Space Frame Example in Ansys

Introduction

This tutorial was created using ANSYS 7.0 to solve a simple 3D space frame problem.

Problem Description

The problem to be solved in this example is the analysis of a bicycle frame. The problem to be modeled in this example is a simple bicycle frame shown in the following figure. The frame is to be built of hollow aluminum tubing having an outside diameter of 25mm and a wall thickness of 2mm.

Verification

The first step is to simplify the problem. Whenever you are trying out a new analysis type, you need something (ie analytical solution or experimental data) to compare the results to. This way you can be sure that you've gotten the correct analysis type, units, scale factors, etc.
The simplified version that will be used for this problem is that of a cantilever beam shown in the following figure:

Preprocessing: Defining the Problem

Give the Simplified Version a Title (such as 'Verification Model').Utility Menu > File > Change Title
Enter KeypointsFor this simple example, these keypoints are the ends of the beam.
- We are going to define 2 keypoints for the simplified structure as given in the following table
  keypoint coordinate
  x y z
  1 0 0 0
  2 500 0 0
- From the 'ANSYS Main Menu' select:
  Preprocessor > Modeling > Create > Keypoints > In Active CS
Form Lines

keypoint	coordinate
x	y	z
1	0	0	0
2	500	0	0

Select: Preprocessor > Modeling> Create > Lines > Lines > Straight Line.
Pick keypoint #1 (i.e. click on it). It will now be marked by a small yellow box.
Now pick keypoint #2. A permanent line will appear.
When you're done, click on 'OK' in the 'Create Straight Line' window.

Define the Type of Element

From the Preprocessor Menu, select: Element Type > Add/Edit/Delete.
Click on the 'Add...' button. The following window will appear:
For this example, we will use the 3D elastic straight pipe element as selected in the above figure. Select the element shown and click 'OK'. You should see 'Type 1 PIPE16' in the 'Element Types' window.
Click on the 'Options...' button in the 'Element Types' dialog box. The following window will appear:
Click and hold the K6 button (second from the bottom), and select 'Include Output' and click 'OK'. This gives us extra force and moment output.
Click on 'Close' in the 'Element Types' dialog box and close the 'Element Type' menu.

Define Geometric Properties

In the Preprocessor menu, select Real Constants > Add/Edit/Delete
Click Add... and select 'Type 1 PIPE16' (actually it is already selected). Click on 'OK'.
Enter the following geometric properties:
```
      Outside diameter    OD:   25
      Wall thickness  TKWALL:    2
  
```
This defines an outside pipe diameter of 25mm and a wall thickness of 2mm.
Click on 'OK'.
'Set 1' now appears in the dialog box. Click on 'Close' in the 'Real Constants' window.

Element Material Properties

In the 'Preprocessor' menu select Material Props > Material Models...
Double click Structural > Linear > Elastic and select 'Isotropic' (double click on it)
Close the 'Define Material Model Behavior' Window.We are going to give the properties of Aluminum. Enter the following field:
EX 70000
PRXY 0.33
Set these properties and click on 'OK'.

Mesh Size

In the Preprocessor menu select Meshing > Size Cntrls > ManualSize > Lines > All Lines
In the size 'SIZE' field, enter the desired element length. For this example we want an element length of 2cm, therefore, enter '20' (i.e 20mm) and then click 'OK'. Note that we have not yet meshed the geometry, we have simply defined the element sizes.(Alternatively, we could enter the number of divisions we want in the line. For an element length of 2cm, we would enter 25 [ie 25 divisions]).

NOTE

Mesh

In the 'Preprocessor' menu select Meshing > Mesh > Lines and click 'Pick All' in the 'Mesh Lines' Window

Saving Your Work

Utility Menu > File > Save as...

Solution Phase: Assigning Loads and Solving

Define Analysis Type

From the Solution Menu, select 'Analysis Type > New Analysis'.
Ensure that 'Static' is selected and click 'OK'.

