Creating Weld Mesh Efficiently Using Discovery and Mechanical
Hi everybody, this is Edwin from Ozen Engineering, Inc. Today, we are going to explore how to create welding using the Discovery Tool, new in the 2024 R1 release, and how to construct a mesh within ANSYS Mechanical.
Discovery Interface
Let's start by navigating to the Discovery interface where I have a typical shell structure extracted from a 3D model. In this case, I've already extracted the shell geometry. By hiding the solids and showing the mid-surface, we can observe gaps between parts due to the geometry mid-surface. This necessitates creating welding in this geometry.
Steps to Create Welding
- Go to the Prepare tab and locate the Welds section.
- Use the Assign tool, specifically the Fillet Weld tool, to create welding across the entire geometry.
- Open the option panel and define a detection distance, for example, 5 millimeters, to capture all gaps between different geometries.
- Select all geometry by dragging a box, and observe the pink lines indicating where the welding geometry will be created.
- Confirm by hitting the OK mark to create the Fillet Weld.
The Fillet Weld is now created, and we can see the continuous seam welding structures that will be used to create a mesh in ANSYS Mechanical.
ANSYS Mechanical
Next, we move to our Workbench project to add and study structural analysis.
- Drag and drop the block and refresh the geometry from the A block.
- Open ANSYS Mechanical by double-clicking the cell.
In ANSYS Mechanical, we have imported our geometry, including the mid-surface from the structural parts and the parts created using the welding tool.
Creating the Mesh
- Select all bodies using Ctrl + A and change the method to Automatic Prime Mesh.
- Modify the element size to 2 millimeters.
- Add weld control and define necessary parameters.
- Model the welding using normal and angled approaches to mimic the seam weld.
- Define two element rows in the welding to divide the surface.
- Use the curves approach for creating welding mesh objects.
- Change curve scoping to body selection and choose the first body.
After configuring, generate the mesh. The mesh is created, showing details of the shell bodies and the welding mesh automatically using guide bodies from Discovery.
Final Adjustments
- Modify the edge mesh size to 1 millimeter.
- Assign structural steel as the material for welding.
- Use the same weld control to create all weldings by activating the worksheet and adding all bodies in one control.
Finally, generate the mesh to see how the shell mesh complies with the welding bodies across the structure, ensuring good behavior for analysis and calculations.
This concludes our demonstration. I hope this will be useful for you. See you next time. Thank you.
Hi everyone, this is Edwin from Ozen Engineering. Today, we're going to see how to create welds efficiently using the Discovery Tool, new in this release, 2024 R1, and how to construct a mesh within ANSYS Mechanical.
Let's go to the Discovery interface, where I have a typical shell structure that we can construct from a 3D model. In this case, I already extracted the shell geometry. We can see that here, hiding the solids and showing the mid-surface.
We can see there are some gaps between the parts created because of the geometry mid-surface. And that's why we need to create welds in this geometry. Then we can go to the Prepare tab and look for the Welds section. We're going to use the Assign tool.
In this case, we have the Fillet Weld tool that allows us to create our welds in our assembly. We're going to use the tool to look through the entire geometry and create welds across all the geometry.
To do so, we're going to open this panel and define a detection distance using, for example, 5 millimeters to be sure we're capturing all the gaps between the different geometry. We can then select all the geometry, and we'll see pink lines showing us where the welding geometry will be created.
Now, let's go to our Workbench project and add a structural analysis study. We'll drag and drop this block and refresh our geometry from the A block. Once the geometry is updated, we can open ANSYS Mechanical by double-clicking in the cell and opening the software.
In Mechanical, we have already imported our geometry. We have new bodies, including the mid-surface from the structural parts and all the parts we have imported. We can see here that we have all these beams, which have been created from the welding tool. We're going to create our mesh.
The first step here is to add a method that will be applied to all bodies. We'll change the method for automatic prime mesh, which will allow us to create our mesh correctly. Then, in the meshing tool, we can modify the element size. Two millimeters will work well. Now, we can add our weld control.
We'll define the different parameters needed to create our bodies. We're going to model our welding using a normal and angled approach, which will create a vertical surface from one face and then another inclination to mimic the welding, the seam weld.
We'll define two element rows in the welding, dividing our surface using two elements. We'll select the way we're going to create our welding mesh objects. In this case, we're going to use the curves approach.
We have several options, but because we previously defined these bodies inside Discovery, we can just use curves, which will be easier for us. We'll change the curve scoping to body selection and choose the first one of them. We'll create just one weld.
Now, we can create, modify some additional controls to have a better mesh. For example, I'm going to modify the edge mesh size instead of 2, which is the default value. I'm going to use 1 millimeter, which is half the element size in the shell bodies.
Then, I'm going to assign some material for my welding. In this case, the structural steel, which is created by default. And now, we have all the configuration ready for creating our first welding body. I like to use this same weld control to create all the weldings in my body.
In doing so, I'm going to change this property, which is named "use worksheet," to "yes." And now, I have activated this table. Hitting this button, I can add all the bodies in just one control, which is very useful for creating curves for complex models.
Then, I can go back to my mesh and create it by hitting "generate mesh." Now, we have our mesh created, and we can see the details here. For example, we can go here and see how the different shell bodies have been meshed.
And the welding mesh has been created automatically using these guide bodies, which were the beams we created from Discovery. We can see how the shell mesh has been modified to be in compliance with our welding bodies. And this is across the whole structure.
We can see the different points, the different joints where we have this good behavior, this good mesh that we can use to support the welding. And the other points that we can use to solve our analysis and to perform any calculations we want considering this welding.
That's it for this video, for this demonstration. I hope it will be useful for you, and see you next time. Thank you.
