# Initial displacement condition

vkr535
Member

Hello Team,

I was trying to simulate a vibration of plate with initial strain(e_xx) condition.

For this, I'm thinking to apply linearly varying displacement as a function of X coordinate. I'm unsure how to apply this displacement as an initial condition. I see that there is an option for initial velocity.

Could you let me know if there is any approach to model initial displacement.

## Answers

@vkr535

You posted in the Explicit Dynamics category. Your questions sounds like you should not be using the Explicit Dynamics solver. Do you have a reason why you would?

You might be better off with the implicit solver. You can put your plate into a Static Structural model and apply a displacement to generate a strain along the X axis.

For study on vibration of small displacements, you can use a linear analysis, which is much faster. What do you want to know about the vibration of this pre-stressed plate? If you want to know its displacement response to a harmonic vibration load, you can use a Harmonic Response analysis. If you want to know about transients, you can use a Transient Structural analysis. In either case, you can link the solution of the Static Structural into the Setup cell of either of those dynamic analyses.

Hello Team,

Thank you for response. I was considering that approach which you suggested, but I was trying to solve only a linear problem without any pre-stress.

The problem was to solve was an explicit linear analysis with non-zero initial displacements and zero initial velocities with the boundary condition U(x=0)=0.Please let me know if I'm missing anything.

Thanks

Vinod

@vkr535

Hello Vinod,

When you say a boundary condition of U(x=0)=0 are you describing the displacement at X=0 (one end of your model) is 0. I assume that means all three directions. A rectangular plate has four sides. What are the boundary conditions on the other three sides?

Once a problem is fully defined, the analyst can choose to solve it using either an implicit solver or an explicit solver.

Your first and second post have conflicting information. Your first post says you want initial strain. If you have strain, you have stress. Your second post says you want to solve a linear problem without any pre-stress. If you don't want any pre-stress, then you can't have an initial strain.

Please provide a complete statement of your problem. If you insert an image, that would be even better.

Hello Team,

" When you say a boundary condition of U(x=0)=0 are you describing the displacement at X=0 (one end of your model) is 0. I assume that means all three directions. A rectangular plate has four sides. What are the boundary conditions on the other three sides? "

--> Yes, the bc's are fixed in all directions. As it is a 2d problem, so both ux and uy are fixed. While on the other 3 edges, they are free.

" Your first and second post have conflicting information. Your first post says you want initial strain. If you have strain, you have stress. Your second post says you want to solve a linear problem without any pre-stress. If you don't want any pre-stress, then you can't have an initial strain. "

--> So, its was basically a 2d plate vibration(longitudinal and NOT transverse), with an initial displacement gradient du/dx(t=0) =0.001 and zero initial velocities( Vx(t=0)=Vy(t=0)=0 )

Below is the attached image of the problem

Thanks

Vinod

@vkr535

Thanks for the complete problem definition. So you have a 1 m long x 0.1 m wide plate. You don't state a thickness, so I assume this is a Plane Strain problem. Fixed support on the left end and a 0.001 m X displacement at the right end. Then you want to let go and watch the vibration.

You can do this most easily in a Transient Structural analysis. You need a 3 step analysis. Step 1 is done with Time Integration Off and has an end time of 1e-5 s. In this time, the Displacement at the right end ramps up from 0 to 1 mm. Step 2 is done with Time Integration Off and has an end time of 2e-5 s. In this step, nothing happens, except that the initial velocity is being set to zero for step 3 because nothing moves in step 2. Step 3 is with Time Integration On and has an end time that depends on how many cycles of vibration you want to observe. Turn on Large Deflection. Under Damping Controls, enter some Damping. You did not specify anything in your problem statement. I choose a damping ratio of 0.05 or 5%.

With that setup, and a 3x25 element mesh, you can get output like this, for the X displacement of the right end.

It will be helpful if you first do a Modal analysis to determine what the natural frequency of the axial vibration is.