4.16 PIPE16 Elastic Straight Pipe

Figure 4.16-1 PIPE16 Elastic Straight Pipe

4.16.1 Input Data

The element X-axis is oriented from node I toward node J. For the two-node option, the element Y-axis is automatically calculated to be parallel to the global X-Y plane. Several orientations are shown in Figure 4.16-1. For the case where the element is parallel to the global Z-axis (or within a 0.01 percent slope of it), the element Y-axis is oriented parallel to the global Y-axis (as shown). For user control of the element orientation about the element X-axis, use the third node option. The third node (K), if used, defines a plane (with I and J) containing the element X and Z axes (as shown). Input and output locations around the pipe circumference identified as being at 0° are located along the element Y-axis, and similarly 90° is along the element Z-axis.

The stress intensification factor (SIF) modifies the bending stress. Stress intensification factors may be input at end I (SIFI) and end J (SIFJ), if KEYOPT(2) = 0, or determined by the program using a tee-joint calculation if KEYOPT(2) = 1,2, or 3. SIF values less than 1.0 are set equal to 1.0. The flexibility factor (FLEX) is divided into the cross-sectional moment of inertia to produce a modified moment of inertia for the bending stiffness calculation. FLEX defaults to 1.0 but may be input as any positive value.

The element mass is calculated from the pipe wall material, the external insulation, and the internal fluid. The insulation and the fluid contribute only to the element mass matrix. The corrosion thickness allowance contributes only to the stress calculations. A positive wall mass real constant overrides the pipe wall mass calculation. A nonzero insulation area real constant overrides the insulation surface area calculation (from the pipe outer diameter and length). A nonzero stiffness real constant overrides the calculated axial pipe stiffness.

Element loads are described in Section 2.7. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 4.16-1. Internal pressure (PINT) and external pressure (POUT) are input as positive values. The transverse pressures (PX, PY, and PZ) may represent wind or drag loads (per unit length of the pipe) and are defined in the global Cartesian directions. Positive transverse pressures act in the positive coordinate directions. The normal component or the projected full pressure may be used (KEYOPT(5)). See Section 14.16.7 of the ANSYS Theory Reference for more information.

Temperatures may be input as element body loads at the nodes. Temperatures may have wall gradients or diametral gradients (KEYOPT(1)). The first temperature at node I (TOUT(I) or TAVG(I)) defaults to TUNIF. If all temperatures after the first are unspecified, they default to the first. If all temperatures at node I are input, and all temperatures at node J are unspecified, the node J temperatures default to the corresponding node I temperatures. For any other input pattern, unspecified temperatures default to TUNIF.

For piping analyses, the PIPE module of PREP7 may be used to generate the input for this element. KEYOPT(4) is used to identify the element type for output labeling and for postprocessing operations.

KEYOPT(7) is used to compute an unsymmetric gyroscopic damping matrix (often used for rotordynamic analyses). The rotational frequency is input with the SPIN real constant (radians/time, positive in the positive element x direction).

A summary of the element input is given in Table 4.16-1. A general description of element input is given in Section 2.1.

Table 4.16-1 PIPE16 Input Summary

Element Name	PIPE16
Nodes	I, J, K (K orientation node is optional)
Degrees of Freedom	UX, UY, UZ, ROTX, ROTY, ROTZ
Real Constants	OD, TKWALL, SIFI, SIFJ, FLEX, DENSFL, DENSIN, TKIN, TKCORR, AREAIN, MWALL, STIFF, SPIN
Material Properties	EX, ALPX, PRXY or NUXY, DENS, GXY, DAMP
Surface Loads	Pressures: 1-PINT, 2-PX, 3-PY, 4-PZ, 5-POUT
Body Loads	Temperatures: TOUT ( I ), TIN ( I ), TOUT ( J ), TIN ( J ) if KEYOPT (1) = 0, or TAVG ( I ), T90 ( I ), T180 ( I ), TAVG ( J ), T90 ( J ), T180 ( J ) if KEYOPT (1) =1
Special Features	Stress stiffening, Large deflection, Birth and death.
KEYOPT(1)	0 - Temperatures represent the through-wall gradient 1 - Temperatures represent the diametral gradient
KEYOPT(2)	0 - Stress intensity factors from SIFI and SIFJ 1 - Stress intensity factors at node I from tee joint calculation 2 - Stress intensity factors at node J from tee joint calculation 3 - Stress intensity factors at both nodes from tee joint calculation
KEYOPT(4)	Element identification for output and postprocessing 0 - Straight pipe 1 - Valve 2 - Reducer 3 - Flange 4 - Expansion joint 5 - Mitered bend 6 - Tee branch
KEYOPT(5)	Used only with the PX, PY, and PZ transverse pressures 0 - Use only the normal component of pressure 1 - Use the full pressure (normal and shear components)
KEYOPT(6)	0 - No printout of member forces or moments 2 - Print member forces and moments in the element coordinate system
KEYOPT(7)	0 - No gyroscopic damping matrix 1 - Compute gyroscopic damping matrix. Real constant SPIN must be greater than zero. DENSFL and DENSIN must be zero.

