INIPS

Bulk Data Entry Defines initial plastic strain values and settings for elements in nonlinear analysis.

Format


(1)	(2)	(3)	(4)	(5)	(6)	(7)	(8)	(9)	(10)
INIPS	`ID`	`ETYPE`	`CIDA`

The following continuation line(s) are optional when ETYPE = SHELL. They can be used to define the sections where initial plastic strain values are applied, and they need to be given before the continuation lines starting with EORS.


(1)	(2)	(3)	(4)	(5)	(6)	(7)	(8)	(9)	(10)
	`SECT`	`NSEC`	`SEC1`	`SEC2`	`SEC3`	etc.

The following continuation lines are used to define initial plastic strain values for an element or a set of elements. They are mandatory and can be repeated as required. Additionally, the optional HARD continuation line can be used to define equivalent plastic strain values and back stress values for an element or set of elements.


(2)	(3)	(4)	(5)	(6)	(7)
`EORS`	`EID`/`ESETID`	`CIDB`			etc.
`VALUE`	`PS1`	`PS2`	`PS3`	etc.
`HARD`	`EQVPLS`	`BKS1`	`BKS2`	`BKS3`	etc.

When ETYPE = SHELL and the SECT line is given, each VALUE line defines initial plastic strain for a shell section; and so, for any shell element (with EID) or shell element set (with ESETID), the number of VALUE lines must be NSEC.

The following optional continuation line is available if initial stress results from the external file (.h3d or .k file) are to be relocated.


(1)	(2)	(3)	(4)	(5)	(6)	(7)	(8)	(9)	(10)
	`RELOC`	`RTYPE`	`PA1`	`PA2`	`PA3`	`PB1`	`PB2`	`PB3`

The following optional continuation line can be used to specify the unit system of the external file. The units can either be defined using field 3 (that is, SI/CGS/MPA/BG) or by specifying units in fields 4, 5, 6 and 7. When fields 3 to 7 are all specified, only field 3 is considered and the following fields are ignored.


(1)	(2)	(3)	(4)	(5)	(6)	(7)	(8)	(9)	(10)
	`UNITS`	`SI`/`CGS`/`MPA`/`BG`	`MASS`	`FORCE`	`LENGTH`	`TIME`

Note: When the UNITS continuation line is defined and the length unit of the external H3D model differs from the current model’s length unit, the external H3D model is scaled to match the current model. In such cases, the RELOC continuation line must also be defined along with the UNITS continuation line. Defining these fields is not mandatory unless model scaling is required. If these entries are not specified, the default unit system is used.

Alternate Format (Initial Plastic Strain from H3D File)


(1)	(2)	(3)	(4)	(5)	(6)	(7)	(8)	(9)
INIPS	`ID`			`ASSIGN`	`SUBID`	`RSTYPE`
	`EORS`	`EID1`/`ESETID1`	`EID2`/`ESETID2`	`EID3`/`ESETID3`	`EID4`/`ESETID4`	`EID5`/`ESETID5`	`EID6`/`ESETID6`	`EID7`/`ESETID7`
		`EID8`/`ESETID8`

Example 1


(1)	(2)	(3)	(4)	(5)	(6)	(7)	(8)
INIPS	7
	`ELEM`	1001
	`VALUE`	3.33e-2	-1.67e-2	-1.67e-2	0.0	0.0	0.0
	`HARD`	5.0e-2
	`ESET`	200
	`VALUE`	3.33e-2	-1.67e-2	-1.67e-2	0.0	0.0	0.0
	`HARD`		50.0	50.0	0.0

Example 2


(1)	(2)	(3)	(4)	(5)	(6)
INIPS	8	SHELL	-1
	`SECT`	2
	`ELEM`	101
	`VALUE`	3.33e-2	0.0	0.0
	`VALUE`	-3.33e-2	0.0	0.0
	`ELEM`	102
	`VALUE`	3.33e-2	0.0	0.0
	`VALUE`	-3.33e-2	0.0	0.0
	`HARD`	3.33e-2	20.0	5.0	0.0
	`HARD`	3.33e-2	-20.0	-5.0	0.0

Example 3 (Alternate Format - Plastic Strain from H3D File)


(1)	(2)	(3)	(4)	(5)	(6)	(7)	(8)	(9)	(10)
INIPS	7			19	3
	`ELEM`	1001	2002	3003

Example 4 (Alternate Format - Plastic Strain from H3D File)


