FEA of welds 3

[chris9]

I'm aware that standards exist for estimating the allowable stress on welds for say 10 million cycles. These standards often take the stress at a distance away from the parent material and this may be about half of the steel wall thickness.

I think the main problem is that most of the weld data is collected empirically by strain gauges and this doesn’t tie up well with FEA models.

From an FEA perspective are there any general guidelines for estimating the allowable stress on the weld? For example if you model the weld as a wedge and find the stress levels on the weld or toe then what would be acceptable for a reasonable durability?

 

[corus]

I don't think modelling the weld will give any acceptable results as the fatigue data implies imperfections in the weld as well as the stress concentration from the weld shape hence it the fatigue life is based on impirical data, and usually assuming a certain probability of failure rather than a known defined number. I have heard that a way would be to assume a crack at the weld toe, of say 0.1mm, and use a fracture mechanics approach to estimating the number of lives to obtaining the critical crack size. This method may be more apppropriate for the many cases in which standard weld assessments don't appear to apply.

corus

 

[chris9]

Corus,

You could say that about FEA of castings because the CAD geometry is rarely an exact match and also imperfections in the castings such as porosity and other defects influence durability. However, for castings I can find allowable stress values or endurance limits to give me a target to work with.

I’m struggling to find a target for welds though. I just need some guidance as to what is an allowable stress on or near a weld without doing a PhD on the subject.

 

[mloew]

Chris9,

Although this is not my area of expertise, I am aware the following commercial products for analysis of welds using the Finite Element Method:
[li]nCode FE Fatigue[/li][li]ESI Sysweld[/li]

I also found this from Googling:
IDAC Welded Joint Analysis of FE Models



Best regards,

Matthew Ian Loew
"I don't grow up. In me is the small child of my early days" -- M.C. Escher

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[corus]

Chris,
Any stress near a weld is allowable, it just depends on how long you want the weld to last. In general, stress endurance limits define an infinite life for a component. For welds this is generally taken as being 10^7 cycles. Some might use a slightly lower figure like 2x10^6 cycles but they're generally the same. Depending on the weld classification then this gives the endurance limit for the weld (or close to the weld). You'll find these values in BS7608 or BS 5500 or whatever the european equivalent is now. ASME give the roughly the same but then you have to apply a factor for the weld type, if I remember.

Matthews links are very good but all these codes depend on the user specifying the weld classification and probably the position of the nominal stress. They're not a magic wand that instantly tells you how long a weld will last but still depend on the idiot pressing the right buttons, even though they give the impression they don't.

corus

 

[ParabolicTet]

for welds, the time-history variation of the load is critical. Say you know the stress under one load case, but often does that loadcase occur and what is the range of values it occurs?

You need to have accurate load data that reflects all applications your part will see in the field. Without this data, you are much better off doing a comparative analysis and compare nominal stress away from welds to a baseline design with a proven field history. This will be much better than trying to design to one stress amplitude for a certain number of cycles, since most real-world parts never see a constant stress range for a fixed number of cycles.

 

[beloka]

Chris
As Corus notes, BS7608 "Fatigue Design and Assessment of Steel Structures" is very helpful. It is often used in design of large rotating equipment such as grinding mills and should provide reliable data.
Another standard that may help is BS7910 "Guide on Methods for Assessing the Acceptability of Flaws in Metallic Structures".
Beloka

 

[chris9]

The reason I asked this question was because a consultant tried to tell me that 360 MPa was an acceptable stress on and around the weld area on a mild steel bracket. The load case used was linear static for one load cycle but in reality the part would get thousands of cycles. The yield stress of the parent material was about 300 MPa. I always thought that for repeated loading, welds were generally less durable than mild steel and therefore I should aim to reduce stress to less than the yield stress of the parent material and probably less than 100 MPa to play it safe.

 

[corus]

Chris,
To obtain the life of a component using the S_N approach then stresses obtained from a linear analysis is the method that is used. Using a static linear load case is also acceptable as all other load cases would just be some factor of your results for that single load case.
In BS 5500, which uses the same data as BS7608, the allowable design stress range for 5000 cycles (say) is between about 300 and 700 MPa depending on the weld classification. The yield stress of the material doesn't come into it for fatigue assessment.
If you're looking at failure of the component against the yield criteria then you also need to look at where the stress is as twice yield is acceptable for secondary stresses.

corus

 

[chris9]

Corus,

Thanks for the input. After having a look at BS7608 I think 360 MPa was too high for the particular application.

 

[ParabolicTet]

another point to remember about welds is that small changes in stress equal big changes in life. this is because there is an exponential relationship between stress and life.

 

[corus]

ParabolicTet is incorrect in what he/she says if you use the S_N relationship described in the design standards. The relationship between stress and life is cubic, ie. if you double the stress then you have an eighth of the life, or an eighth of the number of cycles to failure. Similarly reversing that, half the stress gives eight times the life.

corus

 

[johnhors]

Corus

Cubic is exponential , it's just a more precise description.

