Figure 4.—Area plot

View all elements. .
[eplot]

If the element sizes were not properly determined, then
ANSYS will warm that poorly shaped elements were
created. UTAH2PC will not run an analysis if the model
contains poorly shaped elements. This problem may
occur if the element size changes too rapidly near the area
of mining. To correct this problem, the operator must
first delete the elements generated in the areas outside the
mining regions. Second, the operator must force ANSYS
to slow the rate at which the elements size increases as the
elements radiate away from the area of mining. Finally,
the areas outside the mining regions must be re-meshed.
[aclear,p] Deletes elements from selected areas.
[mopt,trans,1] Slows rate of element growth.

[amesh,p] Re-meshes areas.

Step 3: Output Data

3-1.

3-2.

3-4.

Copy a list of the elements to a file named ELIST.DAT.
[ewrite,elist,dat,,0}

Copy a list of nodes to a file named NLIST.DAT.
[nwrite,nlist,dat,,0]

Select the nodes to be constrained only in the x-direction.
In this example, these are the nodes lying along line x =
3350 (the “bottom” of the model). Do not include the two
nodes at the comers of the model. These nodes are
constrained in the x- and y-directions. Copy a list of these
nodes to a file named UX.DAT.

{nsel,s,p]

{nwrite,ux,dat,,0}

Select the nodes to be constrained only in the y-direction.

3-5,

3-6.

In this example, these are the nodes lying along lines y =
O and y = 2800. Again, do not include the two nodes at
the bottom corners of the model. Copy a list of these
nodes to a file named UY.DAT.

[nsel,s,p]

[nwrite,uy,dat,,0]

Select the nodes that are to be constrained only in the x-
and y-directions. In this example, these are the two nodes
at (3350,0) and (3350,2800). Copy a list of these nodes to
a file named UXUY.DAT.

[nsel,s,p]

[nwriteuxuy,dat,,0}

Select the elements to be cut during the first excavation,
Inthe example, the cut elements are contained within two
rectangles, the first with coordinates (1850,1260).
(1900,1370), and the second with coordinates
(1950,1775), (1870,1520) (figure 1). There are several
steps involved in selecting these cut elements.

. Select nodes within the first set of coordinates. First,

select all nodes between x = 1850 and x = 1900. Then,
from these nodes, reselect the nodes lying between y =
1260 and y = 1370.

[nsel,s,loc,x, 1850, 1900]

[nsel,r,loc.y,1260,1370}

. Select all elements in contact with these nodes.

{esins,0]

". Group these elements into a component named “ekill 1a.”

{cm,ckill1a,elem)

Select the nodes within the second set of coordinates.
First, select the nodes between x = 1950 and x = 1870.


ANSYS5.3
SEP271996
16:48:52
PLOT NO.22
VECTOR

MIN=0,
MAX=.33229

Figure 6.—Displacements around mine openings

Enter the converted stress and displacement files from
load step | into the element tables.
(/input filename, ext]

View analysis results, The following commands will
cause ANSYS to plot the results of the analysis.
[pletab,sxx] Generate a plot of vertical stresses.
[pletab.syy}] Generate a plot of horizontal stresses.

77.

[pletab,txy] Generate a plot of shear stresses.
[pletab,fac] Generate a plot of safety factors.
[plvect,u,,,,vect] Generate a plot of displacements,

Repeat steps 7-5 and 7-6 to review the results from load
steps 2 and 3. Figures 5 and 6 illustrate the resultant
safety factors and displacements around the mine opening,


2-8.

2-9.

. Define element size. There are several

Create areas using the lines created in the
previous steps. This is done by selecting
the lines that bound a region of the
model. In this example, formation 1 was
divided into two areas: area 1, where
mining is to occur, and area 2, which is
located in the same formation as area 1,
but which will not be mined. Formation
2. was defined as area 3, and formation 3
was defined as area 4 (figure 3).

