 |
 |
|
|
||
|
 |
Department of Engineering |
|
|
|
|
| University of Cambridge > Engineering Department > computing help |
Click on the radio button Loads/BCs and change the `Action' to Plot Markers. Under the heading marked Assigned Load/BC Sets select the boundary conditions and loadings you want to be displayed. In the Select Groups category select the groups which has the finite element entities. Then click on the Apply button.
This should erase the markers. If not click on the Reset graphics icon in the top right hand corner. It is the 3rd icon.
The first , (comma) indicates that the degree of freedom in direction 1 is free. If this was a 3-dimensional example then the 3rd degree of freedom is also free becuase it has not been specified. In the above example the 2nd degree of freedom is fixed at 0.
The applied positive pressures are directed in the direction of the positive normal. Applying a negative pressure will be in the direction opposite to it.
Click on the radio button Loads/BCs and and in the form make the following selection :
Action : Create Object : Inertial Load Type : Element Uniform New Set Name : Enter a appropriate name - example : self-wt Target Element Type : 2D or 3D (Make the appropriate choice)Click on the button Input Data... and in the new form in the box marked Trans accel
In the orinial form click on the button Select Application Region... and in the new form select the radio button Geometry or FEM for the `Geometry filter'. Then select the elements or surfaces/bodies. Click on Add and then finally on the OK button.
In the original form click on Apply. This should display yellow arrows pointing in the direction in which the gravity is acting and the magnitude (for this example it will be 1).
The user may have to calcualte the equivalent set of point loads for the individual nodes and specify these as point loads.
If the element sides are 2 noded then the line load is split equally between the 2 nodes. If there are a series of sides then mutiply the line load by the length of the side and apply half to each node. Interior nodes will take contribution from the sides at either side.
If the elements are 3 noded then the total load (line load multiplied by length) is split in the ratio of 1 : 4 : 1 between the nodes. The centre node taking 2/3 rd of the total load and the end nodes 1/6 th of the total load. Again sum the contribution from either sides for end nodes in the interior.
For higher order elements similar factors can be calculated using the shape functions and the principle of virtual work (see any standard book on finite elements).
Consider the situation where lines L1 ans l2 form part of the surfaces which define the geometry (in the figure below). Assume that you also have defined a line L3 which connects points 1 and 3.
Consider the situation where the vertical side between points 1 and 3 is to be retstrained from moving in the horizontal direction. Then this boundary condition should be specified on lines L1 and L2 but not L3 (as a short cut). the reason is when the finite element mesh is created lines L1 ansd l2 are associated with the nodes that are created. Line L3 is not associated with these nodes.
If you attempt to specify the boundary condition on L3 only the nodes at points 1 and 2 will be asssigned that boundary conditions. All the intermediate nodes between points 1 and 3 will not be assigned the boundary condition.
Action : Analyze Object : Entire Model Method : Full RunClick on Step Creation.... In the new form set
Solution Type : Nonlinear Static
Then click on Solution Parameters.... In the new form set
Riks Method = ON Stopping conditions : max Load Multiplier Max Load Multiplier : 1.0
This is illustrated with an example :
First of all choose the following settings :
Action / Object / Method : Create / Spatial / PCL Function
Field Name : < Enter an appropriate name here> Example : pressure
Field Type : <> Scalar <> Vector
Choose Vector for prescribed displacement specification.
Choose Scalar for pressure variation.
Co-ordinate System Type : <> Real <> Parametric
Choose REAL if using the co-ordinates of the new system.
Here the default co-ordinate system (Co-ord 0) which is halfway up the side is not suitable for specifying the pressure variation. It is simpler to create a co-ordinate system with origin coinciding with the base of the side. Lets call this Co-ord 1.
Co-ordinate System : Change the default (co-ord 0) to co-ord 1.Since the pressure variation is scalar enter the relationship in the box marked "Scalar Function".
Example : p = ( 10. - 'Y ) * ( 150. / 10. )
= ( 10. - 'Y ) * 15.
Here click on the appropriate independent variable ('Y)
from the box of the same name whenever you want to use one of this
variable in the equation.
Now click on APPLY to complete creation of the field.
Then open the LOADs/BCs form and give the pressure distribution a name and choose 3D for "Element Type". Then click on the Input Data.... In the new form the name of the previously specified pressure relationship (press) will be listed under the heading Field.
Click on the box marked "Uniform Pressure" and then click on "pressure" entry from the "field" section. Then click on OK and complete the form in the usual manner.
Use the Loads/BCs form and choose : Action / Object / Type = Create / Contact / Element Uniform. Then choose Deform-Deform for "option" for contact between two deformable bodies.
Enter a meaningful name for the contact pair you are about to define, in the box marked New set name.
Click on Input Data... and in the new form choose the contact type to be either General or Tied. Enter appropriate values of Frictional coefficient and limiting shear stress if General was chosen. Initial adjustment tolerance also needs to be specified for both types of contact. Choose a value of about 1% of the largest dimension for this. This is the amount the position of the nodes on either sides can be adjusted to establish contact. Click on OK on this form and then in the main form click on Select Application REgions....
In the new form leave both master and slave surfaces at solid Face if dealing with 3-dimensional solids. If shell elements are involved then it can be set to shell surface.
Set active region to master and then choose the contact surface on the master component. If components of different materials are coming into contact then in general the stiffer of the two is selected as the master.
Similarly set active region to slave and then choose the surface which comes into contact on the slave component. Note that "master" can penetrate into "slave". Also the slave surface should have a more finer mesh. Once both sets of surfaces have been identified click on OK and then in the main form click on Apply.
In a complex assembly with several components there will be several sets of contact pairs needs defining. Repeat this procedure for each pair of such contacts.
However there are situations where there is no choice but to deal with the f.e.mesh. For example consider the situation where a point load is to be applied to node which is coincident with a point which has been used in the generation of the geometry. Then you need to create the mesh and then apply the load to the node in question. Alternatively create the geometry which will give a coincident point where the concentrated load is to be applied apply it the point
Here is a different example : Equal bending moment has to be applied to all the nodes on a particular face. Here the total bending moment is to be equally divided amongst all the nodes. Here one needs to work out how many nodes there is ging to be. Then apply the bending moment divided by the number of the nodes to the geometry.
In the list form chnage the cordinate system to : Coord 1. Select x and this will display a new box for x value. In cylindrical co-ordinate system x would represent the (first) radial co-odrinate. So set the X value to be the same as the radius of the circular hole. Also set the TOL-XYZ to an appropriate value so that only the nodes along the circular hole will be selected. Check that the radio button for Target List is set to A. Now click on Apply. Now click on Add to Group... in the 'List A' form. The 'lista' contents should hopefully have all the nodes along the circular hole. These nodes can be highlighted and cut and pasted into any Select Application Region for nodes for applying a radial load in the Loads/BCs form.
|
|
| | Computing Help |[Finite Elements] | [Engineering Packages] |