Case 1, 2 forces - yes....but, you'll probably have to add constraints to a point here or there to stabilize the model.
Case 2, displacement - yes...make one side constrained and add a displacement constraint to the other end (I think it is under advanced - add a value in the needed direction.)
Yes that is possible, you can use 'inertia relieve' for that. The opposing forces must be (allmost) equal ofcourse.
A deformation can also be done, by using the 'prescribed displacement' in 2015 and 2016. In previous versions you can use 'reference fixture' under advanced fixtures.
Can you post what your geometry looks like? If your geometry and loads and symmetric, you can leverage symmetry such that your constraints will not result in stress singularities.
As others have said, using inertia relieve is an option, but be aware that your displacement field will be polluted by "rigid" body motion (to what extent depends on how well the solver applies the stabilizing springs; applying them yourself is typically a better option).
You can potentially apply point constrains to remove all 6 DoF, but placing them in the proper location will be key.
Thanks for all responses. I attached an ugly figure to show you the geometry and my problems.
- On the left is my geometry: super simple, symmetric and no fillets.
- In the middle is the simulation I run before. Bottom face is fixed and a force is pulling from the topface. It gives me a nice (deformed) result. But... Also a high concentration of stress at the bottom edges (shown in red).
- On the right is my last attempt. Two prescribed displacement at both bottom- and topface. Because of the constraints-error I got, I used a roller/slider suspension on all other four faces. The results round the hole in the middle looks OK, but I also wish to demonstrate the poisson-like effect. With this configuration that is not possible.
Hope this makes sense, still struggling with nice constraints.. And I don't get the principle of how to use inertia relief on this simulation?
stressplate.png 29.5 KB
This model is a classic symmetry problem, and can be modeled with 1/8th symmetry for a solid element model, or 1/4th symmetry for a 2D idealization model (plane stress for example). In your model, you have 3 planes of symmetry for the 3D case and 2 planes of symmetry for the 2D case. For the image you posted, let's assume that the origin is at the center of the hole (and halfway between the front and back surfaces), and the +x-direction is to the right, the +y-direction is up, and the +z-direction is coming out of the screen. You three symmetry cuts would be: (1) along the XY plane, (2) along the XZ plane, and (3) along the YZ plane.
Each surface that you expose with a symmetry cut has a constraint associated with it. The assumption of symmetry is that the solution field (eg displacement, strain, stress, etc) is symmetric. For a 3D model, this simply means that each surface exposed with a symmetry cut is allow to translate in that surface's planer directions, but not in its' normal direction. If you model was made with shell elements (and thereby your symmetry planes create exposed edges), you'd also need to constraint the edge to not rotate along the edge (but allow it to rotate in the other two orthogonal directions). So for your model, the (1) symmetry cut would have a surface constraint to prevent motion only in the z-direction, the (2) cut would prevent motion only in the y-direction, and the (3) cut would prevent motion only in the x-direction.
Also keep in mind that each symmetry cut through a load will cut that load's value. For your model, you have two 1kN loads on the opposite faces, and each of these faces gets cut by two symmetry planes; the result is that you only apply 0.25kN (1kN*0.5*0.5) on each surface.
Inertial relief will add "soft springs" (springs with low stiffness) to your model to prevent rigid body motion. The mathematical description of this is that you can have a ill-conditioned problem if your displacement vector is not sufficiently defined so that solving the system of equations (i.e. using Gaussian elimination to get echelon form) will result in an infinite number of solutions for your displacement (you'll have a zero at your pivot element). These soft springs modify your stiffness matrix and displacement vector so that your problem is no longer ill-conditioned.
A physical interpretation of this in your model is that having equal and opposite loads means the net acceleration on your part is 0, but it does not mean the part has zero velocity (which is required for a static analysis). Also consider that FEA is a numerical method, so you'll never have an exact balance of forces, so your part will want to accelerate in one direction slightly. If you didn't have these soft springs, your model will just "fly off in space". However, these soft-spring will still allow your model to move (the amount and direction is dependent on the stiffness of the soft springs, where they are placed, and how much load imbalance you have), and this motion pollutes your displacement field (ie you can't tell what is due to the deformation of the part and what is due to the part moving is space). If the soft springs have the right value, are placed correctly, and your load imbalance is small enough, then this part motion is typically small enough to be ignored.