Primer - sfepy/sfepy GitHub Wiki
NOTE: The Primer updated for current SfePy? is available at http://docs.sfepy.org/doc-devel/primer.html - the text below uses some now obsolete syntax and is deprecated.
A beginner's tutorial highlighting the basics of SfePy.
Welcome to this updated primer on SfePy, a beginner's tutorial. To get you started, a step-by-step walk-through of the process to solve a simple mechanics problem is presented. The typical process to solve a problem using SfePy is followed: a model is meshed, a problem definition file is drafted, SfePy is run to solve the problem and finally the results of the analysis are visualised.
Figure 1. The ITS
Figure 2. Schematic of the ITS
A popular test to measure the tensile strength of concrete or asphalt materials is the indirect tensile strength (ITS) test pictured in Figure 1.
In this test a circular cylindrical specimen is loaded across its diameter to failure. The test is usually done by loading the specimen at a constant deformation rate of 50 mm/minute (say) and measuring the load response. When the tensile stress that develops in the specimen under loading exceeds its tensile strength then the specimen will fail. To model this problem using finite elements the indirect tensile test can be simplified to represent a diametrically point loaded disk as shown in Figure 2.
The tensile and compressive stresses that develop in the specimen as a result of the point loads P are a function of the diameter (D) and thickness (t) of the cylindrical specimen. At the centre of the specimen, the compressive stress is 3 times the tensile stress and the analytical formulation for these are, respectively:
[ sigma_t=frac{2P}{pi tD} ]
[ sigma_c=frac{6P}{pi tD} ]
These solutions may be approximated using finite element analysis. To solve this problem using SfePy the first step is meshing a suitable model.
Assuming plane strain conditions, the indirect tensile test may be modelled using a 2-D finite element mesh. Furthermore, the geometry of the model is symmetrical about the x- and y-axes passing through the centre of the circle. To take advantage of this symmetry only one quarter of the 2-D model will be meshed and boundary conditions will be established to indicate this symmetry. The meshing program Gmsh is used in this tutorial to very quickly mesh the model.
The ITS specimen has a diameter of 150 mm. Using Gmsh add three new Points (geometry elementary entities) at the following coordinates: (0.0 0.0), (75.0,0.0) and (0.0,75.0). Next add two straight lines connecting the points as shown in Figure 3. Next add a Circle arc connecting two of the points to form the quarter circle segment as shown in Figure 4. Still under Geometry add a Ruled surface (Figure 5). With the geometry of the model defined, add a mesh by clicking on the 2D button under the Mesh functions as shown in Figure 6.
Figure 3. Gmsh add straight lines
Figure 4. Gmsh add circle arc
Figure 5. Gmsh add ruled surface
Figure 6. Gmsh add mesh
That's it, we're done with the meshing. Save the mesh in a format that SfePy recognizes. For now use the medit .mesh format e.g. its2D.mesh.
Hint: Check the drop down in the Save As dialog for the different formats that Gmsh can save to.
If you open the its2D.mesh file using a text editor you'll notice that Gmsh saves the mesh in a 3-D format and includes some extra geometry items that we can delete. I've reformatted the mesh file to a 2-D format and deleted the Edges block. Note that when you do this the file cannot be reopened by Gmsh so it is always a good idea to also save your meshes in Gmsh's native format as well (Shift-Ctrl-S). Click here to download the reformatted mesh file that will be used in the tutorial.
Figure 7. Mesh using medit
You'll notice that the mesh contains 55 vertices (nodes) and 83 triangle elements. The mesh file provides the coordinates of the nodes and the element connectivity. It is important to note that node and element numbering in SfePy start at 0 and not 1 as is the case in Gmsh and other meshing programs.
To view .mesh files you can use a demo of medit available here. After loading your mesh file with medit you can see the node and element numbering by pressing P and F respectively. The numbering in medit starts at 1 as shown in Figure 7 below:
Thus the node at the center of the model in SfePy numbering is 0, and elements 76 and 77 are connected to this node. Node and element numbers can also be viewed in Gmsh - under the mesh option under the Visibility tab enable the node and surface labels. Note that the surface labels as numbered in Gmsh follow on from the line numbering. So to get the corresponding element number in SfePy you'll need to subtract the number of lines in the Gmsh file + 1. Confused yet? Luckily, SfePy provides some useful mesh functions to indicate which elements are connected to which nodes. Nodes and elements can also be identified by defining regions - but more on this later.
