HydroDynamics and Wave Loading

Calculation of loads in Wajac depending on LOAD parameter on SEAOPT command for deterministic load calculation, program versions 6.6-07 to 7.0-01

The calculation of loads from marine growth has been improved and the LOAD parameter has been extended from version 6.6-07 via versions 6.7-09, 6.8-08 and 6.9-05 to 7.0-01. Refer to the attached documentation for updates on each release. Please see the attached document.

Back to top

Can Wajac print Summary of Minimum Base Shear and Minimum Overturning Moment, in addition to max value?

Question:

Can Wajac print Summary of Minimum Base Shear and Minimum Overturning Moment, in addition to max value?

Answer:

By default, summary of maximum base shear and overturning moment of all sea states will be printed in the Wajac listing file. But if the design load is defined as MinBaseShear, MinOMoment or MinBothLoads, then the summary of minimum base shear and minimum overturning moment will be printed in the listing file. It should be paid more attention to that the summary of minimum base shear and overturning moment only relates to the sea states have been defined with Minimum.

Back to top

Cutres: How is the result case numbering for wave loads done

Load case numbering in Cutres can be odd when having many wave directions and wave periods, from a frequency domain analysis. Sestra will sort the cases on wave directions, based on the input in the S#.FEM file From the example in the attachment, using 2 directions and 8 periods:

LC 1 = Stillwater
LC 2 (= 2-0) = heading 1, wave period 1
LC 3 (= 3-0) = heading 2, wave period 1
LC 2-1 = heading 1, wave period 2
LC 2-2 = heading 1, wave period 3
¦
LC 3-1 = heading 2, wave period 2
LC 3-2 = heading 2, wave period 3

Please see the attached document.

Back to top

GeniE: How is the corrosion addition property used in wave load calculation

When a corrosion addition property is assigned to a pipe section beam, the generated FEM file and the wave load calculation will be affected by the combination of Scantling idealization setting in meshing rules and Accurate corrosion addition setting in compatibility rules.

Scantling idealization determines original or corroded dimension is used to FEM generation and wave load calculation.

Accurate corrosion addition determines the beam is corroded from outer surface or inner surface

Take a beam with pile section 2mx50mm as an example, 5mm constant corrosion addition is assigned to the beam. The outer diameter Do, inner diameter Di in FEM file and outer diameter Do in wave load calculation are listed in the below table with different setting combination. The diameter of FEM element can be checked in T1.FEM file, MPRT card can be used to check the diameter used in Wajac.

Back to top

GeniE (All Versions): How are design wave load cases ordered

Symptoms:

GeniE will report the design load with the smAllest phase angle first, i.e. there is no fixed order in the base shear and overturning moment.

Solution:

We acknowledge that this is inconvenient in creating load combinations, as well as in interpreting the results. Until the implementation for this has been changed, a workaround is to create each wave in GeniE twice. You can then specify to retrieve the overturning moment from one wave and the base shear from another wave. This will involve a bit more work in defining the wave load cases, but it will ensure that the load case numbers for overturning moment and base shear are fixed.

Back to top

GeniE MorisonConstant to Wajac

Question: The defined MorisonConstant is assigned to beams. But it is not written into Wajac input file. Where does GeniE write it and how to check the applied Morison coefficients used in wave load calculations?

Answer: In a GeniE workspace, after the defined MorisonConstant is assigned to beams, it is written on SPROHYDR card in the T1.FEM file during the analysis. The SPROHYDR card is as below.

SPROHYDR  1.50000000E+01  2.00000000E+00  6.00000000E+00  5.01000000E+02
          0.00000000E+00  5.02000000E+02  1.14999998E+00  5.03000000E+02
          1.14999998E+00  5.04000000E+02  0.00000000E+00  5.05000000E+02
          1.35000002E+00  5.06000000E+02  1.35000002E+00

Please refer to the document Input Interface Format - Finite Element Model and Load Data Types for detail explanations of this card. User can include the command MPRT into the Wajac input file to make Wajac print out the Morison Coefficients used in wave load calculations for the selected waves and the selected elements.

Back to top

GeniE/Wajac (All Versions): Additional still water levels

There is a limitation in Wajac and GeniE Code check that do not allow to perform code check analysis when currently checked load combination contains additional steel water level.

It is possible to generate results in GeniE for those additional steel water levels by adding dummy load cases, however it is not possible to generate code check, as code check will be performed only for initial water level. For additional water levels hydrostatic pressure will be equal to zero.

