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:
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).
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.
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:
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!!
In this post, I am going to show couple of methods to change the material. In ANSYS, material properties like Young’s Modulus, Poisson’s Ratio for a particular material are available under Engineering Data. You can add these materials to the project. I used the same example project from the structural analysis of a plate.
In the following video, I have shown the following:
How to add material to the project
How to duplicate a material and edit the material properties
How to change material properties inside Mechanical using APDL commands. This method is useful especially if you are lazy enough to go back to workbench project page, add material or duplicate material to edit the material and then update the project to get the material added to the model. Using this method, you can avoid all that and directly edit the material property on the fly. Should be used only for quick checking. Otherwise you may forget the command snippet and wonder about the results.
This post about the modal analysis, “Meshed Connections” in Workbench and “Shared Topology” features in ANSYS.
Modal analysis is a powerful tool for finding out whether all the parts are connected in the way that they are intended to connect.
In the example below, a simple plate structure is modeled in Spaceclaim and first analyzed without any connections. When there are no connections, ANSYS gives an error for rigid body motion when you run it through Structural Analysis, but in modal analysis, it gives zero frequency modes. This means that user gets the opportunity to see all the connections in the model. Not only zero frequency modes, the modes with unwanted motion of the connected parts.
The later part of the video is to add connections through the new feature in ANSYS 16.0 “Mesh Connections” and getting the mode shapes with the correct connections. Then I have suppressed the connections in Workbench and modeled the same connections in Spaceclaim. ANSYS gives different options to reach the same solution. In a perfect world, you only need one. But, sometimes ANSYS gives squeaky errors where the connections can’t be acheived with one method and it might come through with other method. It is always good to have all the options/methods under the armory.
My last post was about structural analysis of a beam model. In this post, I modeled a plate(solid not surface) and meshed it with brick solid elements, applied the loads and solved it for a load in one direction.
As a workshop, please feel free to apply the load in the opposite direction and solve!
In the following video, I have modeled I-beam using ANSYS Spaceclaim and then exported it to ANSYS workbench; applied loads & boundary conditions; solved & post processed the results. Although, there are bunch of similar videos on youtube, I thought it is the best example to start. I hope it is helpful and easy!