GeniE

On this page

ACIS errors documentation

Version: All

ACIS is the geometry modeller in GeniE. There may appear some warnings/errors from verification in GeniE (Tools> Structure> Verify). Some of these warnings/errors may be severe while some may not affect the mesh of the concept model so we recomend you to mesh the model after getting such warnings. If mesh is ok and you are allowed to do further modelling then ignore such warnings. If you are not able to proceed with further modelling then delete the members giving ACIS errors and mesh the model again. Some info about the ACIS errors/warnings are given on the spatial website. The users which are interested in finding more about these warnings/errors may visit the following link,

ACIS_Checker_-_ID_Macros
Types_of_Checks

Back to top

Additional still water levels (GeniE/Wajac)

Version: All

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 codecheck, as codecheck will be performed only for initial water level. For additional water levels hydrostatic pressure will be equal to zero.

Back to top

Applying loads on a full circular beams in GeniE are doubled

The loads are doubled if the beams are either full circle or semi circle.

The proposed workaround is to have 4 beams around the circumference of the tube, and apply a load to each of them.

This can be done by dividing the beams again, such that each covers a sector of 90 degrees. After division, the loads must again be applied to the newly created beams.

Back to top

Best practice for hull modelling in Sesam GeniE

Version: All from 7.3-15

See the Best practice for hull modelling in Sesam GeniE V7 - Rev 4.pdf for both overview and details of how to create typical hull models in GeniE.

Note that especially for modelling of the skin of ship-shaped vessels new functionality has been added to GeniE since this document was written. See the Hull Design Tools -> Create Ship Hull from Transverse Polylines and similar functions.

Back to top

Boolean operation error in GeniE when executing JScript

Version: All from 6.5-04

When executing the following commands in GeniE:

val1 = 1;
val2 = 2;
val3 = 3;

print((val1 <= val2) && (val2 >= varl));
print((val1 <= val2) || (val2 >= val3));

GeniE will throw an exception: JS0001 Cannot convert (line: 1: type -> bool).

The workaround is to use a later version of GeniE.

Back to top

Bulb profiles from Nauticus Hull to Sesam GeniE

Version: All

Bulb profiles are not implemented in Sesam GeniE, and will be substituted by Angle profiles. 

When extruding a 2-dimensional Section Scantlings model from Nauticus Hull to a 3-dimensional GeniE concept model, all Bulb profiles are automatically converted to Angle bars with approximately the same section properties, e.g. the section modulus should be as close as possible.

If the automated procedure doesn't work properly, e.g. the section properties are missing for some of the beams in the concept xml file, the following warning message is issued in GeniE:

Warning:
XML-import problems
While importing/exporting ………:
No  prSection named Bulb….. exists
-> DNV_structure_concept_protocol : model …………

Workaround:

Users must find a substitute profile to use instead of the Bulb profiles. Then there are two options:

  1. Replace the Bulbs with the substitute in Nauticus Hull – Section Scantlings
  2. Keep the Bulbs in Section Scantlings. Attach the substitute profile to the beams that have no profile in GeniE.

See also FAQ no. 00004109 "How to convert small bulb profiles to angle profiles with similar properties".

Back to top

Can't delete object from GeniE, script execution error

Version: All

If you get a script error about unnamed object when trying to delete an object from a GeniE workspace, try the following workaround:

Add all named objects to a named set and export a concept XML file using the option Export subset. Then import the concept XML file into a new workspace.

Back to top

##How to create a dynamic set? Version: All

Besides the 'Create set' option, GeniE gives you tools to create a 'dynamic set'.

The difference between a 'set' and a 'dynamic set' is that dynamic sets are continuously updated when creating new objects.

Today, the only option to create a ‘dynamic set’ is to use GeniE JScript language with the following commands.

The command used to create a dynamic set is:

DynamicSet(AbstractLimit);

Where AbstractLimit is one of the following limit functions:

LimitAbovePlane(Plane3d) – Add to the dynamic set all objects above specified Plane3d();

LimitAnd(AbstractLimit, AbstractLimit) – Combine 2 limit functions;

LimitBelowPlane(Plane3d) – Add to the set all objects below specified Plane3d

LimitBox(Point, Point) – Add to the set all objects that are inside cube spread along main axis between specified points

LimitInOrAbovePlane(Plane3d())  – Add to the set all objects that are above or exactly on the Plane3d();

LimitInOrBelowPlane(Plane3d())  – Add to the set all objects that are below or exactly on the Plane3d();

LimitInPlane(Plane3d()) - Add to the set all objects that are exactly on the Plane3d();

LimitInSet(AbstractSet) – Add to the dynamic set objects from another Set, doesn’t work when you want to add to dynamic set objects from another dynamic set.