Apply Constraints

In the Solution menu, select Define Loads > Apply > Structural > Displacement > On Keypoints
Select the left end of the rod (Keypoint 1) by clicking on it in the Graphics Window and click on 'OK' in the 'Apply U,ROT on KPs' window.
This location is fixed which means that all translational and rotational degrees of freedom (DOFs) are constrained. Therefore, select 'All DOF' by clicking on it and enter '0' in the Value field and click 'OK'.

Apply Loads

In the Structural menu, select Force/Moment > on Keypoints.
Select the second Keypoint (right end of bar) and click 'OK' in the 'Apply F/M' window.
Click on the 'Direction of force/mom' at the top and select FY.
Enter a value of -100 in the 'Force/moment value' box and click 'OK'.
The force will appear in the graphics window as a red arrow.

Solving the System

Solution > Solve > Current LS

Postprocessing: Viewing the Results

Hand Calculations

Deflection

Stress

Results Using ANSYS

Deformation

from the Main Menu select General Postproc from the 'ANSYS Main Menu'. In this menu you will find a variety of options, the two which we will deal with now are 'Plot Results' and 'List Results'
Select Plot Results > Deformed Shape.
Select 'Def + undef edge' and click 'OK' to view both the deformed and the undeformed object.
Observe the value of the maximum deflection in the upper left hand corner (shown here surrounded by a blue border for emphasis). This is identical to that obtained via hand calculations.

Deflection

From the 'General Postproc' menu select Plot results > Contour Plot > Nodal Solution.
Select 'DOF solution' and 'USUM'. Leave the other selections as the default values. Click 'OK'.
You may want to have a more useful scale, which can be accomplished by going to the Utility Menu and selecting Plot Controls > Style > Contours > Uniform Contours
The deflection can also be obtained as a list as shown below. General Postproc > List Results > Nodal Solution ... select 'DOF Solution' and 'ALL DOFs' from the lists in the 'List Nodal Solution' window and click 'OK'. This means that we want to see a listing of all translational and rotational degrees of freedom from the solution. If we had only wanted to see the displacements for example, we would have chosen 'ALL Us' instead of 'ALL DOFs'.
Are these results what you expected? Again, the maximum deflection occurs at node 2, the right end of the rod. Also note that all the rotational and translational degrees of freedom were constrained to zero at node 1.
If you wanted to save these results to a file, use the mouse to go to the 'File' menu (at the upper left-hand corner of this list window) and select 'Save as'.

Stresses

Element Table

From the General Postprocessor menu select Element Table > Define Table...
Click on 'Add...'
As shown above, in the 'Item,Comp' boxes in the above window, select 'Stress' and 'von Mises SEQV'
Click on 'OK' and close the 'Element Table Data' window.
Plot the Stresses by selecting Plot Elem Table in the Element Table Menu
The following window will appear. Ensure that 'SEQV' is selected and click 'OK'
If you changed the contour intervals for the Displacement plot to "User Specified" you may need to switch this back to "Auto calculated" to obtain new values for VMIN/VMAX.Utility Menu > PlotCtrls > Style > Contours > Uniform Contours ...
Again, select more appropriate intervals for the contour plot
List the Stresses
- From the 'Element Table' menu, select 'List Elem Table'
- From the 'List Element Table Data' window which appears ensure 'SEQV' is highlighted
- Click 'OK'
Note that a maximum stress of 64.914 MPa occurs at the fixed end of the beam as predicted analytically.

Bending Moment Diagrams

Element Table

General Postproc > Element Table > Define Table... . Click 'Add...'.
In the window,
1. Enter IMoment as the 'User label for item' - this will give a name to the data
2. Select 'By sequence num' in the Item box
3. Select 'SMISC' in the first Comp box
4. Enter SMISC,6 in the second Comp box
5. Click 'OK'
This will save all of the bending moment data at the left hand side (I side) of each element. Now we need to find the bending moment data at the right hand side (J side) of each element.
Again, click 'Add...' in the 'Element Table Data' window.
1. Enter JMoment as the 'User label for item' - again, this will give a name to the data
2. Same as above
3. Same as above
4. For step D, enter SMISC,12 in the second Comp box
5. Click 'OK'
Click 'Close' in the 'Element Table Data' window and close the 'Element Table' Menu. Select Plot Results > Contour Plot > Line Elem Res...
From the 'Plot Line-Element Results' window, select 'IMOMENT' from the pull down menu for LabI, and 'JMOMENT' from the pull down menu for LabJ. Click 'OK'. Note again that you can modify the intervals for the contour plot.
Now, you can double check these solutions analytically. Note that the line between the I and J point is a linear interpolation.
Before the explanation of the above steps, enter help pipe16 in the command line as shown below and then hit enter.
Briefly read the ANSYS documentation which appears, pay particular attention to the Tables near the end of the document (shown below).Table 1. PIPE16 Item, Sequence Numbers, and Definitions for the ETABLE Commands
node I