4.16.2 Output Data

• nodal displacements included in the overall nodal solution
• additional element output as shown in Table 4.16-2

The direct stress (SAXL) includes the internal pressure (closed end) effect. The direct stress does not include the axial component of the transverse thermal stress (STH). The principal stresses and the stress intensity include the shear force stress component, and are based on the stresses at the two extreme points on opposite sides of the neutral axis. These quantities are computed at the outer surface and might not occur at the same location around the pipe circumference. Angles listed in the output are measured as shown () in Figure 4.16-2. A general description of solution output is given in Section 2.2. See the ANSYS Basic Analysis Procedures Guide for ways to view results.

Figure 4.16-2 PIPE16 Stress Output

The following notation is used in Table 4.16-2:

A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL] (see Section 2.2.2). The O and R columns indicate the availability of the items in the file Jobname.OUT (O) or in the results file (R), a Y indicates that the item is always available, a number refers to a table footnote which describes when the item is conditionally available, and a - indicates that the item is not available.

Table 4.16-2 PIPE16 Element Output Definitions

Name	Definition	O	R
EL	Element number	Y	Y
NODES	Nodes - I, J	Y	Y
MAT	Material number	Y	Y
VOLU:	Volume	-	Y
CENT: X, Y, Z	Center location XC, YC, ZC	-	Y
CORAL	Corrosion thickness allowance	1	1
TEMP	TOUT(I), TIN(I), TOUT(J), TIN(J)	2	2
TEMP	TAVG(I), T90(I), T180(I), TAVG(J), T90(J), T180(J)	3	3
PRES	PINT, PX, PY, PZ, POUT	Y	Y
SFACTI, SFACTJ	Stress intensification factors at nodes I and J	Y	Y
STH	Stress due to maximum thermal gradient through the wall thickness	Y	Y
SPR2	Hoop pressure stress for code calculations	-	Y
SMI, SMJ	Moment stress at nodes I and J for code calculations	-	Y
SDIR	Direct (axial) stress	-	Y
SBEND	Maximum bending stress at outer surface	-	Y
ST	Shear stress at outer surface due to torsion	-	Y
SSF	Shear stress due to shear force	-	Y
S(1MX, 3MN, INTMX, EQVMX)	Maximum principal stress, minimum principal stress, maximum stress intensity, maximum equivalent stress (all at the outer surface)	Y	Y
S(AXL, RAD, H, XH)	Axial, radial, hoop, and shear stresses	4	4
S(1, 3, INT, EQV)	Maximum principal stress, minimum principal stress, stress intensity, equivalent stress	4	4
EPEL(AXL, RAD, H, XH)	Axial, radial, hoop, and shear strains	4	4
EPTH(AXL, RAD, H)	Axial, radial, and hoop thermal strain	4	4
MFOR(X, Y, Z)	Member forces for nodes I and J (in the element coordinate system)	5	Y
MMOM(X, Y, Z)	Member moments for nodes I and J (in the element coordinate system)	5	Y

1. If the value is greater than 0.

2. If KEYOPT(1)=0

3. If KEYOPT(1)=1

4. The item repeats at 0,45,90,135,180,225,270,315° at node I, then at node J, all at the outer surface.

5. If KEYOPT(6)=2

The following tables list output available through the ETABLE command using the Sequence Number method. See Chapter 5 of the ANSYS Basic Analysis Procedures Guide and Section 2.2.2.2 of this manual for more information. The following notation is used in Tables 4.16-3 through 4.16-3b:

Name - output quantity as defined in the Table 4.16-2

Item - predetermined Item label for ETABLE command

E - sequence number for single-valued or constant element data

I,J - sequence number for data at nodes I and J

Node I
Name	Item	E	Circumferential Location
			0°	45°	90°	135°	180°	225°	270°	315°
SAXL	LS	-	1	5	9	13	17	21	25	29
SRAD	LS	-	2	6	10	14	18	22	26	30
SH	LS	-	3	7	11	15	19	23	27	31
SXH	LS	-	4	8	12	16	20	24	28	32
EPELAXL	LEPEL	-	1	5	9	13	17	21	25	29
EPELRAD	LEPEL	-	2	6	10	14	18	22	26	30
EPELH	LEPEL	-	3	7	11	15	19	23	27	31
EPELXH	LEPEL	-	4	8	12	16	20	24	28	32
EPTHAXL	LEPTH	-	1	5	9	13	17	21	25	29
EPTHRAD	LEPTH	-	2	6	10	14	18	22	26	30
EPTHH	LEPTH	-	3	7	11	15	19	23	27	31
MFORX	SMISC	1	-	-	-	-	-	-	-	-
MFORY	SMISC	2	-	-	-	-	-	-	-	-
MFORZ	SMISC	3	-	-	-	-	-	-	-	-
MMOMX	SMISC	4	-	-	-	-	-	-	-	-
MMOMY	SMISC	5	-	-	-	-	-	-	-	-
MMOMZ	SMISC	6	-	-	-	-	-	-	-	-
SDIR	SMISC	13	-	-	-	-	-	-	-	-
ST	SMISC	14	-	-	-	-	-	-	-	-
S1	NMISC	-	1	6	11	16	21	26	31	36
S3	NMISC	-	3	8	13	18	23	28	33	38
SINT	NMISC	-	4	9	14	19	24	29	34	39
SEQV	NMISC	-	5	10	15	20	25	30	35	40
SBEND	NMISC	90	-	-	-	-	-	-	-	-
SSF	NMISC	91	-	-	-	-	-	-	-	-
TOUT	LBFE	-	4	-	1	-	2	-	3	-
TIN	LBFE	-	8	-	5	-	6	-	7	-

Table 4.16-3a PIPE16 Item and Sequence Numbers for the ETABLE and ESOL Commands

Node J
Name	Item	E	Circumferential Location
			0°	45°	90°	135°	180°	225°	270°	315°
SAXL	LS	-	33	37	41	45	49	53	57	61
SRAD	LS	-	34	38	42	46	50	54	58	62
SH	LS	-	35	39	43	47	51	55	59	63
SXH	LS	-	36	40	44	48	52	56	60	64
EPELAXL	LEPEL	-	33	37	41	45	49	53	57	61
EPELRAD	LEPEL	-	34	38	42	46	50	54	58	62
EPELH	LEPEL	-	35	39	43	47	51	55	59	63
EPELXH	LEPEL	-	36	40	44	48	52	56	60	64
EPTHAXL	LEPTH	-	33	37	41	45	49	53	57	61
EPTHRAD	LEPTH	-	34	38	42	46	50	54	58	62
EPTHH	LEPTH	-	35	39	43	47	51	55	59	63
MFORX	SMISC	7	-	-	-	-	-	-	-	-
MFORY	SMISC	8	-	-	-	-	-	-	-	-
MFORZ	SMISC	9	-	-	-	-	-	-	-	-
MMOMX	SMISC	10	-	-	-	-	-	-	-	-
MMOMY	SMISC	11	-	-	-	-	-	-	-	-
MMOMZ	SMISC	12	-	-	-	-	-	-	-	-
SDIR	SMISC	15	-	-	-	-	-	-	-	-
ST	SMISC	16	-	-	-	-	-	-	-	-
S1	NMISC	-	41	46	51	56	61	66	71	76
S3	NMISC	-	43	48	53	58	63	68	73	78
SINT	NMISC	-	44	49	54	59	64	69	74	79
SEQV	NMISC	-	45	50	55	60	65	70	75	80
SBEND	NMISC	92	-	-	-	-	-	-	-	-
SSF	NMISC	93	-	-	-	-	-	-	-	-
TOUT	LBFE	-	12	-	9	-	10	-	11	-
TIN	LBFE	-	16	-	13	-	14	-	15	-

Table 4.16-3b PIPE16 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name	Item	E
STH	SMISC	17
PINT	SMISC	18
PX	SMISC	19
PY	SMISC	20
PZ	SMISC	21
POUT	SMISC	22
SFACTI	NMISC	81
SFACTJ	NMISC	82
SPR2	NMISC	83
SMI	NMISC	84
SMJ	NMISC	85
S1MX	NMISC	86
S3MN	NMISC	87
SINTMX	NMISC	88
SEQVMX	NMISC	89

4.16.3 Assumptions and Restrictions

The element may be used for both thin and thick-walled situations; however, some of the stress calculations are based on thin-wall theory. The pipe element is assumed to have "closed ends" so that the axial pressure effect is included. Shear deflection capability is also included in the element formulation.

Eigenvalues calculated in a gyroscopic modal analysis can be very sensitive to changes in the initial shift value, leading to potential error in either the real or imaginary (or both) parts of the eigenvalues.

4.16.4 Product Restrictions

ANSYS/LinearPlus

• The SPIN real constant (R13) is not available.
• The DAMP material property is not allowed.
• The only special features allowed are stress stiffening and large deflections.
• KEYOPT(7) (gyroscopic damping) is not allowed.