{al.p]

Mesh the model.

factors to consider when setting the ele-
ment size. The smaller the element size,
the greater the number of elements gener-
ated for a given area. The more elements,
the more accurate the results, but the
greater the demand on computer 1e-
sources. Another consideration when set-
ting element size is that stresses will con-
centrate in the region of mine openings and diminish
away from mine openings. Therefore, the elements near
mine openings should be of a relatively small size (for
greater accuracy), while elements away from mine open-
ings can be kept large (to reduce demand on computer re-
sources). It is up to operator experience to determine ex-
actly how to size elements throughout the model. Note
that an analysis can be run with a relatively course mesh
(larger element size) and then rerun with a finer mesh
(smaller element size). If there is no appreciable change
in the results, then there is likely no need to further refine
the element size. However, if the results do change
appreciably, then the model should be recreated with
smaller elements and the analysis repeated, In the ex-

ample, mining will take place in area 1. Therefore, this is”

the area in which stresses will concentrate, and smaller
elements will be required. In addition, smaller elements
will be used to better define the mine openings. In the
example, elements were given an edge length of S feet.
[esize,5]

. Assign proper material numbers to the areas where a

finite-element mesh is to be created. At this point, only
area | is to be meshed, and area 1 is in formation 1, so
each element generated should be assigned material num-
ber I, The material properties associated with material
number 1, as well as all other materials used in the model,
will be listed in a file that will be used later in the analysis,
(see step 4-3).

[mat,1]

. Select and create a mesh for area 1. During this phase,

ANSYS will create a finite- element mesh for the area
selected.
[amesh.p]

Figure 3.—Line plot

D. Create a finite-element mesh for each of the outer areas.
‘These areas do not require the small element size that was
used for area 1. Therefore, a different meshing strategy is
used. In addition to specifying the element size, as was
done in step 2-9-A, the user can also force ANSYS to
create a mesh with a set number of elements along each
line segment. This technique allows the user to vary the
size of elements throughout the model, There is no rule
to specify how many elements should be placed along
each line segment. The operator must use judgment and
experience to make this determination, Again, because
stresses will concentrate around mine openings, smaller
elements should be used around the area of mining, and
larger elements may be used away from the area of
mining. In the example, ANSYS was told to place 20 ele-
ments along the outsides of the model, ‘Ten-foot elements
were placed along the lines closer to area I (figure 4).
{lesize,p]

E. Specify the number of element faces to be placed along
each line division as 1.
{esize,1)

F. Complete the mesh of areas in formation I by generating
a mesh of area 2.
[amesh,p]

G. Set the material number to 2 (for formation 2) and
generate a mesh of area 3.
(mat,2]
{amesh,p]

H. Set the material number to 3 (for formation 3) and
generate a mesh of area 4.
{mat,3]
[amesh,p]


3-7.

3-8.

‘Then, from these nodes, reselect the nodes lying between
y = 1475 and y = 1520.

{nsel,s,loc,x,1950,1870}

[nsel,r,loc,y,1475,1520]

- Select all elements in contact with these nodes.

[esin,s,0]

. Group these elements into a component named “ekill1b.”

{cm ekill1b,elem]

. Group the two components into an assembly called

“ekilll.”
{emgrp,ekilll ekill1a,ekill 1b]

|. Select all nodes and elements in the model.

[allsel]

Select the elements stored in the assembly “ekilll.”
These are the elements to be excavated in the second step
of the analysis.
{emsel,s,ekill1]

Copy a list of these elements to a file named
EKILLL.DAT.
[ewrite,ekill |,dat,.0]

Repeat this process for the elements to be cut for the third
step of the analysis, saving the clement listing as
EKILL2.DAT.

Save ANSYS database and exit the program.
[save]

[finish)

[exit]

Step 4: Prepare Data for Analysis

Run ANS2UT2 from the directory that contains the files

created in step 3. This program will convert the ANSYS output
files into UTAH2PC input files. The program also creates the
master runstream file for UTAH2PC. Consult the UTAH2PC
documentation for more information on UTAH2PC files.
ANS2UT2 will request the following information:

4-1,

42.

Job title. This is an arbitrary title for the UTAH2 run-
stream file and can be up to 80 characters long.