 

[ctmfab]

I'm not sure what code you are trying to satisfy, but from the pressure vessel industry here are a few comments. Got a bit long winded, but I consider fatigue prediction one of the less accurate parts of our work.

We typically tell people during seminars...

"The good lord watches over:
1. Children,
2. Fools, and
3. People that try to predict fatigue failures of PVP geometries with FEA programs.”

========================================
Anyways, here it goes...


As already mentioned, the question depends on what type of load you have. If cyclic, then you need to ensure that the peak stress at the weld toe is within the allowable alternating stress for your given cycles.

You are opening a can of worms here because the stress will tend to be very mesh sensitive unless you use use nodal forces to derive a load on the weld. WRC-474 gives a good approach that helps eliminate the mesh sensitivity issue. Otherwise you are left to determine what mesh density and peak stress is accurate using your engineering judgement.

I would be interested in knowing if anyone has a good approach to the singularity effect at these notches. Plastic analysis is always one option I guess...

Norsok-004 and a few other documents give some guidance on the size of the elements, but that is still a sketchy approach. I belive EN-13445 gives an extrapolation procedure that is fairly good.

If there are no cycles then you are really only concerned with ensuring that your primary loads (sustained loads like weight, pressure, etc) don't cause gross plastic deformation that could lead to collapse.

Welds in vessels are typically "transition" elements going from one shell to another shell and should be stronger than surrounding material. As suggested in WRC-429 and the new Div 2 rewrite, you don't need to check the stresses inside the weld volume since code rules ensure that the stresses in transition regions won't cause problems. Furthermore, the same rotational and extensional deformations that exist in shells won't typically exist in these "transition" regions.

One final thought here is the HUGE safety factors applied in the fatigue curves of PD-5500, En-13445, ASME, AD-merkblatter, API-579, etc. The polished bar fatigue curves used in the current ASME vessel codes have a safety factor of 2 on stress and 20 on cycles (yes 20!). And this just gets you to the mean curve of the original fatigue data (50% failure line)!!!!

The as-welded curves in most European codes is on the order of 99% survival probablility. Again a very large safety factor. The CEN has great data for review of the as-welded curves (free on the net). It is very eye opening to see the huge scatter of data and bit humorus how they apply 3 or 4 standard deviations to contain all the fatigue data.

http://www.paulin.com

 

[JohnnyEnglish]

ctmfab - I have similar FEA weld issues. I am working with ANSYS, and have included a batch file here of a typical case for those interested ANSYS users to run if they wish. Apologies then for the length of this thread, but they do say a picture speaks a thousand words...

Fundamentally, it is a static problem of a vertical bracket welded to a 2m diameter ring. This is a very general case. The material is 5mm sheet steel, and the downward load at the end of the bracket is 10,000N. ANSYS reports the reactions at the weld C of G correctly which is great for me because I can use these forces and moments in my hand calc checks of the weld and the parent material in the more complex cases. However, stresses in the ring material at the top and bottom of the bracket to ring weld are high and do not converge with mesh refinement. This is of course expected in FEA when modelling a re-entrant corner in a shell model. In the batch file, the final plot is of the stresses in the ring, and the element size can be varied with the parameter "elesize".

Does anyone have an idea on how to handle this problem? Are these reported stresses anywhere close to reality? In a static load case with ductile materials, we often ignore the peak stress point as long as the stress drops rapidly away from the hot spot and the general membrane stresses are shown to be less than yield thereby not resulting in plastic collapse. However, what if the problem was one of cyclic loading and fatigue? For any typical case I would take the peak stress and, using a safety factor of 2.5 for a fillet weld, calculate the life from the material S-N curve...but these modelling singularities are prohibitive.

Your input is appreciated.

JE.


/prep7
!********** PARAMETER FOR ELEMENT SIZE **********
elesize = 0.03
!********** ELEMENT DEFINITION **********
et,1,shell63
!********** MATERIAL PROPS **********
mp,ex,1,200e9
mp,prxy,1,0.3
r,1,0.005
!********** GEOMETRY **********
csys,1
k,,1
k,2,1,,1
k,3,1,7.5
l,1,2
l,1,3
adrag,1,,,,,,2
csys,0
arsym,y,all
nummrg,kp
wpro,,90
csys,4
rectng,1,1.1,0.6,0.8
aglue,all
!********** MESH **********
esize,elesize
amesh,all
!********** BOUNDARY CONDITIONS AND LOADS **********
csys,1
lsel,,loc,y,-7.5
lsel,a,loc,y,7.5
dl,all, ,symm
lsel,,loc,z
dl,all,,UZ
ksel,,loc,z,0.8
ksel,r,loc,x,1.1
fk,all,fz,-10000
allsel,all
eplo
finish
!********** SOLUTION **********
/sol
solve
!********** POSTPROCESSING (DISPLAYS STRESS IN RING) **********
/post1
asel,s,loc,x,1
allsel,below,area
/dscale,1,off
avprin,0
plnsol,s,int,0,1
/view,1,1
/ang,1
/rep,fast