Nonconvergence Finite Axis-Symmertic Mixed Problem

[sanshi2000]

I am doing another prblom with follower pressure by axisymmetic element. However, convergent solution can not be reached in my current feap version feap8.3.14. Could you please run the attached problems (Inhk16, Inhk32, Inhk64) in your feap to check wether convergent solution can be reached? By the way, you can use more coarse or fine mesh by decreasing or increasing the value of n at line 8 of one of these input files. Thanks a lot.

Merry Chrismas,
Lei

[sanshi2000]

Happy new year to all. Can anyone share idea on the non-convergence of my previous attach problem? Thanks a lot.

Best wishes,
Lei

[sanshi2000]

Any advise on fixing the problem is reaaaaly appreciated. Is there any document indicating the relationsip between commands in input file and subroutine in feap? The kind of document, where I can find the corresponding subroutine from any command I used in input file, may help me to trace problems when using feap. Thanks a lot in advace.

Best wishes,
Lei

[FEAP_Admin]

To follow the path of execution for Macro commands, first look in program/pmacr.f and find your command in the
data statement for 'wd'.  Now look at the number on the continuation line.  If for example you look at 'disp' you will see that the continuation line number is '3'.  That indicates that the 'disp' command is in the file program/pmacr3.f.
Go to that fine and search for '[disp]' and you will find the relevant code for the 'disp' command.

[FEAP_Admin]

Your problem with non-convergence seems to be related to the mixed option.  If you remove it, then all is well.
But with your Poisson ratio you need mixed.

Most llkely there is a problem with the mixed-axis symmetric tangent.  We will have a look at it.

fyi, a non-ideal work around (will run slow) is to use numerical tangents.  Try inserting the line 'ntan,mate,1' just before you set 'dt,,0.1'

[Prof. R.L. Taylor]

Lei,

Your problem was tested in a pre-release of the next version (which did identify a bug in the axisymmetric tangent).  However, when we run the problem in the release version there is no error.  As far as we can identify, there have been no changes to the element between your version and the current release version.  There was a correction to the follower pressure load (which we provided for you) -- are there any other changes you have made?  If not, can you zip the axisymmetric mixed element (fld2d2 and the 'kine' 'bbar' 'fbar' routines it calls) and post it so we can try to identify where the error may be.

[sanshi2000]

Thanks very very much for your kind help.

With your new subroutine, presld.f, the previous problem has been solved, where I was considering the agreement with axisymmetric and 3d element by analysing inflation of a stretched tube. A brief report on that problem is attached.

But for the current problem, where I am analysing a tube with prescirbed crack, the convergence seem never to be reached as shown in the report attached. I has been seeking the possible reasons, which could be the stress concentration or another rather than feap's bug, since good results are obatins for the previous problem. To confirm that, could you please rerun the attached inputfile 'Inhk_nostretch' in your version, where the mesh size could be reduced by increaing n at the line 8? If convergent, could you also please record the extreme radial displacment, which could be gived by the 3rd colome of the output of 'disp list 1'?   

By the way, 'disp nodes n1 n2 inc' seem not work as expected, only value of one node numerbered by some value independent with n1 and n2 is returned. 

Your time and help are reaaaaaly apperiated. Thanks a lot.

Best wishes,
Lei

[Prof. R.L. Taylor]

First, when you said there was no convergence, we interpreted the comment that the Newton iteration did not converge.   

Your comment concerns the lack of solution convergence with mesh refinement.  These are different things.

In your problem you do have a singularity at the end of the crack.  Thus, as you refine the mesh you will not be able to get a fully converged solution.  For the finite elastic case the tip should experience very large deformations and result in a solution with some finite curvature around the tip, however, with finite elements and a Neohookean material you probably will not be able to achieve a converged solution by subdividing the mesh spaces (a local mesh refinement around the tip could help -- but you will need a good mesh generator to achieve this and keep quadrilateral elements).  If the material is inelastic then there will be a process zone around the tip which needs to be resolved.

[sanshi2000]

Sorry for my confused comment. Thanks very much for your kind advise.

Best wishes,
Lei

[FEAP_Admin]

Adding to Prof. Taylor's comments, I would suggest the following:

1) make a much smaller test case so that you can figure out what to expect; start linear plane strain, move to axis sym, add follower, then finally add finite.

2) note that any crack type singularity will knock the convergence rate down by a factor of the singularity strength (1/2 in the linear case -- more complex in the finite case); so it will not be like a smooth problem.

3) be careful with the tie command.  it is a search command and on some mesh densities it may not get all the correct nodes, sometimes it may miss, sometimes it may grab too many.  You can try to control the behavior with the gap command.  PLOT,OUTLine will help you debug as will examining carefully the list of tied nodes (lookin at the list is tedious but sometimes important, perhaps you can automate the process with a small script).