 |
 |
|
|
||
|
 |
Department of Engineering |
|
|
|
|
| University of Cambridge > Engineering Department > computing help |
Chordal Tolerance refers to the accuracy that will determine the number of straight line segments used when approximating curved lines.
Choose Display from the pull-down menu and then Geometry.... In the form that pops up look for a box marked Display Lines and the value will be 0. Change this to 3 and then click on the Apply button. Then click on the "Refresh" icon and this should display the green lines.
Click on the button marked Define Region.... In the new form set `include' to Geometry. Change this to FEM if the objects are finite elements.
In the box marked Select Groups highlight the group or groups in which the objects reside. More than one group can be selected. Hold down the CTRL key and click on groups to de-select (if you have made a mistake).
Cick on OK in this form and in the original click on Write to report file if you want the requested information written to a file. This will bring up a new form for the report file name. You can choose the default file name (database-name.rpt.01) and click on the Apply button.
There are 2 boxes with the headings :
Then click on Apply button in the original form.
Action : Create Object : Surface Method : Edge option : 3 edgeThen click on the 3 edges which make up the triangular surface.
For any other situation use the 4 curve method.
Action : Transform Object : Surface Method : TranslateThen use the translation vector < 0 0 0 >. Then click on Apply. When Patran puts up the warning message window click on Yes for All. It will be good idea to create a separate geometry group and have it posted before attempting to do this. If different material properties have to be specified to the newly created surface then this will be useful.
Use the wireframe analogy in building up the mesh. Adjacent surfaces should share the side wholly not partly. Otherwise this will lead to mismatching nodes along these sides when the mesh is generated.
If the idea is to create a graded mesh and confine the density of elements to a local region then can use the following scheme to prevent propagation of geometry changes throughout the structure.
The above construction confines the density of the elements to the neighbourhood of surface 1.
The problem arises when you want to add surfaces/solids to a previously created group. The correct procedure is to make that group current before creating the new entities.
Click on the top menu Group and select Set Current .... Then in the new form select the group (to which you want to add entities) from the list under the heading Set Current Group. Then click on Cancel.
The viewport heading should now display this group's name. Now post any other groups you need (example any groups which may contain the points/lines required) to create the surfaces/solids).
Click on the top menu Group and select Post .... Then in the new form select the required groups from the list under the heading Select Groups to Post. Then click on Apply. When you do this make sure that the heading does not change.
Finally the following procedure can be used to move the entities to the correct group. Click on the top menu Group and select Move/Copy .... Then in the new form select the group which has wrongly got the entities from the list marked From Group. Then select the group to which these should belong to from the list marked To Group. Then click on the radio button Move. Then click on Selected Entities.... In the new form click on the entity types you want to move under the heading Geom on. For example if you want to move only surfaces click on the square button marked Surfaces. This will display all the surfaces under the column marked Move. Edit this to list only the surfaces you want to move. Then click on OK. Then click on Cancel in the Group form.
Then post only this group and check the entities in that group.
Set the Axis to be through the center of the circle and perpendicular to the plane of the circle.
Axis : { Point 9 [ x9 y9 1] }
Here Point 9 is the centre of the circle. Point 9 and [ x9 y9 1] represents a line normal to the plane of the circle. Set Total Angle = 360. Click on the box marked 'Curve List' and then select the 2 Point icon from the select menu. Then click on Points 9 and 11 (which from the radius). The circle is denoted as surface 2 in the figure below.
Change the setting to : Transform / Surface / Scale. Set the scale factors accordingly. For example to reduce the vertical axis (y) by half while keeping the horizontal axis (x) the same use : < 1.0 0.5 1.0>. Set the origin to the centre of the circle and then select the circle for the surface.
However if the axes of the ellipse are parallel to the original co-ordinate system then one needs to create a new co-ordinate system (Coord 1) with axes parallel to the axes of the ellipse. Choose : Create / Coord / Axis. Axis : Axis 1 and 2. Enter the co-ordinates for the origin and points on axis 1 and 2.
Origin : [ 0 0 0 ] Point ox Axis 1 : [ 1 1 0 ] Point ox Axis 2 : [ -1 1 0 ]In the above example the new co-ordinate system is at an angle of 45 degrees to the original system. It will have the label Coord 1. Then transform the circle into an ellipse as before but use the new coord system.
