ANSYS中如何解决非线性不收敛的问题？
一、问题描述
3D
1/2对称竖直水泥土加劲抗拔桩，带三块分散板的钢绞线埋于水泥土桩体内，钢绞线分自由段和锚固段。建立了钢绞线杆轴，没有建立分散板，假定其刚度无穷大，其作用是通过与相邻的杆轴节点耦合实现的。没有考虑初始地应力，同时作用了竖向重力和上拔位移。
当材料全部为弹性时，计算很容易收敛，但将土体材料改为弹塑性材料DP时，连第一步都不能收敛，弹性材料和弹塑性材料的收敛历史如下图所示。如何解决非线性不收敛的问题？
弹性材料
弹塑性材料
二、基本理论
1、8.11.2. Overcoming Convergence
Problems
This section provides information to help you fix convergence
problems in a nonlinear analysis. The following topics are
available:
Overview of Convergence Problems
Performing Nonlinear Diagnostics
Tracking Convergence Graphically
Automatic Time Stepping
Line Search
Nonlinear Stabilization
Arc-Length Method
Artificially Inhibit Divergence in Your Model's Response
Use the Rezoning Feature
Dispense with Extra Element Shapes
Using Element Birth and Death Wisely
Read Your Output
Graph the Load and Response History
2、Overview
of Convergence Problems
Some examples may be initially open contact surfaces causing rigid
body motion, large load increments causing nonconvergence, material
instabilities, or large deformations causing mesh distortion that
result in element shape errors.
CHECK, MCHECK,
and CNCHECK commands
help you verify if there are any obvious problems with the model
before you start the solution.
When
you analyze models with large deformations,
some portions of the initial mesh can become highly distorted.
Highly distorted elements can take on unacceptable shapes,
providing inaccurate results. This can cause your nonlinear
solution to stop. When this happens, use the ESCHECK command to perform shape
checking of deformed elements in the
postprocessor (based on the current set of results in
database). This deformed-shape checker helps you to identify the
portions of your model that require different meshing, thereby
allowing them to retain acceptable shapes. Using ESCHECK at
different time points helps you to identify the load conditions
that cause mesh deterioration.
A convergence failure can also indicate a
physical instability in the structure, or it can merely be
the result of some numerical problem
in the finite element model.
3、Performing
Nonlinear Diagnostics
The nonlinear diagnostics
tool NLDIAG can
help you find problems in your model when an analysis does not
converge.
Identify
Regions of High Residual
Forces Issue the NLDIAG,NRRE
command to write the Newton-Raphson residuals from equilibrium
iterations to a file (Jobname.nrxxx).
You can then contour plot the residual
forces via the PLNSOL,NRRE
command, which helps to identify regions of high residual
forces.
Such
a capability can be useful when you experience convergence
difficulties in the middle of a load step, where the model has a
large number of contact surfaces and other nonlinearities. You can
restart the analysis and issue
an NLDIAG,NRRE
command to write out the residuals. By tracking the way the residuals change over several
equilibrium iterations you can identify a portion of your
model where large residuals persist. You can then focus on the
nonlinearities in that area (for example, a contact pair's
properties) instead of having to deal with the entire
model.
Process the Tracked Results Issue
the NLDPOST command
to process the .ndxxx nonlinear
diagnostics files. The command creates
components of elements that violate a certain criterion for a
particular equilibrium iteration (or
iterations).
Monitor the Diagnostics Results in Real
Time The NLHIST command
allows you to monitor results of interest in real
time during solution. Before
starting the solution, you can request nodal data such as
displacements or reaction forces at specific nodes. You can also
request element nodal data such as
stresses and strains at specific elements to
be graphed. Pair-based contact data
are also available. The result data are written to a file named Jobname.nlh.
For example, a reaction force-deflection
curve could indicate when possible buckling behavior occurs.
Nodal results and contact results are monitored at every converged
substep while element nodal data are written as specified via
the OUTRES setting.
4、Automatic
Time Stepping（静态的塑性问题可以不选此项）
This can be important in the following situations:
-
Problems that have
only localized
dynamic behavior (for
example, turbine blade and hub
assemblies) in which
the low-frequency energy content of
the system could dominate the
high-frequency areas.
-
Problems
with short
ramp times on
some of their loads. If the time step size is allowed to become too
large, ramped
portions of the load history may be
inaccuratelycharacterized.
