Showing results for 
Search instead for 
Did you mean: 

Post processing of Advanced Non Linear Analysis SOL601



It is more a educational post than solving particular problem. I was inspired by movie in link below:


If you take a look at this video. How you think we can assess whether the material will start breaking. Ok, the main result that is driving in such simulations is a plastic strain, but as far as I know (maybe I am wrong) the elementns will remain intact even for high strains. Am I right? Another words, are there element types that allows for the model crack initiation and further propagation ? In example, how you would model the stranding of the ship (element types, solver, type of analysis, etc ?)


Any proposals? Maybe you know some interesting publications of non-linear analysis in NX Nastran? I would be thankful of any guidelines and tips introducing into dynanmic and non linear simulations.


Thanks Smiley Happy




Re: Post processing of Advanced Non Linear Analysis SOL601

Solution Partner Phenom Solution Partner Phenom
Solution Partner Phenom


Take a look to the NX NASTRAN ELEMENT LIBRARY manual, you will see the Crack Tip Element type, but unfortunately is not supported by neither FEMAP or NX AdvSym pre/postprocessors GUIs.


NX Nastran crack tip elements include both two-dimensional (CRAC2D) and three-dimensional (CRAC3D) types. You can use the two-dimensional crack tip elements to model surfaces with a discontinuity due to a crack. You use the CRAC2D entry to define the element geometry and the PRAC2D entry to define its properties. You can model a CRAC2D element with temperature-independent anisotropic materials. The 2-D element may be either plane stress or plane strain. The element generates either coupled or lumped mass matrices. The three-dimensional crack tip element is used to model solids with a discontinuity due to a crack.


Also, CRACK PROPAGATION ANALYSIS is a typical calculation procedure in Fatigue Analysis. In many areas of technology dimensioning takes place up to a technical tear (crack length approx. 0.1 to max 1 mm) and the component should not be used beyond this tear point. The reason is that the number of cycles between the initial tear and the complete failure of the component is very short (approx. 5 to 10% of the total fatigue life). The unfavourable relation of use and risk makes any further use inadvisable. 


In aviation and space technology where lightweight constructions of aluminium alloys are used here the number of cycles between the initial tear and failure is much larger and it is common and acceptable to use components with a tear. It is, however, important to know the phase of crack growth and to be sure that the cracks are found during inspection before failure. Fatigue Crack propagation analysis is therefore an important measure for determining the inspection intervals.


When analysing and reconstructing the damage, it is also often important to be able to estimate the crack propagation. Fatigue Damage experts must be knowledgeable on this subject. Really complex, but the procedures exist!!.


Best regards,


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

Re: Post processing of Advanced Non Linear Analysis SOL601

Siemens Phenom Siemens Phenom
Siemens Phenom

The default behavior for multilinear elastic-plastic materials in SOL 601 is to extend the stress-strain data by linear extrapolation of the last two points. In this case, your initial assessment is correct - the elements never fail and remain intact for high strains.


If XTCURVE is set to 0 on NXSTRAT, then the material data table is not extended. If the strain in an element exceeds the last strain value in the supplied data, then that element is considered to be ruptured and is removed from the analysis. No special element types or modeling techniques are needed.

Re: Post processing of Advanced Non Linear Analysis SOL601

Hello dear,

I am need to simulate crack propagation in NX nastran, will you help in explaining the procedure or have any tutorial to share?