An existing liquid engine test stand at the AF Astronautics Laboratory was refurbished and extensively modified to accommodate the static firing of the Titan 34D solid rocket motor (SRM) in the vertical nozzle down orientation. The main load restraint structure was designed and built to secure the SRM from lifting off during the firing. In addition, the structure provided weather protection, temperature conditioning of the SRM, and positioning of the measurement and recording equipment. The structure was also used for stacking/de-stacking of SRM segments and other technological processes. The existing stand, its foundation and anchorage were thoroughly examined and reanalyzed. Necessary stand modifications were carried out to comply with the requirements of the Titan 34D SRM static firing

Glozman, Vladimir

Shipway, George

English

NASA Technical Reports Server

N89-12610
A
TEST STAND FOR TITAN 34D SRlVl STATIC FIRING
Vladimir Glozman
California Polytechnic University
George Shipway
Wyle Laboratories
ABSTRACT
An existing liquid engine test stand at the AF Astronautics
Laboratory has been refurbished and extensively modified to
accommodate the static firing of the Titan 34D solid rocket motor
(SRM) in the vertical nozzle down orientation. The main load
restraint structure was designed and built to secure the SRM from
lifting off during the firing. In addition the structure
provided weather protection, temperature conditioning of the SRM,
and positioning of the measurement and recording equipment. The
structure was also used for stacking/de-stacking of SRM segments
and other technological processes.
The existing stand, its foundation and anchorage were
thoroughly examined and reanalyzed. Necessary stand
modifications were carried out to comply with the requirements of
the Titan 34D SRM static firing. A new superstructure was
designed and erected on top of the modified test stand. The
superstructure was a steel framework consisting of corner and
side columns, horizontal mounting platforms, and cross bracing
elements. Mounting platformelevations and superstructure height
were designed for easy modification to facilitate stacking/de-
stacking procedures and potential testing of different SRMs.
The superstructure and the test stand overall were analyzed
by finite element methods utilizing IMAGES-3D, ANSYS, and NASTRAN
codes. Critical joints, anchors and the environmental enclosure
were evaluated by conventional methods. Analyses were performed
for the specified loads transmitted to the structure from the
SRM, as well as for wind loads, postulated seismic disturbances,
and acoustic pressure. It was determined that the test stand
exhibits a sufficient factor of safety under the most
conservative combination of the applied loads. Stiffness of the
test structure and its dynamic properties were found to be
acceptable.
353
https://ntrs.nasa.gov/search.jsp?R=19890003239 2020-03-20T04:39:21+00:00Z
Specific attention was given to the SRM mounting structure,
which includes a modified thrust pylon, a newly designed pylon
adapter welded into the pylon, and an aft test skirt fixture
connecting the SRM to the pylon through the adapter. Detailed
finite element analysis of the mounting structure with and
without the SRM was performed, and response of the mounting
structure to the ignition transient and other loading conditions
was thoroughly investigated. It was found that stress levels in
all critical elements was below the yield strength of the
selected materials with sufficient safety factor. The stiffness
of the mounting structure and therefore dynamic response of the
SRM during the static firing was shown to be also acceptable.
The modified test stand met all of the design criteria
during the successful firing of the Titan 34D SRM.
INTRODUCTION
The key element in the static firing of the Titan 34D SRM is
the load restraint structure, which stabilizes the rocket and
prevents it from lift-off during the test. The structure was
designed and built utilizing an existing twenty year old liquid
engine test stand at the AF Astronautics Laboratory. This
allowed for the completion of all work for erecting a complex
test facility in a timely, cost effective manner.
The existing stand was analyzed and design modifications
were implemented to permit SRM testing. A new superstructure was
erected on the top of the existing test stand. The
superstructure consists of a steel beam framework with horizontal
mounting platforms and environmental enclosure.
The ability of the existing pylon structure and its
