4.18 PIPE18 Elastic Curved Pipe (Elbow)

Options are available to include various flexibility and stress intensification factors in the formulation. The element can account for insulation, contained fluid, and a corrosion allowance. See Section 14.18 in the ANSYS Theory Reference for more details about this element. A straight pipe element (PIPE16) is described in Section 4.16. A pipe tee element (PIPE17) is described in Section 4.17. A plastic curved pipe (PIPE60) is described in Section 4.60.

Figure 4.18-1 PIPE18 Elastic Curved Pipe (Elbow)

4.18.1 Input Data

Although the curved pipe element has only two endpoints (nodes I and J), the third node (K) is required to define the plane in which the element lies. This node must lie in the plane of the curved pipe and on the center-of-curvature side of line I-J. A node point belonging to another element (such as the other node of a connecting straight pipe element) may be used. 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.

Only the lumped mass matrix is available.

The flexibility and stress intensification factors included in the element are calculated as follows:

ANSYS Flexibility Factor = 1.65/(h(1 + PrX_k/tE)) or 1.0 (whichever is greater) (used if KEYOPT(3)=0 or 1 and FLEX not input)

Karman Flexibility Factor = (10 + 12h²)/(1 + 12h²) (used if KEYOPT(3)=2 and FLEX not input)

User Defined Flexibility Factors = FLXI (in-plane) and FLXO (out-of-plane) (may be input as any positive value)

Stress Intensification Factor = 0.9/h^2/3 or 1.0 (whichever is greater) (used for SIFI or SIFJ if factor not input or if input less than 1.0 (must be positive))

where:

h - tR/r²

t - thickness

R - radius of curvature

r - average radius

E - modulus of elasticity

P - P_i - P_o if P_i - P_o > 0, otherwise P = 0 P_i = internal pressure P_o = external pressure

X_k - 6 (r/t)^4/3 (R/r)^1/3 if KEYOPT(3)=1 and R/r >= 1.7, otherwise X_k=0

KEYOPT(3)=1 should not be used if the included angle of the complete elbow is less than 360/((R/r)) degrees.

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 4.18-1. 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. See Section 14.16.7 of the ANSYS Theory Reference for details.

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 pattern of input temperatures, unspecified temperatures default to TUNIF.

For piping analyses, the PIPE module of PREP7 may be used to generate the input for this element.

A summary of the element input is given in Table 4.18-1. A general description of element input is given in Section 2.1.

Table 4.18-1 PIPE18 Input Summary

Element Name	PIPE18
Nodes	I, J, K - where node K is in the plane of the elbow, on the center of curvature side of line I-J
Degrees of Freedom	UX, UY, UZ, ROTX, ROTY, ROTZ
Real Constants	OD, TKWALL, RADCUR, SIFI, SIFJ, FLXI, DENSFL, DENSIN, TKIN, TKCORR, (Blank), FLXO
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	Large deflection, Birth and death.
KEYOPT(1)	0 - Temperatures represent the through-wall gradient 1 - Temperatures represent the diametral gradient
KEYOPT(3)	Used only if FLXI real constant is not specified 0 - Use ANSYS flexibility factor (without pressure term) 1 - Use ANSYS flexibility factor (with pressure term) 2 - Use KARMAN flexibility factor
KEYOPT(6)	0 - No printout of member forces or moments 2 - Print member forces and moments in the element coordinate system

4.18.2 Output Data

• nodal displacements included in the overall nodal solution
• additional element output as shown in Table 4.18-2

The stresses are computed with the outer diameter of the pipe reduced by twice the corrosion thickness allowance. The direct stress includes the internal pressure (closed end) effect. Also printed for each end are the maximum and minimum principal stresses and the stress intensity. These quantities are computed at the outer surface and may not occur at the same location around the pipe circumference. Some of these stresses are shown in Figure 4.18-2. The direct stress does not include the axial component of the transverse thermal stress. The principal stresses and the stress intensity include the shear force stress component. Angles listed in the output are measured () as shown in Figure 4.18-2. 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 4.18-2 PIPE18 Stress Output

The following notation is used in Table 4.18-2:

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 4.18-2 PIPE18 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
FFACT	Element flexibility factor	-	Y
MFOR(X, Y, Z)	Member forces for nodes I and J (in the element coordinate system)	4	Y
MMOM(X, Y, Z)	Member moments for nodes I and J (in the element coordinate system)	4	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(1, 3, INT, EQV)	Maximum principal stress, minimum principal stress, stress intensity, equivalent stress	5	5
S(AXL, RAD, H, XH)	Axial, radial, hoop, and shear stresses	5	5
EPEL(AXL, RAD, H, XH)	Axial, radial, hoop, and shear strains	5	5
EPTH(AXL, RAD, H)	Axial, radial, and hoop thermal strain	5	5

1. If the value is greater than 0.

2. If KEYOPT(1)=0

3. If KEYOPT(1)=1

4. If KEYOPT(6)=2

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

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 4.18-3 through 4.18-3b:

Name - output quantity as defined in the Table 4.18-2

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
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	91	-	-	-	-	-	-	-	-
SSF	NMISC	92	-	-	-	-	-	-	-	-
MFORX	SMISC	1	-	-	-	-	-	-	-	-
MFORY	SMISC	2	-	-	-	-	-	-	-	-
MFORZ	SMISC	3	-	-	-	-	-	-	-	-
MMOMX	SMISC	4	-	-	-	-	-	-	-	-
MMOMY	SMISC	5	-	-	-	-	-	-	-	-
MMOMZ	SMISC	6	-	-	-	-	-	-	-	-
SDIR	SMISC	13	-	-	-	-	-	-	-	-
ST	SMISC	14	-	-	-	-	-	-	-	-
TOUT	LBFE	-	4	-	1	-	2	-	3	-
TIN	LBFE	-	8	-	5	-	6	-	7	-

Table 4.18-3a PIPE18 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
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	93	-	-	-	-	-	-	-	-
SSF	NMISC	94	-	-	-	-	-	-	-	-
MFORX	SMISC	7	-	-	-	-	-	-	-	-
MFORY	SMISC	8	-	-	-	-	-	-	-	-
MFORZ	SMISC	9	-	-	-	-	-	-	-	-
MMOMX	SMISC	10	-	-	-	-	-	-	-	-
MMOMY	SMISC	11	-	-	-	-	-	-	-	-
MMOMZ	SMISC	12	-	-	-	-	-	-	-	-
SDIR	SMISC	15	-	-	-	-	-	-	-	-
ST	SMISC	16	-	-	-	-	-	-	-	-
TOUT	LBFE	-	12	-	9	-	10	-	11	-
TIN	LBFE	-	16	-	13	-	14	-	15	-

Table 4.18-3b PIPE18 Item and Sequence Numbers for the ETABLE and ESOL Commands

Name	Item	E
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
FFACT	NMISC	90
STH	SMISC	17
PINT	SMISC	18
PX	SMISC	19
PY	SMISC	20
PZ	SMISC	21
POUT	SMISC	22

4.18.3 Assumptions and Restrictions

The element is limited to having an axis with a single curvature and a subtended angle of 0° < 90°. Shear deflection capability is also included in the element formulation. The elbow is assumed to have "closed ends" so that the axial pressure effect is included.

When used in a large deflection analysis, the location of the third node (K) is used only to initially orient the element.

4.18.4 Product Restrictions

ANSYS/LinearPlus

• The DAMP material property is not allowed.
• The only special feature allowed is large deflection.