Job Parameters

Marc > Running an Analysis > Job Parameters

XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">XXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXXX''">

Job Parameters

This subordinate form appears when the Job Parameters button is selected on the Analysis application form. Parameters on this form and its subordinate forms control non-solution specific parameters that generally are placed in the Parameter or Model Definition sections of the Marc input file.

The widgets in the above form are explained in the table below.


Translation Parameter	Description
Marc Version	This can be set to 2007 (default), 2005, 2003 , 2001, 2000, or K7. Some of the forms and settings key off of this setting. This only controls what forms and values are presented to you when setting up an analysis and what is written to the input file. It does not directly control what version of Marc is actually run. This is done via the P3_Trans.ini file on NT or the site_setup file on UNIX. See Analysis Submission Configuration. If 2005, a VERSION,11 parameter is written. If 2003, a VERSION,10 parameter is written. This parameter indicates version specific option formats.
Output File Format	Can be K2, K3, K4, K5, K6, K7, 2000, 2001, 2003 2005, or 2007. The default the same as the Marc Version. This parameter generally places either a 1, 3, 4, 5, 6, 7, 9, 10, 11 or 12, respectively, in the 11th field of the 2nd data block of the POST option. If the Marc Version is the same, then a zero (0) is placed in this field indicating that a POST file of the latest format be written. You cannot set this to a higher version than the Marc Version is set at.
Results File Type	Can be Binary (default), Text, Both, or None. This parameter places either a 0, 1, or 2, respectively, in the 4th field of the 2nd data block of the POST option. If none is selected, no POST option is written.
Assumed Strain	If ON, (default is OFF), places the ASSUMED parameter into the input file. This will force all elements that can deal with assumed strain to use this formulation. This improves the bending behavior of elements 3, 7, and 11. If you wish to control this formulation option for each individual element property set, you must turn this setting OFF.
Constant Dilatation	If ON, (default is ON for Structural/Coupled, OFF for Thermal), places the CONSTANT parameter into the input file. This will force all elements that can deal with constant dilatation (for nearly incompressible analysis) to use this formulation. This affects element types 7, 10, 11, 19, and 20 only and recommended for elastic-plastic and creep analysis. If you wish for each individual element property set to define this separately, you must turn this setting OFF.
Element Centroid Method	If ON, (default is OFF), places the CENTROID parameter into the input file. It is not recommended with non-linear analysis as results are stored at the centroid of each element only and thus it reduces accuracy.
Lumped Matrix	If ON, (default is OFF), places the LUMP parameter into the input file. This is only used for dynamics (lumped mass matrix) or heat transfer (lumped specific heat matrix) and will be ignored for any other analysis type.
Heat Generation Conversion Factor	For Coupled analysis only, this factor can be provided as a conversion factor between inelastic mechanical energy and heat transfer flux. Default is 1.0.
Extended Format	If this is ON, the Marc input file is created in extended format, thus doubling the field width of each entry in the input file. The EXTENDED parameter is placed in the input file. This is ON by default. If Free Field is also ON, the actual field length is only extended when necessary. You cannot turn this OFF if Free Format is ON.
Free Format	If this is set, free field input formats will be used when creating the Marc input file. Fields are separated by commas in the input file but still placed within the normal fixed field width. This is ON by default. You cannot have Extended Format OFF when Free Format is ON.
# of Significant Digits	Defines the number of significant digits to be used when creating the Marc input file. This can be set to any value in the range of three through eight depending on whether extended format is requested or not.
Use Tables: Materials LBCs Contact	Available only when Marc Version is set to 2003 or greater. When this toggle is ON, the TABLE option will be used to write data defined by fields such as time varying loads or temperature varying material properties. Anything that can be described via the TABLE option will be if this option is ON. You can control Materials, Loads and BCs, and Contact tables separately. Additional toggles apprear when this toggle is ON to do so.
Loads on Geometry	If ON, (default is OFF), uses POINTS, CURVES, SURFACES, ATTACH NODES, ATTACH ELEMENT, ATTACH EDGE, and ATTACH FACE options in conjuction with TABLES (Use Tables must be ON also). This associates loads and boundary conditions to geomtric entities directly in the input file using the above options. This is most useful when used in conjunction with adaptive meshing where the mesh can change but the loads remain consistent and not dependent on a node or element number that changes due to remeshing. See the discussion below in Loads on Geometry, 188. Valid only for Marc Version 2003 or greater. Note: This is not fully supported at this time.

Loads on Geometry

The following geometric entities can be written to the Marc input file into the Model Definition section in Marc Version 2003 and beyond.

1. POINTS - this is a simple definition:

Data Block 1: POINTS

Data Block 2: # of points defined

Data Block 3: Point ID, X-coord, Y-coord, Z-coord

For POINTS to be properly used in an input file, FEM nodes must be attached to them via the ATTACH NODE option which is already supported for adaptive meshing (except in that case they are attached to SURFACEs)

ATTACH NODE is used to attach nodes to POINTS in the case of POINT LOAD, POINT FLUX, FIXED DISP, FIXED TEMP and any other nodal based LBC. The typical scenario for this is that one of these LBC types has an application region of Patran points. These points are associated to Patran nodes. Thus the POINTS option is used to write the points to the input file. The ATTACH NODE option is used to associate the associated Patran nodes to the POINTS option. The LBC type is written to the input file with the geometric ids in the blocks requesting the geometry type and IDs.

2. CURVES - this is a bit more complicated:

Data Block 1: CURVES

Data Block 2: # of curves defined

Data Block 3: Curve ID, curve type (always 4 for 2-D NURB curve)

Data Block 4-7: NURB definition

For CURVES to be properly used in an input deck, FEM nodes must be attached to them via the ATTACH NODE option or FEM element edges must be associated using the ATTACH EDGE option. This is dependent on the LBC type being defined.

ATTACH NODE is used to attach nodes to CURVES in the case of POINT LOAD, POINT FLUX, FIXED DISP, FIXED TEMP and any other nodal based LBC. ATTACH EDGE is used to attach element edges to CURVES in the case of distributed loads or films or other element based LBCs. The typical scenario for this is that one of these LBC types has an application region of Patran curves (edges). These curves are associated to Patran nodes or element edges depending on whether the LBC is nodal or element based. Thus the CURVES option is used to write the Patran curves to the input deck. The ATTACH NODE option is used to associate the associated Patran nodes to the CURVES in the case of nodal LBCs. The ATTACH EDGE option is used to associate the associated Patran element edges to the CURVES in the case of element based LBCs. The LBC type is written to the input deck with the geometric ids in the blocks requesting the geometry type and IDs.

3. SURFACES - this is basically same as CURVES:

Data Block 1: SURFACES

Data Block 2: # of surfaces defined

Data Block 3: Surface ID, surface type (always 4 for 2-D NURB surface)

Data Block 4-7: NURB definition

For SURFACES to be properly used in an input deck, FEM nodes must be attached to them via the ATTACH NODE option or FEM element faces must be associated using the ATTACH FACE option. This is dependent on the LBC type being defined.