anchorage to withstand the static load prior to firing and the
thrust load during firing was thoroughly investigated and
necessary modifications have been implemented. A new thrust
restraint fixture was designed to interface with the existing
pylon structure, and to accommodate the SRM aft closure.
Furthermore, the pylon and superstructure assembly were rigidly
connected to provide additional stiffness for the SRM mounting.
Each structure as well as the combined structure were evaluated
for the specified restraint load transmitted from the SRM, as
well as wind load, postulated seismic disturbances and acoustic
pressure. Evaluations were performed by a combination of
conventional and finite element methods using NASTRAN, ANSYS,
IMAGES-3D and other structural codes. Furthermore, due to the
time limitation and the critical importance of the design,
evaluation of the combined structure was performed independently
in two Wyle facilities (Norco, CA, and Huntsville, AL) using two
different structural codes, ANSYS and NASTRAN. The results of
these analySes compared favorably, and subsequent performance of
the test facility during the static firing was the ultimate
verification of the performed design and analytical work.
354
SUPERSTRUCTURE
The 6.7 m x 6.7 m x 16.5 m superstructure (Figure i) was
erected on the top of the modified existing test stand
(Figure 2). The design and analysis of the superstructure was
performed using the IMAGES-3D finite element program.
The main structural elements of the superstructure are:
o Four corner columns.
o Four side columns.
o Three permanent horizontal mounting platforms.
o Two removable horizontal platforms at elevations of
3.2m and 14.5m for the side restraint of 2 segment
and 5 1/2 segment specimens.
o Side diagonal cross bars.
The finite element model of the superstructure (Figure 3)
is comprised of the beam structural elements identified in
Table i.
The model consists of 112 nodes which are connected with a
total of 264 beam structural elements at six different cross
sections, based on the anticipated design. To account for the
weight of stairways, handrails, the mounting platform grating,
and other nonstructural elements, the density of the structural
element material was increased by 20 percent. Weather protection
is provided by side panels and a roof. Wind loading on the side
panels was included; stiffness of the panels was assumed to be
negligible. Because the superstructure iserected on top of the
existing stand, the 36 spring elements were used to represent the
stiffness of the stand. The spring stiffness was determined by
finite element analysis of the existing stand.
The main load conditions as the front and side wind loads of
177 km/hr (Ii0 mph), the postulated ultimate loads on the top of
the superstructure from the attached SRM, and the potential
seismic load were evaluated.
The wind load was represented as a static pressure on the
projected area of the four sides of the superstructure. A
pressure of 250 MPa (36 ksi) applied to the facing side and a
negative pressure of 192 MPa (28 ksi) on the three other sides
was assumed. Two wind directions were evaluated, a front wind
(road to flame side) and a side wind.
The postulated ultimate forces applied by the SRM to the top
of the superstructure were comprised of two elements: two forces
for a total of 144 ton in road-to-flame direction (Z) and two
forces for a total of 41 ton in side-to-side direction (X).
355
The effect of seismic excitation was conservatively analyzed
by quasistatic method applying 0.5g load in three orthogonal
directions simultaneously.
An operating load of 10.6 kN applied to the mounting
platform at the i0 meter elevation and self-weight of the
superstructure was considered in all load cases.
Maximum deflections on the top of the superstructure were
calculated to be:
o due to front wind load;
o due to side wind load;
o due to ultimate side forces
road-to-flame direction
side-to-side direction
6.8 mm
6.3 mm
15.2 mm
48.3 mm
Maximum stress due to wind load was 90 MPa which is below
yield strength of A36 steel with a factor of safety of 2.8. The
maximum stress caused by ultimate top forces of 180 MPa was below
yield strength deflections and stresses caused by postulated
seismic disturbance were substantially smaller of those due to
the wind load.
In addition to the finite element analysis, conventional
methods were used to address buckling of the frame elements and
to evaluate joint connections. Results of these analysis