LimitLine(Point, Point) – Add to the dynamic set all objects that are exactly on the specified line

LimitLower(string, Variant) – Add to the dynamic set all objects with specified property (as string) and value that is lower than specified, e.g. LimitLower("Height",0.3)

LimitLowerInclusive(string, Variant) - Add to the dynamic set all objects with specified property (as string) and value that is lower or equal to specified, e.g. LimitLower("Height",0.3)

LimitNot(AbstractLimit) – Exclude selected limit from dynamic set

LimitNumber(string, Variant, tlLimitNumber) – Check if value of property is within limit

LimitOr(AbstractLimit, AbstractLimit) – Create a dynamic set that is union of two or more existing dynamic sets.

LimitPlane(plane3d, LimitPlane) – Add to the set all objects that are laying exactly on the specified plane3d

LimitString(string, string, bool) – Add to the dynamic set all objects that contains specified name

LimitUppedInclusive - Add to the dynamic set all objects with specified property (as string) and value that is higher or equal to specified, e.g. LimitLower("Height",0.3)

LimitUpper - Add to the dynamic set all objects with specified property (as string) and value that is higher than specified, e.g. LimitLower("Height",0.3)

Examples of Dynamic sets:

//This example adds i.e. web frames to dynamic sets.

//Script will create frames from (FromFrame) to (ToFrame) in spacing of (FrameSpace).

//Script can be modified to be used along Y or Z axis as well.

//***** Dynamic Sets *****// var FromFrame = -5; var ToFrame = 235; var Framespace = 0.8 m; var ActualIndex; var ActualFrameX; var FrameName; var FrameSetArray = Array(); for (i = FromFrame; i < ToFrame + 1; i++)
{
 ActualIndex = i + Math.Abs(FromFrame);
 ActualFrameX = i * Framespace;
 FrameName = "FR" + i;
 FrameSetArray[ActualIndex] = DynamicSet(LimitInPlane(XPlane3D(ActualFrameX)));
 FrameSetArray[ActualIndex].name = FrameName;
}

//This script converts all dynamic set in workspace into regular sets.

for (var namedSetObject in ModelObjects)
{
  if( namedSetObject.supportsType(typeSet) )
  {
    var arrayOfObjectsInSet = new Array();
    var name = namedSetObject.name;
    tempSet = Set();

    for (var objectInSet in namedSetObject)
    {
      arrayOfObjectsInSet.push(objectInSet);
      tempSet.add(objectToAdd);
    }

    Delete(namedSetObject); 
    tempSet.name = name;
  }
}

Back to top

Changing default version of GeniE in Brix Explorer for Sesam

Version: All

Go to folder C:\Program Files\DNVS\Sesam\BRIXExplorer\config

Open sesam.config file in some editor. Check for the location of GeniE in the file. Change it to your desired GenIE version location and save the file. NOw Start Brix and default GeniE version will be picked from your desired location.

Back to top

Changing the File association of the .gni File

If the file association of the .gni file has been set to some specific version and user faces problem opening the file in the right version of the programe. Then it can avoided by deleting the .gni file associations from the registry settings.

"Run---regedit----HKEY_CURRENT_USER---gni_auto_file" and delete the default. Also make sure that all other .gni file associations are deleted.

Back to top

Chords and braces in Genie

When GeniE identifies chords and braces it assesses the following criteria in prioritized order:

  1. Diameter of section
  2. Beams with internal joints
  3. Length of the beams
  4. Names

Cross section thickness is not taken into account.

There was a change order for this in our development database so hopefully it will be corrected soon.

In your case it is the length of the beams that becomes governing. The option you have to overrule it is the "Beams with internal joints". If you join the two beams that you want as cord to one beam the joint becomes an internal joint for that beam. The other two beams will have end joints. This way you can control which one to use as cord.

There is one issue with this. An X joint should actually be modelled with two continuous beams. Then GeniE will know that these beams should be kept straight when you introduce gaps at the ends. It seems like you have accounted for this manually in your model by moving the X joint to make the beams straight. When using one joined and one split beam to control cord/brace you still have to align the beams manually.

I hope you can use this workaround until GeniE accounts for the thickness in joint classification.