Master runstream file name. This is the user-supplied
name of the master runstream file to be created by
ANS2UT2 and provides the input for the UTAH2PC
analysis. Three master runstream files were created for
the example, one for each of the three load steps. The
first (LI.DAT) contains all the data necessary for
UTAH2PC to calculate the state of stress of the model
prior to any excavation. The second (L2.DAT) contains
all the data necessary for UTAH2PC to calculate the state
of stress of the model after the first excavation. The third
(L3.DAT) contains all the data necessary for UTAH2PC.

43.

44,

45.

4-6,

4-7.

4-9,

to calculate the state of stress of the model after the
second excavation.

Material properties file name. This file is provided by the
user and contains material properties for each of the
materials used in the analysis.

Number of different material types. The user is to define
the number of different material types used in the analy-
sis. Note that each of the different material types should
be defined in the material properties file. Three material
types were used in the example analysis, one for each of
the three geologic formations.

ANSYS element connection filename. This is the ele-
ment listing generated by ANSYS (sce step 3-2 above).
The default is ELIST.DAT. ANS2UT2 will convert this
file into a UTAH2PC formatted file named ELIST.UT2.

ANSYS node location filename. This is the node listing
generated by ANSYS (see step 3-1 above). The default is
NLIST.DAT. ANS2UT2 will convert this file into a
UTAH2PC formatted file named NLIST.UT2

ANSYS cut or fill element listing. This is the list of
elements to be cut or filled (see step 3-6-A above). In this
example, the first load step has no cut or fill element
listing. The elements cut in the second load step are listed
in the file EKILLI.DAT. The elements cut in the third
oad step are listed in the file EKILL2.DAT. ANS2UT2
will convert these files into UTAH2PC formatted files.
The name of the UTAH2PC format file is supplied by the
user. ANS2UT?2 will also prompt the user for the name of
a file that UTAH2PC will create and store the number of
each node that is attached to the cut elements.

Gravity loading. Select this option if the first load step is
used to calculate loading by gravity. If gravity loading is
selected, then the material properties file must include the
specific gravity for each of the materials listed.

Initial stress. As an alternative to gravity loading, initial
stress can be provided either from a file (such as the
results from a previous load step) or calculated from
known stress gradients. If the stress gradient is known,
then ANS2UT2 will prompt the user for the following
information.

. Name of the initial stress file to be created.
. Depth to top of model.

. Slope and constant defining stress gradients. Stress is

defined by the formula~

y = mx+b,
where y = stress gradient,
m = slope of gradient,


SUMMARY AND CONCLUSIONS

The technique explained above is one method that will allow
mine planners to generate a two-dimensional, finite-element
model of an underground section of a mine in a relatively
straightforward manner. This model can be analyzed, and
resultant stresses, displacements, and safety factors around mine
openings can be viewed. This information allows a mine planner
to develop mine plans that reduce the potential for rock failure
around mine openings,

Cross sections consisting of several formations of anisotropic
materials can be modeled, but many variables can affect the
accuracy of the model, including the number and location of
joints and fractures, the presence of water, the accuracy of
measurements of material properties and in situ stress, and the
actual geometry of the various formations and openings. It is
therefore critical that a mine planner validate the results of the
analysis by comparing the predicted response of the mine with the

actual response of the mine. The elastic material properties may
be validated by comparing predicted displacements with actual
displacements. Strength properties may be validated by compar-
ing predicted yield zones with observed yield zones (2). These
comparisons will allow a planner to determine if the material
properties used in the model should be modified in order to create
a more accurate model.

REFERENCES

1. Pariseau, W. G., J. C. Johnson, M.M. McDonald, and M. E.
Poad. Rock Mechanics Study of Shaft Stability and Pillar
Mining, Homestake Mine, Lead, SD. (In Three Parts). U.S. Bur
Mines RI 9531, 1995, 20 pp.

2. Pariseau, W.G. Research Study on Pillar Design for Vertical
Crater Retreat (VCR) Mining (contract JO215043, Univ. UT)
USS. Bur. Mines OFR 44-86, 1986, 232 pp.; NTIS PB 86-210960


Simplified Pre- and Post-processing Technique for Performing
Finite-element Analyses of Deep Underground Mines

Mare T. Filigenzi, Mechanical Engineer
National Institute for Occupational Safety and Health
Spokane Research Center
Spokane, WA

ABSTRACT

Two of the major ground control safety issues confronting
underground mine operations today are shaft pillar stability and
the failure of rock around active mine openings. Failure of a
mine shaft can lead to the entrapment of workers. Failure of rock
around active underground mine openings can lead to roof falls,
which in turn can result in worker injuries and fatalities.