Back to top

GeniE: Eigenvalue analysis including HydroDynamic added mass

When performing an eigenvalue analysis for a fixed offshore structure, it is important to take into account the HydroDynamic added mass. After setting up the HydroDynamic environment, the added mass is included as follows.

In the analysis, edit the Wave Load Analysis activity (through the folder tree or the activity monitor). In the top of the dialogue, change the option from Load calculation to Added mass and damping only. This will ignore all possible wave loads in the analysis. On the Added mass and damping tab, check Calculate added mass and Include internal water (if desired). This will include the effects of added mass due to the marine growth and will not neglect the internal water in the flooded beams. After this, Wajac will compute the HydroDynamic added mass and Sestra will take this into account in the natural frequency analysis.

Back to top

GeniE: How to export compartment inertia information to HydroD

There are two ways to export the compartment inertia information to HydroD for HydroDynamic analysis:

Mass Point: The compartment load can be represented as one mass point or several mass points in GeniE. The mass point will be simulated as mass element with the inertia information of each compartment. Dummy Hydro Pressure Load Case: Use the compartment manager to identify compartments. The Compartment Manager automatically identifies all closed volumes (closed by plates and shells). The compartments can be defined by compartment manager. Checking Dummy Hydro Pressure creates not a real load case rather it is used in connection with Wet Surface and HydroDynamic pressure loads computed by HydroD.

The compartment load defined in the GeniE cannot be identified by the HydroD as mass model. The compartment load is represented as pressure load applied on the boundary of the compartment.

Back to top

How to add a point load to a structural analysis with wave loads from HydroD/Wadam

If you add a load manually in GeniE, the important issue is to define this load in a load case not conflicting with the wave load cases created by HydroD/Wadam.

If you have a Morison model included, and want to use the wave loads on the Morison model in the structural analysis, the only recommended option is to define the additional load in a load case following after all the resulting wave load cases. If you have for example 20 wave periods and 10 directions, and include the static load case from HydroD/Wadam, there will be 201 hydro load cases. The additional load case in GeniE should then be put into FEM load case no. 202, or higher. And, for sure, the load case name is not important; it is the FEM load case number that counts. This number may be adjusted by going into the properties of the load case (right-click). A picture from GeniE is attached

If you do not have a Morison model, and you do not need to run fatigue (ok for ULS), you can specify in HydroD that the wave load cases shall start at e.g. no. 5 (WadamRun - Exe. Dir - Result Files - Load Transfer). That means that the first (static?) load case from Wadam will be no. 5, and you can define the additional load in load case 2-4. The wet surface definition in load case 1 is a dummy load, but should not be used for the additional load. Load cases for compartments, if any, should be available for the additional load.

It is of course important (as always) to check the sum of loads in Sestra.lis after the structural analysis has been run. The additional load case should be seen separated from the wave load cases. Please see the attached document.

Back to top

How to convert Sesam wave loads (L#.FEM) to Nastran bdf format

Nastran does not handle complex numbers (e.g. wave loads) the way Sesam does, thus Sesam wave loads cant be easily converted to and calculated in Nastran.

However, in a snapshot (point in time) of a wave from Wasim (on L-file format), the imaginary parts are all zero on both the BRIGAC and BEUSLO cards, and it is therefore possible to convert this information to equivalent Nastran format.

Nevertheless, there are some differences between the Sesam and Nastran implementation of relevant cards, so conversion is not straightforward. NastranToSesam (discontinued) and Sesam Converters only Partially support such conversion.

Here are some details:

Real rotational accelerations on Sesam BRIGAC cards are converted to Nastran RFORCE cards. (Supported, at least for global coordinate system.)

Real translational accelerations on Sesam BRIGAC cards need to be converted to Nastran ACCEL/GRAV cards. (Not supported.)

For translational accelerations (real values, not imaginary) in Nastran, either the GRAV or ACCEL cards can be used, see the attached notes from the Nastran manual. Since BGRAV is applied to the whole model, it is natural to use GRAV since it also applies to the whole model.

Workaround:

The workaround is to use Sestra instead of Nastran for the structural analysis. Please see the attached document.

Back to top

How to create .FEM file for HydroDynamic added mass analysis in Sestra

The implementation of added mass in Sestra requires the wet surface to be a single superelement consisting of three and four noded membrane elements with all nodes super (all translational dofs retained and all rotational dofs free) and coupled to structural nodes (in other superelement). Since GeniE currently can't define all nodes as super (retained), and Patran-Pre doesn't support membrane elements, the following procedure must be used to prepare the model with all membrane elements and all super nodes:

Export a T-FEM file of the wet surface from GeniE with membrane elements.