conformed ability of the superstructure withstand the specified
load with substantial factor of safety.
The environmental enclosure was analyzed by a combination of
conventional and finite element methods and was shown to be
capable of withstanding not only the specified wind load, but
also the acoustic pressure during static firing of the SRM.
A dynamic analysis was performed to obtain dynamic
properties of the superstructure, i.e. resonance frequencies and
mode shapes, with and without the SRM. _ The main results of the
analysis are summarized in Table 2.
EXISTING TEST STAND
The existing iC test stand (Figure 4) was prepared by
removing about 350 tons obsolete and surplus equipment including
large propellant tanks, the liquid motor support and thrust
measurement system, valves and piping_ etc.
A preliminary analysis indicated the necessity of very
limited modification of the stand main frame structure. The
12WF27 beams were changed to stronger 24WF76 beams at the
superstructure interface to the stand and two other weak elements
were replaced with stronger elements.
356
The stand was modeled as a framework (Figure 5) consisting
of 321 beam elements supported at four points. The stand was
analyzed for the same load conditions as the superstructure and
interactive forces from the superstructure were applied to the
finite element model of the stand. The minimum factor of safety
for the wind load was calculated to be more than six against the
yield strength of A36 steel.
The maximum stresses in the stand caused by the abnormal
ultimate load applied to the top of the superstructure was
calculated to be 345 MPa which was below ultimate strength of A36
steel.
The modified stand was also analyzed for a vertical downward
load to determine its vertical load carrying capacity at the
superstructure boundary. A factor of safety of 4.6 against
ultimate strength was calculated for that load condition.
Stiffness properties of the existing stand also were
calculated and subsequently used for a pylon-to-stand connection
evaluation and for creating a general combined finite element
model.
MOTORMOUNTING STRUCTURE
The attachment structure for the mounting of the motor
(Figure 6) includes an existing pylon, newly designed pylon
adapter welded into the pylon, and an aft test-skirt fixture
connecting the motor to the pylon through the pylon adapter. A
finite element analysis of the pylon structure, including a new
pylon adapter, skirt, and a simple (stick) model of the SRM was
performed using the IMAGES-3D and NASTRAN finite element
programs. The model of the pylon is comprised entirely of beam
elements. This assumes that cross sections, particularly those
of the box beam at the top, do not warp. All beam connections
are assumed to be rigid, as are the four support points. All
section properties are based on the drawings of the original
pylon structure.
The pylon adapter model is composed primarily of
quadrilateral and triangular plate elements. The skirt model is
basically a cylinder with a stiffening ring at the bottom. The
SRM is modeled as a beam with section properties based on actual
specimen geometry. The model was subjected to gravity loads in
the three orthogonal directions. This served as a check of the
structural soundness of the model, and also provided information
for evaluating the structures' response to potential earthquake
excitation.
357
The dynamic analysis of the mounting structure with and
without the SRM was performed first in order to obtain the
response of the structure to the ignition transient• The lowest
resonance frequency of the SRM itself as a simple cantilever beam
was computed at 1.96 Hz. The lowest resonance frequencies of the
SRM installed are 1.22 Hz and 1.30 Hz in side-to-side and road-
to-flame direction correspondingly• The dynamic response of the
loaded structure to the ignition transient showed that there was
no amplification of the vertical component of the motor
displacement. However, the horizontal component was 1.7 times
the static• The dynamic load factor was used to adjust the
static force for a load combination calculation• Detailed static
stress analysis showed that the only significant stress of
140 MPa occurs in the pylon adapter upper ring. Stresses in
other parts of the pylon and the adapter were substantially
lower• The maximum stress in the aft test skirt caused by the
abnormal "ultimate" thrust of i0 million pounds canted at six
degrees, was calculated to be 490 MPa. This is below the
