This appendix lists a few guides and suggestions for users transitioning from other analysis codes. The intention of this document is to ease the transition primarily from ABAQUS or the discontinued Patran Advanced FEA product to Marc when doing nonlinear finite element analysis with Patran as the pre/postprocessor. There are four parts:
• Introduction and New Features Section
• Summary - purpose is to alert you to the main points you need to know to avoid having problems and give enough information that an experienced user will not need to read the Reference Section
• Reference Section - gives usage details of topics referred to in the first sections
• Resolving Convergence Problems - that you may encounter when doing non-linear analyses with Patran and Marc (or MSC.AFEA).
Capabilities and Features
The Marc Preference supports all of the nonlinear analysis capabilities that the ABAQUS Preference does (and the discontinued Patran Advanced FEA did), plus a lot more. Capabilities never previously supported or limited in these and other Preferences include:
• Structural, thermal, and coupled thermal-mechanical analysis
• Multi step analysis
• Global and local adaptive re-meshing - including results visualization
• Full 3D deformable body contact
• Multi-body contact (very easy setup) - plus contact tables
• Contact of higher order elements,
• Rigid geometry contact including symmetry planes
• Analytical and discrete definitions of rigid and deformable contact
• Hour glass control for reduced integration elements
• Generalized plane strain elements
• User control over convergence criteria
• Multiple solver options
• Direct Results Access (DRA) - results remain in result file.
• Rigid geometry results visualization/animation
• Input deck reader
• User subroutine access
• Superplastic forming analysis
• Cyclic symmetry
• Axisymmetric to 3D capabilities
• Radiation view factor calculations
• Activation/de-activation of elements
• Conversion of models from other Preferences (solvers)
• Material (elastomer) experimental data fitting
• Domain decomposition - parallel processing
• Beam library
• Rebar modeling plus rebar elements
• Boundary conditions on geometry - in the analysis input deck
• Improved user interface - with one or two button click you can:
• Run a default nonlinear analysis - after model is created
• Monitor analysis - including viewing status files
• View or edit and re-submit input deck
• Read results - postprocess deformed shape
• And much, much more!
Model/Database Conversion: The Patran Advanced FEA Preference no longer exists and has been discontinued. When and old database is opened in Patran 2001 and later releases, all Patran Advanced FEA data is automatically converted to the Marc Preference. The databases are converted with Patran’s normal Preference switching code, which means that only nominal information is converted to the Marc model. Be sure to save copies of your databases. A capability has been implemented in Patran 2001 r2a that significantly increases the complexity level of the model information converted during Preference switching. This capability converts nearly all data from previous (ABAQUS -based) models to the Marc preference. This can be used for all analysis Preferences (if appropriate mapping tables are available) including full model conversion from other solvers such as MD Nastran, MSC.Dytran, ANSYS, LS-DYNA 3D, etc. You turn this new capability on in Patran under Preferences | Analysis
Users should always check converted models for accuracy and completeness. See the Reference Section
for more details on customization (i.e., user control of mapping) and using this new capability with
Note that the ABAQUS input file reader can be accessed via the ABAQUS Preference to import these model and then switch the Preference to Marc.
Consider using these Analysis form defaults (either edit the default static step of the existing template.db, or create a new template.db) for more ABAQUS like defaults:
• Load Increment Parameters
• Change the Time Step Scale Factor from 1.2 to 1.5 (or even 2.0; using smaller values will slow down convergence and may even cause the analysis to exceed the maximum # of cutbacks allowed before decreasing the time step sufficiently).
• Set the Trial Time Step Size to 0.1 (the default of 0.01 causes more increments and larger files than necessary for models that converge easily and the automatic time stepping will cut back if necessary).
• Set the Minimum Time Step to 0.0001 (this typically is the stopping criteria the way it is for ABAQUS, if you do not do this the default stopping criteria of Max # of Cutbacks is used, which is not as easy to define a meaningful number for).
• Set the Max. no. of Steps to 50 (or 100, it defaults to 20 which often isn't enough).
• Turn Quasi-Static Inertial Damping ON and make sure to include a material density
• On some problems it may be helpful to tighten the Relative Residual Force under Iteration Parameters from 0.1 to 0.01. Note that the translator turns the new Autoswitch capability ON by default (when near 0 residual is detected it automatically changes to a displacement criteria)
• Be sure to use Adaptive load increment type with Arc Length Method set to None
• Job Parameters
• Consider changing the Bias on Contact Distance Tolerance (found under Analysis | Analyze | Translation Parameters |Contact Control Parameters |Contact Detection) value to 0.5 or 0.9 as the default. If you run into contact-related convergence problems this is one of the first things to try.
