How do I check if I have reached mesh independence when doing FEA on a cantilever beam subject by a force on one end and the other is fixed. I'm only analysing deformation and stress. I kept on reducing the mesh size hoping that with finer mesh the deformation will become constant but i'm not getting it.
FEA is by nature an approximation of the real world and it is expected that the results should converge to the correct answer the better the model approximates the real part.
The convergence is however element dependant. If you use a single beam (1D) element you should get the same answer as for 1 million beam elements.
I must assume you used solid elements, since if the deflection is not converging it is possibly because you have few elements through the thickness of the part. Single solid elements do not bend so well and therefore need more elements through the thickness so that each element bend less.
What you can do, is to plot the deflection result you get against element size on a graph (and also keep track of the total number of elements in the model and how long each model solves)
Also remember that stresses at a stress concentration can theoretically be equal to infinity and reducing the element sizes at such a location will also start to match this theoretical result (of infinity!) the smaller the elements become, but I am curious why your deflection result does not converge since that is unlikely to change much.
The most common cause of non-convergence is when the loading and /or constraints is changed unintentionally by the user every time the mesh is changed.
Modeling a cantilever beam using beam elements is easiest - A single element will give the correct displacement for an axial force, bending moment, shear force, gravity load and constant distributed load (and any combination of the above).
Using solid elements, not all of these load types will yield the correct result with a single element. Refining the mesh in order to find a converged result can only yield correct results if the models represent the same thing:
Constraints and loads need to be applied distributed over a finite area. Applying point-load and/or point constraint will cause larger deformation as the mesh is refined because the load is being distributed over a smaller-and-smaller area as the mesh is being refined.
If the mesh is very fine, a point load is the same as applying the force on a real structure using a very strong and very sharp needle - it will simply cause a massive indentation locally.
If the load is distributed over an area of (for example) 10mm x 10mm, the load distribution stays the same independent of the mesh density - More nodes are being loaded but each node is loaded with a smaller force, yielding the same normal pressure and same effective force being applied. (The load is applied as a pressure, not a force)
For constraints, look out for constraints on edges or corners only: They are the same as constraining with a very sharp knife-edge or needle respectively, something that is impossible in real life as it would cause an infinite stress to be applied locally. Constraining all nodes on a face again allows a surface area to transfer a load, allowing a finite pressure on the constraint face.
Another common misconception is when a force is being applied to a face: The force you enter is added to EACH node on the face, not distributed evenly. In this case, refining the mesh will increase the load being applied as more nodes are in the applied load area. The best way to apply a load on a solid-element model or shell-element model is using a pressure (or total load), not a force. This will keep the load applied constant when the mesh is being refined while also being closer to reality in how a load is introduced into a structure.