(1)	(2)	(3)	(4)	(5)	(6)
INIPS	8			29	6
	`ESET`	2	5	9
	`ESET`	9	19	29

Example 5 (Specify UNITS of the External File)


(1)	(2)	(3)	(4)	(5)	(6)	(7)	(8)	(9)	(10)
	`UNITS`	SI	KG	N	M	S

Definitions


Field	Contents	SI Unit Example
`ID`	Each INIPS Bulk Data Entry must have a unique ID. No default (Integer > 0)
`ETYPE`	Type of elements for which initial plastic strain is applied. Blank (Default) Applies initial plastic strain for a collection of solid and/or shell elements. SHELL Applies initial plastic strain for a collection of shell elements specifically.
`CIDA`	Coordinate system identification number or flag for the plastic strain components. Blank (Default) The initial plastic strain components are defined in the material coordinate system for solids and in element coordinate system for shells. -2 Components are defined in the material coordinate system. -1 Components are defined in the element coordinate system. 0 Components are defined in the basic coordinate system. Integer > 0 Components are defined in a user-defined (prescribed) coordinate system.
`SECT`	Keyword indicating the start of continuation line(s) for the shell sections.
`NSEC`	Number of shell sections where initial plastic strain is applied for shell elements. No default (1 ≤ Integer ≤ 6)
`SEC(i)`	Through-thickness position for the shell sections. `SEC(i)` must be either all blank or all non-blank, that is, the number of `SEC(i)` must be either `NSEC` or zero; and `SEC(i)` must be given in ascending order if all non-blank. If left blank, this implies the sections are located uniformly through the shell thickness, starting at the bottom surface and ending at the top surface. A Real value is the multiplier to shell thickness to find the location. -0.5 is the bottom surface of the shell element and 0.5 is the top surface. The through-thickness positive direction, pointing from the bottom surface to the top surface, is determined by the right-hand rule and the order in which the grid points are listed on the connection entry. It is the same as the convention for `Z1`/`Z2` of PSHELL. Default = Blank (Blank or -0.5 ≤ Real ≤ 0.5)
`EORS`	Flag indicating an element, or an element SET is selected in the following field. ELEM (Default) Element is selected. ESET Element SET is selected.
`EID`/`ESETID`	Identification number of the element or the element SET to which the plastic strain values apply. No default (Integer > 0)
`CIDB`	Coordinate system identification number or flag for the plastic strain components. Blank (Default) This implies `CIDA` is used. All other options suppress `CIDA`. -2 Initial plastic strain components are defined in the material coordinate system. -1 Components are defined in the element coordinate system. 0 Components are defined in the basic coordinate system. Integer > 0 Components are defined in a user-defined (prescribed) coordinate system.
`VALUE`	Keyword indicating the start of a continuation line for the plastic strain components.
`PS(i)`	Plastic strain components. 4 No default (Real)
`HARD`	Continuation line to define plastic hardening information.
`EQVPLS`	Value of the equivalent plastic strain. Default = Blank (Real)
`BKSi`	Values of the back stresses. Default = Blank (Real)
Alternate Format Description (plastic strain from H3D file)
`ASSIGN`	Identification number of ASSIGN, H3DRES. When `ASSIGN` is specified, `SUBID` should also be specified and the `VALUE` continuation line is not allowed. This field is mandatory for Alternate Format (plastic strain from H3D file). No default (Integer > 0)
`SUBID`	Subcase identification number where initial plastic strain is applied from the H3D file. This field is mandatory for Alternate Format (plastic strain from H3D file). No default (Integer > 0)
`EORS`	Flag indicating an element, or an element SET is selected in the following field. ELEM (Default) Element is selected. ESET Element SET is selected.
`EID#`/`ESETID#`	Identification number of the element or the element SET to which the plastic strain values apply. No default (Integer > 0)
`RSTYPE`	Results type to read in from the specified H3D file. TENS Read in plastic strain tensor only. HARD Read in hardening information including equivalent plastic strain and back stress, if they exist in the H3D file. BOTH Read in plastic strain tensor and hardening information. blank (Default) Read in plastic strain tensor only.
`RELOC`	Activates the Relocation option. 6 The matching grid point ID pairs in the model and external result file are to follow.
`RTYPE`	Relocation type. MATCH (Default) The result from the external result file is relocated using 3 pairs of matching grids in the model (`PA1`, `PA2`, `PA3`) and the external result file (`PB1`, `PB2`, `PB3`). MIRROR The result from the external result file is laterally mirrored according to the plane defined by grid points (`PB1`, `PB2`, `PB3`). Then it is relocated and mapped.
`PA1`, `PA2`, `PA3`	IDs of three non-collinear grid points in the model.
`PB1`, `PB2`, `PB3`	IDs of three non-collinear grid points in model from the external result file that are matched to corresponding grid points in the structure (`PA1`, `PA2`, `PA3`, respectively).
`UNITS`	SI International System of Units Length: Meter = m Mass: Kilogram = kg Time: Second = s Temperature: Kelvin = K Pressure: Pa CGS Centimeter-gram-second System of Units Length: Centimeter = cm Mass: Gram = g Time: Second = s Temperature: Kelvin = K Pressure: Bayre = 0.1 Pa MPA Mega Length: Millimeter = mm Mass: Tonne = tonne Time: Second = s Temperature: Kelvin = K Pressure: MPa BG British Gravitational System of Units Length: Feet = ft Mass: Slug = slug Time: Second = s Temperature: Rankine = R Pressure: lbf/ft² No default
`MASS`	Units of mass. kg (Default) Kilogram lbm Pound-mass slug Slug gram Gram ozm Ounce-mass klbm Kilo pound-mass (1000.lbm) mgg Megagram slinch 12 slugs ug Microgram ng Nanogram uston US ton mg Milligram
`FORCE`	Units of force. N (Default) Newton lbf Pound-force kgf Kilograms-force ozf Ounce-force dyne Dyne kn Kilonewton klbf Kilo pound-force (1000.lbf) mn Millinewton un Micronewton nn Nanonewton
`LENGTH`	Units of length. mm (Default) Millimeter km Kilometer m Meter cm Centimeter mi Mile ft Foot in Inch um Micrometer nm Nanometer ang Angstrom yd Yard mil Milli-inch uin Micro-inch
`TIME`	Units of time. s (Default) Seconds h Hours min Minutes ms Milliseconds us Microsecond nanosec Nanosecond d Day

