# Surface Mesh

## Introduction

Now that we have a geometry, we can start meshing it. We are using Pointwise to generate the surface mesh. This is not a full blown tutorial, more a walk through. If you want to learn more about it, their Youtube channel is highly recommended. You do not have to use Pointwise to generate an overset mesh. ICEM or an other meshing software would work as well.

## Files

Navigate to the directory overset/mesh in your tutorial folder. Either use the previously generated .igs file or copy it from the tutorial folder.


span.prompt1:before {
content: "\$ ";
}
cp ../../../tutorial/overset/geo/onera_m6.igs .


It is possible to script Pointwise. In order to use it, we have to download the script first. You can either download it here or copy it from the tutorial folder.

cp ../../../tutorial/overset/mesh/Semicircle.glf .


## Meshing strategy

Before we start meshing, we have to know how many meshes we create and where they overlap. For this tutorial, 3 different meshes are proposed: near_wing, near_tip and far. The following picture should give an overview:

Now we should estimate the cell count of the mesh. For the purpose of a grid convergence study (GCS) and debugging it makes sense to have differently refined meshes. To limit the amount of work, we will create the finest mesh and coarsen it multiple times.

Usually, the finest mesh is called L0 (level 0) and should have approx 60M cells for this geometry. If every 2 cells are combined in each direction, we get a coarser mesh called L1. This usually goes to L2 for production and L3 for debugging purposes. Additionally, there could be an intermediate level starting at L0.5. It requires a different surface mesh that is sqrt(2) coarser than L0. In this tutorial, we will start at L1 (~8M cells) and end at L3 (~0.125M cells).

## Mesh Generation

### Pointwise overview

If you start Pointwise, it should look something like in the next picture.

1. Object, Layer and Default control

2. Solver information

3. Selection control

4. View control

5. Fast meshing controls

You can control the main view with the following key- and mouse combinations:

zoom

Rotate your mouse wheel. The zoom centers around your mouse pointer.

rotate

Press ctrl and your right mouse button while moving your mouse.

move

Press shift and your right mouse button while moving your mouse.

### Setup Pointwise

Before we actually begin meshing, we have to set some standard values and import our geometry. At first, we set some tolerances for Pointwise

1. Click on File -> Properties

2. Set Model Size to 1. (It is enough, if the order of magnitude is similar)

3. Set Node to 1e-6. The value of Connector should automatically jump to 1e-6 as well

4. OK

Now we have to choose the proper solver. In my case it is CGNS with adf support. If you have compiled the MACH-Framework with hdf5 support, you can skip the last step.

1. Click CAE -> Select Solver

2. Make Sure CGNS is selected.

3. Click OK.

4. Click CAE -> Set Dimension -> 2D (That’s how surface meshes are called here)

5. Click CAE -> Set Solver Attributes (If you have hdf5 support, you can stop here)

6. Select adf for CGNS File Type

7. Click Close

Now we can import the .iges file we created in the previous tutorial.

1. Click File -> Import -> Database

2. Select your .iges File -> open

3. Make sure nothing but Units and From File is selected

4. Click OK

5. You will receive a warning that some entities could not be converted. Just ignore it and click YES

After those steps, the window should look like this (you should probably save at this point):

Few important Pointwise labels:

Block

This is a 3 dimensional Mesh

Domain

This is a 2 dimensional Mesh

Connector

A line constraining the extend of a Block or Domain

Database

An imported geometry

Spacing Constraint

This controls how the nodes lay on a Connector. Further down the line, the Connector controls how the nodes lay in a Domain or Block

### Prepare the Database

To make our live a bit easier in the coming mesh work, we first prepare the database a bit (take a look at the next picture to help guide you).

1. Select the whole database. Just draw a rectangle around it while your left mouse button is pressed

2. Click Wireframe -> Shaded

3. Click on Layers

4. Double click on Description and enter Geo

Because we have two overlapping meshes (near_wing and near_tip), we have to cut the database at an appropriate place. This will indicate where the near_tip mesh will start. The near_wing mesh will go right to the tip of the wing. But because ADflow uses an Implicit Hole Cutting Scheme we only have to make sure, that the near_tip mesh is slightly smaller than the near_wing mesh. This will ensure, that the overlapping region is approximately where we cut the database. In this way we are certain, the solver does not have to interpolate in a critical region (like the wing tip).

