*element_beam_elbow added in R7.1.1.
Internal note:
see ~/doc/elbow
__________________________________________________________________
Date: 2014-01-13 06:14:44 -0800 (Mon, 13 Jan 2014)
Log:
Add options LARGE and NHISV to INITIAL_STRESS_BEAM.
_______________________________________________________
Note the addition of beam bulk viscosity as an option of *control_bulk_viscosity
(2nd edition of the 971 Users Manual).
If you want to input A, Iss, etc. directly, you must use a resultant beam formulation,
i.e., ELFORM=2. With such a formulation, stresses are not calculated because the shape
of the cross-section is unknown. You'll only get forces and moments.
ELFORM 2 is compatible with only a few material types. See the material table at the
beginning of the *MAT section of the Users Manual.
(See also: ~/doc/beam_type2)
ELFORM 1 is an integrated beam formulation. With an integrated formulation, the shape
of the cross-section is defined in the input and so stresses can be computed at the
beam integration points. The parameter CST on Card 1 of *section_beam indicates
whether the section is circular or rectangular. You must give cross-section dimensions
on Card 2 of *section_beam. For circular sections, you give outside and inside diameters
at the two ends. (For a solid circular section, the inside diameter is zero.)
For solid rectangular sections, you give the cross-section width and breadth at the two ends.
For hollow rectangular tubes, it's a bit trickier as you must also use *integration_beam
which is referenced by setting QR/IRID in *section_beam to -IRID where IRID is given
in *integration_beam. In *integration_beam, you can leave NIP and RA blank and set
ICST to 5. On Card 2 of *integration_beam, give the 4 values W, TF, D, and TW are
shown in the figure in the Users Manual.
If QR/IRID in *section_beam is negative, it follows that *integration_beam defines
the location of the integration points.
If QR/IRID is positive and CST is zero (rectangular section), refer to the Figure 5.3
on p. 5.11 of the 2006 Theory Manual (download pdf from www.lstc.com).
If the integration rule is 2x2, 3x3, or 4x4 Gaussian, the locations of the integration points shown
in Figure 5.3 are in accordance with the columns labeled as 2 point, 3 point, and 4 point, resp.,
in the table under *section_shell in the Users Manual.
Integration points for a circular cross-section are positioned sequentially in the
circumferential direction of the cross-section, all at the same distance from the
cross-section center. For example, for 3x3 Guass quadrature, the nine integration points
in the cross-section are 40 degrees apart with the first integration point on a ray
20 degrees off the local s-axis (toward the t-axis) .
An example of an elastic, cantilever beam in simple bending
(http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/hlbeam.9vs16ip.circular.k),
confirms that the radial position of the integration points for a circular cross section is
r = sqrt( (ro^2 + ri^2)/2 )
There appears to be no difference between 3x3 Gaussian and 3x3 Lobatto in the case of a
circular cross section.
For a rectangular section with QR/IRID to 4, which will give 3x3 Lobatto quadrature, and the
integration points will be at the corners (4), edge midpoints (4) and at the center (1).
(Ref: Ticket#2018052410000037)
Axial stresses and bending moments are reported to elout.
In *initial_stress_beam, RULE defines the number and location of the integration points.
NPTS says how many of those integration points are initialized in the
lines that follow. I would guess that 99.999% of the time, you would
want to initialize all the integration points and not a subset
thereof. But the http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/hlbeam.3gaussvs3lobatto.circular.initstress.k
illustrates you don't have to do it that way.
You can get axial strain at beam integration points by setting
BEAMIP (*database_extent_binary) to the number of beam integration points
in your LS-DYNA input deck. Then, after running the model, read d3plot into
LS-PrePost and click History > Int.Pt. > Etype: Beams > (click on any beam element) > Axial Strain > Plot.
STRFLG is not used. elout does not report beam strains.
The strain tensor is not written to elout but
plastic strain at beam integration points is written to elout
(see *database_history_beam and *database_elout in the Users Manual).
http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/hlbeam.4vs9ip.k
After t=0, the cross-section orientation of beams shown in prism mode
(Toggle > Beam Prism) by LS-PrePost is random
UNLESS each beam is given a unique N3 and NREFUP in *control_output is set to 1.
If N3 is not unique to each beam element, the cross-section orientation
of the beams remains correct internally in LS-DYNA, that is, the results are fine. The only
disadvantage is that LS-PrePost has no way to know the cross-section orientation when displaying the
beams as prisms.
__________________________________________________
More regarding use of different materials within *integration_beam...
codes on 07/18/2006 at 04:43:03 (971/rev 8355)
Added ability for beam integration rules to specify a different
part ID at each integration point. Within the same integration
rule, the material types must all be the same (including the
material referred to by the parent part). See below for application.
I have increased the storage in a(n4g) and re-dimensioned the array
rule to (mpubr,4,*) - used to be (mpubr,3,*) - wherever it occurs.
The main changes are in rdintb, wtbir, intrlb, hughbm (and the same
code was added to beswbm, warpbm, hughbm_n - these are the only other
beam elements that use integration rules).
Existing models are unaffected.
Richard Sturt, 18 July 2006
User integration rules for beams can now have different materials
at each integration point. All the materials must be of the same
type (including the material referred to on the main PART card) but
the properties may be different. One use of this is for reinforced
concrete, using *MAT_CONCRETE_EC2 or *MAT_RC_BEAM - these materials
can represent concrete or reinforcement according to the input
properties, so it is possible to position the reinforcement within
the section.
This facility is accessed via *INTEGRATION_BEAM with
NIP>0. For each integration point, the fourth field is now an optional
Part ID. The material referred by that Part will be used at the
integration point.
______________________________________________________
See bugzilla 7763, 7765 for issues affecting *INTEGRATION_BEAM.
7763: Comment #3 from Lee Bindeman 2012-10-10 13:29:07 PDT ---
I found 6 beams have improper location of integration points causing the wrong
beam stiffness, ICST= 14, 16, 17, 18, 21, and 22. I fixed them in trunk, R7.0,
R6.1, and R6.1 at revs 76974 to 76977. Thanks Jim for preparing the simple
data file.
7765:
Concerns beam rule ID number limits and echo to d3hsp
Internal ID limit increasd from 4 to 6 digits; external ID limit is 2*32-1
Echo external ID in d3hsp.
______________________________________________________
More on ELFORM 1...
Yield of H-L beam integration points is based on sigeff = sqrt (sigrr^2 + 3(sigrs^2 + sigtr^2))
where r, s, and t are the beam local axes.
(see http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/spotweld.beam9.k)
The attached 1-beam example illustrates that the beam fails when the
average effective plastic strain reaches the FAIL value specified in mat_024.
Thus the failure strain may be exceeded at some integration points.
http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/beam.cantil.hlyield.k
If mat_003 is used, each IP fails independently.
______________________________________________
The maximum moment is a function of the integration scheme. Stresses are calculated only at
integration points. Based on the location of the integration points, the weighting factors, and the
stresses, a moment is calculated. If you plot the r-stress at the integration points (via elout file), you'll
see that the stress is in accordance with the constitutive model. If you use 4x4 Gauss integration
(QR/IRID=5), the stress profile is more realistic than with 2x2 Gauss integration and the maximum
moment is closer to the analytic plastic moment.
Based on the original 2x2 Gaussian integration, the maximum moment can be calculated as
follows:
M = 4 IP * stress * IP area * moment arm
M = 4 * .0124 * (500 * 1000)/4 * (0.5773 * 500/2) = 894,815
http://ftp.lstc.com/anonymous/outgoing/support/FAQ_kw/mplas_hl_impl.k