. Besides, if I was right, and it is a chipset with its heat sink, not something very large like a building, you will running an incompressible solver, and you will have a velocity inlet, outlet( my recommendation is pressure outlet, otherwise you don't know the free stream pressure at end of the domain, which means you need to use outflow), and again pressure outlet for your horizontal side boundaries. Therefore, we will have rectangular-like boundary in overall. Another point, if your geometry doesn't have fillet or smooth part at the edges, you don't need a CAD file, you simply can create you geometry by creating the connectors. Please, find your answers in descriptions.

1- See the following picture, I created your fins' blocks with a script, written already for answering something similar here, also it has been attached at this post with the parameters that I set for your case, 1*1 square base section and 0.5 for height of the fins. After creating the fins with the script, change the dimension according to your needs and give the lower part the fins appropriate ratio according to your y+, as I did. The ratio that choose is 0.0001, again this depends on your Reynolds number and your desired y+ if your are using a turbulence model.

1-FINS.jpg

2- See the following picture for creating the blocks in the space between fins which indicates the fluid zone. To this end, after creating the fins, create a line connector between two fins, dimension the connector, give a ratio at both side according to your y+, if you had, or your initial delta s. Then, select the connector, and copy and paste it by pressing Ctrl+C and Ctrl+V. A window will open, go to the translate, and select the one side of the connector, and then a corresponding corner of the next fin. The copied connector will be placed at the next space. Again, repeat the copying and pasting with this connector, this time you don't need to specify the translation vector. Repeat this until creating connectors entirely for one side. Then, select all the created connectors at one side, and again do copying and pasting. This time, specify the translation vector for the opposite side of fins. Repeat this for two other sides to create the entire connectors at the space between fins. Next, select all every 4 related connectors for creating structure domain, which means every 4 connectors covering the space between fins at the upper, lower, left and right side of heat sink, and click on assemble domains. This will creates all the domains between fins. Finally, select all every 4 domains which covers the gap between fins, and click on assemble block for creating blocks at once.

2-FLUID_SPCBTW_FINS.jpg

3- See the following pictures for creating the lower part of the fins. This time, you will have connectors at the bottom of the fins in both side. Select all at one side, copy and paste it, go to the translate, and specify the translation vector according to your geometry. Do this for opposite bottom side. Complete the lower part by creating vertical line connector at all corners and copying the horizontal connectors at the side of the heat sink. Select every 4 corresponding domain for creating structured domain, and click on assemble domain. Do similar for creating the bottom block.

3-FINS_BASE_PRT.jpg

3-FINS_FLUIDS_BASEPRT.jpg

4- See the following picture for creating the heat source block. For this purpose, you need to separate the lowest structured domain according to your heat source dimension by selecting the domain, and going to the Edit, Split, and split the domain at two appropriate i location, click OK, then selecting the middle separated domain again and split it at two proper j location. Finally, select the separated domain, corresponding to heat source, go to the Create, Extrude, Translate, and translate it in proper direction and distance.

4-FINS_FLUIDS_BASEPRT_HEATSRC.jpg

Please follow the rest in the next post.

[pdp.aero]

5- See the following picture for creating blocks surrounding heat source at the bottom. Select one of vertical connectors at heat source block corners. Copy and paste it, then translate it in four corner of the heat sink. Create the horizontal connectors, assemble the domains, then assemble the block. You can see the heat source block in the middle of the picture surrounded by other structured blocks.

5-HEATSRC_SRRNDBLK.jpg

6- Next, we are going to create hemisphere-like structured domain around the heat sink, see the following picture. For this, create a circle connector around the heat sink, split it at 15, 35, 65, 85 %. Then, dimension the connectors according to their respective connector on the heat sink edges and create the structure domain.

6-OUTSTR_BASESEC.jpg

7- In this step we are creating a semicircular connectors. Please see the following picture for creating the connector. Then, select the horizontal connector which its center connect to the vertical semicircular connector, and go to the Create, Extrude, Path. Select the vertical semicircular connector as a path. Then, go to the Grid, Merge, and merge the connectors at the opposite side of the semicircular connector.

7-PATH_EXTR.jpg

8- In this step, we will splitting the side connectors which obtained through path extrusion in the previous step, and creating line connectors from the heat sink corners to these points, and give them a ratio at their heat-sink side, please see the next step picture to find out more.

9- In this step, we are selecting every related 4 connectors for creating the domains according to the following picture, and then every related domains for creating the blocks.

9-OUTSTR_BLK.jpg

10-In this step, we are creating the cube-like boundary, dimension the connectors, and creating the unstructured domains. Finally, we are going to the Create, Assemble Special, and select all the unstructured domains, then click on save face. Next, select all the structured domains which obtained from previous step and then click on save face for creating the unstructured block. Finally, we will selecting the empty block, then click on initialize. Please see the following picture to find out.

10-OUTUNS_BLK.jpg

[pdp.aero]

Sorry, due to attachment restriction, couldn't find a space to attach the script, find it here (fins.txt), and modify the parameters base on your needs. I am also clarifying your questions in the following.

Originally Posted by Olds88

Once I make blocks for the heat sink, the heat source, and the fluid between the fins, how do I make a block that encompasses them all to represent the rest of the fluid?

Please see the step 10.

Originally Posted by Olds88

How do I make them share a domain?

You don't need to share domains. You will have three zones, two solid, and one fluid. One solid zone including heat sink, one solid zone including heat source, and one fluid zone including the fluid volume, the wall between the heat source and heat sink could be set through boundary condition's thermal tab in fluent. Please, specify the zones in CAE, Volume Condition. Also, set the upper surface of you heat source which will connect to the heat sink as an interface, then in the fluent set an appropriate boundary condition, which is wall. Note, fluent by default specify the Wall to any boundary which has cells in one side and has not cells in other side, if they didn't specify by user already. In any how, if you couldn't do this, and you do share two domains over each other between the heat sink and heat source, you need to go to the Define, Define Grid Interface in fluent, select one domain from the heat sink zone, and another domain from heat source zone, take a name for interface and create the interface. Your domains don't need to be matched in this case. It will create an non-conformal grid interface between them, and they will have the hanging node value.

Originally Posted by Olds88

When I'm defining the connections between the blocks, what should I set the connection type to?

These is what you need for you problem, velocity inlet at the entry, pressure outlet at the end, pressure outlet at the side boundary, three zones, one interface between the heat sink and heat source, wall.

Originally Posted by Olds88

I was trying to use the blocks between the fins to better control the element size in that area. However, it made things a little confusing once I exported to Fluent. Is there a better way to control the element size between the fins?

Please refer to the step 2.

Also, see the step 8 picture here.

8-CNNT_FOR_OUTSTR.jpg

[Omish]

Hi, sorry I have no answer to your question. I wanted to ask how do you set thermal boundary conditions for you analyzation in pointwise?! I can't do that ,
and when I export it as a "cas." File to Ansys Fluent I can't go to mesh section and add any boundary conditions. Would you please help me with this?