This last recommendation is somewhat controversial, but you will avoid convergence problems in some cases by turning ON Non-Positive Definite
under Translation Parameters | Solver Options
. If you have a run that will not converge, this is one of the first things to try (see section on , 520
for more suggestions).
• ABAQUS incompatible modes = Marc assumed strain
• ABAQUS hybrid = Marc Herrmann element
(requires constant volume formulation)
• Status files: Marc jobname.sts ABAQUS jobname.sta
• Input files: Marc jobname.dat ABAQUS jobname.inp
MD Nastran jobname.bdf
• Output file: Marc jobname.out ABAQUS jobname.dat
Patran Advanced FEA jobname.msg MD Nastran jobname.f06 file
• Results Files: Marc jobname.t16 ABAQUS binary jobname.fil
MD Nastran jobname.xdb
Marc jobname.t19 ABAQUS ascii jobname.fil
This is nearly identical including the requirement to use true stress vs log-plastic strain to define hardening behavior of elastic-plastic materials. If utilities have been installed, Utilities | Fields | Modify | Material Field automates converting from engineering stress-strain to true stress - log plastic strain.
Experimental curve-fitting for elastomers is supported.
Note that Ogden hyperelastic coefficients are different in Marc and ABAQUS.
Marc has all the same element formulations and options plus a few more. The labels and data input for comparable element types is similar. Marc has all of the same element formulations and options as ABAQUS plus a few more (such as generalized plane strain and semi-infinite). One difference is that the Assumed Strain (Abaqus’ Incompatible Modes) and Constant Volume options in the Marc Preference are specified on the Input Properties form rather than via a pull-down menu option.
Marc beam orientation vector should be a vector in the beam XY plane (like MD Nastran) where ABAQUS beam orientation vector is given as the perpendicular to the beam XY plane.
Abaqus axisymmetric models are built in the global XY plane with X = radial, Y = axial, and Z = meridonal (hoop) direction. Marc axisymmetric models are also built in the global XY plane, but are different in that X = axial, Y = radial (think of the way you would lay out a jet engine where X is the station), and Z = hoop. To convert ABAQUS axisymmetric models to Marc:
1. Create a group with all entities
2. Use Group | Transform | Mirror to mirror the model about the Y-Z plane, i.e., select Coord 0.1 under Define Mirror Plane Normal. Make sure to select the toggles that transform all LBC's and element propterties with the model and flip the elements if necessary to keep the element normals in the positive Z direction.
3. Use Group | Transform |Rotate and rotate the model minus (-)90 degrees about the Z-axis.
The Marc work-horse shell element is the Thick Shell (element 75), so this element should be used for most shell applications even though the default may be Thin Shell.
Load/Boundry Conditions (LBC's)
This is nearly identical in that all loads and displacements are total values (not incremental). The major difference is in setting up contact (which is actually much easier to do). Patran does not support pressure loading on 1-D elements, but you can use the LBC option CID Distributed Load to create pressure loads on 1-D elements, including axisymmetric shells.
One difference is in the way removal of LBC sets is handled. ABAQUS removes LBCs gradually over the subsequent step, easing convergence problems. The Marc Preference has this capability when defining contact tables. If you remove a force, pressure, inertial load, or displacement, the LBC will be removed suddenly at the beginning of the step and may cause convergence problems if you have not specifically set up your contact table to do otherwise. If you do not use the contact table but still want the load removed gradually, you can include the LBCs in the subsequent step with zero values so their effect will be removed gradually over the load step. One thing to be aware of though, sometimes Patran fails to include some types of LBCs that have zero as the value. In this case, a work around is to put in a very small number but not zero.
If local cylindrical (or spherical) coordinate systems (c.s.) are required for material and element property orientation usage they must be created manually. In other words, selecting a local cylindrical system on the element property form for material orientation will NOT work the same way as it does for the ABAQUS Preference because the Marc CYLINDRICAL option only applies to nodal quantities. The workaround is to reference the local cylindrical system under the Orientation System input data box, and then reference a spatial field in the Orientation Angle box where the spatial field simply gives the angle in degrees of the element centroid relative to the cylindrical system. Since Patran cylindrical systems give theta in radians, and the rotation angle of the ORIENTATION option is in degrees, this requires a spatial field using the cylindrical system with theta as the only active independent variable and mapping values from 0 to 360 as theta goes from 0 to 2*PI.
ABAQUA uses contact pairs (consisting of two application regions) where a master region can see and prevent penetration of the nodes on the slave region. For contact pair contact Patran puts circle markers on the slave surfaces and arrow markers (pointing toward the slave region) on the master surfaces. For Marc contact Patran puts circle markers on deformable body surfaces and arrows pointing inward on the meshed rigid bodies, and puts hash marks on the inner side of rigid geometry curves. Marc allows geometry to be used to define the rigid body, but does NOT allow tria shells to be used to define the rigid body (only quads) if the geometry is meshed.
