You can define the displacement time history in attribute "Amplitude", and then in Dynamic analysis step, you can assign to nodes using attribute "BCs" for any degree of freedom , then select the defined amplitude for this DOF.

Mr. Kishi,

Can you provide a link to

abaqus?

Hi Kota.

If it's only for initial conditions, you can use the *BOUNDARY command in your model definition (before step definition), if you're writing an input file rather than using Abaqus CAE. (You can select boundary conditions from menu in CAE).

Use with the TYPE=DISPLACEMENT (this is default, so you don't need to specify), TYPE=VELOCITY, and TYPE=ACCELERATION options to define what you need. Do you have access to the manuals? The Keywords manual should give you the information you need, if you look up *BOUNDARY. It is also a way to apply displacements, velocities and accelerations during each step, potentially in conjunction with amplitude data, as suggested above.

You can use node sets (these conditions apply to nodes by default; I don't remember if that can be altered) to define different conditions for different parts of your model.

I've not done dynamic modelling (only static) but I think it'll still work the same. Let me know if you need any further info.

Cameron

The key of the answer is your conditions are initials of constant trough the step.

If you want to hace an initial displacement, I think the best way is put the initial position in the assembly mode with "Translate instance".

A boundary condition is the value of the displacement of the nodes during the time increment of the step. If you want to have a defined movement the best is the boundary condition of the displacement.

So, the acceleration as an initial condition does not hace a physical meaning, has a meaning is trough the step. Velocity has a physical meaning is an initial condition because of the vibration.

Please let me know if I wan not clear.

Hi Kota,

I don't think you should define initial conditions in "Boundary Condition" option, instead, initial disp or velocity should be added in the "predefined fields" option.

The difference is that when defined in BC option, the initial velocity or disp will keep constant for the whole simulation process, while in PF option it would be just added at the starting step, means that the velocity/disp of the object you defined on will change into different values, for instance, if got into contact with another object.

Hello everyone,

Thank you for answering my question!

Hi Sadiq, Jumaa and Cameron,

At first I tried doing such a thing, but I was not able to provide boundary conditions of displacement, velocity and acceleration at the same time.

However, it might be because of other mistakes, so I'll try again.

Hi Bojidarka,

What is a link to abaqus?

Hi Fernando,

I haven't known translate instance, so I try to use this. Thank you.

Hi Frankey,

I thought predefined fields are valid for my analysis, but I couldn't find how to provide initial conditions of displacement and acceleration. If you know how to do this, could you show me the way?

Hi Kota,

I double checked the abaqus GUI and documentation, finding that I'd made a mistake considering initial disp the same as initial velocity.

So it seems that it's not easy to define initial disp or acceleration in ABAQUS/CAE.

But I'm wondering if you could deal with your model in another way, for instance, build up more than 1 steps, calculate the "initial condition" in the 1st step, and then keep going on with your simulation in the following steps with the 1st step ending results as initial condition.

check out the following question, maybe it'll help.

https://www.researchgate.net/post/How_can_I_apply_initial_displacement_u0_in_t0_in_abaqus_explicit

Hi Frankey,

Thanks a lot for your answer. I want to use remeshing technique in my analysis, so I should change the input file step by step. Abaqus includes remeshing technique function, but it can't be applied to dynamic analysis.

Therefore, I should find another way of providing initial conditions.

Kota

Hi Kota,

One option might be a variation of what Sadiq suggested. If you apply movement of any sort with user-defined amplitude, it can call the UAMP subroutine. You can then set up its Fortran code to apply whatever patterns of displacement, velocity and acceleration you need, although I could imagine this getting messy. You could include fields (node-based user-defined variables) or element based state variables (solution dependent variables - STATEV/SDV) to help control behaviour according to regions or other specifics.

I'm surprised Abaqus didn't let you define all three variables. That is unfortunate. I would have expected to at least be able to define the three separately, for additive effect. That's an annoying omission!

Good luck.

Cameron

Hi Cameron,

Thanks a lot for your answer. I haven`t known UAMP subroutine, so I`ll read about UAMP subroutine in the abaqus documentation and decide whether it can be applied to my research. Thank you.

Kota

Hello Kota,

I am assuming you are trying to add initial conditions based on results from another analysis in ABAQUS.

I am unsure about initial acceleration, but for defining initial velocity, Predefined fields could be used. For displacements, the following methods 'might' work-

1. Initial State (Can be found in Predefined fields>other>initial) - This allows you to import the results at a desired step, increment of another analysis.

However, this method does not allow any keyword changes to be made in the new analysis.

2. Solution Mapping (Cannot be used for Dynamic analysis) - Allows mapping a solution from one mesh to another. Try search for *MAP SOLUTION

I hope these should be of use to you.

Kindly let me know in case any other alternate methods work as I am also having a similar requirement.

Thank you.

Best regards,

Amal Jerald