Showing results for 
Search instead for 
Did you mean: 

Welding FEM Simulations system

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Hello everybody,

Do anyone know about welding FEM Simulations module for SIEMENS PRE/POST (FEMAP, NX).

How do you solve this problem - Internal stress in welding and permanent deformation.


Have somebody any tips or solutions???


Thanks for your answer.


Re: Welding FEM Simulations system

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom


I run Fatigue Analysis in weld seams from FEM models created in FEMAP using winLIFE (see, a powerful fatigue analysis tool integrated in FEMAP as an add-on module that take advance of NX NASTRAN results as well.



To perform the fatigue calculation of welded structures, numerous procedures are available. Very early on, Haibach proposed to use strain gauges in front of the weld and used such measurements under service load to make fatigue predictions. He set rules on where and how to use these strain gauges and he showed that reliable results can be obtained. This idea can easily be transferred to calculations with finite elements. Similar to strain gauges, the results of the “measurement points” are used to extrapolate the stresses. This is the way I run using FEMAP + NX NASTRAN to ge stress results + winLIFE to perform fatigue life calculations.


The real structure could be modelled by plate elements (a) or solid elements (b). The size of the elements should correspond to the thickness of the plate to achieve a finite element model with a limited number of elements.


In the case of plate elements the weld is typically not modelled and the finite elements are arranged in the middle of the individual plates (midsurfaces). To calculate the stress in the weld toe by extrapolation, a line of nodes at a certain distance from the weld toe and parallel to the weld seam must exist. In the case of linear extrapolation the two line of nodes must be at 0,4 t and 1,0 t in the direction perpendicular to the weld toe, being "t" the plate thickness.



This video shows how to perform fatigue analysis in weldings with plate elements using winLIFE and the STRUCTURE STRESS CONCEPT METHOD:

If you plan to mesh explicitely the seam welds using 3-D solid elements, I suggest to use hexahedron elements. For the structure stress concept with linear extrapolation, the distance of node line#1 is 0.4 x the thickness of the steel of the weld seam and the distance of node line#2 is 1 x the thickness of the steel of the weld seam. For instance, if the thickness of the steel profile is 7 mm, node line#1 is therefore 2.8 mm and the node line#2 accordingly 7.0 mm away from the fillet weld.


Here you are a VIDEO of a fatigue analysis example with solid elements:


Also winLIFE support the HOT SPOT SEARCH METHOD to perform fatigue analysis of welded structures meshed with Shell elements. Very powerful, I use it a lot because is very easy to setup. For the fatigue life calculation here we use the element stresses projected perpendicularly to the weld toe notch. Since only one element is used for the fatigue life prediction, the increased stress in the weld notch is only recorded to a limited degree of reality and the quality of the prediction is therefore not as good as with a structure stress concept. The critical points of a structure can be found, however, using this method. If required, the hot spots found can then be re-calculated to increase the quality of the prediction.


Within FEMAP you can create automatically the weld elements. The various properties of the sheet metal make it possible to identify the welds. Sheets are looked for which are joined together with nodes. The nodes found are where the sheets meet and show the welds. All elements which lie on these seam nodes are grouped together in weld groups. The groups are created with the command in the winLIFE menu "Create weld groups“.




winLIFE calculates the fatigue life of the welds according to the Hot-Spot Search. The result file created in winLIFE during the calculation process is read back into FEMAP to show the damage sum and degree of utilization. In the following picture the Degree of Utilization = 0.384 is shown in FEMAP.

The degree of utilization of 1.0 signifies the endurance limit is reached. The here reached value of 0.384 means that the endurance limit is used to 38.4%. The safety to endurance limit corresponds to the inverse of the degree of utilization and is 1/0.384 = 2.6.


Best regards,

Blas Molero Hidalgo, Ingeniero Industrial, Director
Blog Femap-NX Nastran:

Re: Welding FEM Simulations system

Solution Partner Creator Solution Partner Creator
Solution Partner Creator

Hello Blas,

thank you very much for your answer, but I was thinking a little different area calculations of weldments. I'm interested in the area of permanent deformation after welding due to temperature and internal stresses. Curl weldments after welding. Tool that will help optimize the order of welds,....

I tried to simulate a manualy:
1st temperature calculation - transient
2nd structural calculation - non-linear material, transient solution and load deformation by temperature increments of 1st calculation.

Finaly I would like to find plastic deformation after welding.
Something like this: 

Re: Welding FEM Simulations system

Solution Partner Experimenter Solution Partner Experimenter
Solution Partner Experimenter



My organisation is support partner to Siemens PLM In India for CAE products. We have customised the software incorporating some research papers findings to predict the Permanent Deformation during and after weldings. It was done for one of the Largest Heavy engineering Organisation in India. It was very successful delivery and oucomes were close to 95% of field data. 

If you want may write me on


- Deepajee