Parametic investigations are performed using several two dimensional finite element formulations to determine their suitability for use in predicting extremum stresses in marine propellers. Comparisons are made of two NASTRAN elements (CTRIM6 and CTRAIA2) wherein elasticity properties have been modified to yield plane strain results. The accuracy of the elements is investigated by comparing finite element stress predictions with experimentally determined stresses in two classical cases: (1) tension in a flat plate with a circular hole; and (2) a filleted flat bar subjected to in-plane bending. The CTRIA2 element is found to provide good results. The displacement field from a three dimensional finite element model of a representative marine propeller is used as the boundary condition for the two dimensional plane strain investigations of stresses in the propeller blade and fillet. Stress predictions from the three dimensional analysis are compared with those from the two dimensional models. The validity of the plane strain modifications to the NASTRAN element is checked by comparing the modified CTRIA2 element stress predictions with those of the ABAQUS plane strain element, CPE4

Gillcrist, M. C.

Parnell, L. A.

English

NASA Technical Reports Server

STRESS CONCENTRATION INVESTIGATIONS USING NASTRAN t
M. C. Gillcristand L.A. Parnell
Naval Ocean SystemsCenter,San Diego,CA
ABSTRACT
Parametric investigations are performed using several two-dimensional finite element formulations to
determine their suitability for use in predicting extremum stresses in marine propellers. Comparisons are
made of two NASTRAN elements (CTRIM6 and CTRIA2) wherein elasticity properties have been
modified to yield plane strain results. The accuracy of the elements is investigated by comparing finite
element stress predictions with e.xperimentally determined stresses in two classical cases: (1) tension in a
flat plate with a circular hole; and (2) a filleted flat bar subjected to in-plane bending. The CTRIA2 ele-
ment is found to provide good results. The displacement field from a three-dimensional finite element
model of a representative marine propeller is used as the boundary condition for the two-dimensional
plane strain investigations of stresses in the propeller blade and fillet. Stress predictions from the three-
dimensional analysis are compared with those from the two-dimensional models. The validity of the plane
strain modifications to the NASTRA_N element is checked by comparing the modified CTRIA2 element
stress predictions with those of the ABAQUS plane strain element, CPE4.
INTRODUCTION
It is common practice in stress analyses of marine propellers to create a three-dimensional (3-D) finite
element model of the blade without hub or fillet and apply a rigid boundary condition at the blade-hub
interface. The stresses nearest the hub are normally the largest. For this reason it is important to know
what influence the absence of the hub and fillet have on the predicted stresses.
One approach to this problem is to perform a full 3-D finite element analysis of the blade, hub and
fillet, a costly and time consuming computational effort. An alternate approach, used at the David Taylor
Naval Ship Research and Development Center (DTNSRDC), is to perform a 3-D finite element analysis of
the clamped blade model (i.e., without hub or fillet) and apply the computed displacements as a boundary
condition for a two-dimensional (2-D) plane strain model of the blade with hub and fillet. This paper
takes the DTNSRDC approach to investigate stress concentrations in the fillet region of a marine pro-
peller blade.
ELEMENT SELECTION
The first step in the finite element analysis is to choose appropriate elements from NASTRAN's ele-
ment library (ref. 1,2). The 20-node hexahedron, CIHEX2, is the obvious choice for the 3-D portion of the
analysis. For the 2-D plane strain analysis, the 6-noded and 3-noded triangular plate elements, CTRIM6
and CTRIA2 respectively, were selected as probable candidates because of the ease with which triangular
elements can be meshed to irregular geometries.
tThisworkwassupportedbytheNavalSeaSystemsCommand(NAVSEA63R5).
154
https://ntrs.nasa.gov/search.jsp?R=19860016360 2020-03-20T14:25:23+00:00Z
The formulation of the triangular plate elements in NASTRAN is based on the assumption of 'plane
stress'. A 'plane strain' solution can be obtained however, by modifying the elasticity coefficients as
described by Schaeffer (ref. 3). The validity of the plane strain modifications to NASTRAN is checked by
comparing the stress predictions of the modified NASTRAN element with those of the ABAQUS plane