Another open source python option to view .mesh files is the appropriately named Python Mesh Viewer.
The next step in the process is developing the SfePy problem definition file.
The programming of the problem description file is well documented in the SfePy user's guide. The problem description file used in the tutorial follows:
# 12/09/2010
# Diametrically point loaded 2-D disk.
from sfepy.mechanics.matcoefs import youngpoisson_to_lame
filename = '/home/grassy/sfepy_wiki/msh/its2D.mesh'
#filename = '/home/grassy/sfepy_wiki/msh/big.mesh'
output_dir = '/home/grassy/sfepy_output' # set this to a valid directory you have write access to
young = 2000.0 # Young's modulus [MPa]
poisson = 0.4 # Poisson's ratio
filename_mesh = filename
options = {
'output_dir' : output_dir,
}
regions = {
'Omega' : ('all', {}),
'Left' : ('nodes in (x < 0.001)', {}),
'Bottom' : ('nodes in (y < 0.001)', {}),
'Top' : ('node 2', {}),
}
materials = {
'Asphalt' : ({
'lam' : youngpoisson_to_lame(young, poisson)[0],
'mu' : youngpoisson_to_lame(young, poisson)[1],
},),
}
fields = {
'displacement': ('real', 'vector', 'Omega', 1),
}
equations = {
'balance_of_forces' :
"""dw_lin_elastic_iso.2.Omega(Asphalt.lam, Asphalt.mu, v, u ) = 0""",
}
variables = {
'u' : ('unknown field', 'displacement', 0),
'v' : ('test field', 'displacement', 'u'),
}
ebcs = {
'XSym' : ('Bottom', {'u.1' : 0.0}),
'YSym' : ('Left', {'u.0' : 0.0}),
'Load' : ('Top', {'u.0' : 0.0, 'u.1' : -1.0}),
}
solvers = {
'ls' : ('ls.scipy_direct', {}),
'newton' : ('nls.newton', {
'i_max' : 1,
'eps_a' : 1e-6,
'problem' : 'nonlinear'
}),
}Download and open the file in your favourite python editor. Note that you will need to change the location of the output directory to somewhere on your drive. For the analysis we will assume that the material of the test specimen is linear elastic and isotropic. We define two material constants i.e. Young's modulus and Poisson's ratio. The material is assumed to be asphalt concrete having a Young's modulus of 2,000 MPa and a Poisson's ration of 0.4.
Note: Be consistent in your choice and use of units. In the tutorial we are using Newton (N), millimeters (mm) and megaPascal (MPa). The sfepy.mechanics.units module might help you in determining which derived units correspond to given basic units.
The following block of code defines regions on your mesh:
regions = {
'Omega' : ('all', {}),
'Left' : ('nodes in (x < 0.001)', {}),
'Bottom' : ('nodes in (y < 0.001)', {}),
'Top' : ('node 2', {}),
}Four regions are defined:
- Omega: all the elements in the mesh
- Left: the y-axis
- Bottom: the x-axis
- Top: the topmost node. This is where the load is applied.
Having defined the regions these can be used in other parts of your code. For example, in the definition of the boundary conditions:
ebcs = {
'XSym' : ('Bottom', {'u.1' : 0.0}),
'YSym' : ('Left', {'u.0' : 0.0}),
'Load' : ('Top', {'u.0' : 0.0, 'u.1' : -1.0}),
}Now the power of the regions entity becomes apparent. To ensure symmetry about the x-axis, the vertical or y-displacement of the nodes in the Bottom region are prevented or set to zero. Similarly, for symmetry about the y-axis, any horizontal or displacement in the x-direction of the nodes in the Left region or y-axis is prevented. Finally, to indicate the response of the load, the topmost node (number 2) is given a displacement of 1 mm downwards in the vertical or y-direction and displacement of this node in the x-direction is restricted.