Export exactly the same model once more but with regular shell elements. Use a different name for the T-FEM file.

Read the model in #2 into Patran-Pre and define all nodes as restrained nodes (translational dofs = restrained, rotational dofs = free). Export T-FEM file with new name.

Check that element and node IDs are identical in the T-FEM files created in #2 and #3.

Copy the lines that contain the restrained nodes from the T-FEM file in #3 into T-FEM file #1

Change the value of NDOF on all BNBCD cards from 6.00000000E+00 to 3.00000000E+00 and remove the values for the rotational dofs, i.e. replace:

BNBCD 1.46100000E+03 6.00000000E+00 4.00000000E+00 4.00000000E+00
      4.00000000E+00 0.00000000E+00 0.00000000E+00 0.00000000E+00

with

BNBCD 1.46100000E+03 3.00000000E+00 4.00000000E+00 4.00000000E+00
      4.00000000E+00
using replace functionality in a text editor.

Use T-FEM #6 for added mass. Use T-FEM file created in #2 for structural strength.

Back to top

How to output a text file of the wave kinematics in Wajac

There are two ways to print the wave kinematics in Wajac.

KPRT this command can be used to print out fluid kinematics at a specified point.

The coordinate of this point is specified relative to the origin of the global coordinate system except for the Z coordinate which is relative to the mudline. The fluid velocity and acceleration are printed in Wajac.lis file. Maximum 100 points may be specified The command is only applicable for deterministic wave load calculation.

OPT9 in OPTI card OPT9 can be set to 1.0 2.0 to print the local data from member load generation.

OPT9 = 1.0, then fort.number files will be generated. OPT9 = 2.0, then prefix_LocalData_<file index>.lis file will be generated. The command can be used for deterministic wave load calculation and irregular wave load calculation. Below is an example in the _LocalData_6.lis file. The file contains the fluid velocity, acceleration, Morison load intensity value of each member.

Back to top

HydroD: Compartments and superelements

Can a superelement be mirrored in Presel and compartments/tanks still be used?

No. If a superelement is mirrored, the compartments will by default be defined across the space between the superelements, at least in Wadam. The centre of the compartment will be computed from the corners of the combined compartment's load case (from both the original and the mirrored superelement). This problem is that the same dummy load cases are defined in both superelements after the mirror operation. The solution is to mirror the superelement in GeniE, and renumber the compartment load cases, to create separate incidents of the superelements (e.g. T7.FEM and T8.FEM) to be assembled in Presel.

An exception is for a centre compartment with one half modelled in one superelement. When mirrored, this will make up the complete compartment.

Back to top

HydroD: Composite model: How to make sure Morison loads are included in the Sestra structural analysis

How to use a composite model (Morison model plus shell model) in a HydroD/Wadam/Wasim load transfer analysis?

In order to use the anchor loads and any other loads from the Morison model in the structural analysis in Sestra, the Morison model has to be part of the structural model.

The recommended method is to use a Single superelement composite model. This means that the complete model can be created in one model, i.e. one superelement (one T#.FEM file), and this file can be read into HydroD as both a Morison model and the Structural model. In this method, all loads, both accelerations, surface pressures and Morison loads, will be part of the same load file (L#.FEM).

More information is found in the Wadam user manual. The HydroD user manual and release notes (for HydroD 6 versions) can also be useful.

If the Morison model is a separate model (T#.FEM, e.g. T2.FEM), Wadam/Wasim will create a load file, e.g. L2.FEM, for the Morison loads, including anchor loads etc. Unless T2.FEM is also a part of the structural model, Sestra will not read the L2.FEM file. Only the L files matching the T files in the structural model will be used.

In this case a superelement model assembled in Presel is required. This means that supernodes (special boundary conditions) need to be defined in the Morison model, e.g. T2.FEM. These need to match the supernodes for the connecting superelements (shell model). Then read T2.FEM into Presel together with the other superelements etc.

Back to top

HydroD: Damping Tutorial

This FAQ describes how to create and use a free surface mesh in HydroD and Wadam. A Sesam Manager zip file is: HydroD 4.10, HydroMesh, Wadam and Postresp are used in this example. Create a new job in Sesam Manager and import the zip file. Open the HydroD_DampingTutorial.pdf file attached to the job and follow the instructions.

