## *EL FILE

Keyword type: step

This option is used to save selected element variables averaged at the nodal points in a frd file (extension .frd) for subsequent viewing by CalculiX GraphiX. The following element variables can be selected (the label is square brackets [] is the one used in the .frd file; for frequency calculations with cyclic symmetry both a real and an imaginary part may be stored, in all other cases only the real part is stored):

• CEEQ [PE]: equivalent creep strain (is converted internally into PEEQ since the viscoplastic theory does not distinguish between the two; consequently, the user will find PEEQ in the frd file, not CEEQ)
• E [TOSTRAIN (real),TOSTRAII (imaginary)]: strain. This is the total Lagrangian strain for (hyper)elastic materials and incremental plasticity and the total Eulerian strain for deformation plasticity.
• ECD [CURR]: electrical current density. This only applies to electromagnetic calculations.
• EMFB [EMFB]: Magnetic field. This only applies to electromagnetic calculations.
• EMFE [EMFE]: Electric field. This only applies to electromagnetic calculations.
• ENER [ENER]: the energy density.
• ERR [ERROR (real), ERRORI (imaginary)]: error estimator for structural calculations (cf. Section 6.12). Notice that ERR and ZZS are mutually exclusive.
• HER [HERROR (real), HERRORI (imaginary)]: error estimator for heat transfer calculations(cf. Section 6.12).
• HFL [FLUX]: heat flux in structures.
• HFLF [FLUX]: heat flux in CFD-calculations.
• MAXE [MSTRAIN]: maximum of the absolute value of the worst principal strain at all times for *FREQUENCY calculations with cyclic symmetry. It is stored for nodes belonging to the node set with name STRAINDOMAIN. This node set must have been defined by the user with the *NSET command. The worst principal strain is the maximum of the absolute value of the principal strains times its original sign.
• MAXS [MSTRESS]: maximum of the absolute value of the worst principal stress at all times for *FREQUENCY calculations with cyclic symmetry. It is stored for nodes belonging to the node set with name STRESSDOMAIN. This node set must have been defined by the user with the *NSET command. The worst principal stress is the maximum of the absolute value of the principal stresses times its original sign.
• ME [MESTRAIN (real), MESTRAII (imaginary)]: strain. This is the mechanical Lagrangian strain for (hyper)elastic materials and incremental plasticity and the mechanical Eulerian strain for deformation plasticity (mechanical strain = total strain - thermal strain).
• PEEQ [PE]: equivalent plastic strain.
• PHS [PSTRESS]: stress: magnitude and phase (only for *STEADY STATE DYNAMICS calculations and *FREQUENCY calculations with cyclic symmetry).
• S [STRESS (real), STRESSI (imaginary)]: true (Cauchy) stress in structures. For beam elements this tensor is replaced by the section forces if SECTION FORCES is selected. Selection of S automatically triggers output of the error estimator ERR, unless NOE is selected after S (either immediately following S, or with some other output requests in between, irrespective whether these output requests are on the same keyword card or on different keyword cards).
• SF [STRESS]: total stress in CFD-calculations.
• SMID [STRMID]: true (Cauchy) stress at the midsurface of a shell. This can only be used for shell elements which have been defined as user elements. It cannot be used of shell elements the label of which starts with S, since these are expanded into volumetric elements.
• SNEG [STRNEG]: true (Cauchy) stress at the negative surface of a shell. This can only be used for shell elements which have been defined as user elements. It cannot be used of shell elements the label of which starts with S, since these are expanded into volumetric elements.
• SPOS [STRPOS]: true (Cauchy) stress at the positive surface of a shell. This can only be used for shell elements which have been defined as user elements. It cannot be used of shell elements the label of which starts with S, since these are expanded into volumetric elements.
• SVF [VSTRES]: viscous stress in CFD-calculations.
• SDV [SDV]: the internal state variables.
• THE [THSTRAIN]: strain. This is the thermal strain calculated by subtracting the mechanical strain (extrapolated to the nodes) from the total strain (extrapolated to the nodes) at the nodes. Selection of THE triggers the selection of E and ME. This is needed to ensure that E (the total strain) and ME (the mechanical strain) are extrapolated to the nodes.
• ZZS [ZZSTR (real), ZZSTRI (imaginary)]: Zienkiewicz-Zhu improved stress [100], [101](cf. Section 6.12). Notice that ZZS and ERR are mutually exclusive.