ATTACH NODE is used to attach nodes to SURFACES in the case of POINT LOAD, POINT FLUX, FIXED DISP, FIXED TEMP and any other nodal based LBC. ATTACH FACE is used to attach shell elements or solid element faces to SURFACES in the case of distributed loads or films or other element based LBCs. The typical scenario for this is that one of these LBC types has an application region of Patran surfaces (or faces). These surfaces are associated to Patran nodes or shell elements or solid element faces depending on whether the LBC is nodal or element based. Thus the SURFACES option is used to write the Patran surfaces to the input deck. The ATTACH NODE option is used to associate the associated Patran nodes to the SURFACES in the case of nodal LBCs. The ATTACH FACE option is used to associate the associated Patran shell elements or solid element faces to the SURFACES inthe case of element based LBCs. The LBC type is written to the input deck with the geometric ids in the blocks requesting the geometry type and IDs.

The actual option that is written is dependent on the Patran goemetric entity in the application region. In general, the same type of geometry is written to the Marc input deck. The edge and face IDs necessary to define and associate FEM with geometry are listed in Vol C under FACE IDS.

The following table shows the applicable load and boundary condition types that can be associated with geometric entities written to the Marc input deck. It also shows the relation between the Patran geometric application region and what is written to the Marc input deck.


LBC Type	Patran Application Region	Required Marc Options	Geometry Type ID
FIXED DISP FIXED TEMP POINT LOADS POINT FLUX INITIAL DISP INITIAL VEL INITIAL TEMP	Nodes	None	2: Nodes ids
	Points	POINTS ATTACH NODES	6: Point ids
	Curves and/or Edges	CURVES ATTACH NODES	5: Curve ids
	Surfaces and/or Faces	SURFACES ATTACH NODES	4: Surface Ids
	Solids	Not yet fully defined ATTACH ELEMENT	3: Volume ids
DIST LOADS DIST FLUXES FILMS	Elements	None	1: Element ids
	Curves and/or Edges	CURVES ATTACH EDGE	5: Curve ids
	Surfaces and/or Faces	SURFACES ATTACH FACE	4: Surface ids
	Solids	Not yet fully defined ATTACH ELEMENT	3: Volume ids

There can be different mixes and matches of geometry types defined for a single LBC. Marc Vol C , Program Input explains that this is handled in the 3rd data block of each LBC type above where the number of geometric types is specified. The 6th & 7th (or 7th & 8th) data blocks are then repeated for each type of geometry.

Solvers / Options

The following form appears for selecting Solvers and other Options on the Job Parameters form. The table below explains each parameter for each solver or option. This places the SOLVER and OPTIMIZE option and the MPC-CHECK parameter into the input deck.


Solver Parameter	Description
Inconsistent MPCs	This option (available for Marc version 2005 or higher) can be set to Reorder (default), Continue or Stop. The order in which ties were applied previously to 2005 was fixed and determined in the order in which they were given in the input deck. For certain options such as CONTACT, INSERT, etc. Marc internally uses ties. With Reorder, Marc applies the constraints in a correct order by forcing an automatic renumbering of all tying equations. For previous behavior, set to Continue of Stop. If an MPC tying conflict occurs the program will continue with warnings, or stop with an error message depending on the setting.
Solver Type	Can be set to Direct Profile, Iterative Sparse, Direct Sparse, Hardware Sparse, Multifrontal Sparse (default) or External Sparse. For Marc 2010 or higher, Pardizo Direct Sparse and MUMPS Parallel Direct solvers are also supported. These are the only Marc solvers supported. This places a 0, 2, 4, 6, 8, 9, 11, or 12 in the 1st field of the 2nd data block of the SOLVER option, respectively.
Non-Symmetric	Places a 1 in the 2nd field of the 2nd data block of the SOLVER option. This is only valid for Solver Type of Direct Profile, Multifrontal Sparse or Pardizo Direct Sparse.
Non-Positive Definite	Places a 1 in the 3rd field of the 2nd data block of the SOLVER option. Valid for all Solver Type selections.
Memory	Specify the amount of work space in words. This can be left blank and the translator will automatically determine this based on model size. It is placed on the 2nd field of the SIZING parameter if supplied.
Bandwidth Optimization	Writes the OPTIMIZE option to the input deck. It is only available for the Direct Prodeck or Multifrontal Sparse solvers and uses the Sloan or Metis algorithms, respectively. This is entered on the second field of the 1st data block of the OPTIMIZE option as a 9 or 11, respectively. Other solvers have their own optimizer and use it by default.
Max. Num. Iterations	For Iterative Sparse solver only. Enters this maximum number of iterations in the 1st field of the 3rd data block of the SOLVER option. Default is 1000.
Stress Analysis Tolerance	For Iterative Sparse solver only. Enters this floating point number in the 1st field of the 4th data block of the SOLVER option. Default is 0.001.
Preconditioner	For Iterative Sparse solver only. Enters a 3, 4, or 5 respectively for Diagonal, Scaled Diagonal, or Incomplete Cholesky (default) preconditioners into the 3rd field of the 3rd data block of the SOLVER option.
Use Previous Solution as Trial	For Iterative Sparse solver only. Enters a 1 if ON (OFF by default) into the 2nd field of the 3rd data block of the SOLVER option.
Out-of-Core Threshold	For Hardware and Multifrontal Sparse solvers only. Enters this integer number in the 7th field of the 2nd data block of the SOLVER option. Default is 100. Represents the number of real*4 words in millions of words. Only for SGI computers running the IRIX operating system.
Number of Processes	Multiple treads can be specified for Pardiso(11) and Multifrontal (8) sparse solvers. The subsequent Marc job is submitted as follows: run_marc -j myjob -nthread ntx Multiple processors can be specified for MUMPS(12) solver. The subsequent Marc job is submitted as follows: run_marc -j myjob -nsolver nsx For DDM, by default the number of processes is set to the number of domains automatically. It can be manually changed if necessary.

Contact Parameters

This subordinate form appears when the Contact Parameters button is selected on the Job Parameters forms. If contact boundary conditions have been defined in the Loads/Boundary Conditions application, this form, together with its subordinate forms, may be used to define most general entries in the CONTACT option. If no contact has been defined, it is unnecessary to modify anything on this form.


Contact Parameter	Description
Deformable-Deformable Method Optimize Constraint Equations	In Double-Sided method, for each contact body pair, nodes of both bodies will be checked for contact. In Single-Sided method, for each contact body pair, only nodes of the lower-numbered body will be checked for contact. Results are dependent upon the order in which contact bodies are defined. This enters a 1 in the 3rd field of the 4th data block. If Optimize Constraint Equations is ON, then a 2 is place in this field. This latter algorithm automatically optimizes the set of contact constraint equations based on the average stiffness of contact bodies, the element edge lengths, and the occurance of sharp corners for deformable, doubled-sided contact only.
Penetration Check	This controls contact penetration checking. sometimes referred to as the increment splitting option. Available options are: Per Increment, Per Iteration (default), Suppressed (Fixed), Suppressed (Adaptive. This enters a 0, 3, 1, or 2 in the 7th field of the 2nd data block, respectively. Per Increment means penetration is checked at the end of a load increment. Per Iteration means that penetration is checked at the end of every iteration within an increment. If penetration is detected, increments are split. Suppress is to suppress this feature for Fixed and Adaptive load stepping types.
Reduce Printout of Surface Definition	This controls reduction of printout of surface definition. This enters a 1 in the 11th field of the 2nd data block if ON.