1. Click on Create -> Planes

2. Choose Constant X, Y or Z

3. Select Y and enter a value of 0.9

4. Click OK (Your view should now look like detail A in the following picture)

5. Select only the upper, lower and trailing edge surface by drawing a rectangle with your left mouse button

6. Click Edit -> Trim by Surfaces

7. Select your freshly created plane (detail A)

8. Make sure Tolerance and Advanced is unselected

9. Click Imprint (Your geometry should now have a different color towards the tip)

10. Click OK

Now we are doing some cleaning up and delete some unneeded surfaces.

1. Rotate your view with pressing ctrl and your right mouse button while moving your mouse until you have a good view on the root surfaces.

2. Select the first root surface

3. Press ctrl while selecting the second root surface

4. Press del on your keyboard to delete them

### Create the near_wing surface mesh

We create the mesh near_wing in a new layer to keep everything orderly.

1. Click Layers

2. Select Show Empty Layers

3. Click with your right mouse button on layer 10 -> Set Current

4. Double click with your left mouse button on the Description of layer 10 and enter near_wing

5. Unselect Show Empty Layers

Because we want to coarsen our mesh multiple times, it is important to think about how many nodes we should have on a connector (Apart from that, it is always good to be multi-grid-friendly). To calculate the number of nodes ($$N$$) per connector, we use this formula:

$N=2^n m + 1$

Where $$n$$ is the number of refinements + 1 and $$m$$ is an integer. For our chord-wise direction, we will use ‘’145’’ Nodes. To save some work, we will set it as default.

1. Click Defaults

2. Make sure Connector is checked

3. Select Dimension and enter 145

4. Select the upper and lower surface of the wing

5. Click Connectors on Database Entities

6. Click on Layers and uncheck the Geo layer

7. Select the two connectors in the middle of the wing (Detail A) and delete them. They showed up because we split the database

8. Select the 6 spanwise connectors (Detail B)

9. Click Edit -> Join

When creating the connectors, we left out the TE. We did this because there were 2 surfaces from OpenVSP. It is less work for us, if we manually create two connectors.

1. Click Defaults

2. Select Dimension and enter 17

3. Click 2 Point Curves

4. Close the root trailing edge (make sure your pointer becomes a cross-hair before you click. This way you are sure the new connector lies on the closest point)

5. Close the tip trailing edge

6. Press OK

Now we initialize the surface mesh.

1. Select everything

2. Click Assemble Domains

3. Select everything

4. Click on the small arrow pointing down next to Wireframe

5. Click on Hidden Line

Now we size the LE (Leading Edge) and TE (Trailing Edge) connectors.

1. Click on All Masks On/Off

2. Click on Connectors

3. Select the LE and TE Connectors by drawing a rectangle like it is shown

4. Click on the input field next to Dimension, enter 73 and hit enter

The surface mesh is now almost complete. We only have to distribute the nodes on it properly by changing the spacing. Usually all Points are distributed according to Tanh. But because we split up the database in the previous steps, we have to remove so called break point at that location.

Note

Break Points give you even more control to distribute your nodes on a connector.

1. Select the LE and TE connectors again.

2. Click on Grid -> Distribute

3. Click on Break Points

4. Click on Delete all Break Points

5. Click on OK

1. Click on All Masks On/Off

2. Click on Spacing Constraints

3. Select the 2 spacing constraints at the LE of the root (A)

4. Click the field next to Spacing and enter 0.0003. Then hit enter

5. Select the 2 spacing constraints at the TE root (B)

6. Apply 7.15e-5 for spacing

7. Select the 2 spacing constraints at the LE tip (C)

8. Apply 0.00016 for spacing

9. Select the 2 spacing constraints at the TE tip (D)

10. Apply 4e-5 for spacing

11. Select the 3 spacing constraints at the tip (E)

12. Apply 0.0025 for spacing

13. Select the 3 spacing constraints at the root (F)

14. Apply 0.04 as spacing

The mesh near_wing is now complete. We will export it later.

