Lesson 01
ANSYS Basics,
Sample 01: simple steel bracket analysis:
The bracket is two parts, the base plate: 200*200mm, 20 mm thick.
The second welded part: 100*200, 20 mm thick.
We will fix this to the concrete column of wall using 4 anchor bolts at the 4 corners
Idea of solution:
Modeling the structure using ANSYS, applying support as point support, and in this case we can get easy the reactions later at each bolt.
Of course we will check the steel bracket against the stresses,
Using a steel: E= 205000 N/mm2
Poisson ratio = 0.3
1- Using ANSYS:
You must note that the power of using ANSYS that the program is empty… strange? No that’s true. That mean the program doesn’t know the units you are using like force, area units… that mean you just start with any units you want then you will get the results in the same units.
For example we will use mm, N, N/mm2 for E, and we will get the stress in N/mm2
Before you start I like to mention that the program looks very difficult and most of us heard that ANSYS is very advance and very difficult, forget that blab la bla. When you start you’ll be amazed it’s easy YES. And after using ANSYS you will start to feel the material behavior.
2- Understanding ANSYS:
ANSYS uses finite elements method (FEM) and before you start with ANSYS its better to have a look and understand what is FEM, its enough to read a few pages about FEM to start with ANSYS.
· Phase 1: Modeling the structure using 1:1 scale and here you have 2 choices:
a- Using the program options and drawing utility to do that. It’s a little long but easy if you have no idea about CAD-3D, and I will link some documents about how to do that later.
b- The easy way is to use AutoCAD 3d then export the file to (SAT), I did prepare the SAT file for you so you can start with it , download the file from here.
· Phase 2: assign material and mesh the structure by using one of the program elements.
· Phase 3: assign the loads and the support.
· Phase 4: analysis.
· Phase 5: reading result.
START NOW,
Open AutoCAD then
File > Export > [ choose ACIS(.sat) ] > select the bracket then ok
Open ANSYS:
- To choose the working directory:
File > change Directory
- Importing the SAT file:
File > import > SAT
- To see the solid shape of or structure:
plotCtrls > style > solid model facets > [choose normal faceting] OK
Plot > replot
Please try the command plot> . . . to see the difference between plotting lines, points..
Your structure shall look as the picture below.
You can take a picture of your structure:
plotCtrls > hard copy > to file
the picture shall be saved in the folder you choose at the beginning, this is important when you want to prepare a report showing the shape or the stresses..
now we have to prepare the volume (solid)
the shape must be one solid, check first how many solids you have
plotCtrls > numbering > VOLU volume numbers
Volume = solid, you will see two colors that mean your structure is two solids.
To make them one:
Preprocessor>Modeling>Operate>Booleans>Add>Volumes. Click on Pick All. now we have added all the volumes into a single volume.
Now you have only one solid
Defining the material:
Preprocessor>Material Properties>Material Models. In the window that
comes up, select
Structural>Linear>Elastic>Isotropic.
Put the numbers in the following:
You finished selecting the material you want to use, STEEL.
Now we have to choose an element for the FEM meshing.
The program have a lot of elements type, don’t worry you will get familiar with It soon, for now just choose the following which can cover almost all steel design.
These elements are used for the small pieces of meshing
Preprocessor>Element Type>Add/Edit/Delete... In the 'Element Types' window that opens click on Add... The following window opens:
After finishing the FEM element type we will do the meshing.
The program has a very useful tool:
Preprocessor>meshing>mesh tool
In the size controls > click SET and enter 10 in the box which is the FEM meshing element size, this number depend on the shape of the structure and the accurate of result you want. To know more check the FEM.
Click MESH > choose the structure > OK
You have the following.
Applying loads and support:
30KN= 30000N
Preprocessor>loads>define loads>apply>structural>force/moment>on nodes
Pick the point where the point load is applied and enter the load value –y
Click OK to see the following.
To apply to support conditions rotate the bracket to see the back of it, you can do that easely by holding Ctrl +right mouse click
Apply the support:
Preprocessor>loads>define loads>apply>structural>force>displacement>on nodes
Choose the four points at the four corners.. Click OK
Hold the movement in the three directions, X Y Z
Your structure is ready for analyzing, save now,
Analyzing:
Solution>solve>current LS
Wait till finish, some time it take a lot of time depending on the structure size and mesh size, and analyzing type.
Reading result:
General postproc>plot results>contour plot>nodal solu
We will choose: stress > Von Mises
Note here the value of 4985 (red color) forget it now we will know what is this later,
Assume we are using a steel 275 grade.
To tell ANSYS: print the stress value between 0 and 275
Plotctrs>style>contours>uniform contours
Enter the numbers in the next box
Check the result you get:
Rotate the bracket and enjoy the stresses values, at each point.
Regarding the BIG Value of stress 4985, because we applied the load at one point only and that is impossible in the real world. So in this point I well get a really very big stress but you can just ignore it.
The gray color in the stress picture showing us where is the area with a stress more than the value we entered 275 (Stress failure).
Regards to all
Nov. 11th 2009