Regards, for Det Norske Veritas AS John Martin Larsen

Global Technical Support DNV Software

Back to top

Conical sections for non-tubulars

Version: All

Description: After applying a non-tubular cone section, GeniE shows the section in the graphical user interface, but will not mesh the segment. Sestra will give an error when trying to analyse.

Explanation: Cone sections for beams are only working for tubular sections. As such, non-tubular variable sections will not get meshed and will subsequently give an error in Sestra.

Workaround: As a workaround, one can apply an average cross-section to the beam segment for which one wanted to have the cone. When GeniE meshes a tubular cone section it will transfer the cone into an equivalent diameter section as well, so in principle one could do the same straightaway in the modeller.

Another method is to model the model the conical segment using plates and connect these to the beams using support rigid links.

Back to top

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

Ensure GeniE generates correct Sestra input file

This is applicable when a user cant use the Automatic generation of input files due to some of the cards not being supported via GeniE GUI or analysis type not supported directly in GeniE. Users can uncheck Automatic generation of input files at any Edit Analysis dialog box (i.e. Linear Analysis). To ensure that all input cards required from GUI are updated in Sestra.inp file when clicking Generate input files, the user needs to follow the below steps:

  1. select the required solver (or any other input)
  2. click "Apply"
  3. click "Generate Input files"
  4. click "OK" to close the dialog box The generated input file may then be edited and will not be overwritten as long as Automatic generation of input files remains unchecked. The contents of Sestra.inp is further described in the Sestra user manual.

Back to top

Error – Mass matrix Max index and NDOF_rmFixedDofs do not match

If when running earthquake analysis in Genie, the below error is issued.

This error is related to the file M1.SIF generated in eigenvalue analysis.

For earthquake analysis, we need run eigenvalue analysis twice with different options. The sequence is mandatory.

  • First run: check the option "Mass Matrix", run the analysis to generate M1.SIF.

If there are supernodes in the structure, then in this step, the user need modify the Sestra.inp file manually to remove the DRED card.

  • Second run: uncheck the option "Mass Matrix", but check the option "Modal Mass Factors", run the analysis to generate R1.SIN and save the modal mass participation factors.

If this error is issued, there are two possibilities:

  • There is no M1.SIF generated in the first run
  • There are supernodes in the structure, but DRED card is not removed manually in the first run

Back to top

ERROR in input on T-file, data is missing for element

Version: All from 7.2-02

If Sestra 8.8-02 aborts with the following error message:

  *** ERROR in input on T-file ***                                                                                                 
      for superelement type     1 on level  1                                                                                      

      Check of T-file (.FEM) revealed the following errors:                                                                        

    * Material data is missing for element 221137                                                                                  
      (the reference number in GELREF1 is zero)                                                                                    
    * Geometry data is missing for element 221137                                                                                  
      (the reference number in GELREF1 is zero)                                                                                    
    * Local coordinate system is not defined for element 221137                                                                    
      (the reference number in GELREF1 is zero)

or Sestra 10 with the error message:

Execution failed!
    Error when fetching beam orientation vector for internal element number 50657. Unable to find the unit vector with transformation id 0.

this is likely caused by some orhpaned and duplicate elements without properties. The orphaned elements come from a bug during import in older GeniE versions, but the issue was fixed in version 7.4-18 (and later). The error may occur in models created in older versions. If you encounter the error use the following script (paste to command line) to simply remove the elements. The script command is available since version 7.3-15.

Me_Analysis1 = MeshEditor(Analysis1);
Analysis1.step(1).DeleteLoads();
Me_Analysis1.RemoveOrphanElements();

Back to top

Exception caught: Database not supported

Version: All

This error occurs when a workspace created in a newer version of GeniE is opened in an older version of GeniE.

To fix this problem, you can either install the older version of GeniE and open it or import the analysis by creating a new Workspace, then selecting File -> Read Command File.

Browse and select the *.js file of the old analysis and click Open.

Alternatively, importing xml file is a better option.

Back to top

Export GeniE model to CAD system

There is no direct way to export GeniE to DWG file. As we know, GeniE indeed can export to CAD system with .SAT format. It is just that Autodesk Inventor is stuck with ACIS v7, while we continuously update ACIS, but it is unfortunately not possible to write out an older version.

Workaround:

  • In some tools, i.e. Solidworks, it is possible to downgrade the SAT file to an earlier version. Maybe it is possible to download some trial of Solidworks to try it out.
  • It is also possible to export from GeniE to PDMS. However, please note that this will not include the “beam section sizes and dimensions”. The only information that is exported is the beam geometry, so the lines of the beam from node to node (without the actual beam section and thickness). If needed, manually add the actual beam section size and thickness in PDMS

The only file that should be exported to PDMS is the *.sdn file (in GeniE, use File > Export > CadCentre PDMS). There is possibility that the PDMS is not compatible with current GeniE version of SDNF export.