### Create the near_tip surface mesh

Now we will create the near_tip mesh. Let’s start with creating a new layer and hide everything unnecessary.

1. Click on Layers

2. Check Show Empty Layers

3. Right click on Layer 20 -> Set Current

4. Double click the Description Field and enter near_tip

5. Uncheck Show Empty Layers

6. Check Layer 0 to make the database visible

7. Hide the mesh near_wing by un-checking layer 10

Now we will create the connectors.

1. Click on Defaults -> enter 201 for Dimension

2. Select everything from the tip to the cut we made earlier

3. Click Connectors on Database Entities

4. Click on Layers -> uncheck layer 0. Now, you should only see the connectors we created

Let’s clean up the generated connectors at the tip TE.

1. Zoom into the tip TE

2. Select the 5 shown connectors (A)

3. Delete them

4. Select and delete the remaining pole (the point with a circle around) (B)

5. Select the 2 connectors that define the outer tip (C)

6. Click Edit -> Join

7. Select the newly joined connector (C)

8. Enter 65 For Dimension and hit enter

9. Click on Defaults and enter 65 for Dimension

10. Click on 2 Point Curves

11. Close the TE again (D)

Next we clean up the root TE.

1. Select the 2 connectors that define the TE (A)

2. Delete them

3. Click on 2 Point Curves

4. Close the Tip again (B)

The last thing to clean up is the tip LE.

1. Select the 3 shown connectors (A)

2. Click on the arrow pointing down next to show

3. Click Hide

4. Select and delete the remaining pole (B)

5. Click on View -> Show Hidden

6. Select the 3 connectors (A)

7. Click on the arrow pointing down next to Hide

8. Click on Show

Now we will dimension the remaining connectors and space the nodes properly.

1. Select the 3 shown connectors (A)

2. Enter 97 for Dimension and hit enter

3. Click All Masks On/Off

4. Click Spacing Constraints

5. Select the 2 spacing constraints at the root LE (B)

6. Apply 0.0008 for spacing

7. Select the 2 spacing constraints at the tip LE (C)

8. Apply 0.0008 for spacing

9. Select the 2 spacing constraints at the root TE (D)

10. Apply 1.3e-5 as spacing

11. Select the 2 spacing constraints at the tip TE (E)

12. Apply 1.3e-5 as spacing

13. Select the 3 spacing constraints at the root (F)

14. Apply 0.01 as spacing

15. Select the 1 spacing constraint at the tip LE (G)

16. Apply 0.0005 as spacing

17. Select the 2 spacing constraints at the tip TE (H)

18. Apply 1.56e-5 as spacing

Next, we split the connectors at the tip to allow a topology where we can achieve a decent quality mesh.

1. Select the tip top connector (A)

2. Click Edit -> Split

3. Make sure Advanced is checked

4. Enter 17 for IJK and hit enter

5. Click OK

6. Select the tip bottom connector (B)

7. Click Edit -> Split

8. Enter 185 for IJK and hit enter

9. Click OK

10. Click on 2 Point Curves

11. Connect the 2 new points (A) to (B)

Since our tip is rounded, we have to project the newly created connector on to our database.

1. Select the newly created connector (A)

2. Click on Edit -> Project

3. Click on Layers

4. Check layer 0 (Geo)

5. Click on Project

6. Make sure Target Database Selection is checked

7. Click Begin

8. Select the upper and lower tip surface (hold down ctrl) (B)

9. Click End

10. Click Project

11. Click OK

Now we actually start meshing.

1. Click on Layers

2. Uncheck layer 0 (Geo)

3. Select the newly created connector (A)

4. Click on the arrow pointing down next to Tanh Distribution

5. Click on Equal

6. Click Edit -> Split

7. Enter 17 for IJK and hit enter

8. Enter 49 for IJK and hit enter

9. Click OK

10. Click on Create -> Assemble Special -> Domain

11. Select 1 connector (B)

12. Click Next Edge

13. Select 2 connectors (C)

14. Click Next Edge

15. Click OK

Next, we mesh the rest.

