Tag Archives: structural

How to do Load Combination-method 4

Published by:


In this method, load combination using Design Assessment in ANSYS Workbench is explained. Design Assessment can be used for Solution Combination, Beam Check(according to AISC, API-WSD etc needs seperate license), Fatigue Check(for beams using FATJACK needs seperate license). Design Assessment has very few post-processing result outputs. To use this method, the analysis has to be linear and the model should be same for all the analysis systems. In the following video, I have used only one analysis system(static structural) with 8 load steps(created in first method). This video explains how to create the load steps 7,8 using the Design Assessment and later compare the results with load steps 7 and 8.

Thanks for reading the post!!

–Vamshi Goli


How to do Load Combination-method 3

Published by:


In this method, the load combination files created using LCWRITE command are used for comparing the results. This method is useful

  • When you just want to send the database file and the results files only instead of sending the complex project with all the details.
  • In other cases, where you want to load the .db file and results files into an external program.
  • If you have lot of cases, instead of numbers, the load case file names help identifying the results easily.

To use this method, before solving the model, Analysis Settings have to be changed as shown in the video below. After solving the model, database file(file.db file) is created along with the two load case files .L1 and .L2. Using the GUI interface(as shown in the video) or by using “LCFILE” and “LCASE” comands, you can load these load case results file and view the results. Here is the video illustrating the process:


–Thanks for reading the post!

—Vamshi Goli!!

How to do load combination in ANSYS–Method 2

Published by:

In the previous post, load combinations using APDL commands are shown. In this post, load combination using multiple analysis systems in the Workbench project page.

With this method, both the analysis systems share the “Model” which includes Engineering Data, Geometry and Mesh. Only boundary conditions(fixed support and force) and post processing are recreated.

In the first analysis system, Vertical Load and Standard Gravity Acceleration Load is applied.

In the second analysis system, along with the vertical load and gravity, 5% force and 10% acceleration is applied in other two directions. The following video shows this method 2.



Look for the upcoming video where the ANSYS load case files are used to post-process the results.

How to do Load Combination in ANSYS—Method1

Published by:


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!!