strain element, CPE4 (ref. 4).
VERIFICATION OF ELEMENT ACCURACY
Success in performing numerical stress calculations by the finite element method depends on the
choice of element and the layout of the element mesh. When properly formulated, the finite element solu-
tion should converge to the exact analytical solution if progressively finer meshes are used. For the circu-
lar hole and fillet geometries investigated in this paper, mesh size can be represented by the dimensionless
ratio, l/r, where l is the length of an element (in the region of interest) and r is the radius of the circular
hole or fillet. Laura, Reyes and Rossi (ref. 5) tried to assess-the accuracy of the constant strain triangular
element in regions of high stress concentration. Finite element predicted stress concentration factors were
compared with photoelastically determined values at the boundary of a slot in a plate subjected to uniax-
ial stress. For element meshes with 1/r equal to 0.13, the difference between numerical and experimental
results was on the order of 10%.
In order to gauge the accuracy of the NASTRAN triangular elements for a given mesh size, comparis-
ons are made between stress results obtained by the finite element method and those obtained by experi-
mental or other analytical techniques. Two stress concentration cases are selected for the comparisons:
(1) a flat rectangular plate with a small circular hole subjected to a uniform tension, a , in the x-direction;
and (2) a filleted bar subjected to in-plane bending. For the case of an infinite plate with a circular hole,
Timc_henko (ref. 6) found that the stress in the x-direction is _r at the edge of the hole and quickly drops
to a away from the hole. For a finite plate with width no less than 4 times the hole diameter,
Tim_henko found that the stresses produced should be within 6% of those produced in the infinite plate,
that is, between 2.820" and 30".
For the sake of comparison, a finite element analysis was performed on a fiat square plate with the
ratio of plate width to hole diameter of approximately 12 to I. The applied stress is a and the theoretical
value of a x at the hole edge should be between 2.8_r and 3_ . Results for the NASTRA_N CTRIA2 ele-
ment are presented in table 1. Mesh fineness in the region of interest is represented in terms of the nondi-
mensional ratio, l/r, where l is the length of an element and r is the radius of the circular hole. Table 1
shows that predicted stresses using the CTRIA2 element are within 6% of the theoretical value when
mesh size values, l/r, of less than 40% are used. The CTRIM6 element yields surprisingly poor results.
Nodal stresses at the edge of the hole range from 1._¢r to 4.3a for very fine meshes (l/r less than 30_).
Averaged nodal stresses yield better results; however, due to the disparity in nodal stresses from contri-
buting elements, there is little confidence in the CTRIM6 predictions. This element is given no further
consideration.
Hartman and Leven (ref. 7) used photoelastic techniques to determine stress concentrations in filleted
barn subjected to in-plane bending as illustrated in figure 1. Stress concentrations of 1.2 to 3.0 were
obtained for r/d values ranging from 0.03 to 0.50, where r is the fillet radius and d is the depth of the bar.
The stress concentration factor, k, is defined as the ratio of the maximum stress at the fillet to the nomi-
nal stress computed by the flexure formula: anom = Mc/I, where c = d/2, I = area moment of inertia and
M = applied bending moment. Table 2 presents NASTRAN CTRIA2 stress predictions in the fillet
region of a flat bar identical to one tested by Hartman and Leven. For this particular case ( r/d = 0.2 ),
155
Hartman and Leven determined the stress concentration to be k = 1.53. The NASTRAN predicted k
value of 1.58 presented in table 2 is in excellent agreement with this, differing by only 3.3% from the
experimentally determined value.
THE 3-D DISPLACEMENT FIELD AS A BOUNDARY CONDITION
The 2-D plane strain finite element analysis of the blade with hub and fillet is predicated on the
hypothesis that the displacement field predicted by the 3-D finite element model can be applied as a boun-
dary condition to the 2-D model. This technique, which is supported by unpublished numerical experi-
ments, is illustrated by the case of a thick plate in bending. A thick rectangular plate lying in the x-z
plane is subjected to out-of-plane bending by the application of a moment along one edge while the oppo-
site edge is fixed; that is, the plate is cantilevered and a moment applied to the free end as illustrated in