1. Select the 2 connectors that form the semi-circle (A)

2. Click Script -> Execute

3. Look for the script you just downloaded and open it.

4. Select all connectors

5. Click Assemble Domains

The last step is to make sure, that the skewed elements at the tip are smoothed. As Assemble Domains didn’t work for the most outer mesh, we will delete this domain first, and create it manually again.

1. Select all domains

2. Click Hidden Line

3. Select the outer most domain and delete it (A)

4. Select all 9 connectors, that define the last remaining domain

5. Click Assemble Domain

6. Select the newly created domain and click Hidden Line

7. Select the 2 domains that define the tip (A & B)

8. Click Grid -> Solve

9. Click on Edge Attributes

10. Make sure Boundary Conditions is checked and set the Type to Floating

11. Click on Attributes

12. Make sure Surface Shape is checked and set Shape to Database

13. Click on Begin and make sure, the tip is selected (it should be)

14. Click on End

15. Make sure Solution Algorithm is checked and set Solver Engine to Successive Over Relaxation

16. Set Relaxation Factor to Nominal

17. Click on Solve

18. Enter 50 for Iterations and hit Run

19. Click OK

Lets check the quality of the created mesh. The most important metrics are Area Ratio and Equiangle Skewness.

1. Select all domains

2. Click Examine -> Area Ratio

3. Click on the Magnification Glass next to max

4. You see, the biggest Area Ratio is ~2.24

5. Click on Advanced

6. Make sure Histogram and Show Histogram are checked

7. As you see, the vast majority of cells has an Area Ratio of less than 1.25. This should be fine

8. Click on Examine

9. Choose Skewness Equiangle for Type

10. As you can see, the most skewed cell has a Skewness Equiangle of ~0.4. This is also fine

11. Click Close

Note

The lower max Area Ratio is, the easier it is to extrude a mesh with pyHyp. If it is more than 2, it can get tricky. Skewness Equiangle describes how skewed a cell is. It should be below 0.8

## Export all meshes for use in pyhyp

The last step is to export the mesh. For pyHyp it is important, that the normals look in the outwards direction. We will set the boundaries manually in pyHyp.

Note

As there has not been found an easy way to figure out which domain in Pointwise corresponds to which domain in pyHyp, it is recommended to orient them all the same way. Then apply the BC for all domains and run the pyHyp script. If an error pops up for one domain, the corresponding BC can be removed. This gets repeated until there are no errors left (This information is repeated on the next page where it probably makes more sense).

Lets start with orienting the near_tip mesh first.

1. Make sure only the layer near_tip is visible

2. Select all domains

3. Click Edit -> Orient

4. Select one domain (It does not matter which one)

5. Click I-J a few times until you are sure, the orange arrow is pointing outwards

6. Click Set Master

7. Select all domains

8. Click Align

9. Click OK

Now we can export it.

1. Select all domains

2. Click File -> Export -> CAE

3. Set near_tip as Filename and save it somewhere

4. Make sure Data Precision and double is checked

5. You can uncheck the rest (It doesn’t really matter. But the files will be bigger if you leave it on)

6. Press OK

Now lets do the same for the near_wing mesh. As we have a symmetry boundary condition, the orientation procedure is slightly more complicated.

1. Make sure only the layer near_wing is visible

2. Select all domains

3. Click Edit -> Orient

4. Select one domain (It doesn’t matter which one)

5. Click I-J until the orange arrow is pointing outwards

6. If the red arrow is not pointing towards the tip, click I and I-J until both conditions are satisfied

7. Click Set Master

8. Select all domains

9. Click Align

10. Make sure all red arrows point towards the tip (if this is not the case, select this domain and repeat step 6)

11. Click OK

Now you can export the mesh near_wing like you did in the previous step.

Congratulations, you managed to create the surface mesh. On the next page, we will extrude it into a volume mesh.