-
Problems
that include structures that are
continuously excited over a range of
frequencies (for example,
seismic problems).
5、Line
Search
Line search
(LNSRCH)
can be useful for enhancing convergence, but
it can be expensive (especially with plasticity). You might
consider setting line search on in the following cases:
-
When your structure is force-loaded (as
opposed to displacement-controlled).
-
If you are analyzing a "flimsy"（脆弱的）
structure which exhibits increasing stiffness (such as a fishing
pole).
-
If you notice (from the program output
messages) oscillatory
（振荡的）convergence patterns.
三、解决方法
1、做好准备工作。通过完全弹性模型的计算结果，熟悉该桩型的受力特点，便于后续采取有针对性的措施。
在ANSYS后处理中通过Results
viewer查找模型中应力或位移最大节点的坐标信息。下图为T=0.01(第一个收敛点，表示荷载较小时刻）的竖向最大应力信息。通过坐标信息，表明最大拉应力产生于桩底之上的桩侧土体。可能是由于桩底的侧摩阻力过大引起的。
桩侧土体竖直面内最大和最小剪应力TXZ（XYZ为圆柱面坐标）如图所示：
根据上图的坐标信息，表明最大剪应力产生于桩底之上的桩侧土体。
通过上图的坐标信息，表明最小剪应力产生于锚固段之上的桩侧土体。可能是由于钢绞线锚固段顶的局部压力引起的。
根据上面的分析，发现桩侧摩阻力对桩侧土体的应力状态影响很大，故需列出桩侧摩阻力分布图，如下：
注：关于如何绘制侧摩阻力图，可参考"ANSYS和EXCEL中如何编程实现“引用某列数值对应的另一列的值”？"http://blog.sina.com.cn/s/blog_9f5beef70102wpl5.html
由上图可知，在桩底（Z=-18000)和锚固段顶（Z=-6000)两处，桩侧摩阻力都特别大，这与上面分析得到的土体中最大应力和位移分布是吻合的。由此可推断出，对于比较难收敛的弹塑性模型，首先要解决桩型受荷初期，上述两处受力较大造成的应力集中问题。
2、可能的解决方法1---放松收敛条件
以模型3Dhorinoholealljiangjiangpile0120151101.txt为例，当为默认的收敛标准（0.001,2范数）时，计算很难收敛，连第一步也难；将收敛标准改为（0.05,2范数）时，不平衡力与收敛容差接近了，但仍无法收敛；将收敛标准改为（0.1,无穷范数）时，第一步和之后的其他步可以收敛。将收敛标准改为 （0.1,2范数）时，第一步就不收敛了，将收敛标准改为 （0.5,2范数）时， 第一步和之后的其他步可以收敛。各收敛标准下的收敛历史如下图所示。
（0.05,2范数）时的收敛历史 不能收敛
（0.1,无穷范数）收敛历史 可以收敛
（0.1,无穷范数）收敛计算信息 可以收敛
（0.1,无穷范数）收敛时刻信息 可以收敛
（0.1,2范数）收敛历史 不能收敛
（0.5,2范数）收敛历史 可以收敛
（0.5,2范数）收敛历史信息 可以收敛
那不断放松收敛标准，虽然最终计算收敛了，是否会影响计算结果呢？还有没有更好的解决方法？
3、可能的解决方法2---更换不同的单元类型
通过放松收敛条件，虽然可以收敛了，但结果可能有错误，需要设计者利用工程经验判别是否可以采用。 继续以上面的模型为例，在收敛标准（0.5,2范数）下，发现这个模型有二个错误，一是土体单元始终无剪切应力，但桩体和钢绞线有剪切应力，且钢绞线的剪切应力很大（因为钢绞线不是纯轴拉，有侧摩阻力作用），二是土体单元始终始终无塑性应变。而之前的完全弹性模型中土体是有剪应力的。造成剪应力丢失的原因可能是非线性收敛标准或者单元类型SOLID285造成的，经过我初步分析，发现产生的原因可能是单元类型SOLID285容易造成剪应力丢失。为了解决非线性收敛问题，需要更换单元类型。具体分析过程详见博文“三维抗拔桩模型为何无剪应力”http://blog.sina.com.cn/s/blog_9f5beef70102wqhh.html
加载中，请稍候......
加载中…
(2015-11-01 09:00:43)