Back to top

Exporting models to SACS

Although it is possible to import models from SACS into GeniE, it is unfortunately not possible to export a model from GeniE to be imported into SACS. No such converter from GeniE to SACS exists.

Back to top

GENIE (All Versions from 6.0-03) Graphics window goes blank

The Windows Update KB3205394 for Windows 7 64 bit systems has the side effect that if the GeniE window is maximized the graphics window goes blank when focus is changed to outside GeniE. The display goes back to normal when refreshing the display (move mouse over model, rotate model etc).

The current workaround is to not maximize the GeniE window, but instead size the window manually (to almost fit the screen). We do not recommend uninstalling security updates.

Back to top

GeniE reports displacements of all FEM Nodes, even if a set has been selected

Question: GeniE reports displacements of all FEM Nodes, even if a set has been selected. Why?

Answer:

In GeniE, three types of results could be generated when printing FEM node displacements via save report.

  1. If in the concept model without any frame joints. Then the displacement of all the FEM nodes will be printed no matter which set is selected. 
  2. If the concept model has frame joints, and then 
    • if the selected set does not include any joints, then no fem node displacement will be printed
    • if some joints are included in the selected set, then only the fem nodes corresponding to these joints will be printed. For such case, the different selected set will generate different fem node displacement report.

Back to top

GeniE SACS Converter soil layers

Question

If a SACS PSI file contains more than one soil ID and the soil layers are different for soil curves with different soil ID, such as below, how does GeniE determine the soil layers and soil curves in the converted GeniE model?

PLGRUP  
PLGRUP PL1         152.40   3.5  21.0  8.00  33.5    28.5 
PLGRUP PL1         121.92   4.0  21.0  8.00  34.5    25.0 
PILE
PILE  101P201P PL1                                                  SOL1  
PILE  102P202P PL1                                                  SOL1  
PILE  111P211P PL2                                                  SOL2  
PILE  112P212P PL2                                                  SOL2

Answer

GeniE assigns soil curves with different ID to pile with different diameters. In a converted GeniE model, the soil layers are determined based on the data of soil layers with the first soil ID in the PSI file. The data of soil curves is linearly interpolated for each soil layer. The linearly interpolated soil curves for all pile diameters are placed at the bottom of each soil layer.

Back to top

Graphic performance via Remote Desktop Protocol

Microsoft Windows Remote Desktop Protocol (RDP) does not allow GPU rendering by default. That means the graphic superiority of host computer cannot be exploited during remote session. This can lead to reduced graphical performance when GeniE try to use DirectX or OpenGL GPU display drivers on the host computer.

This issue can be easily corrected by modifying the group policy on the host computer to allow the use of GPU rendering during a Remote Desktop session. Your IT department might be able to help you to do this.

Back to top

HGLA - Error: System.Collections.Generic.KeyNotFoundException: The given key was not present in the dictionary.

The error message which is listed below can be found during applying HGLA in FEAnalysis in Nauticus Hull

Error: System.Collections.Generic.KeyNotFoundException: The given key was not present in the dictionary.
   at System.Collections.Generic.Dictionary`2.get_Item(TKey key)
   at HGLA.FE.ObjectModel.Geometry.ModelDataProvider.GetElementsOnNode(Node node)
   at HGLA.FE.ObjectModel.Geometry.FeModel.IdentifyAllLongitudinalElementsInDirection(Double x, IList`1& listOfHullGirderBendEffectElem, CalculationDirection direction)
   at HGLA.FE.ObjectModel.Geometry.FeModel.IdentifyHullGirderBendingElements(Double x, IList`1& listOfHullGirderBendEffectElem, CalculationDirection direction)
   at HGLA.FE.ObjectModel.Geometry.FeModel.IdentifyOrGet(Double position, CalculationDirection direction, Dictionary`2 hgbeElements)
   at HGLA.FE.ObjectModel.Geometry.FeModel.GetHullGirderBendingElementsOnPosInDir(Double position, CalculationDirection direction)
   at HGLA.CSRH.Rules.BendMomAdj.Execute(List`1 applicationPoints, DegreeOfFreedom degree)
   at HGLA.CSRH.Rules.BendMomentMidApplier.CalculateAndApplyAdjustment(IWriteStream storage)
   at HGLA.CSRH.Rules.MainApplier.ApplyAndLogBendingMomentInMidship(ICollection`1 summaryResults, List`1 detailedResults, VerticalShearForceApplier vsfd, IBasicCalcProvider basicFromLocalLoads, ISfMomentsCalculator momentsCalculator)
   at HGLA.CSRH.Rules.MainApplier.CalculateAndAdjustToRules(List`1& summaryResults, List`1& detailedResults)
   at HGLA.Main.Program.CalculateAndOutputResults(ExporterOfCsv details, ExporterOfCsv summary, Arguments arguments, LoadDataSource loadDataSource, FemDataSource femDataSource, FeModel feModel, ShearFlowCalculator shearFlowModel, IWriteStream storage, Int32 femLlc, Int32 nhLlc)
   at HGLA.Main.Program.Main(String[] args)
  1    Press Key to END. Application will now exit.