The selected variables are stored for the complete model. Due to the averaging process jumps at material interfaces are smeared out unless you model the materials on both sides of the interface independently and connect the coinciding nodes with MPC's.

For frequency calculations with cyclic symmetry the eigenmodes are generated in pairs (different by a phase shift of 90 degrees). Only the first one of each pair is stored in the frd file. If S is selected (the stresses) two load cases are stored in the frd file: a loadcase labeled STRESS containing the real part of the stresses and a loadcase labeled STRESSI containing the imaginary part of the stresses. For all other variables only the real part is stored.

The key ENER triggers the calculation of the internal energy. If it is absent no internal energy is calculated. Since in nonlinear calculations the internal energy at any time depends on the accumulated energy at all previous times, the selection of ENER in nonlinear calculations (geometric or material nonlinearities) must be made in the first step.

The first occurrence of an *EL FILE keyword card within a step wipes out all previous element variable selections for file output. If no *EL FILE card is used within a step the selections of the previous step apply. If there is no previous step, no element variables will be stored.

There are ten optional parameters: FREQUENCY, FREQUENCYF, GLOBAL, OUTPUT, OUTPUT ALL, SECTION FORCES, TIME POINTS, NSET, LAST ITERATIONS and CONTACT ELEMENTS. The parameters FREQUENCY and TIME POINTS are mutually exclusive.

FREQUENCY applies to nonlinear calculations where a step can consist of several increments. Default is FREQUENCY=1, which indicates that the results of all increments will be stored. FREQUENCY=N with N an integer indicates that the results of every Nth increment will be stored. The final results of a step are always stored. If you only want the final results, choose N very big. The value of N applies to *OUTPUT,*ELEMENT OUTPUT, *EL FILE, *ELPRINT, *NODE OUTPUT, *NODE FILE, *NODE PRINT, *SECTION PRINT ,*CONTACT OUTPUT, *CONTACT FILE and *CONTACT PRINT. If the FREQUENCY parameter is used for more than one of these keywords with conflicting values of N, the last value applies to all. A frequency parameter stays active across several steps until it is overwritten by another FREQUENCY value or the TIME POINTS parameter.

The 3D fluid analogue of FREQUENCY is FREQUENCYF. In coupled calculations FREQUENCY applies to the thermomechanical output, FREQUENCYF to the 3D fluid output.

With the parameter GLOBAL you tell the program whether you would like the results in the global rectangular coordinate system or in the local element system. If an *ORIENTATION card is applied to the element at stake, this card defines the local system. If no *ORIENTATION card is applied to the element, the local system coincides with the global rectangular system unless for shell elements, for which a local system is automatically defined by default (cf. Section 6.2.14). Default value for the GLOBAL parameter is GLOBAL=YES, which means that the results are stored in the global system (the only exception to this is for the shell stresses SNEG, SMID and SPOS, which are always stored in the shell local system). If you prefer the results in the local system, specify GLOBAL=NO.

The parameter OUTPUT can take the value 2D or 3D. This has only effect for 1d and 2d elements such as beams, shells, plane stress, plane strain and axisymmetric elements AND provided it is used in the first step. If OUTPUT=3D, the 1d and 2d elements are stored in their expanded three-dimensional form. In particular, the user has the advantage to see his/her 1d/2d elements with their real thickness dimensions. However, the node numbers are new and do not relate to the node numbers in the input deck. Once selected, this parameter is active in the complete calculation. If OUTPUT=2D the fields in the expanded elements are averaged to obtain the values in the nodes of the original 1d and 2d elements. In particular, averaging removes the bending stresses in beams and shells. Therefore, default for beams and shells is OUTPUT=3D, for plane stress, plane strain and axisymmetric elements it is OUTPUT=2D. If OUTPUT=3D is selected, the parameter NSET is deactivated.