In ABAQUS you typically have to move the contact regions together, but do not need to do this in Marc. In Marc you can give the rigid body an Initial Velocity in the desired direction to move them together.
Marc uses contact body contact (which can include self-contact), where each body is created as a separate application region and contact between the bodies is characterized in the Contact Table. The Contact Table assumes that all bodies will be prevented from penetrating (defined as Touching) all other bodies (including itself), but the contact table and the contact parameters can be modified under Analysis | Step Creation | Solution Parameters | Contact Table. It is located under Step Creation because the contact table can change between analysis steps. Marc's contact body interaction still uses contact pair algorithms, so to avoid penetration follow the same master/slave rules which are to give the lower contact body number to the body with: 1) the finer mesh; 2) the softer material; 3) a convex corner or edge.
Marc's contact boundary detection algorithms are very fast, so it is not a problem to just select the entire body and let Marc figure out the specific regions that will see other bodies. The only problem with doing this is also the most common problem you will have when running contact jobs, and that is the limitation that you cannot apply a displacement constraint to any node that may come into contact. When a node with a constraint comes into contact Marc will give you an error about illegal tieing constraints. One way around this problem when using symmetry in your problem is to use rigid body symmetry planes to define the symmetry conditions (as opposed to defining symmetry conditions with displacement constraints). Another limitation is that nodes that may come into contact should not reference a local coordinate system as their analysis CID. If this happens Marc will stop with a 2011 exit message (version 2001 and prior) or give a warning that the analysis CID has been changed. You can speed up the contact calculations by using the contact table to eliminate checking of bodies that you know will never touch.
Points to Remember: If you are comfortable with Patran and ABAQUS, make sure to get the latest versions of Patran and Marc. Prior versions have too many differences to allow an easy transition. If you must use an older version see FAQ #3 in the Reference Section for suggestions. Make sure P3_TRANS.INI (Windows) or site_setup (UNIX) file points to the appropriate Marc version so you can automatically submit Marc jobs from within Patran.
If you need more information than is found in this document there are two training courses that will provide all the information you will need: PAT 322 is a course covering MSC.AFEA and MAR 120 a course covering Patran /Marc.
Database Conversion: The capability previously mentioned is new to Patran 2001 r2a and will significantly increase the complexity level (and give the user some control in addition) of the model information that is successfully converted during Preference switching between any Preference in the database. This capability should allow easier Preference switching of all solvers such as from ANSYS to MD Nastran, or MD Nastran to Marc (and vice-versa), or MD Nastran to MSC.Dytran, etc. While this capability allows almost all of the model information (including contact, where there are significant differences) to be converted, there are mapping tables. Users should also check these converted models for accuracy and completeness. Users should check the MSC website for updates to these tables. Make sure to save copies of your earlier databases so they can be converted again when and if updated/improved mapping tables become available. When opened, old databases containing the discotinued Patran Advanced FEA Preference are automatically converted to the Marc Preference.
Contact Interaction: As previously discussed, Marc uses contact body contact (which can include rigid bodies), where each body is created as a separate application region and contact between the bodies is characterized in the Contact Table. The contact table is a matrix with entries consisting of Touching, Glued, or Null. The defaults assume that all bodies will be prevented from penetrating (defined as Touching) all other bodies (including itself), but the contact table and the contact parameters can be modified under Analysis | Load Step Creation | Solution Parameters | Contact Table. The contact table is located under Load Step Creation because it can change between steps. Patran puts circle markers on deformable body surfaces and arrows pointing inward on the meshed rigid bodies, and puts hash marks on the inner side of rigid geometry curves.
Marc master-slave contact interaction is defined by the parameters Contact Distance Tolerance, Bias Factor, and Seperation Force (can also use stress). The defaults for all contact bodies are defined on the Analysis | Job Parameters | Contact Parameters | Contact Detection form, but the values for individual contact pairs can be specified as part of the contact table. Master-slave contact interaction is described in the following figures. In this case the rigid body is the master and the deformable body is the slave. In the case of deformable-deformable contact the body created first (listed first in the contact table) is the master.