This is caused due to incomplete definition of the rigid-link.

For bulk carriers and tanker with corrugated bulkhead sometimes do not have plates in centerline in aft end and fore end of the model. In that case, user need to connect beam between independent point of the rigid-link and model. Otherwise, that kind of error can happen.

So workaround for this error is to check connectivity of the rigid-link for structure.

Back to top

How are design wave load cases ordered?

Version: All

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

How do I merge results and load cases from multiple analyses to perform a single code check?

Version: All

This requires some work with both GeniE and Prepost. It basically involves that you merge your analysis results into a single analysis results file, after which a capacity manager is created for doing a code check of this new analysis. The procedure for this is outlined in the attached FAQ document.

Please see the attached document 00003654 Merged analyses code check.

Back to top

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

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.

Back to top

How to change or delete a prescribed displacement?

Version: All

Problem: A load case contains a prescribed displacement (for a support point with prescribed type of boundary condition). How to change or delete this part of the load case and not the whole load case?

Solution: Go to Load Cases folder (or analysis activity if the load is stored there) and double-click the load case. Then double-click Explicit Loads and right-click the relevant prescribed displacement to open Properties to change or click Delete to delete.

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 define your own correction shear forces and bending moments using the slicer in GeniE?

Version: All from 5.1-11

The procedure to create your own slicer including correction shear forces and end moments is described in the attachment. In brief the procedure consists of exporting  a ruleloads xml from Nauticus Hull as for a regular cargo hold analysis with rule loading, and then modifying the target values for correction shear forces and end moments in GeniE.

Please see the attached document 00003913 How to define your own correction shear forces and bending moments using the slicer in GeniE.

Back to top

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 extract and print detailed curve information

Version: All from 6.5-04

The following commands can be used to extract and print detailed information about guiding geometry curves:

Command:

print(<Curve>.GetCurveInformation());

Expected output:

-> Curve Information:

Definition Interval:  [0,22.4768]
Is Closed:            0
Is Self-Intersecting: 0
Is Planar:            1
Is Line:              0
Is Polyline:          0
Is Rational:          0
Number of segments:   4
Degree:               3
Analytic Continuity:        C2
Geometric Continuity:       G2
Analytic Stable Continuity: C2

Command:

print(<Curve>.GeometryToString());

Expected output:

-> BSplineCurve3D{Name[Curve1],Layer[],ControlPoints[Point(10.0000000000:0.0000000000:0.0000000000)
Point(5.9968401846:0.4905205538:0.0000000000) Point(0.2034128748:1.2004085681:0.0000000000)
Point(4.9830908462:4.9492725386:0.0000000000) Point(9.7726718238:9.0147146125:0.0000000000)
Point(3.9542987567:8.1128962700:0.0000000000) Point(0.0000000000:7.5000000000:0.0000000000)],
KnotVector[    0.0000000000    0.0000000000    0.0000000000    7.9056941504   11.4412280564   14.9767619623
  22.4767619623   22.4767619623   22.4767619623],
Degree[3] };

Command:

point1 = <Curve>.EvaluateAtParameter(...parameter...);

Expected output: This command will create a point specified by user name, at curve parameter specified by user.


Command:

Print(<Curve>.GetParameter(...point on the curve...));

Expected output: Command will return curve parameter for the specified point on the curve.


Command:

point = <Curve>.EvaluateAtLocalParameter(... double in [0,1]...);

Expected output: Point on curve will be given when specifying position as parameter. Parameter value between 0 and 1.


Command:

Print(<Curve>.GetLocalParameter(...point on the curve...));

Expected output: Command will return parameter from 0 to 1, from start of the curve to specified point on the curve.


