## 3D Design

Topics related to Ansys Discovery and Ansys SpaceClaim.

#### [ICEM] Airfoil Meshing in icem-cfd

• Aras karimi
Subscriber

Hi everyone,

I want to block the following 3D airfoil in ICEM and create a structured mesh for it.

I blocked it as below, which according to the figure below has 5 blocks, 3 of which are in the front, top and bottom of the airfoil and 2 of which are behind the airfoil.

Now, I have created an initial mesh on the created block, which is as shown in the figure below:

According to the figure above, the mesh in front of the airfoil (front block) has less density than the upper and lower blocks of the airfoil and is not uniform.You might say that the problem can be solved by increasing the number of relevant block nodes. But it is not. I increased the number of nodes. See the figure below:

According to the figure above, the mesh of all three blocks is uniform, but the mesh near the airfoil has a very high density, which does not seem appropriate.

Is there a problem with my blocking, and for example, those two diagonal lines of 45 degrees that are connected from the airfoil to the big half circle of the domain, should they be diagonal or vertical?

I found a picture of a grid on the internet, which seems to be a well-formed uniform front grid of the airfoil, which looks like this:

Is its blocking different from mine?

What kind of blocking strategy should I develop in order to achieve a proper and uniform mesh in front of the airfoil?

Regards
Ansys Employee

Your blocking looks good. You will need to play with edge sizing more to get that similar mesh.

You can try 2D first.

Please go through help manual for more details

Regards,

Keyur

Guidelines on the Student Community

Fluids Engineering Courses | Ansys Innovation Courses

• Aras karimi
Subscriber
I played a lot with the size of the front block edge of the airfoil. I mean this line:

I increased the number of nodes in this block line so that the grid of the front block of the airfoil becomes uniform, and the following figure was obtained:

But if you look carefully at the figure above, you will see that the network in front of the airfoil is very dense and has many more cells than the network on the top and bottom surface of the airfoil.
Do you know what is going on?
The point is that if I want the front block of the airfoil along with the upper and lower blocks of the airfoil to have a uniform grid, so the grid on the leading edge will be very very very small. figure below :

It seems that if one place wants to get better, another place gets worse.

I think the type of blocking should change.

what do you think?

I hope you fully understand what I mean.
Ansys Employee

Please check growth rate while giving edge sizing.

Please go through help manual for more details

Regards,

Keyur

Guidelines on the Student Community

Fluids Engineering Courses | Ansys Innovation Courses

• mjmiddle
Ansys Employee

A good way to think about the blocking is that the structure you intend to create is aimed at getting the grid lines to flow in the directions you want along the geometry and in the farfield with good element angles. The rest should be done by controlling the number of nodes along edges and growth from either end of each edge using the “Edge params.” Your blocking is a good structure because it causes grid lines to flow nicely along the geometry and continuing into the farfield, and the block edges meet the geometry at good angles, in your case close to normal to the blade.
In the second blocking example, this may show a blocking that is easier to get smooth growth ratios on edges between blocks but the edges do not meet the blade at such a good angle. Your picture is zoomed far out and does not show this problem.

With this blocking you could shape the edges using “Blocking > Edit Edge > Split Edge” as below to get better angles:

Either way you must use the “edge params” to set good growth ratios and node counts, so that is the real issue. All edges are candidates for this manipulation except you shouldn’t need to worry about growth ratios on the edges that run along the blade span. These can be uniform.

The “Blocking > Pre-Mesh Params > Match Edges” can be used to quickly match the spacings across blocks:

But you’ll still want to select edge and control growth ratios on side 1 and side 2. You will especially need to control the growth ratios on the edges shown below in your model, but all edges should be carefully set to get smooth mesh size change between blocks:

This fine tuning of node growth is done mostly with the “Blocking > Pre-Mesh Params > Edge Params.” You’ll want to set spacing 1 and 2 on side 1 and 2 of the edge as well as ratio 1 and 2. You can choose different growth laws also, such as bigeometric, biexponential, hyperbolic, etc…

• Aras karimi
Subscriber

I didn’t understand exactly what you meant in the second paragraph (In the second blocking example, this may show a blocking that is easier to get smooth growth ratios on edges between blocks but the edges do not meet the blade at such a good angle. Your picture is zoomed far out and does not show this problem).

What do you mean by the second example of blocking? And you said that ”Your picture is zoomed far out and does not show this problem”.

In the first picture you sent (green grid), did you convert the two diagonal lines, one end of which is connected to the airfoil and the other end to the big semicircle of the domain, into a vertical one? That is, did you convert the diagonal lines into the following form?

