Contact Problem 3

[s89t3]

I have three objects (all different materials). Object one is pushing on object 2 which pushes on object 3. Object 3 is fixed. I would like to conduct a FEA of the surfaces in contact. The actual geometry of the objects are not really important at this point, just the process of introducing 3 seperate objects within the viewport and placing them in contact for analysis. Eventually I would like to pivot Object 1 at different angles and study the differing contact stresses. Any help regarding this issue would be glady appreciated. Also any sugesstions on where I can find Abaqus tutorials regarding a similar issue are welcomed.

Thanks

 

[mrgoldthorpe]

s89t3,

Briefly:
1 Establish and mesh the 3 different objects.
2.Establish on each object surfaces that will be used to provide contact.
3.Establish the surface interaction properties.

Look in the manual (6.5) "22.1.1 Mechanical contact properties: overview". There are several different ways you can do it. If I was doing it I would establish 'slave' and 'master' surfaces as follows.

Object 1 will have a Master Surface for pushing on Object 2. Let's call this surface SURF1M.
Object 2 will have a Slave Surface for being pushed by Object 1. Let's call this surface SURF2S.
Object 2 will also have a Master Surface for pushing on Object3. Call this SURF2M.
Finally, Object 3 will have a Slave Surface for being pushed by Object 2. Let's call this surface SURF3S.

So you establish surface interactions between SURF1M and SURF2S, and between SURF2M and SURF3S. Hopefully, the slave and master surfaces on Object 2 are mutually exclusive since I'm not sure how ABAQUS deals with such over-lapping surfaces.

Finally, take care of boundary conditions on Objects 1 and 2. Before and after contact they may be improperly constrained which can lead to solution problems.

As far as Examples are concerned, take a look in the Example Problems, Bencmarks and Verification Manuals.

I hope this helps.

MRG

 

[as3029]

i am also having similar problem in a stamping analysis.
Say
object 1 - binder (rigid shell)
object 2 - blank (elastic plastic shell)
object 3 - die (rigid shell)

I still have not solved the problem completely, but have the input file eunning under certain circumstances.
Some tips i wish to share with you.
1. The element normals must be opposed to each other (shell elements only)
2. Apply load gradually to avoid contact penetration. You may want to use *Surface bahavior, pressure over-closure=exponential
3. See that the contact constraints do not interfere with applied constraints
It may give you numerical singularty warnings (over constraint checks) or contact over closure if you do not have normals correctly oriented.

if anybody has any more cluse to this problem, please let me also know as similar problem is troubline me too.

 

[corus]

I always displace the objects first to establish contact before applying any loads. Also make sure you adjust the contact surfaces so that overclosure doesn't occur in the option for *contact, ...., adjust=0.
To initially bring the objects into contact use CAE and translate the objects in the assembly module using geometry points on the objects as start and end points for the translation vector.

corus

 

[bassmanjax]

Just to add my £0.02....

A quasi-static ABAQUS/Explicit can sometimes resolve contact problems easier than Standard - especially if you use the 'new' general contact algorithm (*CONTACT). This is only available in Explicit at the moment, but I believe that ABAQUS intend to make this the primary method of defining contact, rather than using *CONTACT PAIR