NOTE: After importing the zip file make sure the HydroD version is 4.10.

There are two purposes of this tutorial:

  1. Show how to create free surface meshes (models) using HydroMesh
  2. Show how to use these models in Wadam for: a. Damping surfaces in moonpools or narrow gaps b. Fixed lids for irregular frequency removal c. Free surface meshes for any of the following uses i. Second-order analysis ii. Wave drift damping or forward speed analysis iii. Offbody points

Back to top

HydroD Wadam: Coordinate systems

The origin of the input system is defined as the origin of the model system after a possible translation in HydroD, this because HydroD will perform the translation by actually changing the various coordinates in the T#.FEM file before it is handed over to Wadam. The global coordinate system of HydroD and Wadam has its origin in the water line, directly above the origin of the input system - normal to the water plane.

When a structural model is translated in HydroD, and used in a load transfer analysis, it is very important to use the translated T#.FEM file in any subsequent structural analysis, in Sestra. The translated T#.FEM file is found in the relevant WadamRun folder within the HydroD workspace.

Back to top

HydroD Wadam: Morison model and beam element type

Before Wadam version 9.7: lease note that the Morison model used in Wadam has to be created by using the standard 2 node beam element.

Beam elements meshed as second/higher order, 3 node, beam elements will be neglected by Wadam.

A typical message in the print file from Wadam, Wadam1.lis is, in section 2.2:

  • nn - ELEMENTS OF ILLEGAL TYPE ARE DETECTED AND DROPPED.

When creating the Morison model in GeniE, this element type is ensured by NOT selecting the option for use of second order elements in the Edit - Rules - Meshing dialogue.

Back to top

HydroD Wasim: T-files created from meshing a .PLN file

HydroD will create a number of T-files when meshing the section model (.pln file). The files are described as follows:

T7301.FEM - mesh of dry part of structure (above sea)

T7302.FEM - mesh of wet part of structure

T7303.FEM - mesh of sea

T7310.FEM - mesh of structure + sea (T7301+T7302+T7303)

T7320.FEM - mesh of structure (T7301+T7302), may be used as panel model

all these models are given in the input coordinate system (same as the section model).

T7310 includes mirror images in the case of symmetry. In addition, the model T7373.FEM is also mesh of the sea, but in the global coordinate system.

T7320.FEM does not contain symmetric parts. It is just the union of the wet and dry part. This superelement model can be used as panel model for Wadam for all loading conditions. This is what actually happens automatically when you import a section model, create the SectionHullMesh and refer to this HydroModel in a Wadam or hydrostatic analysis. The symmetry property is also automatically handled.

T7310 is used if you want to inspect the mesh in Xtract. It is not used for anything in connection with any type of HydroD analysis. Inspecting the mesh in Xtract was important in the old Wasim Manager which had limited graphical functionality, but it is not really needed with HydroD so this file is basically superfluous.

T7373.FEM - mesh of sea in Global coordinate system. May potentially be used as surface model in a Second order or a Wave Drift Damping Wadam analysis or alternatively as an offbody model for Wadam animations. In the last case it is however probable that in the case of symmetry you will want to create a model which includes symmetric parts.

With the possible exception of T7373 (and T7310 if you really want to use Xtract to inspect the mesh) the user should not really need to relate to any of these files. (As mentioned T7320 is automatically used as panel model without any need to specify this for the user).

Back to top

HydroD/Wadam: How to use file names for models in a Multibody analysis

Regarding the T#.FEM files in a multibody analysis, the panel models for different vessels must have a unique'superelement' number (e.g. T1.FEM and T2.FEM). They cannot be distinguished by a prefix in the file name, or by a different path, only.

The reason for this is that HydroD will strip off the path\prefix when copying these files into the Wadam run folder, thus making Wadam see only one of the files, if they both have names like <path\prefix>T1.FEM. Please also remember that this superelement number in the file name needs to be defined in the model, like in GeniE (Edit - Rules - Meshing). Renaming the file from for example T1.FEM to T2.FEM will not work because this number is also given inside the file (in the first line).

Back to top

HydroD/Wadam: Prefix of T#.FEM files

When T#.FEM file are read into HydroD/Wadam, a prefix of the T file will automatically be neglected and only the characters after T will be read by Wadam.

For example, VesselT1.FEM and ShipT1.FEM will have the same name in a Wadam run in HydroD, which is T1.FEM. This will cause trouble if more than one HydroModel exists in one workspace and different T files are read in different places, for example in a multibody analysis.