Contact Detection

This form controls general contact parameters for contact detection. All of these parameters affect the CONTACT option.


Contact Parameter	Description
Distance Tolerance	Distance below which a node is considered touching a body (error). Leave the box blank to have Marc calculate the tolerance. Distance Tolerance is entered in the 2nd field of the 3rd data block.
Bias on Distance Tolerance	Contact tolerance BIAS factor. The value should be within the range of zero to one. This is entered in the 6th field of the 3rd data block. Models with shell elements seem to be sensitive to this parameter. You may need to experiment with this value if you have shell element models that will not converge or penetration appears to occur. A Bias of zero means that the penetration is checked within 1/2 of the Distance Tolerance either side of the element. If during an increment, a node penetrates further than 1/2 of the Distance Tolerance, this may not be detected. Setting the Bias to 0.95 (default), means that 95% of the Distance Tolerance checking is within the element or on the penetrating side of the element.
Suppress Bounding Box	Turn ON this button if you want to suppress bounding box checking. This might eliminate penetration, but slows down the solution.This enters a two(2) in field 8 of the 2nd data block for 3D contact only.
Check Layers	For contact bodies composed of shell elements, this option menu chooses the layers to be checked. Available options are: Top and Bottom, Top Only, Bottom Only. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Ignore Thickness	Turn this button ON to ignore shell thickness. Check Layers and Ignore Thickness combination enters the appropriate flag in the 10th field of the 2nd data block.
Activate Quadratic Contact	Turn this button ON to activate genuine quadratic contact, otherwise, midside nodes will not come into contact and are linearly tied to corner nodes. Activate Quadratic Contact enters a minus one(1) in the 14th field of the 2nd data block. This also affects the Separation Criterion on the next form. Only stress separation criterion is allowed if this is ON.
Activate 3D Beam-Beam Contact	Turn this button ON to activate 3D beam-beam contact. Activate 3D Beam-Beam Contact enters a one(1) in the 13th field of the 2nd data block.

Separation

This form controls general contact parameters for contact separation. All of these parameters affect the CONTACT option.


Contact Parameter	Description
Maximum Separations	Maximum number of separations allowed in each increment. Maximum Separations is entered in the 6th field of the 2nd data block. Default is 9999.
Retain Value on NCYCLE	Turn ON this button if you do not want to reset NCYCLE to zero when separation occurs. This speeds up the solution, but might result in instabilities. You can not set this and Suppress Bounding Box simultaneously. Retain Value of NCYCLE enters a three(3) in field 8 of the 2nd data block.
Increment / Chattering	Increment and Chattering enter the appropriate flag in the 9th field of the 2nd data block. This controls separation within an increment. When Chattering is Allowed, nodes are allowed to separate within an increment if the force/stress on the node is greater than the threshold (Force/Stress Value) in the Current increment (writes a zero to the field), unless Next increment is selected. In this case, if a node, which was in contact at the end of the previous increment, has a force/stress greater than the threshold, the node does not separate until the beginning of the Next increment (writes a one to the field). If Chattering is Suppressed, then if a new node comes into contact in the Current increment, it is not allowed to separate during this increment (writes a two to the field). If Chattering is Suppressed and Next increment is selected, then not only will new nodes coming into contact not be allowed to separate, but also nodes having a greater force/stress than the threshold at the end of the previous increment won’t be allowed to separate until the beginning of the Next increment (writes a three to the field).
Separation Criterion	Separation Criterion enters a zero (1) in the 12th field of the 2nd data block if separation is based on forces. Enters a 1, 2, 3, or 4 if Stresses based on the Derivaition and Relative / Absolute settings. If Activate Quadratic Contact from the Contact Detection form is set ON, only normal Stresses can be used as a separation criterion.
Force Value Stress Value	Force/Stress Value is placed in the 5th field of the 3rd data block. This is the force or stress threshold above which a node is allowed to separate.
Derivation Relative / Absolute	If Stresses are used as the Separation Criterion, then separation is based on either Relative or Absolute nodal stress, where a nodal stress is calculated as a force divided by an equivalent area (Force / Area) or determined by extrapolating and averaging integration point values (Extrapolation). If the contact normal stress on a node exceeds the threshold, the node separates. These settings determine the separation flag written to the 12th field of the 3rd data block. If Activate Quadratic Contact from the Contact Detection form is set ON, only the Extrapolation derivation can be used.

Friction Parameters


Contact Parameter	Description
Friction Type	Available options for friction Type are: None, Shear (for metal forming), Coulomb (for normal contact - default), Shear for Rolling, Coulomb for Rolling, Stick-Slip, Bilinear Coulomb, and Bilinear Shear. Type and Method: places 0, 1, 2, 3, 4, 5, 6, or 7in the 4th field of the 2nd data block depending on fiction type and places a 0 or 1 in the 5th field of the 2rd data block for friction based on nodal forces or nodal stresses respectively for Coulomb fiction. Stick-Slip is a Coulomb type friction.
Method	For Coulomb type of friction models (options 2, 4, and 5 above), there are 2 methods for computing friction: Nodal Stress (by default), Nodal Forces. Type and Method: places 0, 1, 2, 3, 4, or 5 in the 4th field of the 2nd data block depending on fiction type and places a 0 or 1 in the 5th field of the 2rd data block for friction based on nodal forces or nodal stresses respectively for Coulomb fiction.
Relative Sliding Velocity Slip Threshold	Critical value for sliding velocity below which surfaces will be simulated as sticking. Relative Sliding Velocity is placed in the 1st field of the 3rd data block for all friction models except Stick-Slip. For the Bilinear methods, this databox label changes and is for entering the Slip Threshold, which by default is zero, flagging an automatic setting for this parameter.
Transition Region	Slip-to-Stick transition region. Transition Region is placed in the 1st field of the 3rd data block for Stick-Slip model.
Multiplier to Friction Coefficient	Friction coefficient multiplier. Multiplier to Friction Coefficient and Friction Force Tolerance are placed in the 7th and 8th field of the 3rd data block respectively for the Stick-Slip friction model.
Friction Force Tolerance	Friction Force Tolerance. Multiplier to Friction Coefficient and Friction Force Tolerance are placed in the 7th and 8th field of the 3rd data block respectively for the Stick-Slip friction model. This parameter is also used for the Bilinear methods.
Heat Generation Conversion Factor	For Coupled analysis only, this is the conversion factor between energy due to friction and heat generated in a contact analysis. The default is 1.0.