Finite-element analysis has proven to be a reliable method for
predicting stresses and displacements around underground mine
openings. However, this is a complex and time-consuming
technique and is not used as often as it could be in mine planning.
The purpose of this paper is to demonstrate one technique
developed at the Spokane Research Center that allows the user to
create a finite-element model of a two-dimensional section of an
underground mine in a relatively straightforward manner. This
model is then used to calculate stresses, displacements, and safety
factors around mine openings. With this information, mine
planners can evaluate the stability of mine openings as well as the
stability of pillars and mine shafts. This analysis will help de-
velop mining sequences and layouts that minimize stresses in that
section of the mine. This, in turn, should minimize the occur-
rence of shaft failure, roof falls, and other hazards associated with
underground mining.

INTRODUCTION

The prediction of stresses and displacements around
underground mine openings has proven to be a difficult challenge.
However, the rewards of such predictions can be substantial. If
a mine planner knows that a particular sequence or configuration
of excavations will lead to unacceptably large displacements in
the rock mass, and that these displacements may affect shaft
stability, the planner can modify that sequence or configuration in
order to maintain the integrity of the shaft. Such modifications
can also minimize stresses in and around mine openings, which,
in tur, can reduce the occurrence of roof falls and other hazards
associated with the failure of rock.

Finite-element analysis has proven to be an effective method
for predicting stresses in rock mass caused by underground
mining (1). These earlier studies relied upon the UTAH2PC
finite-element program for the analysis of underground mining
near a mine shaft. The UTAH2PC code can analyze a two-
dimensional section of an underground mine in which there are
several formations having anisotropic material properties. ‘The
program can also analyze multiple cut-and-fill operations.

However, UTAH2PC does not have an automatic finite:
element mesh generator. Each node of the finite-element mesh
must be manually located, and each element must be explicit!y
defined. This leads to a tremendous amount of labor and book-
keeping for an analyst using this program, as well as a reduction
in the flexibility of the analysis. If the analyst wishes to modits
the geometry of the mine openings or geology, the nodes and
clements of the finite-element mesh must be manually relocated
and redefined, or the mesh must be regenerated.

Many finite-element analysis programs are available today
that include automatic mesh generators and intuitive, user
friendly interfaces (ANSYS, COSMOS/M, PATRAN. cic.).
These programs will automatically create a finite-element mesh
with all the necessary nodes and elements. However, many of
these programs are intended for mechanical engineering design
and are not suitable for models possessing the anisotropic
material properties or brittle-failure criteria associated with rock

‘As a solution to these problems, researchers at the Spokane
Research Center, Spokane, WA, have developed a finite-element
pre- and postprocessing procedure that takes advantage of the
automatic mesh-generating capabilities of ANSYS, a commercial
ly available, finite-element analysis program, while at the sume
time utilizing the analytical capabilities of the UTAH2PC finite
element code. With this procedure, a user can model two-dimen
sional sections of underground hard-rock mines, even those witl:
multiple formations and anisotropic materials. These models cn
be used to plan mining sequences and layouts that will avoid the
creation of regions of unacceptably high displacements or stress
concentrations.


4-10.

411.

4-12.

4-13.

414,

4-16.

4-17,

4-18.

4-19,

4-20.

x
and b

= depth in feet,

= constant.

In the example, the initial stress for load step 1 was
defined by the following formulae.

o, = 0.1X +1000

and a, = 0.01X + 1000.
These formulas were provided to ANS2UT2, which
applied these values to all of the elements in the model
and saved the results in the file STRESS.UT2.

Boundary node listing. The boundary node listing is gen-

erated by ANSYS (see steps 3-3, 3-4, and 3-5 above).

