contact problem ,too many attempts...

[Newuser2006]

hallo every body,iam a new user to abaqus and i want to simulate to sheet metal deformation.this sheet of metal is in contact with a rigid mould,with some openings in the mould.the load is applied as uniform pressure on the the sheet and is supposed to deform the sheet where the openings are.the problem now is that it is taking too many attempts for the first increment,and the Time/LPF Inc column is always decreasing.so wha is the problem?contact definition or rigid body definition.maybe some find the problem quite easy so please help me.by the way where can i find more information about working with abaqus rather than in the manual.
regards

 

[bfillery]

Dear Newuser2006

It sounds as though you may be getting rigid body motion. If so, there are several options.
1) If your geometry is supposed to be coincident to start, you can try to adjust the initial surface positions of the contact pair ref ABAQUS 6-6EF 29.2.5
2) Attached weak springs to prevent rigid body motion
3) As an initial step, prescribed a small known displacement to the sheet to initiate contact onto the mould. In a subsequent step you can apply the required pressure and remove the this intial displacment.

Hope this helps

bfillery

 

[Newuser2006]

thanks for fast reply and please continue helping me
i try to explain again what is happening,
1)in the first srep the sheet and mould are in contact,i give also the mould(rigid body)small displacement to confirm the contact,after many increments step one is completed
2)step 2 begins after i made the initial increment very very small,1e-016,then after 7 increment it stops and says error too many increments
so the question is now why is this error?and why i had to start with so small initial increment
thanks

 

[Yoman228]

It may be due to some snap though motion. if that the case I will try using *the stabilize option or using Riks.

*Static, stabilize=0.0002

Stabilize option is easier if you not interest the post buckling behaviour before the time step finish. And you will have to check the energy within the system to ensure there is not too much damping.

 

[corus]

You could also try *contact controls, automatic tolerances as that usually works. You sometimes get 'chattering' where one point opens and closes. You can get the nodes in contact printed so you can see where the problem may lie. The automatic tolerances might fix that. It doesn't sound like rigid body motion as you'd get an error about negative eigenvalues.

corus

 

[bassmanjax]

If it's sheet metal forming, you may be better to use ABAQUS/Explicit to solve the problem as quasi-static. Not only that, but if the model is 3D, you can use the general contact algorithm.

If you need the final shape of the sheet, you can run a springback analysis by importing the results of the Explicit forming step into a static Standard analysis.

Regards

Martin

 

[Newuser2006]

Thanks for all replies.
bassmanjax what you said is really interesting,but i did not understand anything from it,iam still new to abaqus.
actually the simulation worked good for a simplified model,but now i imported the full real mould (3d structure)and iam not able to use it as rigid body.why ?and what to do?should discret rigid bodies be meshed? thanks

 

[bassmanjax]

Hi

If you have your mould geometry in 3D, then you will have to mesh it with rigid elements - see the rigid element library in the ABAQUS Users Manual for the 3D element types. I think they're R3D4 (4 node) and R3D3 (3 node). I'm at home at the moment, so I don't have access to the docs...

You can then tie all the rigid elements together to form a rigid body, for this you also need to define a ref point in CAE as the reference node. Any boundary conditions for the rigid body are applied to the ref point only. So if you don't want the mould to move, just fix all translations and rotations on the ref point.

If you go down the route of using Explicit, you can use general contact. This is dead easy to set up, because all you need to do is set *CONTACT, ALL EXTERIOR to include all elements in the model, deformable and rigid.

In Explicit, your pressure load will have to have an amplitude curve the loads are related to step time. This is well covered in the docs.


Have a look through the example problems to get a feel for how Explicit models are generated. There's also a decent section in the docs on how to transfer results between Explicit and Standard should you want to do springback.

Regards

Martin