We provided the material constants in terms of Young's modulus and Poisson's ratio, but the linear elastic isotropic equation used requires as input Lamé’s parameters. The youngpoisson_to_lame function is thus used for conversion. Note that to use this function it was necessary to import the function into the code, which was done up front:
from sfepy.mechanics.matcoefs import youngpoisson_to_lameHint: Check out the sfepy.mechanics.matcoefs module for other useful material related functions.
That's it - we are now ready to solve the problem.
One option to solve the problem is to run the SfePy simple.py script from the command shell:
$ <sfepy path>/simple.py its2D_1.pyNote: For the purpose of this tutorial it is assumed that the problem definition file (its2D_1.py) is in the same directory as the simple.py script. If you have the its2D_1.py file in another directory then make sure you include the path to this file as well.
SfePy solves the problem and outputs the solution to the output path (output_dir) provided in the script. The output file will be in the vtk format by default if this is not explicitly specified and the name of the output file will be the same as that used for the mesh file except with the vtk extension i.e. its2D.vtk.
The vtk format is an ascii format. Open the file using a text editor. You'll notice that the output file includes separate sections:
- POINTS (these are the model nodes)
- CELLS (the model element connectivity)
- VECTORS (the node displacements in the x-, y- and z- directions.
Notice that the y-displacement of node 2 is -1.0 as we set it as a boundary condition.
SfePy includes a script (postproc.py) to quickly view the solution. To run this script you need to have Mayavi installed. From the command line issue the following (with the correct paths):
$ <sfepy path>/postproc.py its2D.vtkThe postproc.py script generates the image shown in Figure 8, which shows the average displacements in the model. Cool, but we are more interested in the stresses. To get these we need to modify the problem description file and do some post-processing.
Figure 8. Mayavi visualisation of solution
SfePy provides functions to calculate stresses and strains. We'll include a function to calculate these and update the problem material definition and options to call this function as a post_process_hook. Save this file as its2D_2.py.
from its2D_1 import *
from sfepy.mechanics.matcoefs import stiffness_tensor_youngpoisson
def stress_strain(out, pb, state, extend=False):
"""
Calculate and output strain and stress for given displacements.
"""
from sfepy.base.base import Struct
ev = pb.evaluate
strain = ev('de_cauchy_strain.2.Omega(u)')
stress = ev('de_cauchy_stress.2.Omega(Asphalt.D, u)')
out['cauchy_strain'] = Struct(name='output_data', mode='cell',
data=strain, dofs=None)
out['cauchy_stress'] = Struct(name='output_data', mode='cell',
data=stress, dofs=None)
return out
asphalt = materials['Asphalt'][0]
asphalt.update({'D' : stiffness_tensor_youngpoisson(2, young, poisson)})
options.update({'post_process_hook' : 'stress_strain',})The updated file imports all of the previous definitions in its2D_1.py. The stress function (de_cauchy_stress) requires as input the stiffness tensor - thus it was necessary to update the materials accordingly. The problem options were also updated to call the stress_strain function as a post_process_hook.
Run SfePy to solve the updated problem and view the solution (assuring the correct paths):
$ <sfepy path>/simple.py its2D_2.py
$ <sfepy path>/postproc.py its2D.vtkIn addition to the node displacements, the vtk output shown in Figure 9 now also includes the stresses and strains averaged in the elements:
Figure 9. Mayavi visualisation of solution with stresses and strains
Remember the objective was to determine the stresses at the centre of the specimen under a load P. The solution as currently derived is expressed in terms of a global displacement vector (u). The global (residual) force vector (f) is a function of the global displacement vector and the global stiffness matrix (K) as: f = Ku. Let's determine the force vector interactively.
In addition to solving problems using the simple.py script you can also run SfePy interactively. This requires that IPython be installed. To run SfePy interactively, use isfepy:
$ <sfepy path>/isfepyOnce isfepy loads up, issue the following command:
In [1]: pb, state = pde_solve('its2D_2.py')The problem is solved and the problem definition and solution are provided in the pb and state variables, respectively. The solution, or in this case, the global displacement vector (u), contains the x- and y-displacements at the nodes in the 2D model.