Direct Text Input

This widget is to facilitate the input of the Marc input data that cannot be created using the functionality available in the Marc Preference. All data input here will be appended to the Marc Parameter or Model Definition data sections. There is no error checking available for invalid input. Information in this form is saved and associated with the job.


DTI Parameter	Description
Additional Parameter Input	Text in this area will be placed in the Parameters section of the input deck just before the END keyword.
Additional Model Definition Input	Text in this area will be placed in the Model Definition section of the input deck just before the END OPTION keyword.
Write at Beginning/End	This toggle specifies whether the text is written at the beginning of the section or at the end of the section. For Parameters this is written at the top of the input deck after any TITLE parameters or just before the END statement. For the Model Definition, this is written either just after the END statement or just before the END OPTION statement. End is default.
Parameters Section Model Definition Section	These toggle between defining input for Parameters or Model Definition.
Clear	This clears the text in the text data box for the section that is selected.
Cancel	This closes the form without any changes saved.
Apply	This closes the form and saves the changes made to both sections.
Read From File	This will populate the text data box with text from the indicated deck. This brings up a typical deck browser to select the deck. Both the Parameter and Model Definition sections can be populated separately by reading a deck.


Note:	Direct Text Input, 332 (DTI) is also available in the History section of the Marc input deck when creating Load Steps. This feature is not available for MSC.AFEA.

Groups to Sets

This functionality will convert any selected Patran group that contains nodes and/or elements into Marc element and node sets using the DEFINE option and place the SETNAME parameter in the Parameter section or the input deck.


Groups/Sets Parameter	Description
Select Groups to Translated to Sets	Lists all groups available. Select all the groups you wish to translate in this list box and it will place them in the Groups Translated to Sets list box.
Groups Translated to Sets	Lists all groups that will be translated. Clicking on a group name in this list box will remove it.
Translate Group Members Into:	Either Node Sets or Element Sets (both OFF by default) will create the appropriate DEFINE option in the input deck. No error checking is done for duplicate element or node IDs between groups
OK	Closes the form and saves the information.
Cancel	Closes the form and does not save any changes.

Example: A group called “wing” with both elements and nodes will be written as:

DEFINE, NODE, SET, wing_N	
list of nodes	
DEFINE, ELEMENT, SET, wing_E	
list of elements

The name of the set is the group name with the words _N or _E appended.


Note:	In Marc the set names are limited to 12 characters. Group names must therefore be unique in their first 10 characters.

Restart Parameters

This subordinate form appears when the Restart Parameters button is selected on the Translation Parameters form. This places a RESTART or RESTART LAST option in the input deck and invokes the Marc solver with the -r parameter on the run_marc script when submitting a restart job.


Note:	For a restarted job, the CONNECTIVITY and COORDINATES and other Model Definition information is not written to the input deck, thus reducing the input deck size. Only the necessary information is written.


Parameter	Description
Restart Type	You can Write restart data, Read restart data and Read and Write restart data. The default is None for no restart data.
Create Continuous Results File	If when restarting a job, you wish the results form the previous run to be copied into the new POST deck, then turn this ON. This will place the RESTART or RESTART LAST options before the POST option in the input deck. Otherwise they are placed after the POST option which flags Marc not to copy the results to the new POST deck. If you turn this ON, you must have a restarname.t16 and/or restartname.t19 deck in your local directory or the Marc analysis will fail.
Last Converged Increment	Writes a RESTART LAST instead of a RESTART option. ON by default.
Reauto Complete Unfinished Loadcase Immediate Remesh	Reauto is OFF by default. This is used for changing conditions on restart of a problem in an autoloading sequence. This places a REAUTO option in the input file. If Complete Unfinished Loadcase is ON then a 1 is placed in the 3rd field of the REAUTO options and the preveious set of history data is completed or teminated. If this is OFF, then any additional data needed for the REAUTO option are extracted from the first Load Step information for the restart job. Only if the Restart Type is set to Read or Read and Write is the REAUTO written or the toggle visible to the user. The Immediate Remesh toggle writes a 1 to the 9th field or the REAUTO and forces a remesh if Global remeshing is turned ON. See note below on example of usage.
Restart from Increment	Defines the increment to be read from the file specified in the Select Restart File form. This is entered in the 3rd data field on the 2nd card of the RESTART option. It is only requested when Restart Type is set to Read or Read and Write. The last increment on the restart file is used for the RESTART LAST option when Last Converged Increment is ON.
Increments Between Writing	Defines the number of increments between writing data to the restart file. This is entered in the 2nd data field on the 2nd card of the RESTART option. It is only requested when Restart Type is set to Write or Read and Write. When Last Converted Increment is ON, this is the 4th field of the 2nd data block of the RESTART LAST option.
Select Restart File...	This brings up a file browser to select the restart file when the Restart Type is set to Read or Read and Write. This file is specified on the command line for invoking the Marc solver using the -r option.


Note:	The most common usage of the REAUTO option is as such: a user runs a job to, say, 50 increments. The job fails to converge or for some reason the user wishes to restart the job with different conditions at, say, 20 increments. The first job must be run and restart information written (Restart Last toggle OFF). The second run is done by reading restart data from increment 20 of the previous job and turning ON the Reauto toggle and the Complete Unfinished Loadcase toggle. The previous loadcase (Load Step) is then terminated or completed at 20 increments and the job restarted using the new load case (Load Step) information for the new job.

Adaptive Meshing

In general this form allows for turning ON or OFF adaptive meshing on a Local or Global basis. It writes the appropriate ADAPTIVE and/or REZONING parameter and option or ADAPT GLOBAL option to the Marc input deck. It also allows for ATTACH NODE and SURFACE options to be written to the input deck.

General Adaptive Parameters

Global adaptive remeshing is mostly used in contact analysis where entire deformable contact bodies must be remeshed because the element distortion becomes too great and the analysis fails to converge. Local remeshing can be used in any general analysis.

This table below lists the general adaptivity parameters valid for both Local and Global adaptivity. Local adaptivity allows for mesh refinement about specific user-defined zones of a finite element mesh based on certain criteria. Global adaptivity allows for remeshing of entire deformable contact bodies.


