How to couple MANATEE to ANSYS using an existing ANSYS model ?

Coupling MANATEE to ANSYS to compute FRF using an existing ANSYS model is not automated yet within MANATEE. However, the concept stator coupling method can be adapted.

How the current coupling works

MANATEE can automatically generate a "concept stator" model in ANSYS. This "concept stator" cannot integrate any complex topologies, such as:

Complex topology with frame
Complex topology with frame

To simulate such topologies, it is important to first understand how the coupling works when it generates a "concept stator". To summarise MANATEE will automatically:

  • generate an APDL script that defines everything (geometry, mesh, boundary conditions, loads, run, save result...)
  • call Ansys to run the computation
  • convert the resulting displacements to FRF.

The generated APDL script code can be split in two main parts "Geometry" then "Simulation". Below are listed (in order) all the main steps of the APDL script to define and run the simulation from a new ANSYS model:

Geometry part
  • Define element type
  • Define material
  • Draw a tooth in 2D and set 2D mesh on each line
  • Extrude the 2D tooth and 3D mesh
  • Duplicate tooth volume to get the global machine mesh
  • Create specific components to store the nodes where loads, boundary conditions,... will be applied
Simulation part
  • Define a modal analysis
  • Set damping properties
  • Set boundary condition on Lam_Bottom and Lam_Top components (if needed)
  • Then for each wavenumber r (radial and/or tangential):
    • Define the load to be applied on the tooth tip "TX" components
    • Define simulation and run
    • Define post-process saving displacement from Yoke_ext component

Note that the generated APDL script is readable with any text editor and contains some comments to understand its content and find all these steps.

How to adapt the concept stator coupling to an existing ANSYS model

The "concept stator" coupling was defined to have the geometry part independent from the simulation part within the APDL script. Therefore as long as an ANSYS model contains the correct components, the simulation part can be used without any change. Below are listed the main steps required to compute the FRF of an existing ANSYS model with MANATEE:

  • Adapt the existing ANSYS model to match MANATEE requirements (machine position, component setup)
  • Generate an APDL script (simulation part only)
  • Run the simulation manually in ANSYS
  • Compute the FRF from the displacement in MANATEE.

The FRF results can then be used in MANATEE for further simulation.

Adapt the model to match MANATEE requirements

To be able to skip the geometrical part of the APDL script, ANSYS model should include:

  • Geometry and mesh
  • Materials
  • Components

MANATEE requirements are the same as for the coupling to Optistruct:

  • Machine axis should be Z
  • Machine should be centered on the origin of the coordinate system (machine between z=L/2 and z = -L/2)
  • The nodes for the load application of the first tooth tip (T0 component) have cylindrical coordinates (Rint, 0, z). All the other tooth tip components are numbered in trigonometrical order.
  • All the load application components "TX" represent a cylinder whose axis is along Z
  • Lam_Bottom and Lam_Top components contain nodes of lamination both ends. These components are used to set boundary conditions. In free-free case, there is no need to define these components.
  • In case of a complex boundary condition, it should be directly defined in the ANSYS model. MANATEE simulation should then set boundary condition to free-free (to avoid the APDL script from adding other boundary conditions)
  • Yoke_ext is the component that contains the nodes where displacement are computed. It should correspond to the lamination or the frame exterior.

Here are given component examples:

Component examples: Lam_Bottom (left), TX (center), Yoke_ext (right)
Component examples: Lam_Bottom (left), TX (center), Yoke_ext (right)
Generation of the APDL script

Once the ANSYS model has been updated, the next step is to generate the simulation part of the APDL script. MANATEE project and machine files can be based on the “concept stator” ones. In particular, in the project file the Ansys FRF workflow is selected with:

Input.Simu.is_mechanics=1; % Run the mechanical module
Input.Simu.type_mech_workflow = 4; % Wave FRF workflow
Input.Simu.type_FEA_model = 2; % Ansys

In the MANATEE project file, Input.Simu.FRF_FEA_proj is set with the name of a dedicated APDL generation project.

Input.Simu.FRF_FEA_proj = 'my_APDL_gen_script';

The APDL generation project is created by coping/pasting/adapting the file Mechanics\APDL\Projects\default_APDL_gen. Below are listed the modifications to do in this script to generate only the simulation part for an existing ANSYS model:

  • Removing ANSYS path (Input.Simu.FEA.ansys_path) and 2D mesh parameter (Input.Simu.FEA.N_list)
  • Setting Input.Simu.FEA.NLay to the number of nodes in each TX component + 1.
  • Adding the following line :
    Input.Simu.FEA.is_geo_gen = 0;

Then the following command line should be used to generate the script:

run_MANATEE('<Your MANATEE project name>')

The resulting APDL script will be available in the folder Mechanics/APDL/Results.
Note that the execution will end with an error as MANATEE cannot run ANSYS.

Run the simulation manually in ANSYS

First, the updated ANSYS model needs to be opened in ANSYS Mechanical. Then, the generated APDL script can be run. At the end of the simulation the results will be stored in the FRF_displacement.txt file.

Post-processing in MANATEE

Finally FRF results can be obtained using the following MANATEE command script:

convert_APDL_FRF(file_path, projname, r, is_rad)

This function parameters are:

  • file_path: Path to the FRF_displacement.txt file
  • projname: Name of the project (for the result file)
  • r: wavenumber list
  • is_rad: 1 for radial, 0 for tangential, 2 for both

Starting from version 1.08.02, a 5th optional parameter is added to convert_APDL_FRF: is_mm (default value 0): 1 if the existing ansys model is in [mm] to convert the resulting displacement to [m]

All the computed FRF will then be available in "projname".mat
Note that r and is_rad parameters must be the same as the one that generated the APDL script.

Previous Next