tensile strength of 620 MPa for normalized 4130 alloy steel.
PYLON ANCHOR YIELD ANALYSIS
Pylon anchor yield analysis was critical• It preceded all
other analyses, because the existing 40 steel anchors were
imbedded in concrete and, thereforei could not be replaced. Each
anchor is 57.1 mm (2.25 in.) in diameter and 11.6 m long and is
made of quenched and tempered 4340 steel• Detailed analysis was
performed taking into account anchor/concrete relative stiffness
and the anchor/concrete interface• Eventhough the anchors can
withstand the abnormal "ultimate" thrust of i0 million, maximum
thrust force must be limited to 8.6 M based on yield of the
anchors, and to only 7.2 M to maintain the joint. But even the
smallest allowable thrust is substantially higher than that
predicted and recorded during the SRM test.
COMBINED MODEL ANALYSIS OF THE TEST STAND
After design and modification of the main elements of the
test stand were completed, the finite element analyses of the
stand were carried out. A combined finite element model of the
superstructure, test stand, pylon assembly and SRM were developed
on the NASTRAN and ANSYS finite element computer codes and
carried out by two independent teams• These analyses were aimed
to verify the design effort and also examine the stand-pylon-SRM
interfaces• Therefore, the three following cases were analyzed:
• Free standing pylon with the SRM without any attachment
to the restraining structure•
• Pylon with the SRM attached to the superstructure at the
top level by means of struts•
358
. Pylon attached to the stand at the second platform level
with the SRM attached to the superstructure at the top
level.
The analyses of the combined model were performed for
different load conditions: thrust load, wind load, seismic
disturbances, etc. The analyses took into account the transient
nature of the thrust force and the SRM mass decay during the
burnout.
The results of the combined model analyses gave additional
information about static and dynamic behavior of the stand. They
were in good agreement with the previously obtained data, and
therefore, verified overall new design and modification of the
test stand and the pylon.
Performance of the test stand during the SRM static firing
was in good correlation with analytical predictions. No trace of
damage, malfunction, or any structural problems have been noticed
during the test. The measured stresses, eigenvalues, and
eigenvectors were very close to those obtained during design and
analytical activities. Overall the test stand performed
exceptionally well and met all design criteria during the
successful firing of the Titan 34D SRM.
LIST OF FIGURES
i. Superstructure framework.
2. Main structure of the test stand for Titan 34D SRM firing.
3. Finite element model of the superstructure.
4. Test stand IC.
5. Finite element model of the modified test stand iC.
6. Finite element model of motor mounting structure.
LIST OF TABLES
i. Superstructure node and beam element summary.
2. Resonance frequencies of superstructure, Hz.
359
TABLE 1
SUPERSTRUCTURE NODE AND BEAM ELEMENT SUMMARY
•-ELEV'.
M
IkODE
VIEW
IkttvlBER
92-104
/_ 105-112
[ 66-78
53-65
40-52
/ 27-39
14-26
I 1-13
COLUMN
CORNER SIDE
W12 X 58 Wl;_ X 26
25-28 53-56
21-24 19-52
17-20 45-48
13-16 41-44
9-12 37-40
5-8 33-36
1 -4 29-32
INNER
157-i64
117-124
97-104
77-84
57-64"
PLATFORM W12 x 26
OUTER
185-192
165-180
145-152
125-132
105-112
85-92
65-72"
CORNER CROSS
153-156 197-200
133-136
113-116
93-96 192-196
SIDE
Two 6X4Xl_
233-264
225-232
217-244
209-216
201-208
" SECTIONS W16 X 67
360
TABLE 2
RESONANCE FREQUENCIES OF SUPERSTRUCTURE, HZ
Mode Description
Global rocking side-to-side
Global rocking road-to-flame,
Global torsion
Local side column bending
Lower platform (local)
Upper platform (local)
Without
Specimen
z¢.29
With
Specimen
2.58
2.59
7.41
/4.29
8.66, 8.71
8.71, 8.73, 8.75
361
ORIGINAL PA:C_
O,F _o QUALITY.
FIGURE 1
SUPERSTRUCTURE FRAMEWORK
362
iii!i
i!iii
iiill
iiiiiiiiiiiiiiii_
_iiiiiiiiiMiM!i!iil
ORIGINAE PANGS IS
OF POOR QUALFI_
FIGURE 2
MAIN STRUCTURE OF THE TEST STAND FOR TITAN 34D SRM FIRING
(., <J
363
FIGURE 3
FINITE ELEMENT MODEL OF THE SUPERSTRUCTURE
364
ORIGINA.UPA_G_
OF POOR QUALIT_
i!i!i!iiiil...'...iiiiiiiiiiiiiiiiii
FIGURE 4
TEST STAND IC
365
!
\
\/
\
\\
FIGURE 5
FINITE ELEMENT MODEL OF THE MODIFIED TEST STAND IC
366
SRM
AFT SKIRT
PYLON ADAPTER
PYLON
FIGURE 6
FINITE ELEMENT MODEL OF MOTOR MOUNTING STRUCTURE
367


Test stand for Titan 34D SRM static firing

Abstract

Similar works

Full text

Available Versions

NASA Technical Reports Server