This can be done using “Blocking > Move vertex”.  Aren’t you wrong?

Yes, I use “Mach Edge” to adjust the size of the elements of the blocks next to each other.

I made the diagonal lines of the left block vertical with the “Move vertex”, which turned out as follows:

Now I produced the following network on it, which is as follows:

Is this network what you say it is? If so, good uniformity is not created in front of the airfoil.

I use  bigeometric  growth law for all lines. Is it correct? What are the uses of  biexponential  and  hyperbolic  growth laws?

Regards.

• mjmiddle
Ansys Employee

This is a picture you sent of your second blocking:

As Keyur and I said, your first blocking is the one that makes the better angles:

Either way, you are not going to get real nice transitions in mesh unless you set good spacings and growth ratios with the edge params, so that is the important thing you need to do, regardless of which blocking scheme you choose. The choice of growth law is up ot you. I listed popular laws for CFD meshes. Any of the laws with "bi" in front mean growth from both sides. "Geometric" is linear growth. There is also Geometric1 and Geometric2 and other laws that have a 1 or 2 at the end. This means growth for side 1 or side 2. Exponential growth should be obvious. You can look up hyperbolic growth with some online searches. It is a general term used in CFD meshes.

The blocking I used is shown in the last picture of my previous post. Except to match the grid picture of your first post, I moved the two left-most vertices to vertical positions. These are the same two blocking schemes you proposed.

• Aras karimi
Subscriber

I think you did not understand my meaning correctly. The mesh network is not the color of the network produced by me, but I found its photo on the Internet.

Look, I blocked like this first:

Then the grid I generated looked like this:

Now the left block does not have a uniform grid. See the photo above.

Then I increased the number of the mesh block on the left side, which became like this:

Now, the problem with this network is that the front of the airfoil has a very, very high density. I have a problem with this.

I found a picture of this network on the internet, which I think is a good and uniform network:

How is this blocked?

I hope you understand what I mean.

Regards

• mjmiddle
Ansys Employee

Your blocking is better than the one you found on the internet. That one has bad transition seen in the farfield, and it probably has this problem if you were to zoom in close to the blade:

One of your previous pictures showed you already knew how to create this blocking structure:

You can get more gradual transition of mesh sizes by setting better edge params and moving vertices. ICEM CFD has some smoothers but the orthoganol/elliptical smoothers are not very good. Only the quality smoother is decent. You can smooth better if you write the mesh out to Fluent or CFX and smooth there.

Whether you choose the blocking structure of the one seen on the internet, or yours, the thing you need to do is set edge params for gradual grow of node distributions between blocks. Moving vertices of blocks to spread out high density regions and condense sparse regiosn can help this a bit, also.

• Aras karimi
Subscriber

The problem of unwanted network transmission found on the Internet in Farfield can be solved with the “Match Edge”.

I write the network on Fluent. I didn’t really notice the smoothness of the network. In which areas do you mean the smoothing of the network?  How can I do this?

I use “Match Edge” for the gradual growth of nodes in blocks next to each other, but there is still mesh density in the front block of my mesh (not internet mesh). Please see the following photo:

Another question: How can I apply a precise and desired distance for a smaller block near the airfoil? I created it with split block but I didn’t find an option to adjust its spacing :

I heard that “split block” is not needed to account for a smaller block near the airfoil and ICEM has an option that automatically creates a smaller block near the airfoil. Do you know anything about this?

Sorry, I have too many questions. Due to lack of time, I had to ask my questions at once.

Regards

• mjmiddle
Ansys Employee

The "Match Edges" sets the spacing on one side of each of two edges you select on opposite sides of a connected vertex. I gave a previous picture on suggested edges to match edges, but you can try lots of edge pairs connected across a vertex:

Use "Blocking > Move Vertex > Set Edge Length" to directly set the blocking edge length.

You can also use "Set location" in this menu to set xyz locations of vertices.

The block splitting you are thinking about is called an O-grid, but you don't need to do this in your blocking because the entire farfield region up to touching the blade is an O-grid type. You don't need to split through a radial edge as in your last picture because it's structurally the same grid. You only need to control the node spacings and ratios on the radial edges of the O-grid to control the growth away from the blade.

I have said this many times: Your blocking structure is good; all you need to do is control the spacings and ratios on the block edges to get good growth and smooth transition between blocks. You cna do this entirely with the "Edge Params" button. The "Match Edges" is a convenience function.