In [2]: u=state()
In [3]: u
Out[3]:
array([ 0. , 0. , 0.22608933, ..., -0.12051821,
0.05335311, -0.0677574 ])
In [4]: u.shape
Out[4]: (110,)
In [5]: u.shape=(55,2)
In [6]: u
Out[6]:
array([[ 0. , 0. ],
[ 0.22608933, 0. ],
[ 0. , -1. ],
...,
[ 0.05272529, -0.13954334],
[ 0.16780587, -0.12051821],
[ 0.05335311, -0.0677574 ]])Note: We have used the fact, that the state vector contains only one variable (u). In general, the following can be used:
In [7]: u = state.get_parts()['u']
In [8]: u
Out[8]:
array([ 0. , 0. , 0.22608933, ..., -0.12051821,
0.05335311, -0.0677574 ])In [9]: K=pb.mtx_a
In [10]: K
Out[10]:
<93x93 sparse matrix of type '<type 'numpy.float64'>'
with 1063 stored elements in Compressed Sparse Row format>
In [11]: print K
(0, 0) 2443.95959851
(0, 6) -2110.99917491
(0, 13) -332.960423597
(0, 14) 1428.57142857
(1, 1) 4048.78343529
(1, 2) -1354.87004384
(1, 51) -609.367453538
(1, 52) -1869.0018791
(1, 91) -357.41672785
(1, 92) 1510.24654193
(2, 1) -1354.87004384
(2, 2) 4121.03202907
(2, 3) -1696.54911732
(2, 47) 76.2400806561
(2, 48) -1669.59247304
(2, 51) -1145.85294856
(2, 52) 2062.13955556
(3, 2) -1696.54911732
(3, 3) 4410.17902905
(3, 4) -1872.87344838
(3, 41) -130.515009576
(3, 42) -1737.33263802
(3, 47) -710.241453776
(3, 48) 1880.20135513
(4, 3) -1872.87344838
: :
(90, 80) -1610.0550578
(90, 85) -199.343680224
(90, 86) -2330.41406097
(90, 89) -575.80373408
(90, 90) 7853.23899229
(91, 1) -357.41672785
(91, 7) 1735.59411191
(91, 49) -464.976034459
(91, 50) -1761.31189004
(91, 51) -3300.45367361
(91, 52) 1574.59387937
(91, 87) -250.325600254
(91, 88) 1334.11823335
(91, 91) 9219.18643706
(91, 92) -2607.52659081
(92, 1) 1510.24654193
(92, 7) -657.361661955
(92, 49) -1761.31189004
(92, 50) 54.1134516246
(92, 51) 1574.59387937
(92, 52) -315.793227627
(92, 87) 1334.11823335
(92, 88) -4348.13351285
(92, 91) -2607.52659081
(92, 92) 9821.16012014
In [12]: K.shape
Out[12]: (93, 93)One would expect the shape of the global stiffness matrix (K) to be (110,110) i.e. to have the same number of rows and columns as u. This matrix has been reduced by the fixed degrees of freedom imposed by the boundary conditions set at the nodes on symmetry axes. To restore the matrix, temporarily remove the imposed boundary conditions:
In [13]: pb.remove_bcs()
sfepy: updating variables...
sfepy: ...done
sfepy: updating materials...
sfepy: Asphalt
sfepy: ...done in 0.00 sNow we can calculate the force vector (f):
In [14]: f=pb.evaluator.eval_residual(u)
In [15]: f.shape
Out[15]: (110,)
In [16]: f
Out[16]:
array([ -2.86489070e+01, 8.63500981e+01, -1.33101431e-13, ...,
1.35003120e-13, -5.32907052e-14, 4.26325641e-14])Remember to restore the original boundary conditions previously removed in step [13]:
In [17]: pb.time_update()To view the residual force vector, we can save it to a vtk file. This requires creating a state and set its DOF vector to f as follows:
In [18]: state = pb.create_state()
In [19]: state.set_full(f)
In [20]: out = state.create_output_dict()
In [21]: pb.save_state('file.vtk', out=out)Running the postproc.py script on file.vtk displays the average nodal forces as shown in Figure 10.