name item e Definition
MFORX SMISC 1 Member forces at the node
MFORY SMISC 2
MFORZ SMISC 3
MMOMX SMISC 4 Member moments at the node
MMOMY SMISC 5
MMOMZ SMISC 6
Note that SMISC 6 (which we used to obtain the values at node I) correspond to MMOMZ - the Member moment for node I. The value of 'e' varies with different Element Types, therefore you must check the ANSYS Documentation files for each element to determine the appropriate SMISC corresponding to the plot you wish to generate.

node I

name	item	e	Definition
MFORX	SMISC	1	Member forces at the node
MFORY	SMISC	2
MFORZ	SMISC	3
MMOMX	SMISC	4	Member moments at the node
MMOMY	SMISC	5
MMOMZ	SMISC	6

Command File Mode of Solution

The above example was solved using the Graphical User Interface (or GUI) of ANSYS. This problem can also been solved using the ANSYS command language interface. To see the benefits of the command line clear your current file:

From the Utility menu select: File > Clear and Start New
Ensure that 'Read File' is selected then click 'OK'
select 'yes' in the following window.

Copy the following code into the command line, then hit enter. Note that the text following the "!" are comments.

/PREP7   ! Preprocessor
K,1,0,0,0,    ! Keypoint, 1, x, y, z
K,2,500,0,0,  ! Keypoint, 2, x, y, z
L,1,2     ! Line from keypoint 1 to 2
!*
ET,1,PIPE16   ! Element Type = pipe 16
KEYOPT,1,6,1  ! This is the changed option to give the extra force and moment output
!*  
R,1,25,2,  ! Real Constant, Material 1, Outside Diameter, Wall thickness
!*  
MP,EX,1,70000  ! Material Properties, Young's Modulus, Material 1, 70000 MPa
MP,PRXY,1,0.33    ! Material Properties, Major Poisson's Ratio, Material 1, 0.33
!*  
LESIZE,ALL,20           ! Element sizes, all of the lines, 20 mm   
LMESH,1    ! Mesh the lines
FINISH                  ! Exit preprocessor
/SOLU          ! Solution
ANTYPE,0                ! The type of analysis (static)
!*
DK,1, ,0, ,0,ALL  ! Apply a Displacement to Keypoint 1 to all DOF
FK,2,FY,-100   ! Apply a Force to Keypoint 2 of -100 N in the y direction 
/STATUS,SOLU     
SOLVE     ! Solve the problem
FINISH

Note that you have now finished Postprocessing and the Solution Phase with just these few lines of code. There are codes to complete the Postprocessing but we will review these later.

Bicycle Example

Now we will return to the analysis of the bike frame. The steps which you completed in the verification example will not be explained in great detail, therefore use the verification example as a reference as required. We will be combining the use of the Graphic User Interface (GUI) with the use of command lines.
Recall the geometry and dimensions of the bicycle frame:

Preprocessing: Defining the Problem

Clear any old ANSYS files and start a new fileUtility Menu > File > Clear and Start New
Give the Example a Title
Utility menu > File > Change Title
Defining Some VariablesWe are going to define the vertices of the frame using variables. These variables represent the various lengths of the bicycle members. Notice that by using variables like this, it is very easy to set up a parametric description of your model. This will enable us to quickly redefine the frame should changes be necessary. The quickest way to enter these variables is via the 'ANSYS Input' window which was used above to input the command line codes for the verification model. Type in each of the following lines followed by Enter.
```
       x1 = 500
       x2 = 825
       y1 = 325
       y2 = 400
       z1 =  50
    
```
Enter Keypoints

