Hi scudelari,
I like to create a batch file (.BAT) to run the model or models from a command line. The batch file essentially becomes my “documentation” so that I can find the information whenever I need it. These commands can be entered individually in a command window, too. (Type “CMD” in the Windows “Start > Search programs and files” search bar.)
The overall steps are as follows:
- Do a Check Model whenever you are ready to do the analysis. “Analysis > Analysis > Check Model”.
- You may need to exit the software before you try to run the analysis from the command line or batch file. I did not test this step.
- View any folder with Windows Explorer.
- Create a batch file (right-click > New > Text Document) and change the filename AND extension (to .BAT). Note that you may need to set the “Tools > Folder Options > View” to display the file extensions; that is, uncheck “Hide extensions for known file types”. (If the .TXT extension is now shown when you create the new text document, then your extensions are hidden.)
- Right-click the batch file and choose “Edit”. Copy or type in the text of the batch file given below.
- You need to change the drive designations K: and J: to a drive that is not already in use.
- You need to change the path "C:\Program Files\Autodesk\Simulation 2014" to the location where your software is installed.
- You need to change the ‘folder with the model’ to the location of your model. “my model” is the name of the .FEM file that you normally open, and “.ds_data\5” is the design scenario that you want to analyze. (The design scenario folder contains the file “DS.ASD” that the processor reads.)
- You need to change the processor name “pppp” to the appropriate name. The list below is from the Help.
- There are various runtime options which you can see by entering “K:\pppp.exe -help” in a command window.
Contents of the batch file (copy or type this text)
:: use a drive substitution for the folder with the ADSK Sim Mech software
subst K: /d
subst K: "C:\Program Files\Autodesk\Simulation 2014"
:: use a drive substitution for the folder with the model
subst J: /d
subst J: "C:\Simulations\junk nf.ds_data\4"
:: run the analysis
K:\ssap1.exe "J:\ds" -run
pause
List of processors
- Linear static stress: ssap0 filename -run
- Natural frequency (modal): ssap1 filename -run
- Transient stress (modal superposition): ssap2 filename -run
- Response spectrum (modal superposition): ssap3 filename -run
- Transient stress (direct integration): ssap4 filename -run
- Frequency response (modal superposition): ssap5 filename -run
- Critical buckling load: ssap6s filename -run
- Random vibration (modal superposition): ssap7 filename -run
- Natural frequency (modal) with load stiffening: ssap8s filename -run
- Weight and center of gravity: ssap9 filename -run
- Static stress with nonlinear materials, MES with linear materials, MES with nonlinear materials, and MES Riks Analysis: apak4 filename -run
- Steady-state heat transfer: ssap10 filename -run
- Transient heat transfer ssap11 filename -run
- Electrostatic: esap filename –run
I piece these instructions together from these pages in the Help:
- Perform Analyses - Run Simulation
- Schedule Analyses