Figure 10. Average nodal forces
The forces in the x- and y-directions at node 2 are:
In [22]: f.shape = (55,2)
In [23]: f[2]
Out[23]: array([ 375.26022639, -604.89425239])Great, we have the vertical load or force apparent at node 2 i.e. 604.894 Newton. Since we modelled the problem using symmetry, the actual load applied to achieve the nodal displacement of 1 mm is 2 x 604.894 = 1209.7885 N. Applying the indirect tensile strength stress equation, the horizontal tensile stress at the centre of the specimen per unit thickness is 5.1345 MPa/mm and the vertical compressive stress per unit thickness is 15.4035 MPa/mm. The per unit thickness results are in terms of the plane strain conditions assumed for the 2D model.
Previously we had calculated the stresses in the model but these were averaged from those calculated at Gauss quadrature points within the elements. It is possible to provide custom integrals to allow the calculation of stresses with the Gauss quadrature points at the element nodes. This will provide us a more accurate estimate of the stress at the centre of the specimen located at node 0. The code below outlines one way to achieve this.
from its2D_1 import *
from sfepy.mechanics.matcoefs import stiffness_tensor_youngpoisson
from sfepy.fem.geometry_element import geometry_data
from sfepy.fem import Field,FieldVariable
import numpy as nm
gdata = geometry_data['2_3']
nc = len(gdata.coors)
def nodal_stress(out, pb, state, extend=False):
'''
Calculate stresses at nodal points.
'''
# Calc point load
u = state.vec
pb.remove_bcs()
f = pb.evaluator.eval_residual(u)
f.shape = (pb.domain.mesh.n_nod,2)
P = 2. * f[2][1]
# Calc nodal stress
pb.time_update()
ev = pb.evaluate
stress = ev('dq_cauchy_stress.ivn.Omega(Asphalt.D,u)')
sfield = Field('stress', nm.float64, (3,), pb.domain.regions["Omega"])
svar = FieldVariable('sigma', 'parameter', sfield, 3,
primary_var_name='(set-to-None)')
svar.data_from_qp(stress, pb.integrals['ivn'])
print '\n=================================================================='
print 'Load to give 1 mm displacement = %s Newton ' % round(-P,3)
print '\nAnalytical solution'
print '==================='
print 'Horizontal tensile stress = %s MPa/mm' % round(-2.*P/(nm.pi*150.),3)
print 'Vertical compressive stress = %s MPa/mm' % round(-6.*P/(nm.pi*150.),3)
print '\nFEM solution'
print '============'
print 'Horizontal tensile stress = %s MPa/mm' % round(svar()[0][0],3)
print 'Vertical compressive stress = %s MPa/mm' % -round(svar()[0][1],3)
print '=================================================================='
return out
asphalt = materials['Asphalt'][0]
asphalt.update({'D' : stiffness_tensor_youngpoisson(2, young, poisson)})
options.update({'post_process_hook' : 'nodal_stress',})
integrals = {
'ivn' : ('v', 'custom', gdata.coors, [gdata.volume / nc] * nc),
}The output:
==================================================================
Load to give 1 mm displacement = 1209.789 Newton
Analytical solution
===================
Horizontal tensile stress = 5.135 MPa/mm
Vertical compressive stress = 15.404 MPa/mm
FEM solution
============
Horizontal tensile stress = 4.58 MPa/mm
Vertical compressive stress = 15.646 MPa/mm
==================================================================Not bad for such a coarse mesh! Re-running the problem using a finer mesh provides a more accurate solution:
==================================================================
Load to give 1 mm displacement = 740.779 Newton
Analytical solution
===================
Horizontal tensile stress = 3.144 MPa/mm
Vertical compressive stress = 9.432 MPa/mm
FEM solution
============
Horizontal tensile stress = 3.148 MPa/mm
Vertical compressive stress = 9.419 MPa/mm
==================================================================To wrap this tutorial up let's explore SfePy's probing functions.
As a bonus for sticking to the end of this tutorial see the following problem definition file that provides SfePy functions to quickly and neatly probe the solution.
from its2D_1 import *
from sfepy.mechanics.matcoefs import stiffness_tensor_youngpoisson
def stress_strain(out, pb, state, extend=False):
"""
Calculate and output strain and stress for given displacements.