The default is UX.DAT, UY.DAT, UXUY.DAT.
ANS2UT2 will convert these three files into a single
UTAH2PC formatted file named BOUND.UT2.

Screen output filename, This is a file that will contain the
UTAH2PC runstream output. This file name does not
require an extension. The first four characters of this file
name will be used as the first four characters for
UTAH2PC stress and displacement output files.

Number of load steps. This is the number of increments
to reach final load. Usually 10 increments are sufficient.

Maximum number of iterations per load. This is the
number of iterations allowed per load step. A value of 80
was used in the example analyses.

Iteration interval. This is the number of iterations be-
tween printing of residuals and should be less than the
maximum number of iterations. A value of 20 was used
in the example analysis.

Type of analysis. Analyses include plane stress, plane
strain, axially symmetric, elastic, or elastic-plastic. The
type of analysis used in the example problem was an
elastic-plastic analysis with a quadratic yield condition.

Caving. An elastic-brittle analysis can be pursued by
selecting the caving analysis. This program option is
somewhat experimental and should be used with care.

Batch runstream. Some data files can be skipped during
a sequential batch run consisting of several back-to-back
program passes. Select this option if this action is
desired.

UTAH2PC to write output files. Select this option if
UTAH2PC is to save output files (recommended).

Input units. If metric units are used in the model, then
“yes” should be selected. Otherwise, the default is “no.”

Error value. ‘The program will exit the equation solver

when the residuals are reduced to a value less than the
error value. A value of | is recommended.

4-21. Orf value. An over-relaxation factor is used to accelerate
the equation-solving procedure. Orf should be between I
and 2 (1.86 recommended)

4-22. Xfac and Yfac. These are the scale factors used to con-
vert the measurement units in the mine plans into inches
or millimeters, as appropriate.

4-23, Bfac and Sfac. These are scale factors used to change
elastic properties (efac) or strength properties (sfc)

Load step 1 consists of applying the initial stress field to the
model. During load step 2, the resultant stresses from load step
1 are applied to the model, and the first excavation takes place.
During load step 3, the resultant stresses from load step 2 are
applied to the model, and the second excavation takes place.

Step S: Analyze Data

Run UTAH2PC from the directory containing the files created
in step 4. UTAH2PC will prompt the user for the name of a
runstream file (as created in step 4-2) and will then perform the
analysis. Output includes cartesian stresses and element safety
factors, element principal stresses and strains, and node force and
displacements. For the example analysis, UTAH2PC was
executed three times, once for each of the three load steps.

Step 6: Prepare Results of Analysis

Run CONVERT from the directory that contains the files
created in step 5. This program converts Cartesian stresses, ele-
ment safety factors, and node displacement files generated by
UTAH2PC into a format ANSYS can read. CONVERT will
prompt the user for the name of the UTAH2PC output file to be
converted and the name of the ANSYS input file to be created.

Step 7: Review Results of Analysis

7-1, Run ANSYS from the directory that contains the ANS YS
files created in step 6.

7-2. Resume the original modef database.
[resume,filename,db} filename,db is the file name and
extension of the ANSYS database. The default is file.db.

7-3, Enter the ANSYS postprocessor.
[/post 1]

7-4. Create element tables that are to contain the stresses and
safety factors generated by UTAH2PC in step 5 and con-
verted into ANSYS format in step 6.
[etable,Sxx]
[etable,Syy]
{etable,Szz]
[etable,Txy]
[etable,Fac]


REQUIREMENTS FOR SOFTWARE

1. Computer-aided design (CAD) software capable of saving
drawing files in IGES format. Third-party programs are available
that will convert other drawing formats (such as DXF) into an
ANSYS format.

2. ANSYS version 5.0 or later (pre- and postprocessor only).
This program is used to create the finite-element mesh and view
the results of the analysis.

3. ANS2UT2.EXE. This program is used to convert ANSYS
‘output files into UTAH2PC input files and create a UTAH2PC
runstream file.

4, UTAH2PC.EXE.' This program is used to perform the finite-
element analysis.

5. CONVERT.EXE? This program is used to convert
UTAH2PC results files into ANSYS input files.

REQUIREMENTS FOR ANALYSIS

1. Vertical section map of the area of the mine to be analyzed.
This map should illustrate the major geologic features of that
section.

