Introduction to FEA with Solidworks and Cosmos Works
This note provides a brief introduction to using Cosmos Works for simple modeling of components. The first example will be to look at a 90o angle cantilever beam loaded assymetrically. This is tedious to do by calculation and a clear example of where modern sophisticated FEA packages can save time.
It should be noted that on our system the FEA package, Cosmos Works, can only be accessed via Solidworks, not directly.
i) Start Solidworks
ii) Set the units to SI, Newtons, kg, m, seconds.
iii) Click on 'Sketch', the three planes appear, click on the x-y 'Front' plane. This rotates the selected plane into the plane of the screen.
iv) Using 'Line', starting at the origin, sketch the approximate profile of the 0.05 x 0.05 x 0.005 angle section (which is to be in AISI 1020 steel, 1 m long and loaded with 100N at the free end). Use the 'Smart Dimension' to change the dimensions to those required.
v) Put an internal fillet 0.005 between the internal edges. Failure to include a finite fillet between internal edges gives rise to significant errors.
vi) Exit Sketch and click on 'Extruded Boss or Base' and put in the length of 1. Click OK and the beam will be extruded.
vii) Specify the material. Click on the appropriate icon in the model tree on the left and select the appropriate material.
viii) Save the model and start Cosmos Works.
ix) From the Cosmos Works menu, click on 'Study' and select 'Static'.
x) Apply the load. Zoom in on one end of the beam, select 'Loads / Restraints', click on force, select the end face and enter 1000 in the appropriate box on the left. For a direction, click on an edge parallel to the 'y' direction. Click OK. If the load is in the opposite direction to that required, tick the 'Reverse Direction' box.
xi) Restrain the beam. A significant problem when specifying restraints in FEA is that they are absolute, which is not possible in real life. It is therefore very easy to over constrain a component making it over stiff and under estimating the deflection. Considerable care is needed to avoid errors of this type.
The names used for the restraints are not very always accurately descriptive. We will use 'Reference Geometry'. This involves, with the top window on the left shaded pink, selecting the entity, vertex, edge or surface, to be restrained and then clicking in the lower smaller box in the left hand window, so it becomes shaded pink, then picking on an edge parallel to the direction in which the entity is to have no movement (or in some situations, a specified displacement).
Rotate the beam and zoom in on the other end.
Restrain, using 'Reference Geometry' the end face in the z direction (perpendicular to the end face) against translation in the z direction. This is important as it allows Poisson contraction effects to occur.
Restrain, using 'Reference Geometry' the outer upright edge (which is lying parallel to the y axis) from translation in the x direction.
Restrain, using 'Reference Geometry' the outer horizontal edge (which is lying parallel to the x axis) from translation in the y direction.
xii) Save the model, mesh it the run it.
xiii) Check the results. The deformed shape should show that the beam has twisted, moved down and sideways.
2 Stress Concentrations
Originally stress concentrations were worked out mathematically which was satisfactory for simple configurations. More complex configurations could only be determined by experimental work which was time consuming and not very accurate. The development of FEA made it possible to compute (geometric) stress concentration factors fairly easily. Modern modelling tools and the power of modern computers make complex geometries straightforward to assess. Examples are shafts with changes in section, grooves (eg valve stems) and holes.
As stress concentrations are usually adjacent to small features, such as holes and grooves, it may well be necessary to enter small dimensions into the meshing controls form to ensure that the results of the computation are sufficiently accurate in these regions.
To demonstrate the stress concentration caused by small holes in a beam, the example in 1, above, was modified by putting a 6mm diameter hole slightly (5mm) below the top of the beam and 30mm from the restrained end, see diagrams above. The maximum stress then moved from the end of the beam to the hole and the maximum stress by the hole was 102 MPa, whereas the maximum at the restrained end was 34MPa. This indicates a stress concentration factor of about 3.
3 Interference fit - Effect of Radial Pressure
The configuration and text below,
describe an interference fit. There is no information about the constraint of the inner bore nor of the fillet radius at 'd'. It was assumed that diameter A = 60mm, B = 55mm, C = 50mm and the length W was 50mm.
One eighth of this component was modelled and by using 'Reference Geometry' restraints the symmetry of the 1/8
portion modelled could be represented.
It was assumed that there were no restraints on the inner bore moving inwards.
To investigate the interference fit a radial inward pressure was applied to diameter 'B' of 1MPa.
This was modelled with fillet radii of 1mm and 0.2mm at 'd'.
Results are summarised in the table below:
|Location||Fillet d: 1mm radius||Fillet d: 0.2mm radius||Fillet d: 0.1mm radius|
|By open end, 55mm diameter||~ 11MPa VMEQ||~ 11MPa VMEQ||~ 11MPa VMEQ|
|Half way along 55mm dia surface||~ 6.5MPa VMEQ||~ 6.5MPa VMEQ||~ 6.8MPa VMEQ|
|In fillet 'd'|| ~ 7.5MPa VMEQ
~ 7.5MPa sigma 1
|~ 9.5MPa VMEQ|| ~ 10MPa VMEQ
( ~ 12.5MPa sigma 1)
|The values above were obtained using meshes generated by the default settings chosen by the software.
For the results below a finer mesh (by a factor of 10 smaller than the default) was specified for the region of the fillet.
| ~ 18MPa VMEQ
~ 21MPa sigma 1
For fine detail it is critical to specify accurate internal fillet radii and ensure a suitably fine mesh is generated in these regions.
Further information to be added.
David J Grieve, 23rd November 2007.