So T#.FEM files are needed to be assigned with different recognized numbers, like VesselT1.FEM and ShipT2.FEM.

Please also remember that this superelement number in the file name needs to be defined in the model, like in GeniE (Edit - Rules - Meshing). Renaming the file from for example T1.FEM to T2.FEM will not work because this number is also given inside the file.

Back to top

HydroD: How to include compartments when using multiple instances of the superelement in Presel

It is not possible to reuse superelements with compartment definitions in HydroD. The only exception is if a compartment is actually split in two or more superelements, e.g. at the centre line of a vessel.

The reason for this is that the load case definitions for compartments must be unique in the 1st level models. Reused superelements will have the same load case numbers as the original, modelled, superelements. Load combinations in Presel are not used for these dummy load cases. HydroD, Wadam and Wasim will read the definitions as created in the 1st level model only.

The way to do this with superelements is to create more superelement T-files in GeniE, with specific load case numbers for the compartments in each; one superelement for each location in the complete model. Or, alternatively, not use the superelement technique this way.

Back to top

HydroD: How to include mooring stiffness into the motion analysis

The anchor stiffness is included by way of a Morison model. Given a Morison model, normally created in GeniE, mooring stiffness may be added by an anchor element or a TLP element and the corresponding anchor/tlp properties.

The Morison model may consist of one or more beams only, with their nodes giving positions for the mooring elements.

To include the mooring force into a load transfer analysis, the Morison model must normally be assembled with the shell structural model in a superelement assembly (using Presel).

Alternatively, a restoring matrix may be defined directly.

Back to top

HydroD: How to select filling fractions for sub model

If the whole compartment in the sub model is fully wet or dry, then the filling fraction for that compartment can be defined to be 1 or 0.

If a compartment is not completely modelled in the sub model, and it is partly filled only, then some special technic is needed for filling fraction defined.

Go to GeniE first, using the global model and look at the interesting compartment. Carefully select the wetted/submerged internal compartment surface in the sub model, according to the filling fraction, assign them wet surface property. Then apply the correct load case number.

Then run submod (the same as before).

Import into HydroD the modified sub model with only partly defined wetted internal surface.

Assign filling fraction for this compartment to be 1.

So the correct internal wet surface will be generated from HydroD and read into Wadam/Wasim.

Also remember to define the correct Compartment points, typically taken from the global analysis, from Wadam.lis or from HydroD information.

Back to top

HydroD: How to use (old) quasi-static load transfer option and local structure model with HydroD

The calculation of static load inside a compartment may be difficult when the tank is not modelled completely.

When using the (old) quasi-static method, defining Compartment points in HydroD is required (in the Loading Condition) to give Wadam the correct position of the acceleration and zero pressure points. The correct position may typically be found from the compartment data for the global, complete, model. Right-click a compartment and select Information.

If the local model contains parts above the free surface of the compartment (but still not the complete comparment), HydroD cannot remove properly the wet part of the compartment above the actual free surface, as in normal cases.

To avoid this problem, the best way is to remove the wet surface, or dummy hydro pressure, from the elements above the free surface. This must be done in the modeller, e.g. GeniE or Patran-Pre.

In some cases, simulating a high filling fraction (like almost full) may be done by defining a full tank with a reduced density.

Back to top

HydroD: Why is there some times a problem in using a model from Patran-Pre

If a material and thickness is not properly defined, the T#.FEM file from Patran-Pre will not be correct.

The thickness record (GELTH) is written to the T-file with zero thickness for shell elements that have no property defined in Patran-Pre. Reading of this T-file by other programes (e.g. HydroD, Wadam or Sestra) will result in error termination.

Back to top

License error: invalid host when starting old Sesam programs (HydroD 4.10, Sestra 8.8, Profast)

License error: invalid host when starting old Sesam program (HydroD 4.10, Sestra 8.8, Profast) HydroD4.10, Sestra 8.8, Profast, and some other old Sesam programs, are not compatible with the latest dongle driver on some windows systems. The walkaround is to downgrade the dongle driver to 11.15.

  1. Delete the HASP folder in registry editor, as shown below. This will uninstall the license dongle driver.
  2. Install License dongle driver 11.15, which can be downloaded from (copy link if not working)

Back to top

Postresp: How to define off body points for Postresp in a HydroD and Wadam analysis

To use off body point results in Postresp, specific off body points must be defined in HydroD, using coordinates given in the Global coordinate system, i.e. having the origin in the still water line.

