Assembly and interaction

[dureiken]

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

 

[Yoman228]

If the contact area do not change. I will just tie the serface together.

Otherwise using the hard contact should be fine as long as both surface is not rigid.

 

[dureiken]

both surface are in steel

i tried to launche the job but it doesn't work because of :

The system matrix has 3 negative eigenvalues.

 

[bassmanjax]

Could be that the surfaces are overclosing to much in the first increment - try reducing the initial time step size.

Regards

Martin

 

[dureiken]

I put :
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.

 

[bassmanjax]

If the surfaces are more or less coincident at the start, then you may well need an even smaller time increment than 1e-4.

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

 

[dureiken]

The both surface are exactly the same.

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.

 

[bassmanjax]

If the surfaces start off as coincident, then ABAQUS will need a very small time step to start the analysis, possibly as small as 1e-9.

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

 

[bkal]

From your initial description I got an impression that you have not defined that the surfaces which are adjacent to each other are in contact, so your upper part is actually not supported - hence negative eigenvalues. Basically, in the Interactions module you need to specify that two surfaces can contact - just putting them close to each other does not help.

 

[dureiken]

I tried to put a space between two parts but the same errors.

If you have the time to look I put the file on a ftp :

http://74.114.free.fr/abaqus/

Thanks for your help

 

[Yoman228]

I had a look on the model. There are a few things that need to be done as following.

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.

 

[dureiken]

ok thanks a lot it works but at the step 1, the block is moving long the beam, like if it was sliding on the surface. I think maybe it's because the local axis aren't the same than the global one ?

 

[dureiken]

step 0 :

Step 1:

 

[bassmanjax]

I've had a quick look also and I would agree with Yoman on his points.

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

 

[bassmanjax]

You don't have any boundary conditions on the block. Try constraining two of the vertical faces such that the block can only move vertically.

Regards

Martin

 

[Yoman228]

you can also put some friction between the surface. my experence tell me that steel to stel is around 0.3 to 0.5.