CW_Design_Tutorial_1.doc

CosmosWorks Design Tutorial #1

(Draft 1 6/28/06)

Introduction

This is simply a restatement of the CosmosWorks online design scenarios tutorial with a little more visual detail supplied on the various menu picks and thought processes that are covered in the version supplied with the software.  In this lesson, you use design scenarios to investigate the effect of changing the applied loads and some dimensions of the part on the static analysis results.  The part is supported and loaded as shown in Figure 1.  The total force will be specified and it will be divided between various regions of the hanger.  The force on the central hanger (FCenter) is twice the force on each of the side hangers (FSide).   You will study the effect of changing the total applied force, thickness and height of hangers, and the thickness of the back plate on the stress distribution in the part.

Figure 1  The assembly of interest

First you need to switch to the CosmosWorks Manager by clicking its icon, .  Start a new study by:

1. Double click on the Part Name à Study
2. In the Study panel, assign a Study name.
3. Pick Analysis typeàStatic
4. Select the Mesh TypeàSolid Mesh. 

When the analysis menu expands you will see that the second item is associated with parameters. That is where you will have access to the definition of the parameters chosen by you to control, or define, the design scenarios.

Design parameter selection

To begin that process you should have planned ahead and identified the items (geometry, loads, restraints, etc.) that you want to see varied.  Then you have to input those design parameters.  The following parameters, in Table 1, have been chosen to define the design scenarios of interest here:

                                                                      Table 1

You can begin adding design parameters by defining the total force of interest:

1. In the CW Manager right click ParametersàEdit/Define to open the Parameters panel.
2. Since you are beginning with an empty list select Add.
3. The Add Parameters panel appears. Enter the Name à FTotal and add a comment.
4. Select the FilteràStructural Loads, and pick TypeàForce.
5. Finally set the initial Value and Units (say 120 lbs here as seen in Figure 2), OK.

Figure 2  Beginning the design parameter definitions

Then the entered data will appear in the top line of the Parameters panel.  Continue defining force parameters in a similar fashion. The next one will be given in terms of a parametric expression of the now know total force:

1. In the Parameters panel select Add again.
2. The Add Parameters panel appears. Enter the Name à FCenter and add a comment.
3. Select the FilteràStructural Loads, and pick TypeàForce and desired Units.
4. This time you want a parametric equation so check Expression.
5. Enter the relation, (FCenter =) FTotal/3, OK, as seen in Figure 3.
6. The second parameter appears in the Parameters panel.
7. Carry out the same sequence of steps for the last force parameter, FSide.  The only difference is the Expression which is (FSide=) FTotal/6.  The results for the last two force definitions are seen in Figure 3.  They will also appear as the next two lines in the Parameters panel.

Figure 3  Using expressions to relate parameters

The next design parameters will be part dimensions picked from the graphics display.  To assure that they are visible to pick:

1. Select the SolidWorks icon to open that Manager panel.
2. Right click on AnnotationsàShow Feature Dimensions.  See Figure 4.
3. Knowing that we are interested in Boss-Extrude3, expand it and open Sketch5 so the dimensions you want will be available to pick with the cursor.  (Here is an example where renaming Boss-Extrude3 to something related to the part would have been helpful.)
4. While it is not required for the design scenarios, remember that it may save time in later design reviews to change the dimension name to match the design parameter name that you are getting ready to assign.  In the graphics area select dimension 0.308472 (D1) àPropertiesàDimension PropertiesàNameàHeightàOK.  This is shown in Figure 5.

Figure 4  Turn on dimension displays to aid picking geometric parameters

Figure 5  Renaming the hanger height dimension

Now you are ready to continue defining the class of design parameters that are part dimensions:

1. Parameters panelàAdd.
2. In Add Parameters panelàNameàHeight.  Add a comment.
3. FilteràModel dimensions (see left of Figure 6).
4. In the graphics area pick the above dimension (0.308472 in).  Note that the Type àLinear Dimensions, Unitsàin, Value, and full Model dimension name are automatically inserted.  Check them and pick OK (Figure 6 right).
5. Repeat this process, including renaming the dimension, for the hanger thickness of 0.023000 as seen in the top of Figure 7.  In Add ParametersàNameàThickness.
6. The final dimension parameter is the back plate thickness of 0.060000 (top right of Figure 7).  Simply pick it (without renaming) and give it the parameter nameàBack_T, OK.
7. Now the initial design parameters are complete as seen in the Parameter panel of Figure 8.

Figure 6  Select the hanger height design parameter via a graphs pick

Figure 7  Rename and pick the hanger thickness as a parameter

Figure 8  The completed geometric and force design parameter definitions

Linking force or restraint parameters to the analysis model

The three geometric parameters are now related to the solid model, but we have not yet linked the two free force parameters (FCenter and FSide) to the finite element model.  Before doing that the basic material properties and restraints for the analysis will be defined as sketched in Figure 9:

1. In the CosmosWorks Manager menu, SolidàEdit/Define MaterialsàSteelàAllow steel.
2. Right click on Loads/RestraintsàRestraintsàOn cylindrical face.  Select the top two cylindrical holes and set Circumferential component = 0.  Either of those will eliminate a rigid body motion (RBM) about the vertical (z-) axis.  The zero circumferential displacement around the full circle includes two points where the x-displacement will also be zero and two points with zero y-displacements.  Thus, rigid body translations in x- and y- directions are prevented (now takes care of 3 of 6 RBM).
3. Right click on Loads/RestraintsàRestraintsàOn flat face.  Select the top surface of the back plate.
4. Set the normal (z-) component to zero, OK.  That will eliminate the possible RBM of a z-displacement, x-rotation, and y-rotation (6 of 6).

...