2. The location of all existing and proposed mine openings.

3. Material property data along each axis of anisotropy for each
of the important geologic features of the section map. These data
should include-

Elastic modulus.

Shear modulus.

Poisson’s ratio.

Compressive strength.

Tensile strength.

Shear strength.

Angle of inclination of the axis of anisotropy with the
x-axis,

Specific gravity, if gravity loading is to be applied to the
model.

BH OmmDNe>

4, In situ stress. This stress can be caused solely by gravita-
tional loading or it can be input as a formula where vertical,
horizontal, and shear stresses are functions of depth.

‘UTAH2PC was written by William Pariseau of the University
of Utah under contract with the U.S. Bureau of Mines and is available
at no cost from the Spokane Research Center, NIOSH, Spokane, WA
99207.

*ANS2UT.EXE and CONVERT.EXE were both written by
researchers at the Spokane Research Center of the U.S. Bureau of Mines
and are available at no cost from the Spokane Research Center, NIOSH,
Spokane, WA 99207.

5, Measurements of displacement of the rock mass as mining
progresses, This information is required to calibrate the finite-
element model.

SYMBOLS

6, = Vertical stress.

0, = Horizontal stress.

X = Depth in feet.
EXAMPLE PROBLEM

An example analysis has been provided to illustrate the
technique. Figure 1 shows the geometry of the geology and
proposed mine openings used in this example. The mine consists
of three major formations. In situ stress is given by the following
formula. :

o, 0.1X + 1000

and 0, = 0.01X +1000.

The model used to illustrate this technique contained 11,955
nodes and 11,952 elements and took approximately 6 hours to
create and analyze on a 66 MHZ Pentium PC with 64 megabytes
of RAM. Text appearing inside square brackets [ ] is a command
issued to ANSYS.

PROCEDURE

Step 1: Create Data for Analysis

1-1, Begin by digitizing mine drawings using a CAD program.
Either horizontal or vertical sections may be digitized and
modeled. If vertical sections are to be analyzed, then the
drawing should be digitized so that mine depth increases
along the positive x-axis, as shown in figure 1. This is
necessary to accommodate UTAH2PC’s coordinate
system, which defines positive x as pointing down. The
drawing should include only major geologic formations.
Note that in the example, an extra line segment was added
to break formation | into two sections. This was done to
isolate the area of formation 1 in which mining is to
occur. The purpose for this isolation will be explained
later. Avoid overlapping and concurrent line segments ,
(figure 2). ANSYS will not generate a finite-element
mesh if these conditions are present.

Step 2: Create Finite-Element Mesh

2-1. Export the final drawing in an IGES format. If the CAD
program does not have IGES export capabilities, then
contact your ANSYS distributor for other available
translators.


3350

L 2800

Increasing depth ——————t

Formation 3

Formation 2

has

Extra line:

rake

| 1800, 1570
no,

KEY 1950, 1475
a /
sesanoxnaon

1770, 1340
0,190
1850, 1260

2-4,

2.5.

2.6.

Figure 1.—Mine plan

2-2. Run ANSYS from the directory that contains the IGES

format file created in step 1.

2.7.

Incorrect

Correct

Figure 2.—Line configuration

Input the IGES format file. This step will read in
all of the line segments created by the digitizing
process in step 1.

[/aux15]

liges fname,ext] (filename,ext is the name and
extension of the IGES file created in step 2-1.)
[finish]

Enter the ANSYS preprocessor.
U/prep7}

Define element types to be used, This step will tell
ANSYS to use three- and four-node, two-
dimensional elements when creating the finite-
‘element mesh.
[et, 1,plane42]

View line segments. The plot should look
identical to the digitized mine elevation drawing
created in step 1-1

[plot]

Merge coincident keypoints. Keypoints are the
points that define the ends of each line segment
By issuing the following command, any keypoints
which are within a radius of 1 unit from each other
will be merged together into one keypoint. This
step will eliminate extraneous keypoints that might
have been created during the digitizing process.
[nummerge,kp, 1]