*element_beam_elbow added in R7.1.1. Internal note: see ~/doc/elbow __________________________________________________________________ RE: Shift of neutral axis due to int.pt. damage or failure Author: lpb Date: 2019-03-04 17:50:49 -0800 (Mon, 04 Mar 2019) New Revision: 10900 Modified: trunk/Vol_I_Keyword/SECTION_BEAM.docx Log: Added a description for a new option called NAUPD. This neutral axis update option causes the neutral axis of integrated beams to be recalculated when damage or failure occurs at one or more integration points. 11. NAUPD. Integrated beams have integration points arranged about a neutral axis. Axial stress at each point will generate both an axial force and a moment at each node. The moment is proportional to the distance from the neutral axis. For a pure axial load, the moments cancel and only the force remains. However, if damage or failure occurs at one or more integration points, then the moments will no longer cancel and an axial load will produce moments at the nodes. To prevent this default behavior, set NAUPD to 1 to activate the neutral axis update option. With this option, the neutral axis will be updated such that partially failed elements will continue to generate balanced moments during axial loading. This option applies to beam forms 1, 9, 11, and 14 when used with material types 3, 98, 100, 124, and 158. __________________________________________________________________ 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 See bug 15474 regarding output of beam strains. 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