Shell bolt model - Contact clearance

[ahkrit]

Hi!

Based on my previous post (

https://www.eng-tips.com/viewthread.cfm?qid=492174)

I would like to have another question regarding this paper:

https://files.engineering.com/getfi...09-62fb984f5c66&file=edgetosurfacecontact.PNG

It says at the contact definitions (3.2. Contact) that between rigid surfaces and hole edges the finite tracking is used, as it allows also for clearances.
But Abaqus documentation says the opposite, that clearance can be used only with Small-sliding.

https://abaqus-docs.mit.edu/2017/English/SIMACAEKEYRefMap/simakey-r-clearance.htm

Could someone help me out in that topic please? How is it meant in this paper?

I also built up the same model, it works fine if there is no gap between hole and the rigid surface. But if i would like to model a standard bolted joint with gap (0,5mm for example) then i get the following errors for the kinematic coupling between Master node(=beam end node = rigid body reference node) and on of the hole node:

https://files.engineering.com/getfi...063d-4bd5-ab7c-1143e9df2d44&file=warnings.PNG

The simulation is with 2 steps. 1st step is the pretension, it runs nice, but in 2nd step this warning pops up and does not converge.
How could i solve this issue?

Thanks!

 

[FEA way]

In the article, they mention clearance not as a special keyword used to specify precise initial clearances for small-sliding contact but as a naturally occurring clearance in the model. They only adjusted the contact tolerance to account for it.

Gaps between the parts in static analyses often lead to rigid body motions and thus should be avoided. There are several ways to handle such problems. Check the article "Simulation of a Parking Pawl Mechanism with ABAQUS/Standard and ABAQUS/Explicit" written by D. Ramnath and P. Andrade. It discusses various approaches to contact convergence issues.

 

[NRP99]

What is your second step? Have you fixed the length of bolt for the applied pretension force in first step? How many DOf's fixed in the kinematic coupling? Load of model before fixing the bolt length?

Image of model or result would require to understand the problem. Anyway this is warning and if non-convergence is happening after say some increments you can understand by seeing the results what exactly is happening?

 

[ahkrit]

All BCs are according to the paper defined. The kin coup as well, so 3,4,5 DOFs are coupled between master nodes and hole nodes.
In first step one end of the beam is fixed and the two end nodes of the plates.In 2nd step prescribed displacement applied in X direction.(see pics attached)

The difference is clearly the gap, that is the reason why the model cannot handle it. With *CONTACTCONTROL, STABILIZE it does run quite well until the last time step, where it gives back the same Warnings and then divergence occures.
Of course in DOF direction 1 and 2 no constraints are given as the gap is bigger and there is no contact as the joint is not slipping(load is below the limit).
Any ideas how it should be solved?

Unfortunately i cannot find this article.

 

[FEA way]

Right, it seems that this article can’t be found so easily anymore. Too bad, it features a really nice summary of various approaches to such issues. Another interesting paper on this topic is titled "Getting Bodies into Contact - the Despair and Joy" and written by R.J. Tyrrell. I would also recommend the "6 Tips solving non convergence with Abaqus FEA" blog post on Simuleon’s website.

Anyway, you could try these methods:
- automatic stabilization in step settings
- discrete springs or dashpots
- dynamic implicit analysis (maybe even explicit but it will be better to start from implicit quasi-static)
- contact damping

 

[NRP99]

Some observations .
-Use of 4 node quad elements is recommended. Do not use quad/triangular mix if the geometry is simple. Triangular elements are stiff elements.
-Why you are using the rigid surface is not understandable. I have not read the paper. For bolt joint, beam is sufficient.
-You have shown second step in which you applied displacement. Did you fix the length of bolt for pretension before applying any load? Insert step and just fix the length of bolt before any load. This is recommended practice.
- Mesh looks coarse. Use biasing/small size to enhance/fine mesh near the holes. Mesh refinement can solve any contact related problems. In fact most contact convergence problems incur due to insufficient mesh density.
- Check below general points for convergence issues

General points to achieve convergence.