Comments

INIPS and IPSADD should not have the same ID.
The INIPS Bulk Data Entry is selected by the Subcase Information Entry INIPS.
Initial plastic strain is only supported for nonlinear static analysis (both small and large displacement analysis). Initial plastic strain is supported for solid elements (CHEXA, CPENTA, CPYRA and CTETRA) and shell elements (CQUAD4, CTRIA3, CQUAD8 and CTRIA6), only.
Initial plastic strain is currently not supported for:
- Solid elements with user-defined material in LGDISP analysis.
- Elements with MATMDS material.
For initial plastic strain of solid elements, the following 6 plastic strain components are needed for each VALUE:
- $PS1 - ε_{xx}^{p}$
- $PS2 - ε_{yy}^{p}$
- $PS3 - ε_{zz}^{p}$
- $PS4 - ε_{xy}^{p}$
- $PS5 - ε_{yz}^{p}$
- $PS6 - ε_{zx}^{p}$
Where x, y, and z are the axes of the coordinate system selected via CIDA and CIDB.
For initial plastic strain in element or material coordinate system of shell elements, the following 3 plastic strain components are needed for each VALUE line:
- $PS1 - ε_{11}^{p}$
- $PS2 - ε_{22}^{p}$
- $PS3 - ε_{12}^{p}$
Where 1 and 2 are the first two local directions in the element or material coordinate system.
For initial plastic strain in the basic or a prescribed coordinate system of shell elements, the following 6 plastic strain components are needed for each VALUE line:
- $PS1 - ε_{xx}^{p}$
- $PS2 - ε_{yy}^{p}$
- $PS3 - ε_{zz}^{p}$
- $PS4 - ε_{xy}^{p}$
- $PS5 - ε_{yz}^{p}$
- $PS6 - ε_{zx}^{p}$
Where, x, y, and z are the axes of the basic or prescribed coordinate system.
Alternate Format (Plastic strain from H3D file):
1. VALUE continuation line is not allowed for the Alternate Format when plastic strain is sourced from the H3D file.
2. For shell elements, currently only the equivalent of NSEC=2 is supported (Z1 and Z2 layers) to apply the plastic strain, as the number of layers where plastic strain data is available can be identified from the H3D file.
3. Currently, only H3D files output from OptiStruct and HyperForm are supported.
Relocation continuation line:
The RELOC entry and its related fields define three matching grid point pairs on the model and the external result file. The result from the external file is relocated (translated and rotated, as required) such that the three non-collinear grid points PB1, PB2 and PB3 coincide with PA1, PA2, and PA3, respectively.