How to do Load Combination in ANSYS—Method1


This post is about how to combine the loads, create load cases in ANSYS. Almost all professional projects will have load cases and load combinations. Although it varies from industry to industry, load combination is common. I am going to use the following terms very often. The best way I remember them are:

Load Step: a particular step in which you apply a load and have results loaded on to the database file(db file) after you solve.

Load Case: a results file which is a combination of one or more load steps results.

In general, you can define a load step anyway you want only during the pre-processing. Whereas you can define the load case file during post-processing.

In the following video, I am taking the previous example of cantilever I-beam to apply loads and combine them.

The loads I applied on the I-beam are :

Load Step 1: Apply a load of 1000N in X direction

Load Step 2: Apply a load of 1000N in Y direction

Load Step 3: Apply a load of 1000N in Z direction

Load Step 4: Apply an acceleration of 9.81m/sec^2 in Z direction

Load Step 5: Apply an acceleration of 9.81m/sec^2 in Y direction

Load Step 6: Apply an acceleration of 9.81m/sec^2 in X direction

The desired load combination is:

Load Combination 1: Load Step 3 + Load Step 4 –which is vertical load plus vertical acceleration due to gravity

Load Combination 2: Load Step 3 + Load Step 4+ 5% of Load Step 1+ 5% of Load Step 2+10% of Load Step 5+10% of Load Step 6     — which is vertical load+ vertical acceleration+ 5% in lateral directions and 10% acceleration in lateral direction.


The steps involved for load combination:

Step 1: Create Load Steps and Solve

Step 2: Convert Load Steps to Load Cases

Step 3: Use commands “LCOPER” and “LCFACT” to combine the load cases

Step 4: Create additional load steps by using “RAPPND”. Yes, you can convert the load cases to load steps so that you can view the view the results in Workbench via Mechanical. If you only create load cases, then you are limited to use classic ANSYS. In the video, I change the the step number to see the results on the fly!! Very useful command.

Step 5: Create seperate load case results file by using “LCWRITE”. This is useful for classic ANSYS users, as they can load the db file and results file(LCFILE command) and view the results / extract results.


This is a lot of information for first time user. It takes time to get the terminology and methods. Hope the following video makes things clear!!



4 thoughts on “How to do Load Combination in ANSYS—Method1


    can you tell me please how to apply self weight(i.e dead load) of a structure along with a dynamic load(i.e a time varying load) in ansys mechanical apdl?

    1. admin Post author

      Just apply gravity to include self weight and Force seperately. Sorry, lot of spam comments, I missed your comment.

  2. ubuntuvps

    After a load case combination is performed for structural line elements, the principal stress data are not automatically updated in the database. Issue

    1. admin Post author

      Working with APDL commands have lot of issues with workbench updates. I always clear the solve data and re-run the model if it does not take lot of time. Also, double check your results with .rst file as shown in “APDL only” method.

Leave a Reply

Your email address will not be published. Required fields are marked *