Learning Forum

[user deleted]

How can I specify the size of layers within a 2D mesh extrusion in Ansys Workbench? In Ansys APDL there is the possibility of defining a "Spacing Ratio", but in Ansys Workbench I do not see this option anywhere.

I attach two images: What I want to obtain and have in APDL (Left) and what I currently have in Workbench and is not what I want to obtain (Right)

 

Explaining a little better what I want to obtain, is that the last layer of the 10 of the extrusion is 10 times larger than the first, that is, the layer furthest from the initial surface is 10 times larger than the layer furthest from the initial surface. close to the initial surface

 

[user deleted]

The only way I have found has been to define each layer one by one, as shown in the attached image, but it is a very slow process, I would like to know if this can be defined in some way in the first extrusion.

 

[peteroznewman]

Use a Sweep Bias Type on the Sweep Method and type a value larger than 1 (such as 5) to put small elements near the Source face.

[user deleted]

Could you give me some other indication, because I can't get anything, I get the following error: "Mesher failed to initialize"

[peteroznewman]

In Mechanical, right click on Mesh and Show Sweepable bodies.  If your geometry does not highlight in green, try adding a Mesh Method called Multizone to the body.

[user deleted]

I don't understand why you have to add a multizone method, could you explain it a little more. By the way, I get a mapped mesh but it seems to me that it doesn't take into account the specified sweep method. I have attached an image of the result obtained.

 

[user deleted]

By adding a side size on the four main edges and adding 10 divisions with a bias factor of 10, I got just what I wanted. Also, I had to add a multizone method. What I have to do now is to make a more precise mesh on the external face with triangular elements, as shown in the images I attached in my first post. Below, I show you two images of what I just did.

 

[peteroznewman]

The only way I know to get triangles on the external face is to use the Mesh Method Sweep as I showed above.

The reason your geometry is not sweepable is because the topology of the external face and the opposite face are not identical. For example, if one face has an extra vertex that the other face does not, or if one face has an imprinted curve on it that the other face does not.  Furthermore, the four edges along the sweep direction must have no vertices on the edge, only corner vertices. 

The easiest way to repair the geometry is to open it in SpaceClaim and go to the Repair tab. Click the Extra Edges button to remove any imprinted curves. Click the Split Edges button to remove those.  If you have extra curves on one face that you need to keep, then you must create those same curves on the opposite face. On the Design tab, use the Project button to project the imprinted curve to the opposite face.

[user deleted]

It is now resolved, thank you very much