Command:

point = <Curve>.EvaluateAtLengthFraction(... double in [0,1]...);

Expected output: Point on curve will be given when specifying position as parameter. Parameter value between 0 and 1.


Command:

vector = <Curve>.TangentVector(...point on the curve...);

Expected output: Command will return tangential vector at specified point on curve.


Command:

radius = <Curve>.CurvatureRadius(...point on the curve...);

Expected output: Command will return curvature radius at specified point on curve.


Command:

vector = <Curve>.CurvatureVector(...point on the curve...)

Expected output: Command will return curvature vector length at specified point on curve.


Command:

<Curve> = Curve.VectorCurvatureFunction(...no points...,...scale factor...);

scale factor - real numbers R

number of points - Natural positive numbers

Expected output: For given curve, the curvature function will be displayed.

Back to top

How to import complex result cases into GeniE?

Version: All from 6.1-05

If complex result-cases have to be imported into GeniE, they have to be converted into a static result-case at a specific phase angle.

This can be done by scanning the result-cases in Xtract/Framework to find out the worst phase angle.

Then in Prepost, create a new result-case which will contain the complex result-case at that specific phase angle.

Now import the updated results file into GeniE and code check the complex result-case at the specified phase angle.

Back to top

How to import external result into GeniE to do plate code check

To import an external result file into GeniE for a plate code check, follow these steps:

  • Prepare FE model:
  • Open an existing workspace XXX.gnx that includes the same mesh as result file.
  • Alternatively, import T#.fem file into a new workspace (Make sure not to check the option “Create analysis activity” when importing T#.fem file).

  • Import external result file:
  • Ensure that the analysis activity only includes mesh activity before importing external result file. If the analysis activity includes the structural (Sestra) analysis activity, uncheck the option “linear structural analysis”.

  • Then import external result file into workspace (*File->Import->*External Results SIN file) and check the option “create load cases”. Result cases matches with existing load cases. For result cases without match, load cases will be created with names .loadCase(N).

  • Combined result cases can be defined with relevant load factor for further capacity check

  • Capacity Check:
  • Create a new capacity manager
  • Select the current analysis activity and apply the relevant rule.
  • Perform the plate code check or beam code check using the result cases

Back to top

How to resolve missing nodes for segmented piles?

Version: All from 7.0

Symptoms: The number of nodes/displacements reported by Splice is less than the number of soil layers reported by Splice when a pile with a segment change is used.

Cause: At segment changes, the default mesher in GeniE creates longer pile elements, to make sure that the same number of elements is generated. However, in case of a segment change, an additional node is required at the segment change. As a result, Splice receives less nodes than soil layers from GeniE, and hence reports less displacements than soil layers.

Solution: This issue was addressed in GeniE V7.0, but is only solved when using GeniE’s partial mesher. To solve the issue, use the following steps:

  1. In the folder tree on the left-hand side of the GeniE window, right-click on your analysis and select Choose mesher > Use partial mesher to enable GeniE's partial mesher.
  2. Next, edit the mesh activity settings by right-clicking on the meshing step in the folder tree or in the activity monitor. Make sure to set the mesher to ‘always regenerate mesh’.
  3. Remesh and re-analyse the model. Additional nodes are now created along the pile. In particular, additional nodes are generated at the segment ends. This makes sure that each soil layer receives one node (or two in case of a segment change). As a result Splice will compute the displacements corresponding to these nodes.

Back to top

How to solve "Unknown error in HOOPS display kernel during update" error?

If you receive an error message while using GeniE with the following message:

Display update failed.

Unknown error in HOOPS display kernel during update.

Display service unexpectedly crashed. Save workspace and restart application.

Please report issue to DNV Software

Please follow the steps below to solve this issue:

Terminology
The following documentation refers to “graphics drivers” and “GeniE graphics drivers”.

The graphics driver is the system level software provided by your Graphics Card supplier (most likely Intel, NVIDIA or ATI) to interface between Windows and the GPU. This is supplied with your operating system or graphics card.

The GeniE graphics driver is the software used by GeniE to interface with the graphics driver defined above and is supplied with GeniE.

There are several “GeniE graphics drivers” provided. At the time of writing these are OpenGL, OpenGL2, DX9, DX11 and Auto. The default is Auto. This setting will attempt to choose the best GeniE graphics driver based on the hardware on your particular machine.

Step 1: Upgrade your graphics driver.
Check to see if there is a newer version of the graphics driver or drivers for your machine. Note that some laptops in particular may have more than one GPU from different vendors, typically Intel and NVIDIA or Intel and AMD.

