I am performing SOL 101 analysis. I realize in my .f06 output there is a "Grid point singularity table" that shows failed grid points. What does it mean?
Should I always use:
PARAM, AUTOSPC, YES
and what are the implications of using this command?
Thanks in advance!
The AUTOSPC parameter is ON by default in NX Nastran solver since a few versions ago, then no worry if you forgot to issue it explicitly.
NX Nastran automatically identifies and constrains singularities in the stiffness matrix using a parameter called AUTOSPC. When you add PARAM,AUTOSPC,YES to your input file, NX Nastran automatically removes degrees of freedom that are either unconnected or very weakly coupled to the finite element model.
If singularities remain in the stiffness matrix at the grid point level, the NX NASTRAN software automatically outputs a Grid Point Singularity Table (GPST) after the Grid Point Singularity Processor (GPSP) executes. The table lists singular degrees-of-freedom in the global coordinate system. You can have the software automatically constrain singular degrees-of-freedom using the PARAM,AUTOSPC,YES option, then any identified singularities with a ratio smaller than PARAM,EPZERO (default = 1.E-8) will be automatically constrained with single-point constraints.
The NX NASTRAN software prints the GPST in the .f06 file. The GPST lists all singular degrees-of-freedom, in the global coordinate system, and the ratio of stiffness between the softest and stiffest degree-of-freedom for the grid point. It also lists any degrees-of-freedom that the software automatically constrained.
To reduce the size of the *.f06 file you can set OFF the printing of the GPST, simply including in the bulk data PARAM,PRGPST,NO and the printout of singularities is suppressed, except when singularities are not going to be removed.
But please note you should always review the Grid Point Singularity Table carefully to understand which DOFs were singular and why. Automatic constraint generation can mask actual modeling errors.
I'm having the same outputs in my .f06 when I run SOL 101 or even SOL 105.
I have been looking the nodes that were pointed in the list, and it's all the points that are not connected with Surface to Surface Gluing. I don't understand why .. the problem is only on rotationnal DOFs, but I think it is wierd that the listed points are all the others nodes not set in Surface to Surface gluing...
What do you think the problem could be?
I think it slows down the analysis, am I wrong?
Thanks in advance,
Hello Elaine, hello Mixi,
may be the message also occurs if different parts of mesh are not connected e.g. when duplicate nodes are not merged and decoupled sub meshes without constraints are formed.
An eigenfrequency analysis will uncover it due to additional rigid body motion forms with (nearly) zero eigenfrequencies.
Glueing: It can also fail if search distances between gluing regions are too small or glueing regions do not fit in projection. I think sometimes negative search distances can also solve gluing problems. I also made at once the mistake to use one region both for source AND target region. NX did not give me a warning message.
Singularity in rotational DOFs: I made the experience that shell elements with midside nodes can also produce such singularities at their midside nodes without visible reason. It can drive you mad. AutoSPC couldn't solve that problem in my case. Linear shell elements do not have that problem.
BAILOUT=-1 was the way I choosed.
If you couple shell nodes with beam elements which are pointing into normal direction of shell element at coupling node, it also can produce singularities at rotational DOFs if the beam is not restrained against free rotation. Thin shell elements do not have a stiffness for their rotational DOF in normal direction. For linear elements you can define an artifical rotational stiffness with a special parameter. But it does not work with parabolic shell elements with midside nodes.
Best wishes, Michael
Hello Elaine, hello Trixi,
one additional information about "GRID POINT SINGULARITIES" at rotational DOFs:
They also occur at NODES (Grid points) of SOLID elements (hexahedrons, tetrahedrons, pyramids, ...). As these elements do not link to rotational DOFs of nodes the rotational DOFs of linked nodes remain unlinked in most cases and have therefore no stiffness parameters (stiffness matrix at that DOF is singular). In a model fully created with solid elements you will therefore have ALL its nodes in the GRID POINT SINGULARITY TABLE.
They will be constrained automatically because AUTOSPC=YES is set by default and you will be informed about that, too.
*** USER INFORMATION MESSAGE - SINGULARITIES FOUND USING EIGENVALUE METHOD
*** 242139 SINGULARITIES FOUND 242139 SINGULARITIES ELIMINATED
But the f06 file can grow up to many Megabytes in file size without having ANY important information in that table. That's really annoying. Setting off "printing GPST" by setting PRGPST to NO is a really good way in that case.
Best wishes, Michael