ABAQUS explicit/Analysis

[mj345]

Hello All,

Thank you for your quick response. I am doing drop test using Abaqus/explicit. having couple of questions.

1. While assigning element types, Do I need to choose the standard or explicit option?
2. How to choose the total step time for analysis?
3. If I want to include the gravity in the analysis, Do I need to give in Initial step or in the Step-1?

Appreciate your response.

kind regards,

 

[FEA way]

Since it's Abaqus/Explicit analysis, select explicit in element type. Total time step should correspond to the time period of the event that you are simulating (keep in mind that the bigger step time is the it takes to solve the problem). Loads can only be created in analysis step, not in initial step so the same applies to gravity load. However in drop tests it is usually better to place the falling object right above the target and apply initial velocity to it than simulate whole free fall with gravitational acceleration.

 

[mj345]

Thank you for quick response FEA way.

 

[mj345]

Hello FEA Way,

One more question while applying general contacts between the shell elements(generated @mid surface and assigned thickness).
Does it consider the thickness by default or Do I need to mention thickness in surface properties?

Kind regards,

 

[FEA way]

Sure, Abaqus automatically accounts for shell thickness in general contact. You only have to edit this setting (in Edit Interaction --> Attribute Assignments --> Surface Properties) if you want to use non-default thickness (argument value other than ORIGINAL).

 

[mj345]

Hi FEA Way,

Thank you for the reply its very much helpful. I am doing the drop test using Abaqus/Explicit and have the information about the dropping distance(X inches).
I want to apply velocity to the falling object,as per my understanding the velocity is same as the distance/per second(X inches/sec).
Please let me know your ideas.

Kind regards,

 

[FEA way]

Since you know the dropping distance, you can calculate velocity using the simple formula: v=sqrt(2gh), where h is your dropping height. Of course this ignored the air resistance. Then place the model right above the ground and apply initial velocity with magnitude equal to this calculated value.

 

[mj345]

Thank you for your quick response.

 

[mj345]

Hello All,

I am doing drop test using ABAQUS/Explicit, Is there any option to enter the initial and final velocity of the dropping object?

your help is appreciated.

Kind regards,

 

[FEA way]

There are two ways to define velocity in Abaqus - either as initial condition (Create Predefined Field --> Step: Initial --> Mechanical --> Velocity) or as boundary condition (Create Boundary Condition --> Step: Step-1 --> Mechanical --> Velocity/Angular velocity). In the first case velocity will initially have defined value but the body will be able to change the magnitude and value of its velocity during analysis (in this case slow down and bounce due to impact). In the second case the body will have prescribed velocity that will remain as defined during the whole analysis (so that the body won't slow down or change the direction of motion). In impact analyses initial velocity is always used. You can place the body right above the ground and apply the value of terminal velocity, as I explained before. However if you want to simulate the whole free fall anyway (which is not recommended) then you can place your model at some height above the ground and use gravitational acceleration to drive it towards the target.

 

[mj345]

Thank you FEA way,

Analyzed the model with the first case like defining velocity as an initial condition. But when I plot the deflection history as graph,did not see any bumping back behavior after the impact.
Deflection showed as a straight line after impacting. Then I thought it might be because of having the damping(Bulk viscosity applied to the model as default option).
So in next iteration bulk viscosity made to zero still having the same behavior. Is there anything do I need to check in the analysis?

kind regards,

 

[FEA way]

Can you share some pictures of your model’s setup (geometry with applied BCs) and results ? Make sure that all units (especially for material properties) are consistent. That’s a common reason of such errors. Also verify your contact definition.

 

[mj345]

Hello FEA way,

Thank you and can't share the data as I am working from the client location.

I have one more question for you regarding the material properties.

Mechanical Properties English
Tensile Strength, Ultimate 58000 - 79800 psi

This is for ASTM A36 Steel and values are taken from Matweb, Is this Engineering stress or the true stress?

Kind regards,

 

[FEA way]

I'm not 100% sure which value they provide but this is most likely engineering stress.