Mechanical Stress Analysis of High-Speed Electric Motors Using Ansys Mechanical and Motor-CAD

Hello everyone, this is Botan from Ozen Engineering. In this video, I will show you how you can run your mechanical simulation analysis for your high-speed electric motors by using Ansys Mechanical and Motor-CAD.

Before going to the details of this video, I would like to show you the blog that I created for this simulation workflow. Here, I explain all the steps in detail to show you how you can also simulate the same thing for your projects.

Basically, all you need to do is just change some features and settings to adjust the simulations for your project. Now, let's get started with Ansys Mechanical. In order to get the results of mechanical stress simulations, first, we need to create a Workbench workflow.

Here, I imported my geometry from Ansys Maxwell into the Ansys Static Structural. Here, as you see from the left side, we have multiple tools that we can use in Workbench.

I basically drag the Static Structural and drop it next to the Maxwell model, and I use Maxwell 2D for my electric motor geometry. You can also perform this simulation in Maxwell 3D. Now, let's check out the geometry of the electric motor that is used for this simulation.

As you see, this is one part, one fraction of the electric motor. This is a template motor provided in Motor-CAD. Here, we have 48 stator slots and 8 numbers of poles in the rotor. Since this simulation is related to the rotor, we don't need the stator and the coils.

We don't need to remove these parts in Maxwell; all we need to do is couple the geometry into the SESIC structure by using simply drag and drop, and couple with the set structure. Then, you have to double-click the model to open Ansys Mechanical.

Here, if you follow the blocks as well, I unsuppressed the rest of the motor except for the rotor. Now, it's time to assign the thickness of this 2D model.

You can also simulate a 3D model of your electric motor in Ansys Mechanical, but since the 2D version is way faster and pretty close to the 3D model, I would like to show you how you can do it in 3D.

Once you choose all of the materials, you have to assign the thickness as the thickness of your lamination material. And then, you can basically choose any material for your laminations, for our magnets, and shafts. After completing the geometry part, it's time to create the contacts.

Here, in electric motor stress simulations, the connections are one of the most important parts of the stress simulations. Since these magnets are attached to the rotor by using some adhesive or feeding methods, we have to simulate this phenomenon.

Here, as you see in my geometry, I created a small gap from the bottom side of the motor of the magnets compared to the rotor. And the top part is basically touching the outer part of the rotor, which is simulating the bonded simulation.

But since these are not the bonded models, these are somehow attached to each other, we have to provide the friction between the magnets and the rotor.

That's why, in order to create the accurate connections, first, you have to come to contact and make this tolerance slider to 100. If you make those to 50 or negative values, Ansys Mechanical will detect very tight gaps, for example, it will detect this edge and the corner of the magnet as a contact, and this will lead to inaccurate results of your simulation.

All we want is to simulate the connections between this edge and rotor edge. That's why we are giving the tightest tolerance value for the connections.

After assigning this value, you can right-click the contacts and create automatic connections, and Ansys Mechanical will automatically detect the connections of your electric motor. The next step is the mesh.

The mesh is also very important for electric motor stress analysis since we don't want to run our simulations too long and we want to get the maximum accuracy.

As you see, the rotor main part has one solid chunk of metal, and we don't need to assign so many mesh values here since these will be the same thing for the rest of the geometry. What we want to do is basically assign more mesh around the corner and the edge of the magnet or the rotor slots.

In order to do that, you have to come to sizing and activate the capture curvature, and we have to make the curvature normal angle 7. If you make this value smaller, this will capture more angles around the corners and edges.

Connecting the meshes between the parts, in order to do that, we have to right-click the mesh and insert a Mesh Connection Group. This will create a block here that detects the connection mesh between the parts.

Here, same as the connections, we have to make the tolerance slider as the maximum; otherwise, the mesh will detect some connections between very small gaps.

For example, here, there is a gap between this mesh and this mesh, and if you make this tolerance a bit smaller, this will detect the connected mesh between these two points. In order to prevent that, you have to choose the smallest tolerance value.

After generating the mesh, it's time to assign the boundary conditions. Here, I have the rotational velocity to simulate the rotating part of the electric motor at 15,000 RPM. And it is rotating around the z-axis.

The last thing is frictional support, which is assigning because we don't want to simulate the rest of the electric motor since this is one friction, and we want to achieve the same thing for the rest of the electric motor.

Here, we have to choose the frictional support and assign these four edges to limit the simulation within this boundary. After assigning the static structure, we have to come to solutions and insert the results that we want to see.

Here, I would like to see the equivalent von Mises stress, which I already assigned, and choose the bodies for the results that you want to see in your electric motor. Here, I assign all the bodies since I want to see the whole electric motor stress simulations under the rotation.

After you solve your model, you will see the results as seen in this picture. Here, as you see, the maximum stress occurs at the corner of the magnet slots.

This is due to the mechanical saturation happening around the narrow and small gaps and parts of the electric motor, and since there is not enough corner and radius of this slot, this will increase the maximum stress of this point.

But since this value material is less than the yield strength of the lamination material we assigned, this motor is considered safe at 15,000 RPM. This is how we can simulate the mechanical simulation in Ansys Mechanical. Now, I would like to show you how we can do it in Motor-CAD.

In Motor-CAD, if you go to open template and open the E10 electric motor, you will have the same model in your Motor-CAD simulation. And Motor-CAD is very straightforward. All you have to do, first, increase the mesh density of the model.

To do that, come to input data, settings, and calculation, and reduce this value from 0.2 to 0. 1. And then, once you go to calculation, we have to assign the shaft speed of the electric motor, which is 15,000 rpm, and we have to include the magnets, and the new feature that comes with Motor-CAD, we can include the shaft with the radial interference.

I assigned a 0.02 coefficient, which you can try different values based on your models. After you solve the rotor stress model, you will see that Motor-CAD will automatically solve the simulations by assigning the boundary condition itself.

And once we achieve the same results from Motor-CAD, we can compare the Ansys Mechanical simulation results and the Motor-CAD results. As you see, both simulations simulate the maximum stress results at the same part of the electric motor, which is the magnet slot edge and corners.

Here, Motor-CAD predicts 368 MPa values, and Ansys Mechanical predicts 413 MPa. This shows the two different workflows of Ansys Mechanical and Motor-CAD.

This is everything about this video, thank you for listening to me, and if you have any questions, please contact us at https://ozeninc.com/contact for more information.