The easiest way to upgrade a graphics driver is to start “Device Manager”, open the “Display Adapters” tab, right click on one of the available GPUs and select “Update Driver Software”. Select “Search Automatically for update driver software”.

If Windows finds a newer driver follow the instructions to install it and restart GeniE.

If you have more than one GPU listed in the “Display Adapters” setting then you can try updating all of them. On a hybrid laptop the default settings are normally that one GPU, typically from Intel, runs when the laptop is on battery and the higher performance GPU, typically from NVIDIA or AMD runs when the laptop is connected to an external power source and/or an external monitor. These settings can be over-ridden but that is machine specific.

In some cases Windows may not find a new driver but you may find a new driver on the website of your computer manufacturer or on the website of your GPU manufacturer. In some cases the latter will not install as the computer vendor has not approved it.

A note on GPU graphics drivers: Graphics techniques used in most modern design systems such as GeniE are very complex as are the third party drivers that transfer the graphics commands from the CPU to the GPU. Bugs are relatively common and upgrading, or downgrading, driver versions is something every design professional is likely to have to do at some point. If there are no problems then don’t upgrade, but if serious problems are encountered then seeing if a newer version is available should always be the first step - unless of course the problems started after a driver version upgrade, in which case reverting to an older more-stable version would be recommended.

If a problem such as this is resolved by changing a driver version (Step 1) , by changing the GeniE Graphics Driver (Steps 2 and 3), or by disabling GPU hardware acceleration for your entire machine (Step 4) then it would be useful if you could report the GPU type and driver version to DNV GL Support. In some cases, if we can reproduce the issue, we may try to follow up with the GPU manufacturer to try to get the bug fixed.

Step 2: Try different GeniE Graphics Drivers
If Step 1 does not solve your issue, you can try changing the GeniE Graphics Driver. This can be done in View->Options->General->Select Graphics Device.

Assuming you are using the default “Auto” then try in turn DX11, DX9, OpenGL2 then OpenGL in turn.

Starting GeniE with command line options It is necessary to load or create a new workspace in order to change this option. It is therefore possible the error dialog may prevent the setting from being changed. If so you can start GeniE with a command line option that specifies the desired graphics device.

Starting GeniE with command line options is described in Section 4 of Volume 1 of the GeniE documentation. On a command line type “GeniEr /?” to display a help dialog listing the available command line options. For example, to select “opengl” start GeniE with “GeniEr /graphicsdevice=opengl”. Note that this command line option only overrides the option currently set in the View Options dialog - it does not change it. Therefore if you find you can successfully start GeniE this way then you may wish to also change the Select Graphics Device option once you have a workspace loaded.

Step 3: Force GeniE to ignore GPU graphics
If none of the GeniE graphics drivers used in step 2 work then you can force GeniE to ignore the GPU and execute all graphics commands on the CPU. This means that GeniE will not access the third-party graphics driver installed on your machine.

This option is “Hardware Acceleration”, also in the View->Options->General tab. The corresponding command line option to turn off GPU based hardware acceleration is “/hardwareacceleration=off”.

For this setting we strongly recommend you choose the OpenGL driver e.g. “GeniEr /graphicsdevice=opengl /hardwareacceleration=off”.

Step 4: Disable GPU acceleration on your entire machine:
Obviously this should only be a last step as it will affect the performance of other GPU hardware-accelerated applications as well as GeniE although it could quickly be used as a first check to see if the problem is GPU-related or elsewhere.

  1. Choose Start > Control Panel.
  2. Double click Personalization and select Display Settings.
  3. Click Advanced Settings.
  4. Click Change Settings on the Troubleshooting tab.
  5. Move the Hardware Acceleration slider to None.
  6. Click Apply and then click OK to accept the new setting and close the dialog box.
  7. Click OK to close the Display Properties dialog box.
  8. Restart Windows.

If, after trying all these steps, this error is still present or GeniE crashes then it is likely there is an issue elsewhere. In this case please send your model and data to DNV GL support as there may be a specific issue caused by the data you are using.

Back to top

How to solve 'HOOPS has reported graphics errors with dx9 startup' message?

Version: 6.4-08

If DirectX 9 isn't properly installed on your PC, you may receive the following message in GeniE:

HOOPS has reported graphics errors with dx9 startup

If the GeniE graphics window is not functioning ...

