Cancel
Showing results for 
Search instead for 
Did you mean: 

Fatal Error 2083 TA1NLE

Valued Contributor
Valued Contributor

I am running a non-linear anaysis I have done many times before, but now I am getting this error.  Any ideas where to look? 

 

I could maybe modify the input deck, but I don't have the enterprise version so a modified deck would not work.   I have to figure it out through the femap gui.  Using nonlinear static.

 

 *** USER WARNING MESSAGE 2083 (TA1NLE)
     FOR ELEMENT          393 MID3 REFERENCE TO A MATS1 IS IGNORED
     BECAUSE NX NASTRAN SHELL THEORY IS A 2-D REPRESENATION OF PLASTICITY.

 *** USER FATAL MESSAGE 2083 (TA1NLE)
     FOR NONLINEAR MATERIAL PROPERTIES REFERENCED ON THE PSHELL ENTRY,
     MID4 MUST BE BLANK AND MID1 AND MID2 MUST REFERENCE THE SAME MAT1/MATS1 ENTRY COMBINATION.
     User information:
     For nonlinear material properties referenced on the PSHELL entry,
     MID4 must be blank and MID1 and MID2 must reference the same
     MAT1/MATS1 entry combination.

 

7 REPLIES

Re: Fatal Error 2083 TA1NLE

Phenom
Phenom

The warning message is advising that the Transverse Shear will only use the linear properties of the plate material, and not the non-linear plasticity part of the plate material that has been specified for the relevant property.

 

However, the FATAL error message presumably occurs because you have an entry in the Memb-Bend Coupling field of the plate property.  You can check / edit this easily within Femap by looking at the plate property(ies).  The default is that Memb-Bend Coupling is ignored.  You probably have it set to a material (possibly "Plate Material") which is obviously a non-linear material.  I suggest you refer to Remark 6 of the PSHELL entry in the NX Nastran Quick Reference Guide, which comes with your installation of Femap.

Re: Fatal Error 2083 TA1NLE

Valued Contributor
Valued Contributor

I did not see anything in the Memb-Bend Coupling, but some of the PSHELL had different materials for the Bending and Transverse Shear....After changing them to "Plate Material" so it was consistent, the problem persists.

 

Re: Fatal Error 2083 TA1NLE

Phenom
Phenom

So how did some of the elements end up with different materials for bending and transverse shear?  Did the model originate in Femap, or was it an imported bdf?  The question is, do you know why some of the pshells have separate bending to plate material (eg. an attemtp to represent corrugated sheet in linear analysis)?  

Anyway, the message tells the story.  The warning message is saying the plastic material is being ignored for transverse shear.  But it is also saying that the bending material must be the same as the plate material itself [for non-linear analysis].  It lists the element number (393), so that is the starting point for checking the property thoroughly.  If all the properties had the defaults (which may substantially change the engineering, by the way), this message will not appear.

 

 

Re: Fatal Error 2083 TA1NLE

Valued Contributor
Valued Contributor

After importing a model (*.dat/bdf/inp/...) I wanted to consolidate some of my materials.   So, I used Modify, Update Elements, Material, by element.   This changed the first material, but the material for the bending and shear was left as the original.  

 

I changed this and checked the PSHELL settings.   I also did a test model (attached).   If the step size is too large or the strain too big it gives this warning and then a bunch of warnings and a fatal error.   At load 350 lbs it works fine, but at 400 it will not solve and gives this:

 

 *** USER WARNING MESSAGE 2083 (TA1NLE)
     FOR ELEMENT           26 MID3 REFERENCE TO A MATS1 IS IGNORED
     BECAUSE NX NASTRAN SHELL THEORY IS A 2-D REPRESENATION OF PLASTICITY.

 *** USER FATAL MESSAGE 6288 (SITDR2)
     UNABLE TO CONVERGE WITH ITERATIVE METHOD.
1    NONLINEAR ANALYSIS                                                    FEBRUARY   3, 2016  NX NASTRAN  8/25/13   PAGE   228

 

Somewhere along the line my setting got changed.   Model has been acting strange...maybe it is getting corrupted....save often.

Re: Fatal Error 2083 TA1NLE

Phenom
Phenom

The second problem you posted is fully unrelated to the first, other than both are for a non-linear analysis.  Convergence difficulties in non-linear analysis can be due to a whole range of reasons, not least of which is the possibility that your real structure (as modelled) cannot support the load you wish to apply.  It is also "path dependent", so can be sensitive to some of the choices you make about increments, iterations and convergence tolerances (and arc-length methods and automatic increment bisections etc etc) .  Linear analysis simply needs a mathematically viable set of equations and has no care whether you apply 1N or 1e9 N.  Non-linear analysis is a much closer attemtp to model the real world, so is an order of magnitude more complex.  There is never a "one size fits all" approach to non-linear analysis settings, due to the wide range of types and severity of non-linearity.

 

And finally, the chances that this problem is related to model corruption or saving, is (for better or worse) less than 0.5%.  Femap is one of the most robust programs I have ever used.  Not perfect, but very, very solid.  If you ever have an actual problem with models saving successfully, the first place to check is whether your hard disk is failing or the SSD is approaching its write cycle limits.

Re: Fatal Error 2083 TA1NLE

Valued Contributor
Valued Contributor

Thanks for the input.   You gave me some good areas to look at.  

 

The model seems to be running now.   Basically it had to do with my step settings.   I'm still not sure why it had me going on a wild goose chase looking at my PSHELL settings when it was the step size it did not like. 

 

I will have to look into your suggestion on how to get set the thickness on the elements rather than separte PSHELL entries...it would have saved me some time debugging.

Re: Fatal Error 2083 TA1NLE

Phenom
Phenom

So, just a bit of general advice...

Femap encourages the same tiered structure as the general Nastran structure. ie.

Plate (and solid, and beam and most others) elements reference a property, which references a material.  I can promise you, this methodology is one of the great foresights for model editing developed by the Nastran guys way back in the 60's.

 

Thus, your model should have as many plate properties as you have distinct requirements for thickness and material.  Eg. if you had 5 thicknesses and two materials, but one material only needs to have two thicknesses out of the 5, then you need 7 properties.  Then when you need to update "materials", then you would actualy use Modify -> Update Elements -> Property ID to change the elements from referencing one of the existing properties, to another of the existing properties.  If your change to the elements required a different property not amongst the 7 existing combinations, then you would create another property first.

 

And if all the elements which are 3mm thick need to change to 3.5mm, then that is an edit to the property (no edit or update required to elements, or any need for a new property)

 

Of course, if all you needed to do was to change one of the materials so it had non-linear behaviour, then you simply make that change to the material itself, and then all the properties which use that material (and elements which use those properties) are automatically "updated", because of the hierarchy - no need to Modify -> Edit anything other than the material itself.

 

I hope that tells you something you did not already know.