Further calculations can be done in Postresp on the results in these off body points.

The off body point grid is used for visualization & animation in Xtract only.

Back to top

Prepost: Use of CREATE HydroDYNAMIC-INTERFACE

Prepost can convert results from a structural results file R#.SIN, based on frequency domain wave loads, to a HydroDynamic type of results file, like G1.SIF, for use in Postresp.

This is for example relevant if statistical calculations are needed for structural responses of stresses or displacements, because Postresp cannot read the R file directly. The command syntax is typically:

OPEN, SIN-DIRECT-ACCESS, ' ' R100, OLD, READ-ONLY CREATE HydroDYNAMIC-INTERFACE, ' ', G1, 1 NODAL-DISPLACEMENTS 1 X END

Please see the user manual for Prepost for details.

Notice that this command is only available if the S#.FEM file is available when running Sestra, together with the T#.FEM and L#.FEM files.

Back to top

Presel HydroD Xtract: Display of beam elements from Equipment vertical mass option

The display of beam elements from the equipment vertical mass option is different in Presel, HydroD and Xtract.

Presel and HydroD will show the "vertical mass" beam elements as beam 'tents', i.e. without eccentricities, in the same way as for the option "beams and mass" from equipments.

Xtract will show the vertical beam elements, i.e. with eccentricities, when the beam cross section is shown. In wireframe mode of beam elements, the eccentricities are not shown. The beam elements are shown in the same way as for the option "beams and mass" from equipments.

Back to top

Sesam: How to enable stochastic fatigue for a submodel with no local wave loads

Including local loads like wave loads is normally recommended in a submodel analysis. However, if the wave loads are not important for the submodel analysis, the local wave load analysis may be skipped. In that case the file S#.FEM, required for stochastic fatigue, needs to be created for the submodel.

The S#.FEM file has to be present when Sestra is run for the submodel, together with the T#.FEM file(s) - and L#.FEM file(s) for possible local loads. If not, no stochastic fatigue can be computed later.

As the wave load cases for the submodel have to match the wave load cases for the global model, the global S#.FEM file (e.g. S1.FEM) can be copied and renamed to the submodel superelement number (e.g. S4.FEM).

Renaming the file is okay because the contents are Sestra commands. (Renaming a T#.FEM model file is not okay.)

Please notice that the contents of the S#.FEM file are described in the Sestra user manual.

Back to top

Wadam/Sestra: Mass information has to exist in structure model for load transfer and later strength analysis

If you want to do load transfer in HydroD and strength analysis in Sestra, mass information has to exist in your structure model.

For the mass related issues, Wadam/HydroD will calculate inertial loads from the mass information. These loads will contribute to calculation of the global forces and motions.

Also the accelerations will be transferred into Sestra. When you do the structure analysis, Sestra will only use the acceleration load from Wadam and the mass from the structure model to add gravity effect. So, your structure model should have mass information, similar to the mass input in HydroD/Wadam.

Back to top

Wadam: How are not-flat elements handled in a panel model

All panels in a Wadam analysis are adapted to be flat panels. For both lower and higher order shell and solid elements, Wadam will adjust the nodes into a flat , 3 or 4 noded, panel. This also when there is an out-of-plane issue with the lower order elements. This means that the normal vector of the panel may be different from the original normal vector of the element, which again can be an issue for example in the use of tolerances in a Wadam load transfer analysis. Wadam will use the definition of the wet surface, or dummy hydro pressure, in load case 1, for both shell and solid elements, to select the panels. This is described in more detail in the Wadam user manual, section 2.1.2.

After a Wadam analysis, there will be a file called panelT1.fem in the Wadam run folder. This is the actual panel model used in the calculations, after Wadam has handled the original panel model, including any cutting of the model at the water line etc. This model can be displayed in for example Xtract, as verification.

Back to top

Wadam: How to interpret the printed balance of mass and buoyancy in section 2.7 in Wadam.lis

First, the vertical tolerance is given in HydroD, relative to the characteristic length. Wadam will stop if the tolerances are exceeded.

Any imbalance between mass and buoyancy will be printed as a vertical resultant force (F3), and as a distance/translation in length unit, at the bottom of section 2.7 in Wadam.lis. The translation is for information only, no translation will be performed by Wadam. A distance of for example 0.5 means that the vessel should be translated up by 0.5 length units to achieve perfect balance.

The individual values for mass and buoyancy are printed in the same section.

