General Mechanical

General Mechanical

How to give revolute joint in 2D Explicit Dynamics?

    • samyak1902
      Subscriber

      I was wondering how to make a body-to-ground revolute joint in 2D. When I define the geometry analysis type as "2D", this revolute joint is not available. I can make this revolute joint in 3D, but I want to use 2D instead of 3D in order to reduce my simulation time.


      I want to give a revolute joint to the shaft hole in the file attached below.



      Is there any way to make a revolute joint in 2D? I would appreciate any inputs!

      Thank you for your valuable time.

    • peteroznewman
      Subscriber

      You can create a Cylindrical Coordinate System at the center of each gear, and add a Displacement Constraint of X=0 because in a Cylindrical Csys, X is Radial.


      I would like to know why did you choose Explicit Dynamics to simulate two gear teeth?  What is your simulation goal?


      If it was to see the gear teeth turn and go in and out of mesh, you could do that in Rigid Dynamics with a lot less time spent computing results.


      If it was to look at the stress in the gear teeth, you would be better off in Static Structural looking at a model with just a few teeth on each gear as others have done.


      Attached is a working ANSYS 19.1 model.

    • samyak1902
      Subscriber

      Hi Peter,


      I want to calculate the Hertzian contact stresses in a spur gear assembly. I also want to plot the variation of stresses with respect to time for different depths. Earlier, I used Static Structural with 3D model for finding the stresses but it was taking a huge amount of time. So, I started to work on explicit dynamics but it is also taking a large amount of time so thought to solve the model for 2D case.


      I am attaching the reference paper which I want to validate and also an ANSYS model for 1 tooth. The major problem which I am facing is the huge amount of time taken by simulations.


      Regards


      Samyak


    • Sandeep Medikonda
      Ansys Employee

      Hi Samyak,


        Are you able to provide details of what your analysis settings are? An explicit analysis doesn't guarantee speed, it depends on the time step calculated based on the smallest element in your model. So, What is the total end time and your time step? 


        Your mesh looks extremely refined which could be causing problems. Partition your model only simulate only the area of interest. 


        Also, We have a few verification examples in the help that you might find helpful, these are from MAPDL though.



      Regards,
      Sandeep
      Best Practices to post on the Student Community

    • peteroznewman
      Subscriber

      Hi Samyak,


      If you want to study Herztian stresses, you don't want Explicit Dynamics, you want Statics. If the 3D Statics model was taking too long, use a 2D Statics plane strain model. That will reduce time much more than a 2D Explicit Dynamics model would.



      I also want to plot the variation of stresses with respect to time for different depths. 



      When you say "depths" what do you mean?  Do you mean face width?


      The variation in stress with respect to time is the same as different angles of the gears in a static solution to get the contact point to one side or the other of the pitch circle.


      Regards,
      Peter

    • samyak1902
      Subscriber

       Hi Sandeep,

      I have attached the screenshot of the analysis settings. I want to analyse the simulation for time in which tooth starts its contact upto the time when it leaves the contact which is approximately 0.00825 seconds. I have done the meshing so fine because I want to plot the variation of stresses with respect to time for different depths. By depth, I mean the depths under the surface of the contact point.

      Regards,


      Samyak


    • samyak1902
      Subscriber

      Hi Peter,

      By depth, I mean the depths under the surface of the contact point and not the face width.

      In my case the loading conditions are:
      1. The rotation speed of 600RPM is to be applied on the surface of the shaft hole of the driving gear.
      2. The 35 Nm torque is to be applied on the shaft hole of the driven gear.

      Is it possible to simulate gears in static structural on the basis of given loading conditions as both the gears will be moving?

      Regards,
      Samyak

    • Sandeep Medikonda
      Ansys Employee

      Hi Samyak,


        You don't have any mass scaling on to speed up the simulation and have a very small element size as well. I would expect this simulation to take a long time in explicit, remember in explicit your time is proportional to the characteristic length.


        I would recommend you to do something in static structural as peter suggests and the way some of the other he pointed out to have done.


      Regards,
      Sandeep

    • samyak1902
      Subscriber

      Hi Sandeep,

      In my case the loading conditions are:

      1. The rotation speed of 600RPM is to be applied on the surface of the shaft hole of the driving gear.
      2. The 35 Nm torque is to be applied on the shaft hole of the driven gear.

      Is it possible to simulate gears in static structural on the basis of given loading conditions as both the gears will be moving and none of them will be fixed? 

      Regards,
      Samyak

    • Sandeep Medikonda
      Ansys Employee

      Samyak,


        The boundary conditions are not a concern and can be used/simulated. You only need to account for the rigid body motion. In Static structural, you are solving [K]{u}={f}, whereas in an explicit analysis since the time frame is small you solve the full equations of motion, i.e., [M]{a}+C{v}+[K]{u}={f}. i.e., you are accounting for the inertial effects.


        In the examples that peter provided, other community members have analyzed it in static structural.


      Regards,
      Sandeep


       

    • peteroznewman
      Subscriber

      Hi Samyak,


      In Static Structural, you can perform a multi-step solution. Have the gear teeth oriented in CAD at the angle where the tooth first comes into contact. Let's say for example that the gear rotates by 10 degrees from first contact to last contact.


      Create a model with a Revolute joint on each gear center. On one Revolute, apply the load of 35 Nm. On the other Revolute, apply a displacement of 0 degrees for Step 1. In each of the next 10 steps you will increase the angle on the displacement by 1 degree.


      What that will do is load up the gear teeth in step 1 then each subsequent step you will have the teeth at another angle where you can plot the stress. In step 2 and beyond, if you have a frictional contact, the sliding friction force will be acting on the tooth surface as well as the normal contact pressure.


      You need a fine mesh to show the Hertzian stress below the surface, so you definitely don't want to use Explicit Dynamics.


      You can add a rotational velocity Inertial load to each gear to account for the stress generated by the rotational velocity.


      Regards,
      Peter

Viewing 10 reply threads
  • You must be logged in to reply to this topic.