frame vertices

We are going to define 6 keypoints for this structure as given in the following table (these keypoints are depicted by the circled numbers in the above figure):
keypoint coordinate
x y z
1 0 y1 0
2 0 y2 0
3 x1 y2 0
4 x1 0 0
5 x2 0 z1
6 x2 0 -z1
Now instead of using the GUI window we are going to enter code into the 'command line'. First, open the 'Preprocessor Menu' from the 'ANSYS Main Menu'. The preprocessor menu has to be open in order for the preprocessor commands to be recognized. Alternatively, you can type /PREP7 into the command line. The command line format required to enter a keypoint is as follows:
```
 K, NPT, X, Y, Z
```
where, each Abbreviation is representative of the following:
```
 Keypoint, Reference number for the keypoint, coords x/y/z
```
For a more detailed explanation, type help k into the command lineFor example, to enter the first keypoint type:
```
 K,1,0,y1,0
```
into the command line followed by Enter.As with any programming language, you may need to add comments. The exclamation mark indicates that anything following it is commented out. ie - for the second keypoint you might type:
```
 K,2,0,y2,0 ! keypoint, #, x=0, y=y2, z=0 
```
Enter the 4 remaining keypoints (listed in the table above) using the command line
Now you may want to check to ensure that you entered all of the keypoints correctly:
Utility Menu > List > Keypoints > Coordinates only
(Alternatively, type 'KLIST' into the command line)
If there are any keypoints which need to be re-entered, simply re-enter the code. A previously defined keypoint of the same number will be redefined. However, if there is one that needs to be deleted simply enter the following code:
```
 KDELE,#
```
where # corresponds to the number of the keypoint.

keypoint	coordinate
x	y	z
1	0	y1	0
2	0	y2	0
3	x1	y2	0
4	x1	0	0
5	x2	0	z1
6	x2	0	-z1

y1 = 325

Changing Orientation of the Plot

To get a better view of our view of our model, we'll view it in an isometric view:

Select Utility menu bar > PlotCtrls > Pan, Zoom, Rotate...'

In the window that appears (shown left), you have many controls. Try experimenting with them. By turning on the dynamic mode (click on the checkbox beside 'Dynamic Mode') you can use the mouse to drag the image, translating and rotating it on all three axes.
To get an isometric view, click on 'Iso' (at the top right). You can either leave the 'Pan, Zoom, Rotate' window open and move it to an empty area on the screen, or close it if your screen is already cluttered.

Create Lines

line	keypoint
line	1st	2nd
1	1	2
2	2	3
3	3	4
4	1	4
5	3	5
6	4	5
7	3	6
8	4	6

Again, we will use the command line to create the lines. The command format to create a straight line looks like:

  L, P1, P2 
  Line, Keypoint at the beginning of the line, Keypoint at the end of line

For example, to obtain the first line, I would write: ' L,1,2 '
Note: unlike 'Keypoints', 'Lines' will automatically assign themselves the next available reference number.

Enter the remaining lines until you get a picture like that shown below.
Again, check to ensure that you entered all of the lines correctly: type ' LLIST ' into the command line
If there are any lines which need to be changed, delete the line by typing the following code: ' LDELE,# ' where # corresponds to the reference number of the line. (This can be obtained from the list of lines). And then re-enter the line (note: a new reference number will be assigned)You should obtain the following:

Define the Type of Element
Preprocessor > Element Type > Add/Edit/Delete > AddAs in the verification model, define the type of element (pipe16). As in the verification model, don't forget to change Option K6 'Include Output' to obtain extra force and moment output.
Define Geometric Properties
Preprocessor > Real Constants > Add/Edit/DeleteNow specify geometric properties for the elements
```
 Outside diameter    OD:   25
 Wall thickness  TKWALL:    2
```
Element Material Properties

Preprocessor

 MP, LAB, MAT, C0
 Material Property,Valid material property label, Material Reference Number, value

To enter the Elastic Modulus (LAB = EX) of 70000 MPa, type: ' MP,EX,1,70000 '
To set Poisson's ratio (PRXY), type ' MP,PRXY,1,0.33 '

Mesh Size

Preprocessor > Meshing > Size Cntrls > ManualSize > Lines > All Lines

Mesh

In the 'Preprocessor' menu select 'Mesh' > 'Lines' and click 'Pick All' in the 'Mesh Lines' Window

Saving Your Job

Utility Menu > File > Save as...

