Welds in FEM

[mrmartins]

Hi. During struture simulations how do I specify the welded unions between the parts/bars composing the structure?

Thanks

 

[corus]

It depends on what you want from your model. If you're not interested in the weld loads per se then just use a single continuum for your model.

corus

 

[mrmartins]

Thanks a lot for your answer. I am not interested in the welds, but isn´t important to define the mechanical resistance of the welds?

 

[Drej]

When you weld a structure it becomes continuous. As corus says above a single, continuous, continuum is the way to go if you don't need analysis information on your welds. The mechanical resistance (of the weld) as you've stated will be modelled implicitly by your continuous mesh, since the weld is assumed to be of the same strength of the parent material. Usual disclaimer here that the weld in reality will of course NOT be the same strength and will produce a HAZ and its geometry will be non-uniform etc. etc..


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[corus]

If you have a full penetration weld then the stiffness of the weld will be at least the same as the parent material (presuming the correct weld material has been specififed).
The same principle would apply in general to fillet welds.
Generally if the throat thickness of the weld, or the total throat thickness at the joint, is equal to or larger than the parent plate then the weld stiffness won't be a factor.

corus

 

[crisb]

Normally modelling welds as a continuum works fine but there are occasions when it will not be realistic......2 wide thick plates welded together at their edges will behave differently under transverse loading to a single plate of twice the thickness.

 

[mrmartins]

Thanks a lot to everybody for your comments. So as I understant I can consider the welds as continuous media, and the only thing I need to check is the quality of the welds to be sure that they are at least as resistant as the rest of the material, maybe perform some mechanical tests to some welds. What do you think?

 

[cloche]

Exactly. You can "get rid" of the weldments in the FE model, exception made for these welds which have low quality factor (i.e. they could incorporate cracks, discontinuities, thermically altered zones on the base material, and have induced stresses). Anyway, modeling without the welds is GENERALLY (see exception provided by Crisb) "safer" since:
- it reduces resistant area with respect to reality
- it induces stress concentrations at the corner/edges (of course you have to properly interprete these concentrations)

 

[ncc212]

mrmartins, (and other contributors)

i'd be interested to know how you get on with your weld modelling.

Other than yield and ultimate, which will need to be in the dirction of the weld and across the weld, I am unsure how you will enter the test results into the material model. I am thinking more of the fracture toughness, which will almost without doubt be significantly lower than the parent plate.

In turn will you not need to calibrate the descritisation of the mesh around your weld? I can't see how an element can be partially cracked (other than specific crack elements such as ZenCrack which i have heard of but not personally used.)Therfore the crack would step its' way along the elements. This would seem unrealistic other than for a macroscopic model i.e. where the element size equaled the metal grain size (bit unwieldy for any realistic sized structure). In turn if your tests are Charpy (strain rate 1s^-1) is this applicable to your loading/strain rate?

Any way of taking the macroscopic behaviour of the weld outwith the FE model?

Apologies if it's a case of more questions than answers but just bulking the welds in with the rest of the structure just doesn't sit right if you know what i mean.

 

[trainguy]

In our practice (railway vehicle engineering),

We model the structure without the welds, assuming they will be effective in transmitting the loads.

We later verify the validity of that assumption by extracting from the FEA the nodal forces at weld locations, and then we use hand calculations with code specified weld strengths.

Clearly, for full pen welds, this approach is unnecassary because if the parent metal is not overstressed, neither is the weld, but for fillet welds, esp. intermittent ones, this is a crucial step in the structural analysis/design.

I also agree with crisb's comment as it is a common error with junior/inexperienced FE analysts.

tg

 

[Modey003]

When FEA modeling a weld I would definatly start with a homogeneous contiuum model since the stiffness of the weld joint isn't significantly effected by weld quality (pores, intergranular oxide/sulfur inclusions etc...). Also, you will need to account for any thermal-mechanical residal stresses from the welding process.

Weld joint stress concentrations by using a saftey factor. Also, in the saftey factor should include the lower material strength found in welds due to pores and inclusions. My advice to you is to work with a materials engineering guy who know the details of welding.

Regards
Modey

 

[gwolf]

It all depends on the geometry of the weld as other posters have said, however:

In general for a continuous weld you model it as a continuum but use different material data when analysing for strength and fatigue. Here fatigue is the critical one because welds are usually as strong as the parent material after allowing for any change in properties because of the heat. The big difference comes in fatigue strength.

You also need to consider whether the weld has been dressed to smooth it out. There will be a factor of about 10 difference on fatigue life between dressed and un-dressed welds.

The basic rule of thumb is not to put a weld in a high stress area if you can avoid it. You would need to give more information on your particular components, materials weld geometries etc to get a more specific answer.