• Aras karimi
Subscriber

OK, so if you say that my initial blocking is fine, so there are two strategies:

1- If I want the mesh on the surface of the wing to be uniform, then the mesh density of the front block will be different from the upper and lower blocks of the wing, which is as follows:

(Strategy 1)

2- If I want the mesh density of the front, upper and lower wing blocks to be uniform, so the mesh on the wing surface will be different, which is as follows:

(Strategy 2)

And these two things really bother me.

Do you agree with these 2 events?

Therefore, I must accept one of these two strategies. Which one do you recommend?

• mjmiddle
Ansys Employee

A uniform mesh would be the same element size throughout. You do not want a uniform mesh for a CFD model. You want small elements at the surface, and growing in size gradually from the surface as well as throughout the mesh (between blocks). Use the “Edge Params” to set spacings and ratios to get gradual growth from the surface as well as between blocks. Your last picture looks appropriate for a CFD mesh. Different element sizes in the mesh anywhere will necessitate denser mesh regions than other regions. You must only ensure that mesh sizes grow gradually between these regions, not abruptly. It sounds like you need some learning on what should be done in the mesh for a CFD analysis. I’m sorry but I can’t keep responding to this post anymore if you essentially keep asking what are in content the same questions over again.

• Aras karimi
Subscriber

Therefore, it is not a problem to condense the network in one area of the network, only the edges of adjacent blocks should have a good growth ratio.

What is the appropriate ratio number for the edges of adjacent blocks? 1.1 or 1.2 or...

I checked the aspect ratio of the grid, which reported values of 1-31500, which is a very high number and shows most of the very large elements produced behind the airfoil:

I increased the number of nodes in the block lines behind the airfoil, which reduced the aspect ratio, but the total number of cells in the grid increased significantly.

Is there a need to create a smaller block near the airfoil and also cut the block behind the airfoil so that the mesh is small only in those areas?

Regards

• mjmiddle
Ansys Employee

Growth ratios between 1 to 1.3 are typical, but it depends on your CFD solver. Aspect ratios also depend on your CFD solver. High aspect ratios are not preferred anywhere except in the boundary layer. But these are all questions about the CFD solver. Get to know the requirements of your CFD solver.

• Aras karimi
Subscriber

Hi Dear mjmiddle,

After creating the domain around the airfoil in Design Modeler, I enter ICEM for meshing. After entering ICEM, the front Face of the domain is incomplete.

The domain was created in Design Modeler without any problems:

After that, I enter ICEM for meshing:

According to the figure above, the front face of the domain is incomplete. (The black face is the selected face and the green face is the back face of the domain).

Is this a serious problem or just a graphical display?

If it is a serious problem, how can I fix it?

After creating the mesh on it, which options should I choose in the mesh check section so that I can make sure that the generated mesh is free of problems?

Thankyou

Regards

• mjmiddle
Ansys Employee

You had this mesh and geometry working together previously. What did you do different? The picture is very zoomed out. Zoom in to see what it's doing. Did you load the old blocking onto a new geometry or create a new blocking on this geometry? I think it may be blocking projection problems.

Or you may have a missing geometry surface.

There are lots of way to diagnose projection probems, and some may show an issue while others do not. After computing mesh, right click in the model tree on "Edges > Show Association." If that doesn't show anything try "Edges > Projected Mesh Shape" to see how the edges form when mesh is computed. "Pre Mesh > Scan Planes" can show something the other methods didn't show. A quality check such as determinant or angle, then selecting the lowest histogram bar can help show you what is wrong. Face projections don't get set unless you purposefully set them (default projects to nearest surfaces), but you can display that too using "Faces > Face Projection" from the model tree.

As for the error and possible problem checks, it opens the panel with the default options used for the mesh dimension type (2D or 3D). There is a "Set Defaults" button to return to those if you have turned some on/off. Go to the help to understand what each of these mean. Some may only be necessary depending on the solver you want to use, such as whether boundary elements are required (uncovered faces and missing internal faces checks). If you created a blocking and the quality checks are high enough such as determinant and angle, then the mesh will most likely be free of errors. A lot of these errors occur with tetra and prism and possibly after smoothing. Certainly after manual mesh editing, you could get lots of errors.

Have you gone over the "Introduction to ANSYS ICEM CFD" course from the Ansys Learning Hub? ICEM CFD is in maintenace mode and no longer supported. I see a "course dates" course there, but I don't see a self paced course anymore where you could download the materials.