Refer. Coordinate Sytsem : Coord 1
Alternatively the above segment can be divided into a inner and outer surface using an intermediate circle (radius 15). For the outer surface mesh seeds are assigned in the same way as before.
For the inner surface the size of the elements can be controlled using Create / Mesh Control / Surface in the Finite Element form and assigning a Global edge length of 2.0. The created mesh is shown below :
The surfaces shown on the right can be superimposed on the geometry shown on the left becuase there is an exact match. Whereas in the case of the geometries shown below the surfaces shown on the right cannot be super-imposed on the surfaces shown in the left. Because ther are no common points/lines/surfaces.
However there is no need to resort to the use of super-imposed surfaces just to specify a different thickness. PATRAN allows for different regions of the mesh to be assigned different thickness. It is sufficient to divide the region to be assigned a different thickness into separate surfaces. For example the inner annulus consists of 4 surfaces. These are separate from the rest of the geometry. The inner annulus (consisiting of 4 surfaces) can be assigned a different thickness from the one to the rest of the geometry. This eliminates the need for the use of super-imposed surfaces.
For 2D PLANE STRESS analysis this thickness is specified in the Properties form.
In this method one makes a copy of the original journal file under a different name. For example plate0.db.jou is copied to plate1.db.jou. Then edit this file and change the line which has the database name to correspond to the new journal file name. Then search for the dimensions you want to change and replace these with the new values. Then save and exit this file. The journal file is a text file and all these changes can be carried out using the standard text editor. It is also possible to edit and remove any sequence of commands that is not wanted. However be careful not to delete any lines which might be relevant any subsequent operation.
Then start up PATRAN in the usual manner and choose File / Utilities / Rebuild.... Then choose the newly modified journal file and click on Apply. This will run through the journal file and re-create the new mesh.
The second method is useful if you plan to carry out a series of parametric studies where a number of variables are to be changed and the planned changes are substantial.
Here the journal file from a original analysis is copied under a different name as before. Then all the values (whether it be dimensions or material properties or mesh division) which are to be changed are replaced with parametric names. Then these parameters are grouped together and set to new values towards the top of the journal file. This is illustrated with an example :
uil_file_rebuild.start("/export/msc/patran8/patran80/abaqus.db", @
"/amd_tmp/rasp-16/users3/abcd1/p8/pipe2.db")
db_set_pref( 303, 3, 0, FALSE, 0.00099999998, "" )
STRING asm_create_grid_xyz_created_ids[VIRTUAL]
$ pipe outer radius
REAL pipe_out_rad
$ pipe inner radius
REAL pipe_in_rad
$ intermediate radius
REAL int_rad
$ final radius - marks the extent of the circular region
REAL fin_rad
$ no. of elements - layer (mesh divisions)
INTEGER lay_elno
$ no. of elements radially in a 45 deg segment
INTEGER rad_elno
...
$
pipe_out_rad = 0.5
pipe_in_rad = 0.487
int_rad = 0.7
fin_rad = 1.2
lay_elno = 3
rad_elno = 3
...
$#
asm_const_grid_xyz( "1", "[0 0 0]", "Coord 0", asm_create_grid_xyz_created_ids )
$# 1 Point created: Point 1
asm_const_grid_xyz( "2", "[`pipe_out_rad` 0 0]", "Coord 0", @
asm_create_grid_xyz_created_ids )
$# 1 Point created: Point 2
asm_const_grid_xyz( "3", "[ `int_rad` 0 0]", "Coord 0", @
asm_create_grid_xyz_created_ids )
$# 1 Point created: Point 3
asm_const_grid_xyz( "4", "[ `fin_rad` 0 0]", "Coord 0", @
asm_create_grid_xyz_created_ids )
$# 1 Point created: Point 4
...
mesh_seed_create( "Surface 34.4 33.4 40.4 39.4 38.4 37.4 36.4 35.4 ", 1, `rad_el
no`, @
0., 0., 0. )
|
|
| | Computing Help |[Finite Elements] | [Engineering Packages] |