Solution Phase: Assigning Loads and Solving

Close the 'Preprocessor' menu and open up the 'Solution' menu (from the same 'ANSYS Main Menu').

Define Analysis Type

Solution > Analysis Type > New Analysis... > Static

Apply Constraints

 
 DK, KPOI, Lab, VALUE, VALUE2, KEXPND, Lab2, Lab3, Lab4, Lab5, Lab6
 Displacement on K, K #, DOF label, value, value2, Expansion key, other DOF labels

 DK,1,UX,0,,,UY,UZ

^th

 DK,5,UY,0,,,UZ

^th

Apply the constraints to the other rear wheel location (Keypoint 6 - UY and UZ).
Now list the constraints ('DKLIST') and verify them against the following:
If you need to delete any of the constraints use the following command: 'DKDELE, K, Lab' (ie 'DKDELE,1,UZ' would delete the constraint in the 'z' direction for Keypoint 1)

Apply Loads

FK, KPOI, Lab, value, value2
Force loads at keypoints, K #, Force Label directions (FX, FY, FZ), value1, value2 (if req'd)

FK,3,FY,-600

FKLIST

FKDELE,3,FY

Solving the SystemSolution > Solve > Current LS

Postprocessing: Viewing the Results

To begin Postprocessing, open the 'General Postproc' Menu

DeformationPlot Results > Deformed Shape... 'Def + undef edge'
- You may want to try plotting this from different angles to get a better idea what's going on by using the 'Pan-Zoom-Rotate' menu that was earlier outlined.
- Try the 'Front' view button (Note that the views of 'Front', 'Left', 'Back', etc depend on how the object was first defined).
- Your screen should look like the plot below:
Deflections

Go to Utility menu > PlotCtrls > Numbering... and turn on 'Node numbers'. Turn everything else off.
Note the node numbers of interest. Of particular interest are those nodes where the constraints were applied to see if their displacements/rotations were indeed fixed to zero. Also note the node numbers of the seat and crank locations.
List the Nodal Deflections (Main Menu > General Postproc > List Results > Nodal Solution...'). Are the displacements and rotations as you expected?
Plot the deflection as well.General Postproc > Plot Results > (-Contour Plot-) Nodal Solution select 'DOF solution' and 'USUM' in the window
Don't forget to use more useful intervals.

Element Forces

Select 'Element Solution...' from the 'List Results' menu.
Select 'Nodal force data' and 'All forces' from the lists displayed.
Click on 'OK'.
For each element in the model, the force/moment values at each of the two nodes per element will be displayed.
Close this list window when you are finished browsing.
Then close the 'List Results' menu.

StressesAs shown in the cantilever beam example, use the Element Table to gain access to derived stresses.
- General Postproc > Element Table > Define Table ...
- Select 'Add'
- Select 'Stress' and 'von Mises'
- Element Table > Plot Elem Table
- Again, select appropriate intervals for the contour plot
Bending Moment Diagrams

Element Table > Define Table...

Plot Results > Line Elem Res...

MechDocs Blog

Tuesday 18 September 2012

Space Frame Example in Ansys

Introduction

Problem Description

Verification

Preprocessing: Defining the Problem

Solution Phase: Assigning Loads and Solving

Postprocessing: Viewing the Results

Command File Mode of Solution

Bicycle Example

Preprocessing: Defining the Problem

Solution Phase: Assigning Loads and Solving

Postprocessing: Viewing the Results

1 comment:

Advertisement

Subscribe Us

Labels

Popular Posts

About The Author

Blog Archive

Labels List

Subscribe Here

Know Us

Search

Recent

Slider(Do Not Edit Here!)

Popular

Comments

Author

Main Nav

Banner Ad

Labels

Contact Us

Flickr

	`EX 70000`
	`PRXY 0.33`