• Aras karimi
Subscriber

No no mjmiddle, don't judge too soon Look, I don't do any blocking on the new geometry, only when I come from the design modeler of the ICEM, the front surface of the domain is incomplete.

Look at the pictures above that were gridded and I sent was a symmetrical 3D airfoil that after drawing in Design Modeler, when I enter ICEM (without any blocking), the surfaces are complete and have no problems:

Now my new geometry is an asymmetric airfoil, after drawing it in Design Modeler, when I enter ICEM without doing anything, I see that the front surface of the domain is incomplete: see the following pictures:

What is the reason for this problem?

Once again, I tried the same asymmetric airfoil with a longer cord length, this time only one end piece of the airfoil is incomplete: see the photos below: (This is my main geometry)

I ask one question, you quickly say you don't know ICEM and take a course, which I don't think is the right behavior. I have been working with ICEM for about a year.

How can I make sure that the incompleteness of the surface does not cause problems in my generated mesh?

mjmiddlelook, my geometry is an asymmetric airfoil, and when I draw it, I come to ICEM for gridding, without doing anything, I see that the front surface of the domain is incomplete at the end of the airfoil. Doesn't this cause problems?

I generated his mesh and looked at all the mesh quality check parameters, all of which had very high values.

But what can be said about the geometry that a much bigger part of it is incomplete?

I hope you will answer me much sooner than last time

Regards

• mjmiddle
Ansys Employee

OK, it's just a geometry problem at this point. I see no blocking listed in the model tree. You can try to view the surfaces better. Use full display by one of the methods shown below:

You can view in wireframe/full also.

If the problem is still there, you must have done something wrong in DesignModeler. Did you draw the geometry entirely in DM or did you import it?

You can work with imperfect geometry with the blocking by setting associations to walk across problems, but it gets a bit painful. You can use face-to-surface associations to interpolate. You can make edge splits (not block splits) and set the association different on the edge segments. Move the new edge splits to the end of the best parts of the curve, and set a none association on the segment that crosses problems and gaps.

You can recreate curves and surfaces in ICEM CFD.

Such a simple geometry should not have problems though. It's better to fix what you did wrong in creating the geometry in DM.

If you have not gone over the Introductory ICEM CFD training, you should. Even when customers submit support cases, we require them to take a training in the subject first, so that we are not just duplicating work that is described in training. If you don't have ALH access, I think a lot of the basic ICEM tutorials can be found on YouTube.

• Aras karimi
Subscriber

I drew the whole geometric model in Design Modeler.

By using the 'Solid Full Flat Display' option, the display of the surfaces was changed from incomplete to full.

It's just very strange why this is happening when the entire geometry model was drawn in Design Modeler and is fine.

Anyway, the display problem is fixed. thank you

• Aras karimi
Subscriber

Dear mjmiddl,

I want to create a periodic mesh on the domain below, and the front page of the domain (purple color) will be named Periodic 1 and the back page of the domain (blue color) will be named Periodic 2:

I need to establish a Translational Periodic boundary condition. I created a mesh structure. Now please help how can I apply this boundary condition?

The front surface of the domain is located at the origin of the coordinates, and the back surface of the domain is located in the -Z direction and at a distance of -0.2 meters from the origin of the coordinates. (In other words, the span length of the airfoil is 0.2 meters)

Earlier, I read that I should first come to this section and select the type of boundary condition. There is also a parameter called offset. What number should be written?
I went to ICEM Help and found the following:

I’m still confused and I don’t know what number should I put for the offset ?
And what should I do next?

If you help me, I will thank you a thousand times.

Regards

• mjmiddle
Ansys Employee

This post has become a long run-on of changing topics. Can you submit this to a new post?

• Aras karimi
Subscriber

Yes, I brought it up in the post below a few days ago and still haven’t gotten a response.

https://forum.ansys.com/forums/topic/creation-of-periodic-b-c-in-icem/#post-314453

I would be grateful if you could help me

Regards

• Aras karimi
Subscriber

Dear  mjmiddle,

Is it necessary to make the mesh at the end of the airfoil smaller or should it grow uniformly to the end of the trailing edge according to the shape below?

• mjmiddle
Ansys Employee

I'm not sure. That's a question that concerns what the solver really needs. For a knife edge, I don't think it needs to be smaller, but I'm not sure. You usually find out when the CFD solver has convergence problems or results don't look accurate in that region. If you are using CFX or Fluent which are Ansys products, you can ask in a new post for that CFD solver.

• Aras karimi
Subscriber

Thankyou