"""
from sfepy.base.base import Struct
ev = pb.evaluate
strain = ev('de_cauchy_strain.2.Omega(u)')
stress = ev('de_cauchy_stress.2.Omega(Asphalt.D, u)')
out['cauchy_strain'] = Struct(name='output_data', mode='cell',
data=strain, dofs=None)
out['cauchy_stress'] = Struct(name='output_data', mode='cell',
data=stress, dofs=None)
return out
def gen_lines(problem):
from sfepy.fem.probes import LineProbe
mesh = problem.domain.mesh
ps0 = [[0.0, 0.0], [ 0.0, 0.0]]
ps1 = [[75.0, 0.0], [ 0.0, 75.0]]
# Use adaptive probe with 10 inital points.
n_point = -10
labels = ['%s -> %s' % (p0, p1) for p0, p1 in zip(ps0, ps1)]
probes = []
for ip in xrange(len(ps0)):
p0, p1 = ps0[ip], ps1[ip]
probes.append(LineProbe(p0, p1, n_point, mesh))
return probes, labels
def probe_hook(data, probe, label, problem):
import matplotlib.pyplot as plt
import matplotlib.font_manager as fm
def get_it(name, var_name):
var = problem.create_variables([var_name])[var_name]
var.data_from_any(data[name].data)
pars, vals = probe(var)
vals = vals.squeeze()
return pars, vals
results = {}
results['u'] = get_it('u', 'u')
results['cauchy_strain'] = get_it('cauchy_strain', 's')
results['cauchy_stress'] = get_it('cauchy_stress', 's')
fig = plt.figure()
plt.clf()
fig.subplots_adjust(hspace=0.4)
plt.subplot(311)
pars, vals = results['u']
for ic in range(vals.shape[1]):
plt.plot(pars, vals[:,ic], label=r'$u_{%d}$' % (ic + 1),
lw=1, ls='-', marker='+', ms=3)
plt.ylabel('displacements')
plt.xlabel('probe %s' % label, fontsize=8)
plt.legend(loc='best', prop=fm.FontProperties(size=10))
sym_indices = ['11', '22', '12']
plt.subplot(312)
pars, vals = results['cauchy_strain']
for ic in range(vals.shape[1]):
plt.plot(pars, vals[:,ic], label=r'$e_{%s}$' % sym_indices[ic],
lw=1, ls='-', marker='+', ms=3)
plt.ylabel('Cauchy strain')
plt.xlabel('probe %s' % label, fontsize=8)
plt.legend(loc='best', prop=fm.FontProperties(size=8))
plt.subplot(313)
pars, vals = results['cauchy_stress']
for ic in range(vals.shape[1]):
plt.plot(pars, vals[:,ic], label=r'$\sigma_{%s}$' % sym_indices[ic],
lw=1, ls='-', marker='+', ms=3)
plt.ylabel('Cauchy stress')
plt.xlabel('probe %s' % label, fontsize=8)
plt.legend(loc='best', prop=fm.FontProperties(size=8))
return plt.gcf(), results
materials['Asphalt'][0].update({'D' : stiffness_tensor_youngpoisson(2, young, poisson)})
# Update fields and variables to be able to use probes for tensors.
fields.update({
'sym_tensor': ('real', 3, 'Omega', 0),
})
variables.update({
's' : ('parameter field', 'sym_tensor', None),
})
options.update({
'output_format' : 'h5', # VTK reader cannot read cell data yet for probing
'post_process_hook' : 'stress_strain',
'gen_probes' : 'gen_lines',
'probe_hook' : 'probe_hook',
})Probing applies interpolation to output the solution along specified paths. For the tutorial, line probing is done along the x- and y-axes of the model.
Notice that the output_format has been defined as h5. To apply probing first solve the problem as usual:
$ <sfepy path>/simple.py its2D_4.pyThis will write the solution to the output directory indicated. Then run the SfePy probe.py script on the solution:
$ <sfepy path>/probe.py its2D_4.py <sfepy output path>/its2D.h5The results of the probing will be written to text files and the following figures will be generated. These figures show the displacements, normal stresses and strains as well as shear stresses and strains along the probe paths. Note that you need matplotlib installed to run this script.
Figure 11. Response along x-axis
Figure 12. Response along y-axis
The end.