### 1.3.4. Workflow in Stand Alone Operation

The difference between Stand Alone operation and WB Integration is that the several steps or operations have to be performed manually. The following is an overview of these steps:

1. Generate the ANSYS input file in Workbench or Mechanical APDL, including the loads and boundary conditions (*.inp, *.dat or *.cdb).

   From Workbench:

   In the Mechanical application, select the analysis and select Tools > Write Input File to write a *.dat or a *.inp file.

   Figure : Write Input File

   Alternatively, in the project schematic, you can update the Setup status. A ds.dat file is written in the project folder SYS-X/MECH. This file can also be used as Pre-processing Model in ACP.

   From Mechanical APDL:

   In Mechanical APDL, use the command CDWRITE to write a .cdb file, which can be used as a preprocessing model in ACP.

       cdwrite,db,file,cdb

2. Start ACP

3. Import the ANSYS Model in ACP.

   ACP supports the .dat, .inp and .cdb file formats. Import the model into ACP by selecting File > Import Pre-Processing Model or by right-clicking the Models object in the tree view and selecting Import Pre-Processing Model.

   Figure : Import ANSYS Model Using the Context Menu

4. Define the Materials, or copy the materials from the ACP Material Databank.

   For more information on defining materials, see Material Data.

   For more information on using the Material Databank, see Material Databank.

5. Create laminate sequences.

   See Usage Reference and Composite Modeling Techniques for detailed information.

6. Update the model after any change in the ACP definition (layup definitions) or change of the input model.

   After any modification in the input model, the input file must be reloaded (see Model).

   After any change in the ACP definition, the database must be updated. Use the Update button in the toolbar.

7. Send the model to the ANSYS solver (Solve Current Model) or export the new analysis file (Save Analysis Model). For more information, see Model.

8. Switch between ACP Pre and ACP Post.

   Click on the parent object in the tree view to switch between ACP Pre and ACP Post. You may also right click the parent object to call up the contextual menu and select ACP Post.

   Figure : Switch Between ACP Pre and Post

9. Import the results.

   In the ACP Post mode, solutions can be imported to evaluate the strength of the composite structure. In the tree view, import the result files by right clicking the Solution object. See Solutions for more details.

10. Perform composite postprocessing.

    Use definitions to define which results are evaluated in postprocessing. Plot these values in the scene for representation on the geometry or use sampling points for representation through the lay-up.

11. Save the composite definitions.

    Use the File menu or right-click the Models object in the tree view to use the contextual menu.

Release 18.2 - © ANSYS, Inc. All rights reserved.