Rigid Body Contact 2

[a2joe]

Hi All,

I am new to Abaqus, so any help would be appreciated.

I am trying to model interaction between 2 rigid bodies, a sphere and a plate. I have constrained the 2 bodies initially to have point contact. My goal is to apply a vertical displacement to the sphere for the second step to cause penetration, to obtain contact force, area and stress. I cant get Abaqus to do that. Any ideas? I have defined reference points on both parts to apply BCs to the rigid bodies (Initially both fixed. Second, translation in the -1 direction for sphere). I think I am messing up the interaction properties.

Also, for rigid bodies I cannot assign material and section properties, so how does Abaqus compute the contact parameters?

Thank you for your help

 

[bassmanjax]

Contact between two rigid bodies is not possible in ABAQUS - one of the bodies has to be deformable. You could try meshing one of the bodies and giving it a high Young's Modulus.

Regards

Martin Stokes CEng MIMechE

 

[huaijuliu]

Totally agree with 2nd floor.
And the rigid surface should be the master surface.

 

[dezsit]

Hello,

As far as I remember, you can define contact between two rigid bodies (for example between two meshed discrete rigid bodies)
But there are a lot of limitation regarding the used surface (for example cannot be both of them analytical rigid), the used algorithm, etc. See the User manual, Rigid body definition (or sg like that) chapter

There is not necessary to assign any section or material, if your bodies are either analytical or discrete rigid. In these cases you should define a reference point to the part and assign an inertia element, to describe the mass and inertia properties.
You can use rigid body constraints, in this case you should define the section and material properties as in case in any deformable body, and use the constraint "Rigid body"

I hope, this helps,

Br.
DT

 

[a2joe]

Thanks for the help guys

I tried 2 meshed discrete rigid bodies, but that didnt work. Maybe my interactions were wrong.

I cant assign mass or inertia properties because I eventually want to apply these to human bone models obtained from MRI scans so its a lot of extra work to figure those out.

So I am now trying what you guys suggested; defining them as deformable and using rigid body constraints.

My question would be: if I use rigid body constraints for deformable parts, will abaqus give a rigid body contact solution or a deformable one?

Thanks once again; Martin, Hua and DT

 

[dezsit]

Hello

Contact between two discrete rigid surface is allowed only in explicit general contact (but i'm not sure)

If you use standard solver, and contact pair algorithm, you can use only surfaces which are "rigidized" by rigid body constraint (here the base body is deformable), and not discretized by rigid elements (as in case of the discrete rigid body)
It is not necessary to use inertia properties, if your simulation is static, and do not necessary to take into account the gravity as load,

if both parts are rigid in your analyises, there is not contact stress

If the goal of your current analysis is to verify the kinematics of your system for example, it is ok to use only rigid bodies (as in case an MBS simulation),
but to investigate the stress state of your parts due to contact interaction, you should use deformable bodies

Br.
DT.

 

[Elabbasi]

I agree with what DT said. Rigid to rigid contact is supported only for explicit dynamic analysis and there is no contact area to consider and no stresses will be obtained. If you want stresses you need truly deformable bodies, even if they are quite stiff, and you might need a fine mesh around the contact area. It's ok to do a static analysis, also avoid an implicit dynamic analysis. You can however take into account the gravity load so that the weight of the bodies are accounted for in the force equilibrium.

Contact between a rigid sphere and a rigid plate will always only occur at one point (the location of that contact point will change). You can get an estimate of contact stresses and contact area however based on the contact forces resulting from your FE analysis (these should be accurate). You should use the contact force together with some analytical expressions (Hertzian contact for example) to get the stresses and contact areas. The contact area should be much smaller than your mesh size if the 2 bodies are nearly rigid.


Nagi Elabbasi

http://www.veryst.com