figure 2. Using sixteen CIHEX2 isoparametric brick elements, a 3-D finite element model is constructed
and solved for displacements and stresses. A 2-D model in the x-y plane is created using CTRIA2 ele-
ments. Displacements computed by the 3-D model at nodes 5 through 7 are applied as a displacement
boundary condition to the corresponding nodes in the 2-D model. Stresses are then computed using the
2-D model. Table 3 presents stress predictions from both models at nodes l, 2, 3 and 4 along the top sur-
face of the plate. With the exception of node 1 located on the rigid boundary, stress predictions from the
two models differ by less than 2%. Similar results are obtained for the bottom surface of the plate. Since
the 3-D model composed of isoparametric brick elements can be expected to yield reasonable stress predic-
tions at locations away from the boundary, these results support the assertion that the 3-D displacement
predictions can be applied as a boundary condition to the 2-D model in order to obtain reasonable stress
predictions.
PROPELLER MODELS
A 3-D and 2-D finite element propeller blade model are constructed for the purpose of analyzing the
stresses in the blade root region. The 3-D blade model without hub or fillet consists of 40 CII-IEX2 brick
elements and is presented in figure 3. Figure 4 shows a 2-D model of a blade, hub and fillet cross section
composed of 243 CTRIA2 elements. Maximum stress is usually developed at the base of the blade in the
midchord region. For this reason, the 2-D analysis is based on a planar slice through the blade, hub and
fillet in the vicinity of the midchord. The plane of interest is illustrated in figure 3 by superposition of a
2-D model on the 3-D model. R is the propeller radius measured from the center of the hub. Nodes 1, 2
and 3, located at approximately 0.36R, correspond to nodal points on both the 3-D and 2-D finite element
models. Hydrodynamic and centrifugal loads are applied to the 3-D finite element model in order to
predict the displacements at nodes I, 2 and 3. These displacements are then applied to corresponding
nodes on the 2-D planar model as a displacement boundary condition, ensuring that all out-of-plane
degrees-of-freedom are constrained.
Several 2-D plane strain propeller models are analyzed in order to investigate the sensitivity of root
stresses to fillet radius. The propeller under consideration has a fillet of constant radius, r, which is
approximately one half the blade thickness, d. Table 4 presents stress predictions from both NASTRAN
and ABAQUS 2-D analyses of the blade with hub and fillet. The extremum stresses (those of greatest
absolute value) are the compression stresses developed in the fillet on the low-pressure face of the blade
(see figure 4). The stress values presented in the table vary less than 40/o over a range in r/d values from
0.37 to 0.56. The 3-D NASTRAN analysis of the clamped blade without hub or fillet predicts a maximum
156
stressvaluewithin3e_ of the2-D NASTRAN predictionsand within4_o of the2-D ABAQUS prediction.
Thistechniqueofcombiningthe 2-D and 3-D finitelementanalysesto predictfillets ressesispredicated
on theassumptionthatthe planestrainconditionexistsintheregionofthe2-D planarslice.Itisreassur-
ing to notethatthe 3-D analysispredictsout-of-planedisplacementsan orderof magnitudesmallerthan
thein-planedisplacements.Thisresultlendscredenceto theassumptionofplanestrain.
SUMMARY AND CONCLUSIONS
Parametric investigations were performed using several two-dimensional finite element formulations to
determine their suitability for use in predicting root stresses in marine propellers. Comparisons were made
of two NASTRAN elements, CTRIM6 and CTRIA2, wherein elasticity properties were modified to yield
plane strain results. The accuracy of the elements was investigated by comparing stress results obtained
by the finite element method with those obtained by experimental or analytical techniques for two stress
concentration cases: (1) a fiat rectangular plate with a small circular hole subjected to uniform tension,
and (2) a filleted bar subjected to in-plane bending. For both cases, the CTRIA2 element was found to
provide stress predictions within about 5% of the expected value (experimental or theoretical) so long as
the mesh size parameter, l/r, did not exceed about 15%. Furthermore, it was discovered that when the
CTRIM6 element was used, the solution did not appear to converge. The plane strain modification to the
NASTRAN element was checked by comparison with the ABAQUS plane strain element, CPE4. NAS-