General Adaptivity Parameter	Description
Adaptivity Type	Selects either Local (default) or Global. Global will remesh only the selected contact bodies. Local will rezone or remesh only the localized areas defined by the selected groups. If Local is selected, the ADAPTIVE option and parameter are included in the input file. For a purely linear analysis with no load increments specified, an ELASTIC parameter is included to force the remeshing. If Global is selected, the ADAPT GLOBAL option is included in the input file and the ADAPTIVE and REZONING parameters. Also, if necessary, the appropriate ELASTICITY or PLASTICITY parameters are written. None is the default in which no adaptive meshing is allowed and all widgets are dimmed.
Upper Bounds Multiplier	This specifies the upper bounds on the problem size before the analysis is automatically terminated. The number of nodes, element, contact segments, contact nodes and fixed degrees-of-freedom are determined automatically from the initial model. The factor will scale these values up for adaptive meshing purposes. The default is to double (2) the size of the model before termination. The scaled maximum number of nodes and elements are placed on the ADAPTIVE parameter in 2nd and 3rd fields respectively. The SIZING parameter continues to contain the number of nodes and elements from the original mesh. The scaled maximum fixed degrees-of-freedom is placed in the 5th field of the SIZING parameter and replaces the original number from the original model. The scaled maximum number of contact segments and contact nodes are placed on the CONTACT option in the 2nd and 3rd fields of the 2nd data block respectively. This is determined by selecting between the largest of the (multiplier) times the deformable body entities or the rigid body entities and NOT the sum of the two.
Continue if Upper Bounds Exceeded	This will place a one (1) in the 4th field of the ADAPTIVE parameter and flags the program to continue with the previous mesh if the upper bounds have been exceeded.
Increment Frequency	For Local adaptivity, this parameter flags a remesh after the specified number of increments. When the Adaptivity Type is Local, enters the integer number (default = 1) into the 3rd field of the 2nd data block of the ADAPTIVE option.
Snap to Geometry	If this toggle is ON, the ATTACH NODE and SURFACE options are written. Typically, you need to have at least three nodes associated to a curve, or surface/solid edge for geometry snap to work. First the nature of the problem is determined (2D or 3D). For 2D problems, curves are written as NURBs to the SURFACE option and if a surface is supplied, the edges are written as NURBs to the SURFACE option. For 3D problems, surfaces are written as surfaces and if a solid is supplied, the faces are written as surfaces to the SURFACE option. These geometric entities must be placed in the group comprising the adaptive meshing zone in addition to the elements that make up the remeshing zone. All nodes associated to these geometric entities are placed in the ATTACH NODE option. For Local adaptive remeshing only.
Existing Zones	This is a list of adaptive remeshing Zones that have been created. They consist of a Zone name associated to a group (for Local adaptivity) or a deformable contact LBC (for Global adaptivity) and the associated parameters. If you select an existing Zone, you may change its parameters when you press the Apply button. If you rename it in the Zone Name data box, a new Zone with the modified settings will be created.
Zone Name	Enter a Zone name in this box. On Apply, this name will be created and will become visible in the Existing Zones list box.
Select a Group Select a Deformable Contact LBC	For Local adaptivity, this list box lists all Groups. The Groups must have a list of elements that define the remeshing zone. This list of elements will be written to the Marc input file as an element set in a DEFINE option for each Zone that is defined. For Global adaptivity, this works the same way except the label is changed to select Deformable Contact LBCs from which the list of elements is derived. This defines the 3rd field of the 3rd data block of the ADAPT GLOBAL by identifying the contact body ID also. The group names must be unique within the first 10 characters. The “_E” qualifier is appended to the group name after the 10th character to denote that an element set (DEFINE) has been created from the entities in the group.
Apply	Creates the Zone which consists of all the parameters plus the selected Group or Deformable Contact Body.
Delete	Will delete the selected Zone.
OK	Closes the form saving any settings on the form.
Defaults	Will set the default widgets for either Local or Global. It does not set the Adaptivity Type widget however; only the widgets for Local or Global depending on which it is set to.
Cancel	Will close the form without saving any setting on the form.


Note:	Group names associated with each zone are limited to 10 characters. They will be truncated if they exceed this limit. The names are used to define element sets in the input file and are appended by “_E.” For this reason they should be unique in the first 10 characters.

Local Adaptive Meshing

The general procedure for setting up a Local adaptive remeshing analysis is as follows:

1. Set the Adaptivity Type to Local

2. Enter a Zone Name. This can be anything you like.

3. Select a Group to be associated to this Zone. This group must be created in the Patran Group application and must contain the nodes and elements of the region of the model in which the adaptive remeshing is to occur. The default_group can be selected in which case the entire model (in general) is part of the remesh Zone.

4. Select Adaptive Mesh Criteria. Use must turn ON the Use Criterion toggle for each particular criteria to be active. You can turn on as many as you like. Only Node in Contact is ON by default because it does not need any user intervention. All other Criteria requires user input to define what will trigger a mesh adaptivity.

5. Press the Apply button to create the Zone with the associated criteria and group.

6. Repeat this for each Zone to be set up.

This table list the parameters that are specific to Local adaptivity criteria. See also the forms below:


Local Adaptivity Parameter	Description
Maximum Levels to Adapt	This places the given integer in the 2nd field of the 3rd data block of the ADAPTIVE option. Two (2) is the default.
Criteria	Selects the Local adaptive criteria to use. The options are: Mean Strain Energy, Zienkiewicz-Zhu Stress, Zienkiewicz-Zhu Strain Energy, Location within Box, Node in Contact, Maximum Solution Gradient, Equivalent Stress, Equivalent Strain, Equivalent Plastic Strain, User Sub. UADAP. Although Node in Contact is the default, no adaptivity will be done unless at least one of these is turned ON. See next parameter. The selection made here places a 1, 2, 2, 4 or -4, 5, 8, 9, 9, 9, or 10 in the 1st field of the 3rd data block of the ADAPTIVE option respectively.
Use “Criteria” Criteria	This toggle must be ON to use the selected Criteria. The label of this toggle changes and the Criteria is substituted by the name of the Criteria. They are actually separate toggles for each Criteria. The number of Criteria that are turned ON is placed in the 1st field of the 2nd data block of the ADAPTIVE parameter. The 3rd and 4th data blocks are repeated for each Criteria turned ON. All are OFF by default except Node in Contact.
f1, f2, f3, f4, f5, f6	These values are written to the ADAPTIVE option in the 1st through 6th fields of the 4th data block respectively. Some have defaults. Others are dependent on the model size and other factors.
Unrefine	For the Location within a Box criterion, the ability to unrefine the mesh is turned ON with this toggle. If ON, it places a -4 instead of a 4 in the 1st field of the 3rd data block of the ADAPTIVE option.
Absolute	For the Equivalent Stress/Strain criteria, this selects whether f1 or f2, f3 or f4, or f5 or f6 are written.

Mean Strain Energy and Zienkiewicz-Zhu Stress

Zienkiewicz-Zhu Strain Energy and Location within Box

Node in Contact and Maximum Solution Gradient

Equivalent Stress and Equivalent Strain

Equivalent Plastic Strain and User Sub. UADAP

Element in Cutter Path and Temperature Gradient

Global Adaptive Meshing

The general procedure for setting up a Global adaptive remeshing analysis is as follows for any given job:

1. Set the Adaptivity Type to Global

2. Enter a Zone Name. This can be anything you like.

3. Select a Deformable Contact Body to be associated to this Zone. This body must be created in the Patran Loads/BCs application.

4. Select Adaptive Mesh Criteria. (2D or 3D) You must at a minimum:

• Select a mesher (Advancing Front is default for 2D)

• Give a Target Element Length or Target Number of Elements

• Select Remesh Criteria (default is to remesh every 5 increments)

You have control of many parameters to influence the meshing.

Press the Apply button to create the Zone with the associated criteria and body.

Repeat this for each Zone to be set up.