Notice that the resulting force in a following structural analysis in Sestra may differ from the results in Wadam. This is mainly because of potential differences in the normal vectors of the models, due to different mesh of the panel model and the structural model. Differences in the mass distribution between the mass used in HydroD/Wadam and the mass of the structural model are also important.

Back to top

Wadam: How to solve error from drift force calculation with pressure integration

When drift forces from all degrees of freedom is wanted, the pressure integration method is used. This puts more strict requirements to the mesh of the panel model, especially at the waterline. (The alternative is to calculate only the horizontal drift forces.)

If Wadam stops, you may see the following message in the file poten.log:

Error in evaluating Rankine matrix

If this is the case, please inspect the panel model closely, with respect to the waterline. Avoid defining the waterline just above the element borders of the model, as Wadam will cut the panel model at the waterline. This may result in tiny and badly shaped elements.

It is most useful to check the file panelT1.FEM, created by Wadam (found in the Wadam run folder). This is the panel model actually used in the calculations, after being cut at the waterline (and at the sea bed).

It may be useful to put on the element labels, to more clearly view any small elements at the waterline. An example from Xtract is shown in the attachment, where some additional element labels are shown above the main ones. Please see the attached document.

Back to top

Wadam: Load transfer analysis with NO MATCH written in Wadam.lis.

Problems with NO MATCH' stated in Wadam.lis for a load transfer analysis should in general be inspected. This means that the listed elements (in the structure model) will have no wave pressure in the structural analysis, and subsequently problems with lower accuracy and increased reaction forces may occur. Local results at these elements will also be affected.

A good way of checking this issue is to plot the pressures in Xtract, from reading the T#.FEM file for the structural model (the L#.FEM file will be read automatically). Elements without pressure will show up as grey elements, without colour contours, when the pressures are displayed.

A work around may be to increase the load transfer tolerances defined in HydroD. If this is not sufficient, the panel model and structural model should be inspected. If there are only a few of these elements, the message can normally be neglected.

Notice that this may also indicate that the definition of the wet surfaces (dummy hydro pressure) in the structure model is not correct. Wadam will find all such elements defined in load case 1, both on the outside and inside of the model.

Example:

  * 2023                   NO MATCH   (24, 1, 0)

 ** A TOTAL OF   29 LEGAL ELEMENTS IN ACTUAL OCCURENCE NO.       2
   OF SUPERELEMENT TYPE      23 DID NOT MATCH!

The numbers in the brackets, (24, 1, 0), indicate that Wadam will search up to 25 panels to find one that can match with the structural element. The load transfer tolerances are used, out of plane/distance and normal vector angle, (dist, ang, 0).

Back to top

Wajac: What are ILLEGAL ELEMENTS

Question: When running the model, Wajac produces the warning below. How to identify the illegal elements so that you can decide whether this issue needs corrected

Answers: This warning indicates that there are illegal elements in the model, which will lead to the reported structure mass in " W E I G H T A N D B U O Y A N C Y S U M M A R Y" is incorrect as they are not counted in the mass calculation.

Please notice that only beam type BEAS is supported by Wajac. So any other beam type like truss elements (TESS), second order beam elements (BTSS) will be issued as illegal elements.

Back to top

Wajac (All Versions): HydroDynamic results file generations takes too long

If you are running Wajac and it takes hours in finishing while generating HydroDynamic results file G1.SIU then please check as follows, There may be a wrong entry on OPTI card. If you change OPT3 option from 3 to 2 then it will work fine. Please make sure that all the entries are at correct positions. For spacings, please see user manual. OPTI 0. 0. 2. 0. 0. 0. 0. 0.

Back to top

Wajac (All Versions): Waveloads and Buoyancy including eccentricities

The OPT8 under the OPTI command governs the consideration of element eccentricities in load calculation. It applie to both wave and buoyancy calculation. If OPT8 = 0 or blank, eccentricities will be taken into account for calculations of both wave & buoyancy load, and if OPT8 = 1, eccentricities will not be considered in both wave and buoyancy calculations.

Back to top

Wajac (All Versions): Wind loads without wave loads

If you want to compute only wind loads on the structure then you have to use a dummy wave load condition with it in GeniE. This is a limitation. Dummy wave load condition might have calm sea condition, buoyancy may optionally be switched off.

Back to top

Wajac (All Versions): HydroDynamic added mass in eigenvalue analysis run

Create a dummy loadcase with fem loadcase number 11. Now create dummy waveload condition and add Wajac activity to the analysis. Select Added mass and dampling tab for calculation and click Apply. Now waveload case has fem number 12. 1 to 10 are the eigenmodes.

