Four Point Contact Analysis for steel pipe in ABAQUS/CAE

[Linus86]

Hello,

I am relatively new to ABAQUS CAE and i have been facing this problem for the past three weeks (asked every one i know but not many people have working knowledge on ABAQUS).

I am trying to model a contact analysis of four points on a pipe as shown in the picture in the link. The two semi circular model on the top will be moving at a displacement of about 50mm downwards on the pipe. While the two semi circular model at the bottom will be supporting the pipe. At the end, i am trying to analyze the stresses induced on the pipe when it undergoes four point bending.

For the pipe, I am using deformable solid with both the plastic and elastic data.

For the four Semi circular model support, I model it as analytical rigid.

I am using surface to surface contact with frictionless interaction.

Now the problem i am facing is when I am submitting the job for analysis, I keep getting this two errors "There is zero FORCE everywhere in the model based on the default criterion...." and "The strain increment has exceeded fifty times the strain to cause first yield at 1890 points".

Also, i am able to complete the analysis but the results is definitely not what i have intended it to be (when i click the deform model in the visualization module, the model changes to some weird looking thing).

Do i need to model the semi circular support as a discrete rigid instead? And what could be done to solve the two warnings above?

Thank you very much.

 

[Fabi0]

How did you define your contact?
What kind of element did u use to mesh?
It seems a hertz contact, so have you consider that seeding in contact area depend on the size of the contact area?
Boundary condition are ok?

As you can see, there's a lot of thing that can't be undestand by you attached picture

Fabi0

 

[Linus86]

Hi Fabi0,

Thank you for your reply.

For my contact,
- I am using a surface to surface contact interaction in the initial Step.
- The master surface is the rigid part Choosing the outer surface.
- The slave surface is the outer shell of the pipe.
- Sliding Formulation: Finite Sliding
- Discretization Model: Surface to surface
- Contact Tracking: Single Configuration (State)
- And the rest is default setting.
- I have define a total of four contact interaction property one for each rigid support.

For the Boundary Conditions,
- For the pipe, I have apply XSYMM (U1=U2=U3=0) on the half face of the pipe as i have only drawn have of the pipe and can take it as symmetry ciondition (applied in initial Step).
- For the top two semi circular part, i have constrain the five degrees of freedom except U2 where i have applied a displacement of - 50 (Applied in the next Step).
- For the bottom two semi circular part, i have constrain all five degrees of freedom (Applied in initial Step).

For the Mesh Element,
-I am using a C3D20R with default setting.
- My global seed size is 20.

The other thing i am unsure about is the number of steps i need to run this job as i currently only have two step (the initial and apply displacement step).

Thank you.

 

[corus]

You'd be better using a quarter symmetry model sod having only one upper and one lower support. That way you can halve the model size and get quicker run times.

If you're using finite sliding then you're better using NLGEOM=ON in your step definition. For the plots you have now, make sure the deformation scale factor is set to some reasonable value so you don't get weird looking deformation plots. Posting a picture of the deformation would be easier to explain though.

Tara

 

[Fabi0]

Of course you must use NLGEOM=ON like corus say.

You have meshed it all by the global seed? I believe you have to refine the mesh in the contact area...for hertzian contact you must consider that the contact area is very small compered to the model.
By using the quarter simmetry you can increase the refinement of the mesh without having to much elements in your model.

The zero force warning is ok for the early increment of the analysis, because i suppose you have applyed the displacemnt with a ramp, but in the last increment it should disappear, control it in the .msg file.

The distortion may be a problem of element dimension, because if the element in the contact zone is too big, only a few node, maybe just one, came into contact: in this way there's too much stress in this node. You can also try to reduce the minimun time incrementation in the step module.

 

[Fabi0]

PS: number of step looks ok, but you must set small time increment and a small time start!

 

[portliner]

The symmetry of the pipe should be imposed by U1=0 only as I can see. The two lower circular parts all six DOF should be fixed. Use C3D20 in the contact zones, they are recommended in regions with high stress gradients. Use *Pre print, contact=yes to check the initial contact status.

/Stig