Note:	Although you can set up multiple zones for a given job, only one deformable body can be associated with a zone. If the same deformable body is associated with more than one zone, only the first one encountered will be used in the zeroth increment. You may select the zones per Load Step when you set up your load stepping sequences. See Load Step Selection, 334.

Below is a discussion of 2D and 3D Global adaptive meshing. This table lists the parameters that are specific to Global adaptivity. The adaptive meshing is for either 2D or 3D mesher technology. What is presented to you in the form is based on this switch.


Global Adaptivity Parameter	Description
Mesher	Selects the mesher to use when a remesh is necessary. Choices are Advancing Front (2D default), Overlay, Delaney, or Tetrahedral (3D default). This places a 2, 3, 4, or 11 in the 1st field of the 3rd data block of the ADAPT GLOBAL option. For 3D shell models, this places 12 or 19 in the data block for triangular or quadrilateral shell meshes, respectively. For 3D hex meshes, this places a 5 in the same data block.
Increment Frequency	This parameter flags a remesh after the specified number of increments. Valid for all 2D and 3D meshers. The toggle must be ON to enable the data box. By default this criterion on ON. For Marc Version 2003 or greater, if this is ON, a 1 is placed in the 1st field of the 4th data block. The value (default=5) in the data box is placed in the 2nd field. For Marc Version 2001 or less, a 1 is placed in the 1st field of the 4th data block. The value (default=5) in the data box is placed in the 4th field.
Immediate Remesh	This parameter forces a remesh before the analysis begins. Valid for all 2D and 3D meshers. For Marc Version 2003 or greater, if this is ON, a 7 is placed in the 1st field of the 4th data block. For Marc Version 2001 or less, if this toggle is ON, a one (1) is placed in the 9th field of the 4th data block.
Advanced...	This button brings up a form to allow you to set the remeshing criteria This is described in the table and form below.
Target	Previous Mesh Size is the default. For Marc Version 2000 or less, only Element Length is valid. No. of Elements is disabled if not 2001 or greater.
Element Length: No. of Elements:	This label changes depending on the Target that is selected. If Target is Element Length, the databox accepts a real value. If Target is No. of Elements, the databox accepts integer values. Both are blank by default. If Target Element Length is supplied, this fills out the 2nd field of the 5th data block of the ADAPT GLOBAL option. If No. of Elements is supplied this fills out the 4th field of the 5th data block. If neither is supplied, both fields should be left blank. This flags Marc to use the same number of elements as the previous mesh. Only Target Element Length is valid for Marc Version 2000 or less.
Elements	For Advancing Front: All Quads is the default. All Quads places a zero (0) in the 1st field of the 5th data block of the ADAPT GLOBAL option. All Tris places a two (2) and Mixed places a one (1). For Overlay only All Quads is allowed. For Delaunay only All Tris is allowed.

The Advanced criteria form is valid for all meshers, 2D and 3D, however, only various remesh criteria are valid as described below. All parameters in this table affect the ADAPT GLOBAL keyword option.


Parameter	Description
Strain Change	This parameter flags a remesh if a change in equivalent strain greater than that specified is detected. This is only valid for Marc Version 2003 or greater. If this is ON, a 5 is placed in the 1st field of the 4th data block. The value in the data box (an real) is placed in the 3rd field. The default is 0.4.
Element Distortion	This parameter flags a remesh if the element distortion is to be used as a remesh criterion. This is only valid for 2D. The databox value is to indicate the greatest allowable quadrilateral distortion above which triangular elements are added. For Marc Version 2003 or greater, if this is ON, a 2 is placed in the 1st field of the 4th data block. For Marc Version 2001 or less, a one (1) in the 2nd field of the 4th data block and the databox is not applicable.
Penetration	This parameter flags a remesh if penetration is detected. For Marc Version 2003 or greater, if this is ON, a 6 is placed in the 1st field of the 4th data block. The data box default is blank (=2*contact tolerance). If the data box has a value and it is enabled it is placed in the 3rd field. For Marc Version 2001, if this toggle is ON, a one (1) is placed in the 3rd field of the 4th data block and the data box value is placed in the 10th field. For Marc Version 2000 or less, if this toggle is ON, a one (1) is placed in the 3rd field of the 4th data block and the data box is not applicable. This is only available if the mesher is for Quad elements.
Angle Deviation	This parameter flags a remesh if internal element angles change beyond a specified limit. The angle deviation is measured from the undeformed state and is 40 degrees by default. Thisis for 2D meshers only. For Marc Version 2003 or greater, if this is ON, a 3 is placed in the 1st field of the 4th datablock. The value in the databox is placed in the 3rd field. For Marc Version 2001 or less, if this toggle is ON, a one (1) is placed in the 6th field of the 4th data block and the angle deviation for Quads in field 7 and for Tris in field 8.
Aspect Ratio	This parameter flags a remesh if the elmeent aspect ratio becomes larger than that specified. This is only valid for Marc Version 2003 or greater for 2D meshers. If this is ON, a 4 is placed in the 1st field of the 4th data block. The value in the data box (an real) is placed in the 3rd field. The default is 10.0.
Valume Control	This turns ON the volume control flag for 3D meshers. A 1 is placed in the 7th field of the 5th data block for Tet mesher or the 9th field for the Hex mesher. For 3D solid meshers, it also defines the volume ratio control placed on the 3rd field of the 4th data block.
Minimum Element Edge Length	Controls the minimum element edge length. This is blank by default and optional in which case the minimum edge length is 1/3 the Target Element Length. Fills out the 7th field of 5th data block for 2D or the 2nd field for 3D. This is a real value greater than zero. Only valid for Marc Version 2001 or greater and is only valid for the 2D Advancing Front, Delauney and Tetrahedral meshers.
Maximum Element Edge Length	Controls the maximum element edge length for 3D. This is blank by default and optional in which case the maximum edge length is 3 times the Target Element Length. Fills out the 10h field of 5th data block. This is a real value greater than zero. Only valid for Marc Version 2003 or greater.
Curvature Control Subdivisions	This is ON by default with a value of 36 for the Subdivisions for 2D meshers. For 3D meshers it is OFF with a default value of 10. Fills out the 5th field of 5th data block with the Subdivisions value for 2D or the 8th field for 3D. This is an integer value greater than or equal to -1. (-1 is used to obtain uniform outline points.) Only valid for Marc Version 2001 or greater and only valid for the 2D Advancing Front, Delauney and Tetrhedral meshers.
% Change of No. of Elements	Forces the new number of element in the new mesh not to exceed a percentage of the original number of elements. A maximum of five remesh trials are used to fulfill this requirement. This is blank by default and optional in which case no such control is enforced. Fills out the 8th field of 5th data block. This is a real value between 0 and 100. Only valid for Marc Version 2001 or greater and is only valid for the 2D meshers.
Smoothing Ratio	This is 0.8 by default and optional. Fills out the 6th field of 5th data block. This is a real value between zero and one (0-1). Only valid for Marc Version 2001 or greater and only valid for the 2D Advancing Front and Delauney meshers.
Feature Vertex Angle	For Tetrahedral mesher, defaults to 100 degrees and is placed in the 3rd field of the 5th data block. For the 2D meshers, defaults to 120 and is placed in the 3rd field of the 5th datablock.
Feature Edge Angle	For the Tetrahdral mesher, defaults to 60 degrees and is placed in the 4th field of the 5th data block.
Coarsening Factor	For the Tetrahedral mesher, defaults to 1.5 for interior elements and is placed in the 5th field of the 5th data block.
Transition Factor	For Advancing Front mesher, placed in the 9th field of 5th data block.
Outside Refining Levels	This is blank by default. Fills out the 2nd field of 5th data block. This is an integer value between zero and two (0-2). Only valid for Marc Version 2001 or greater and only valid for the 2D Overlay mesher.
Inside Coarsening Levels	This is blank by default. Fills out the 3rd field of 5th data block for the 2D Overlay mesher or the 2nd field of the 6th datablock for the 3D Overlay mesher. This is an integer value greater than or equal to zero (2D mesher will always use one (1) regardless of the number you place in the databox). Both the toggle and the databox are only valid for Marc Version 2001 or greater.
Change Element Type	Placed the appropriate element type in the 4th field of the 3rd data block. Some element types are not supported for remeshing. If you experience an error message from Marc stating that the selected element type is not supported, instead of modifying your properites in Patran, specify one of these element types to be used when remeshing is necessary.

