Tag Archives: Workbench

Bolt Modeling in ANSYS—Method 1

Published by:

Hello All,

It’s been a long time since I have posted a tutorial. I have lot of topics ready for this blog but it is difficult to find apt models to suit the blog’s purpose of making the tutorials as practical as possible.

In this post, I have chosen a simple model for extracting shear loads for the bolts. Bolt modeling using line elements is explained. There are at least 5-6 other methods where you can model the bolts differently. Here is the link for the blog which explains in detail about the bolt modeling methods:

An Overview of Methods for Modelling Bolts in ANSYS

Line method is generally used for global analysis. By global analysis, I mean that all the components of the assembly are modeled and analyzed using a single analysis. This method is a conservative approach where large safety margins are common. Pretension is not included in this method. Note: In this video, beam elements are directly connected to the shell elements with a single node-to-node connection. In general, care should be taken to distribute the load to the nodes around the beam element (which is usually the size of the washer area).

 

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:

Hello,

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!!