Assembly and interaction
Assembly and interaction
(OP)
Hi,
I want to study stress on a simple example : a HEB beam with a cube on the superior face.

I created 2 parts, I put them well in the assembly module, face on face, and i want to simulate a simple surface to surface contact.
In load module I put gravity on the both parts and "encastrement" on the face of the beam.
But I want to know exactly how to simulate the contact on Abaqus in order to check the stress into the beam due to the weight of the second part.
Thanks
I want to study stress on a simple example : a HEB beam with a cube on the superior face.

I created 2 parts, I put them well in the assembly module, face on face, and i want to simulate a simple surface to surface contact.
In load module I put gravity on the both parts and "encastrement" on the face of the beam.
But I want to know exactly how to simulate the contact on Abaqus in order to check the stress into the beam due to the weight of the second part.
Thanks





RE: Assembly and interaction
Otherwise using the hard contact should be fine as long as both surface is not rigid.
RE: Assembly and interaction
i tried to launche the job but it doesn't work because of :
The system matrix has 3 negative eigenvalues.
RE: Assembly and interaction
Regards
Martin
RE: Assembly and interaction
1E-04 in initial increment size
and the results were :
Time increment required is less than the minimum specified
The system matrix has 3 negative eigenvalues.
RE: Assembly and interaction
You could try using an amplitude curve for scaling the gravity load so that it is zero at time t=0 and 1 at time t=1.0. That way, the gravity is applied over the whole step rather than instantaneously at the start of the step.
Regards
Martin
RE: Assembly and interaction
I put : 0 at step 0 and 1 at time 1
new errors :
Too many attempts made for this increment
The system matrix has 3 negative eigenvalues.
RE: Assembly and interaction
Try putting a small gap between the block and the beam to start with, say 0.01mm.
I'm sure that the problem you are seeing is because ABAQUS cannot resolve the contact in the first increment.
Regards
Martin
RE: Assembly and interaction
RE: Assembly and interaction
If you have the time to look I put the file on a ftp :
http://74.114.free.fr/abaqus/
Thanks for your help
RE: Assembly and interaction
1) The contact property needed to be defined. Under Interaction Property manager/ mechanical/ Normal Behaviour/ Hard contact.
2) I will place both object touching each other before the analysis.
3) On the Edit Interaction choose the option of Specify tolerance foe adjustment zone. I choose 1e-5 in your model (note that this number has to be smaller then any mesh size next to the contact surface) and the model.
RE: Assembly and interaction
RE: Assembly and interaction
Step 1:
RE: Assembly and interaction
I do think that you may do better to adopt a different modelling strategy. If you are only interested in the stresses in the beam, you don't need to model the block as a deformable object - model it as a flat, rigid plate (R3D4) to represent the 'footprint' of the block on the beam. You'll need to create a reference point for the rigid plate, so attach a mass element to it (Property module > Special > Inertia > Create > Point Mass) - this will be the mass of the steel block.
Set the boundary conditions on the ref point so that the plate can only translate in the vertical (gravity) direction.
Regards
Martin
RE: Assembly and interaction
Regards
Martin
RE: Assembly and interaction