User Subroutine File

This functions as a normal file browser. Two options exist. The titles are changed to indicate that a FORTRAN file must be selected. The Filter uses a *.f* to find all .f or .for files in the specified directory if the Option is Select Subroutine File. This is the default.

When the job is submitted, the

run_marc -j jobname -u user_sub

command is ultimately given. The toggle Save Executable can be turned ON in which case the job is submitted with:

run_marc -j jobname -u user_sub -sa yes

The new executable will automatically be called by the name of the user subroutine with a .marc appended to the end (.exe on Windows). This executable remains in the submittal directory or scratch directory specified. It is not deleted after job execution.

If the Option is Use Existing Executable then the titles and filters are changed as indicated. The job is submitted with:

run_marc -j jobname -pr user_sub.marc

where usersub.marc is the executable name (or usersub.exe on Windows).

If you turn ON the Remote Exe. toggle, then you can specify the exact path to an existing Marc executable on a remote host (this should only be used when submitting jobs to a remote host).

Activation of various subroutines is also flagged from the Activate Routines button. This is explained below.


Note:	Using an existing, compiled and linked Marc executable is generally only meant to work on a local machine since the executable is machine dependent. It will not work for a remote submittal unless you explicitly identify the remote location of the executable using the Remote Exe. toggle. If the job cannot find the given path on the remote machine, the job will fail.

Activate Subroutines

A button called Activate Routines on the Select User Subroutine File brings up this form, which allows for various subroutines can be activated. These are general functions do not require much special input, but are global for the analysis in general. Other functions that are or may be specific to a particular material or element property or to a specific load are generally activated in the Materials, Properties, or Loads/BCs applications.

All toggles are OFF by default.


Contact Routines	Description
uMOTION	Enters the UMOTION option after the CONTACT option. Not valid for Thermal analysis. Option is not written if no contact bodies exist.
UFRICtion	Enters the UFRICTION option after the CONTACT option. Not valid for Thermal analysis. Option is not written if no contact bodies exist.
UCONTACT	Enters the UCONTACT option after the CONTACT option. Not valid for Thermal analysis. Option is not written if no contact bodies exist.
UGROWRIGID	Write a UMOTION, 2, option after the CONTACT option. This is not valid for Thermal analysis and is not written if no contact bodies exist.
SEPFOR / SEPSTR	If this toggle is ON, writes a comment after the CONTACT option: $....user subroutine sepfor or sepstr has been flagged
UHTCOEf	Enters the UHTCOEF option after the CONTACT option. Only valid for Thermal and Coupled analysis. Option is not written if no contact bodies exist.
UHTCON	Enters the UHTCON option after the CONTACT option. Only valid for Thermal and Coupled analysis. Option is not written if no contact bodies exist.
IMPD, ELEVAR, ELEVEC	If this toggle is ON, a UDUMP option is written with all the nodes and elements of the model specified in the 2nd data block (a blank line indicates all nodes/elements). A negative Post code must have been selected also in the Element or Nodal Output Requests form which then invokes user subroutine PLOTV or UPSTNO.


Material Routines	Description
WRKSLP	Writes a -1 to the 1st field of data block 2 of the WORK HARD option. This is not applicable if TABLES are being used, but only if WORK HARD is written. No data blocks after block 2 are written if this is activated. If this is ON, then it is activated for ALL plastic models.
CRPVIS	Write the VISCO ELAS parameter to the input deck.


Other Routines	Description
UTRANform	If this toggle is ON, the UTRANFORM option is written after COORDINATE data. Datablock three includes the list of nodes supplied. However this list is broken up into more than one list if necessary. What determines the division of this list into multiple lists is the reference coordinate frame associated to the nodes. There will be one list for each reference coordinate frame. Thus data block 2 indicates the number of reference coordinate frames and then data block 3 repeats itself for each reference coordinate frame. The actual reference coordinate frame is unimportant as the user subroutine will deal with the real definitions of the coordinate transformations. If the list is left blank, no list is written.
UFXORD	If this toggle is ON, the UFXORD option is written after COORDINATE data. Datablock two includes a list of nodes supplied and can be left blank. This will use the same nodes as UTRAN. Generally these two are not used together.
USDATA	If this toggle is ON, the USDATA option is written with the integer value of the data box placed in the 2nd field near the top of the Model Definition section.
IMPD, ELEVAR, ELEVEC	If this toggle is ON, a UDUMP options is written with all the nodes and elements of the model specified in the 2nd data block (blank line). A negative Post code must have been selected also in the Element or Nodal Output Requests form which then invokes user subroutine PLOTV or UPSTNO.
UFORMS	If this toggle is ON, for the selected MPCs, the Tying type will be written as a negative number, thus invoking User Subroutine UFORMS. This works for all MPC types that write the TYING option except Overclosure (does not work with Explicit, Sliding Surface, and RBE MPCs since they do not write the TYING option).

Rebar Selection

When this button is selected a listbox becomes available to associated 2D rebar layers to the job. Please keep in mind the following when running jobs with rebar elements.

1. 2D rebar layers are created using the Rebar Definition tool. See Rebar Definition Tool, 159.

2. Analysis jobs must be axisymmetric or plain strain in order to activate and create rebar elements in the input file.

3. The Marc Version must be set to 2003 to allow selection of 2D rebar layers.

4. Only the 2D rebar layers selected will be translated to the input file. The exception is:

5. If separate rebar element properties have been defined outside of the Rebar Definition tool, they will be translated to the input file regardless and in addition to what is selected here.


Note:	If you delete a 2D rebar layer in the Rebar Definition tool, obviously the association to the job will be lost. This is up to the user to manage.