Figure B‑1 Contact Procedure
No contact is assumed as long as the deformable body does not come within the contact region (zones 2,3). Marc detects contact when the deformable body falls in the contact region (cases 2, 3 in Figure B‑2
) and applies a seperation force to prevent the bodies from pulling apart and the contact condition is defined as closed
. This same contact interaction model is used for deformable to deformable body contact where the master body is the one that comes first in the contact table. As mentioned previously, contact interaction is defined by the parameters Contact Distance Tolerance
, D, (see Figure B‑1
- by default Marc uses 1/20th
of the element edge length), Bias Factor
, B (see Figure B‑2
- Marc default on this is 0 but you can override this value on the Analysis | Job Parameters | Contact Parameters - Contact Detection
form) and Seperation Force
. The bias factor offsets the contact region as shown in Figure B‑2
Figure B‑2 Contact with Bias Factor
Note that in the case of contact penetration ( i.e., the node moves past the contact zone), the increment will split (if allowed). Splitting is when the load increment, which relates to the amount of penetration, is reduced until the node falls in the contact zone. If there is a problem with chattering (a condition where a particular node jumps into and out of contact thus preventing the increment from converging), you can go to Job Parameters | Contact Control Parameters | Seperation and set the Chattering toggle to Suppress. If you suppress chattering Marc will simply ignore this node after a few cycles of opening/closing.
Marc has a Glued contact option that is similar to ABAQUS tied contact. By defining two bodies as glued, slave nodes cannot penetrate, separate, or slide relative to the master surface. If glued contact is activated both the normal and tangential displacement of the node are constrained. It can be used for bonding surfaces together permanently and is frequently used for mesh refinement purposes. Bodies to be glued together are defined by a G on the contact table. By using glued contact and specifying a small separation force a condition of infinite friction can be modeled. Prior Marc versions required the user to specify a large separating force but the default in Version 2001 and beyond is that separation is
A capability was added in Marc 2001 to do stress-free initial contact. This capability is available in ABAQUS using the Initial Adjustment Tolerance on the Rigid - Deformable LBC form. Using this option in Marc, any slave node that falls within the contact zone defined by the Contact Distance Tolerance is projected to lie on the master surface such that any gaps or overlaps present in the initial model will not introduce undesired stresses. This can be activated in the contact table.
Frequently Asked Questions
Below are a few frequency asked questions of Patran Advanced FEA users switching to the
1. I have heard about a new Marc-based MSC.AFEA product. Exactly what is this MSC.AFEA product and what does the name stand for?
The MSC.AFEA product is an interlocked version of Patran and Marc that will have a reduced price, but will restrict access to Marc features that are not supported by the Patran and the Marc Preference. It also requires that Patran and Marc be run on the same machine. Inter-locked means that the user will NOT be able to hand-edit the input deck and submit it directly to Marc, or to submit the job to a Marc installation on another computer.
The name MSC.AFEA is derived from the combination of MSC and AFEA. The MSC part comes from the company title, MSC Software, and the AFEA part was selected due to name recognition of the discontinued Patran integrated non-linear analysis product sold by MSC software called Patran Advanced FEA.
2. Does MSC.AFEA or the Marc Preference have all the capabilities of Patran Advanced FEA?
It has everything and a lot more. The only item that is not supported to the same extent is in the area of random vibration analysis, although it is possible to do this in Marc with user subroutines. In addition to having all of the capabilities it also has much more as listed in Capabilities and Features
. The combination of Patran and Marc (MSC.AFEA) is one of the most powerful, and easy to use, software combination available for nonlinear FEA available anywhere. Just about anything you could do in Patran Advanced FEA can be done just as easily in MSC.AFEA.
Will my old Patran Advanced FEA models run directly in Marc?
See the above Reference Section
titled Database Conversion
. As much data as is possible is converted. Even after using the new mapping capabilities, models containing more advanced features such as nonlinear material models, gap and beam elements, multi-stepping, mpc's and more complex capabilities that vary from one solver to the next in their implementation will likely require those features to be recreated (or at least checked) after the database Preference has been changed.
3. My company is not planning to upgrade Patran 2003 for a while. Can I still use Patran to build my Marc models?
You should convert as soon a possible. The Marc Preference in Patran 9.0 and earlier had not kept up with changes in the latest releases of the Marc solver. In addition, there were several code defects, documentation errors and other deficiencies that made it difficult to build and completely run Marc models from earlier versions of Patran. There are also compatibility issues when you switch to Patran 2001 from version 9.5 and earlier in that the session and journal files Patran builds and uses as backup are not compatible, although the Marc Preference databases should successfully convert.
The major capability missing in the Marc Preference of earlier version before 2001 is multi-stepping. In versions 2000 r2 and earlier you could do multi-stepping by using restarts, which was fully supported. The only thing to remember about multi-stepping in Marc using restarts is that the loads default to incremental loads and not total values. If you want to move the end of a cantilever beam down 1 unit in step 1, and then over 1 unit in step 2 you would have to apply a displacement of -1.0 in the vertical direction in step 1, and in step 2, apply a vertical displacement of 0.0 and a horizontal displacement of one.