Back to top

Wajac (All Versions): Marine Growth Weight and Buoyancy always on

When defining a loadcase with sea water level and Marine Growth, the vertical load due to Marine Growth is always the vectorial sum of its weight and buoyancy. This is independent of turning on or off the buoyancy calculation and only applies to the amount of Marine Growth that is submerged. all other Marine Growth is neglected.

Back to top

Wajac (V6.2-01 from All): Error in Dean Stream function seastate parameters

For Dean Stream function theory to be used for computation of wave kinematics, the three errors which are computed should sum up to higher than 0.0001, if less than 0.0001 then we get error for this wave theory. Below is a link which has a flash window for inputting the sea state parameters.

After you click on 'calculate', the errors are listed to the left side in a window, the three errors are

  • Wave Height Error:
  • Mean Sea Level Error:
  • Bernoulli RMS Error:

Sum of these three errors should be higher than 0.0001.

http://www.coastal.udel.edu/faculty/rad/streamless.html

Back to top

Wajac (V6.2-01 from All): Height of breaking wave

print in Wajac .lis file:

Error: The wave height is exceeding the breaking wave height

Height of breaking wave is computed using the following equation:

Hb = 0.142 * L

where L is the wave length and Hb is height of breaking wave

L = (g* T^2)/(2*pi);

If you are using any other theory than Airy wave theory, Wajac will still consider wavelength computed by Airy wave theory. Rest of the calculations will be based on actual wave-length computed by relevant selected wave theory but only the comparison for height of breaking wave is done on the basis of airy wave theory wave-length. This will be corrected in the future versions.

Back to top

Wajac: Dean Stream function....Current

The implementation of Dean Stream Function is according to Dean, R.G.: Stream Function Representation of Nonlinear Ocean Waves, Journal of Geophysical Research, Vol. 70. No. 18, 1965 Dean, R.G.: Relative Validities of Water Wave Theories, Journal of the Waterways and Harbours Division, ASCE, 1970 as given in the reference list of Sesam:Wajac.

There is also a very nice web calculator for stream function wave kinematics developed by Professor Dean at Univ of Delaware,

Back to top

Wajac: HydroDynamic coefficients have not been specified by the Wajac analysis control data.

Wajac can give the following Warning saying that HydroDynamic coefficients have not been specified by the Wajac analysis control data.

*** WARNING: HydroDYNAMIC COEFFICIENTS HAVE NOT BEEN SPECIFIED BY THE Wajac ANALYSIS

    CONTROL DATA. ENSURE THAT THE COEFFICIENTS ARE SPECIFIED ON THE Sesam INTERFACE FILE ***

This warning means that you did not specify a HydroDynamic coefficient in the Wajac input file manually. However, an easier way in most cases is to specify those coefficients directly in GeniE, so that hydro coefficients are included in the *T.FEM file.

Both ways are correct, but if you choose to use GeniE to specify coefficients, it will give you the warning mentioned above.

Back to top

Why is there a mismatch between the loads reported in Wajac.lis and Sestra.lis?

In some cases, the wave loads reported in Wajac.lis might not match those in Sestra.lis.

An obvious reason can be errors in the load transfer, but another reason which is not related to an error is the following.

The cause of the difference between Wajac and Sestra can be due to non-zero Cdx and/or Cmx components (drag and inertia coefficient along the member) specified in the Morison coefficients in the model.

Wajac will use the Cdx and Cmx components to calculate the loading on the model, and will find the overturning moment and base shear including these loads. However, the loads are only used by Wajac to compute the overturning moment and base shear. As such, these values are correct and the correct phase angle is found for the wave loads. The wave loads for those phase angles are then used in Sestra, but without the Cdx and Cmx components of the load. These are only used to find the overturning moment and base shear and will not be used in the structural analysis afterwards. If the Cdx and Cmx components of the Morison coefficients are set to zero, the values in Wajac.lis and Sestra.lis will be the same. Otherwise, the values in Wajac will be different due to the added Cdx and Cmx component used for the Wajac determination of the phase angles of maximum overturning moment and base shear.

Hence, adjusting the Cdx and Cmx values to 0, which is how Sestra gets the loads from Wajac, makes Wajac and Sestra report the same. Note that the main difference is that in the case the Cdx and Cmx are not equal to zero, the phase angle found at which the maximum base shear occurs may change compared to when Cdx=0 and Cmx=0.

Back to top