Radiation Viewfactors

This form appears when you press the Radiation Viewfactors button. This button is only available when

1. The Analysis Type is set to Thermal or Coupled analysis.

2. Radiation boundary conditions have been created under the Loads/BCs application.

This form or application is used to flag a thermal radiation analysis and calculate the radiation viewfactors which are stored in a file and accessed when the job is submitted. The parameters on the form are described here


Parameter	Description
Thermal Radiation	This is OFF by default. It must be turned ON for a thermal radiation analysis to proceed. All widgets in the View Factor Controls frame below remain disabled if this is OFF. If this is ON, the widgets are enabled. This parameter flags the thermal radiation analysis and means that a RADIATION parameter and the VIEW FACTOR option are placed in the input deck.
Temperature Units	Can be Celsius (default), Kelvin and Fahrenheit. This places a 1, 2, or 3 in the 4th field of the RADIATION parameter, respectively.
Stefan-Bolzmann Constant	Default value is shown above. This is the 4th field of the RADATION parameter.
Number of Rays	This is the number of rays used in the MonteCarlo simulation to determine the radiation viewfactors. This is input to the viewfactor program and not the Marc input deck. This controls the accuracy of the viewfactor calculation. The higher the number, the longer the compute time.
Analysis Type	The is either 2D, 3D or Axisymmetric. This is input to the viewfactor program and not the Marc input deck. 2D analysis refers to analysis in two dimensions such as plane strain. Shell elements are considered 3D analysis since they perform in three dimension even though they are 2D type elements.
Symmetry Planes	If this is ON, then the Symmetry Plane data boxes are activated. Otherwise they are disabled.
Symmetry Plane 1/2/3	These are inputs to the MonteCarlo simulation and are select databoxes for accepting planes in any way that Patran allows selection or definition of a plane. Symmetry Plane 3 is only activated if the Analysis Type is 3D.
Number of Entities	This widget is always disabled and is for informational purposes only. See explanation below.


Note:	RADIATION parameter Field 2 is always set to 2 and field 3 is always set to 0.

Here is an explanation of how this works:

1. The Analysis Type is set to Thermal or Coupled

2. Radiation LBCs are created.

3. Thermal Radiation is turned ON in this form; the Temperature Units and Stefan-Boltzman Constant changed if necessary.

4. Change the Number of Rays if desired and set the Analysis Type. At this point, the program detect the existing Radiation LBCs and counts the number of entities in the application regions of all the Radiation LBCs but separated by number of element edges and element faces. This value is reported in the Number of Entities data box.

These entities are the number of element edges or element faces (but not both). If a geometric entity is in the application region, it is evaluated to determine the associated element edges/faces. If no Radiation LBCs exist, a message to that effect is issued, however you probably can’t get this far if there are not any defined. If 3D analysis is set but no element faces are available, the number of entities is zero. If 2D or axisymmetric is set but no element edges are available, the number of entities is zero. The reported number does not mix element edges and faces.

5. Set the Symmetry Planes if desired. If the select databox is left empty, that plane is assumed inactive. The input to the program is a location and a vector.

6. Pressing the Calculate button to create the viewfactors. The ratio of the number of emanating rays from any given entity that hit another entity that has radiation defined to those that don not hit it is the view factor (in the most simplistic explanation).

While the view factor calculation is going on, a Percent Complete form/widget appears if more than say, 20 entities need viewfactor calculations.

If the user presses the Cancel button the calculation is terminated prematurely.

7. The calculation of the thermal radiation view factors is written to a file called jobname.vfs.


Note:	If you change the jobname after doing the view factor calculation the correct file will not exist in this case. A warning that the file does not exist is issued if this is the case. You will need to rename the file or recalculate the viewfactors.

When the job is submitted it is submitted with the -vf option specifying the view factor file name as such:

run_marc -j jobname -vf jobname.vfs

The Radiation LBCs themselves do not get translated into the input file, but are part of the input to the view factor calculator. The two Temperatures at Infinity (top and/or bottom) are passed into the program and written to the view factor file. Below is a description of the view factor file itself:

Block 1 - Header

Line 1

10  int     iver    Version #

10  int     nobj    Number of objects

10  int     nray    Number of rays used in computation

Block 2 - Objects

Line 1 repeated nobj times

10  int     obj     Object number

10  int     eid     Element id

10  int     face    Face or edge number

15  float   tinf    Temperature at infinity top

15  float   tinf    Temperature at infinity bottom

Block 3 - View Factors repeated nobj times

Line 1

10   int    obj     Emitting object number

10   int     nz     Number of non zero viewfactors

Line 2 repeated nz times

10  int     obj     Incident object number

15  float   vfs[4]  Four view factors

                    Emit        Incident

               1     out          out

               2     out           in

               3      in          out

               4      in           in

where : out - outer normal of element according to connectivity

         in - the other side


Note:	For line elements, out means the right hand side as you travel from node 1 to node 2. For shells, out is defined by the right hand rule for the connectivity of the nodes.

Cyclic Symmetry

This is a capability in Marc Version 2001 and greater. The translator places the CYCLIC SYMMETRY option in the input deck.


Temperature Parameter	Description
Cyclic Symmetry	This toggle turns this option ON. Only if this toggle is ON does the frame and its contents become active for input. If the toggle is OFF, no CYCLIC SYMMETRY data will be written to the input deck.
Cyclic Symmetry Axis	This is a vector that can be selected graphically by all the current methods in Patran. Coord 0.3 (the z-axis) is the default. The three direction cosines are placed in fields 1-3 of the 2nd data block of the CYCLIC SYMMETRY option.
Point on Symmetry Axis	This is a point that must lie on the symmetry axis. If left blank, the origin is used. It can be picked graphically by all the current Patran methods. The coordinates are placed in fields 1-3 of the 3rd data block of the CYCLIC SYMMETRY option.
Number of Repetitions	This is used simply to calculate the Angle. The default is two (2). Thus 360/2 is 180. So 360 is always divided by this number and placed in the Angle data box.
Angle	This is placed in the 1st field of 4th data block. This box is always disabled. The number is calculated and set by the Number of Repetitions.
Suppress Rigid Body Motion	If this toggle is ON, a -1 is placed in the 1st field of the 5th data block. If it is OFF, a zero is placed there instead.

Cyclic Symmetry is valid for:

1. Only continuum elements (solids, 2D solids). However, the presence of beams and shells is allowed, but there is no connection of shells to shells, so that shell part can, for example, be a turbine blade and the volume part can be a turbine rotor. The blade is connected to the rotor and if there are 20 blades, 1/20 of the rotor is modeled and one complete blade.

2. Nonlinear static analysis including remeshing as well as coupled analysis.

3. Pure heat transfer.

4. All analyses involving contact.

5. Eigenvalue analysis such as buckling or modal analysis, harmonic analysis, and transient dynamic analysis. However, there are restrictions in the case of modal analysis which are described in more detain in Marc Volume A: Theory and User Information, Chapter 9, Cyclic Symmetry.