TRAN and ABAQUS 2-D plane strain analyses were performed on a propeller model yielding stress pred-
ictions which differed by only a few percent.
A combined 2-D and 3-D analysis of a thick plate in bending demonstrated the validity of applying
predicted displacements from the 3-D analysis as a displacement boundary condition to the 2-D model in
order to predict stresses in the plate. This technique was then applied to the analysis of root stresses in a
marine propeller blade. It was found that extremum stresses develop in the fillet on the compression face
of the blade and that these stresses are rather insensitive to small changes in the fillet radius. Further-
more, it was demonstrated that there is no significant difference in the extremum stresses predicted by the
3-D clamped blade analysis and the 2-D blade-hub-fillet analysis..Although the close proximity of the
_-xed displacement boundary condition in the 3-D model may distort the stress field in the root region, it
does not appear to adversely affect the prediction of extremum stress.
REFERENCES
1. The NASTRAN Users Manual, Vol. 1, NASA Scientific and Technical Information Office, Washington,
• D.C., June 1985.
2. The NASTRAN Theoretical Manual, NASA Scientific and Technical Information Office, Washington,
D.C., Jan 1981.
3. Schaeffer, H.G., MSC/NASTRA.N Primer: Static and Normal Modes Analysis, Wallace Press, Inc., Mil-
ford, New Hampshire, Jan. 1982, pp 271-272.
4. ABAQUS User's Manual, Hibbit, Karlsson and Sorensen, Inc., May 1984.
157
5. Laura P.A., Reyes J.A. and Rossi R.E., Numerical Experiments on the Determination of Stress Con-
centration Factors, Strain, vol. 10, no. 2, Apr. 1974, pp 58-63.
6. Timoshenko, S.P. and Goodier, J.N., Theory of Elasticity, 3rd ed., McGraw-Hill, New York 1970, pp
90-92.
7. Hartman, J.B. and Leven, M.M., Factors of Stress Concentration for the Bending Cases of Fillets in
Flat Bars and Shafts with Central Enlarged Section, Proceedings of the Society for Experimental
Stress Analysis, vol. 9, no. 1, 1951, pp 53-62.
158
TABLE 1. STRESS AT THE EDGE OF A SMALL CIRCULAR HOLE IN A SQUARE FLAT
PLATE SUBJECTED TO TENSION a, IN THE x-DIRECTION.
Mesh size Stressf Percent difference from
I/r a_ infinite plate value
0.64 2.42cr 19.3
0.36 2.86cr 4.7
0.26 2.84cr 5.3
0.22 2.86cr 4.7
t NASTRAN predictions using triangular plate element CTRIA2.
l ----element length
r = radius of hole
= applied stress
ex = stress in x-direction at the centroid of an element located at edge of hole
TABLE 2. STRESS CONCENTRATION IN A FILLETED BAR SUBJECTED TO
IN-PLANE BENDING.
Mesh size Stress Concentration t Percent difference from
l/r k ' experimental value*
0.140 1.46 4.9
0.025 1.58 3.3
t NASTRAN predictions using triangular plate element CTRIA2.
l -- element length
r = fillet radius
* Experimental value -- 1.53 (see reference 7).
159
TABLE 3. PLATE STRESSES PREDICTED BY NASTRAN 2-D AND 3-D MODELS
Node Model Dimensionless Percent
Number Stress* Difference
1 3D 1.221 14.0
2D 1.392
2 3D 1.106 0.8
2D 1.096
3 3D 1.011 0.4
2D 1.015
4 3D 1.000 1.2
2D 1.012
* The major principal stress at node 4 predicted by the 3D analysis has a dimensionless stress value of
1.000. The other stress values listed in the table are major principal stresses presented in terms of
the unit stress at node 4.
160
TABLE 4. EXTREMUM STRESS PREDICTIONS BASED ON 2-D PLANE STRAIN
ANALYSES OF THE BLADE, HUB AND FILLET.
Finite Element Number Mesh Fillet Extremum
Element Type * of Size Size Stress **
Code Elements l/r r/d
NASTRAN CTRIA2 243 0.03 0.37 0.985
NASTRAN CTRIA2 243 0.03 0.46 0.974
NASTRAN CTRIA2 243 0.12 0.56 1.00
ABAQUS CPE4 136 0.40 0.46 0.968
r _ fillet radius
d _ blade thickness at hub
l _ element length in region of extremum stress
* CTRIA2 refers to the NASTRAN CTRIA2 element modified for plane strain. CPE4 refers to the
ABAQUS plane strain quadrilateral element.
** The extremum stress predicted by the 3-D blade model has a dimensionless stress value of 1.0. The
stresses listed in the table are presented in terms of this unit stress.
161
L/2 _-
r/d = 0.2
L/D = 2
D/d = 3
K = 1.53 determined photoelastically by
Hartman and Leven (ref. 7).
, Figure 1. A filleted bar in a field of pure bending.
162
, 3D MODEL
2
4
7
Y
z, X
Figure 2. 3D and 2D thick-plate models.
163
Figure 3. 2D blade, hub and fillet model superimposed on a 3D propeller blade 
model composed of 40 CIHEX2 elements. 
Figure 4. 2D Model of blade, hub and fillet showing detail of upper fillet.
Model is composed of 243 CTRIA2 elements.
165


Stress concentration investigations using NASTRAN

Abstract

Similar works

Full text

Available Versions

NASA Technical Reports Server