[li]Increase steps of the analysis. For contact analysis, its better to first establish contact in the initial steps and then apply loading. To establish contact use displacement loads. For the two parts to be contacted, move one part with very small displacement like 0.01/0.1. This is to tell Abaqus there is contacts between parts.( Abaqus/or any FEA software is not smart enough, I guess. ) At later step, deactivate/remove the displacement load and apply small load (10%) and in next step apply full load.[/li]

[li]Refine mesh at penetration locations. Most of the problems in contact convergence are solved by refining the mesh at the master as well as slave surface. Use of linear brick/quadratic tet is always recommended. Contact with linear brick elements is smooth but not so with quadratic tet. For different material properties different elements are recommended. Check which elements is suitable for your analysis in Abaqus manual or example problems.[/li]

[li]Use contact stabilization. this will apply the damping force to counter large contact force application locally at the contact. But make sure the damping energy (ALLSD) is very less number than internal energy of the model (ALLIE). (Its not always recommended, though)[/li]

[li]Use step stabilization. This will introduce the damping forces to counter large contact force application and will slowly apply contact forces/assembly loads to achieve convergence at complete part/assembly level. But make sure the damping energy (ALLSD) is very less number than internal energy of the model (ALLIE). (Its not always recommended, though)[/li]

[li]Sometimes its better to use general contact than surface to surface contact. I feel general contact algorithm is robust than the surface to surface contact. But if model size is too big then this may get warnings of memory exceeded. Give it a try.[/li]

[li]Sometimes changing step initial increment size has also help achieve contact convergence. Some problems are solved by 0.1/0.01/0.001 initial increment size and some problems are solved by initial increment of 0.1/0.2/0.5/1.[/li]

More tips on contact convergence on - Link-1. Or just google "contact convergence in Abaqus", "your specific error/warnings" and "solving non convergence with Abaqus FEA Simuleon".

 

[ahkrit]

@FEA way

This is the part where the article writes about the edge to surface contact (bolt clearance between shaft and hole):
"For contact between the hole and the rigid surface, the
classical node-to-surface contact search was used. Also a finite
sliding tracking approach was used which means that any arbitrary
relative separation, i.e. any finite sliding or rotation of the contact
surface is allowed [20]. To accurately model the clearance between
the bolt and the laminate, a contact tolerance was set to a value of
10 microm."

Maybe i do not understand but for me it seems like that it does want to model the initial distance between shaft and hole edge, or not?
Also in Table 2 it shows different clearances for the comparison.
But in case if it was modelled with clearance (gap between shaft and edge = gap between rigid surface and shell hole edge) then it should also have singularity issues with rigid body motions. I do get this convergence issue in that way, even though everything is modeled the same way. On the other hand pretension is applied, and as in a fully built 3D model (all parts modeled with 3D elements, contact between surfaces and surfaces-bolt head)it should hold the parts together as long as the connections can slip.
Still does not work for smaller loads.

Any idea what the problem is?
How could i calculate it as static analysis?

 

[FEA way]

The paper that you are referring to is titled "A global bolted joint model for finite element analysis of load distributions in multi-bolt composite joints" and written by P.J. Gray. The authors clearly say that they set the contact tolerance (not clearance) to 10 µm. But maybe they meant something else than regular adjustment tolerance by this imprecise statement. Check the documentation chapter "Adjusting initial surface positions and specifying initial clearances in Abaqus/Standard contact pairs". In addition to the approach used only with small-sliding contact, this chapter also describes some alternative methods that are applicable to finite-sliding formulation as well.

 

[SWComposites]

That paper has a completely horrible way of modeling a bolted joint. Use of rigid elements is completely unrealistic.

 

[ahkrit]

@SWComposites

how would you modell it in an efficient way? including preloading.