The parameter OUTPUT ALL specifies that the data has to be stored for all nodes, including those belonging to elements which have been deactivated. Default is storage for nodes belonging to active elements only.

The selection of SECTION FORCES makes sense for beam elements only. Furthermore, SECTION FORCES and OUTPUT=3D are mutually exclusive (if both are used the last prevails). If selected, the stresses in the beam nodes are replaced by the section forces. They are calculated in a local coordinate system consisting of the 1-direction , the 2-direction and 3-direction or tangential direction (Figure 74). Accordingly, the stress components now have the following meaning:

• xx: Shear force in 1-direction
• yy: Shear force in 2-direction
• zz: Normal force
• xy: Torque
• xz: Bending moment about the 2-direction
• yz: Bending moment about the 1-direction

For all elements except the beam elements the parameter SECTION FORCES has no effect. If SECTION FORCES is not selected the stress tensor is averaged across the beam section.

With the parameter TIME POINTS a time point sequence can be referenced, defined by a *TIME POINTS keyword. In that case, output will be provided for all time points of the sequence within the step and additionally at the end of the step. No other output will be stored and the FREQUENCY parameter is not taken into account. Within a step only one time point sequence can be active. If more than one is specified, the last one defined on any of the keyword cards *NODE FILE, *EL FILE, *NODE PRINT or *EL PRINT will be active. The TIME POINTS option should not be used together with the DIRECT option on the procedure card. The TIME POINTS parameters stays active across several steps until it is replaced by another TIME POINTS value or the FREQUENCY parameter.

The specification of a node set with the parameter NSET limits the output to the nodes contained in the set. Remember that the frd file is node based, so element results are also stored at the nodes after extrapolation from the integration points. For cyclic symmetric structures the usage of the parameter NGRAPH on the *CYCLIC SYMMETRY MODEL card leads to output of the results not only for the node set specified by the user (which naturally belongs to the base sector) but also for all corresponding nodes of the sectors generated by the NGRAPH parameter. Notice that for cyclic symmetric structures in modal dynamic and steady state dynamics calculations the use of NSET is mandatory. In that case the stresses will only be correct at those nodes belonging to elements for which ALL nodal displacements were requested (e.g. by a *NODE FILE card).

The parameter LAST ITERATIONS leads to the storage of the displacements in all iterations of the last increment in a file with name ResultsForLastIterations.frd (can be opened with CalculiX GraphiX). This is useful for debugging purposes in case of divergence. No such file is created if this parameter is absent.

Finally, the parameter CONTACT ELEMENTS stores the contact elements which have been generated in each iteration in a file with the name jobname.cel. When opening the frd file with CalculiX GraphiX these files can be read with the command “read jobname.cel inp” and visualized by plotting the elements in the sets contactelements_st_in_at_it, where is the step number, the increment number, the attempt number and the iteration number.

Starting with version 2.14 of CalculiX the selection of “S” (stress) automatically triggers the output the stress error estimator “ERR” as well. This can only be avoided by selecting NOE in a position after S (either immediately following S, or with some other output requests in between, irrespective whether these output requests are on the same keyword card or on different keyword cards).

First line:

• *EL FILE
• Enter any needed parameters and their values.
Second line:
• Identifying keys for the variables to be printed, separated by commas.

Example:

*EL FILE
S,PEEQ


requests that the (Cauchy) stresses and the equivalent plastic strain is stored in .frd format for subsequent viewing with CalculiX GraphiX.

Example files: beamt, fullseg, segment1, segdyn.