  • Please make sure DirectX is installed correctly. The DirectX End-User Runtime can be installed using the Sesam Installer or from the Microsoft Website
  • The graphics driver can be changed manually

Open a workspace in GeniE and choose View->Options->General Tab->Select Graphics Device

To toggle different graphics devices click the icon to the left of the "Select Graphics Device" text

To solve this, please download and install DirectX 9 from Microsoft's website:

http://www.microsoft.com/en-us/download/details.aspx?id=8109

After the download has finished, unzip the files to a folder on your hard drive. Double click the DXSetup.exe file to start the installation. 

After you have installed DirectX 9, you can modify the Graphics device to use in GeniE by navigating to View|Options and select the General tab.

There, you will be able to select Graphics Device DirectX 9, OpenGL or OpenGL2 by clicking on the icon in front of "Select Graphics Device".

Back to top

Import ANSYS model to Genie

There is a converter from ANSYS to Sesam (GeniE) which is part of our utility software called Prepost. Please refer to Sesam_Ansys.pdf (located in Prepost installation folder) document for Ansys (*.cdb) conversion. The conversion from Ansys to Sesam is explained in section 3.2. Basically, it only consists of a READ command to read in the Ansys file and a WRITE command to write out the Sesam FEM file. Below is the Prepost input example:

OPEN ..
READ ANSYS, ' ' FileName 0 1
WRITE FEM-FORMATTED, ' ' T1 1

Use Sesam Manager to create a job with a Prepost activity and start Prepost from there.

Please note that only older Ansys database versions are supported. Version 10 should work fine. There have been some updates for version 12 or 13, but not all options may be supported (refer to the attached document).

Back to top

Improving Compatibility When Reading Old JS files into Higher Version

Some model errors were happened when reading old format JS files to build GeniE workspace. These JS file may be generated by the customer self-develop tool. To avoid model error, it needs to set the compatibility option when reading JS file into GeniE. It is recommended to select V3.3-38 or older.

Back to top

Keyboard Shortcut commands for GeniE

In the Attached page are the various usefull keyboard shortcut commands for GeniE.

Please see the attached document Short Cut key.

Back to top

Midnodes incorrectly positioned, not in the middle of the edge or out of line

When using 2nd order elements in GeniE, the midnodes are placed at the parameter position 0.5 of the curve between the end nodes. For some models, the parametrization is non-uniform; this may lead to distorted mesh, missing mesh, or wrongly positioned midnodes. This can happen if the underlying geometry description is distorted.

Enabling "Uniformized face parametrization" from the Edit > Rules > Meshing menu will will better align the midnodes correctly , but it can have negative impact on performance. The alternative is to recreate the plate/shell to get a better parametrization, or manually use mesh edit functionality to move nodes a little (the mid nodes will follow and snap to correct position).

Back to top

Modelling issue: red exclamation mark on beam

Question: what does the red exclamation mark mean?

Answer:

When the beam which has an offset depending on the intersection of two other beams. Then, for some reason, one of these two beams is deleted (e.g. it is joined with another or the user has delete it directly). The offset can not be defined anymore. For such issue, we will give an exclamation mark to remind the user. 

So please check the questioned beam to check if there is abnormal offset. Below is an example.

This issue relates to Bug 16075.

Back to top

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 (available from the Sesam Input Interface Format/download/public/sesam/user-documentation/knowledge-articles-files/ACCEL.pdf){target="_blank" rel="noreferrer nofollow"}

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

Out of memory

Version: All

Sometimes a memory error similar to this is displayed:

CMofaMainApp: Exception caught os_err_out_of_virtual_memory - os_get_adress_space:VirtualAlloc(0x38000000, 201560064) failed

Since GeniE employs a database called Objectstore, there is a limit on the maximum total size of the database. By default this limit is 128MB, but by defining an environment variable OS_PSE_AS_SIZE, the maximum size can be increased up to approximately 1GB (OS_PSE_AS_SIZE = 0x20000000). If you are using 64 bit computer then you may use 0x40000000 (applies to versions V5.1-11 and V5.2-04 and onwards).

If this environment variable is defined too large, the application will not start. Also notice that the change above will make databases created prior to this change unreadable. To import such databases you must first set the variable back to the value it had when the database was created. Please see the attached screenshot (Env_var_1.JPG) on how to set this variable.

Using 64 bit version of GeniE might solve such problems too.

Please see the attached document How to set environment variables.

Back to top

Partially split plates warning

What does the Partially split plates warning mean?

Partially split plates warning intended to warn user that some elements are having improper geometry or mesh so user can check it. Partially split plates are not always a source of problem but GeniE warns about this because it is not uncommon that users wanted to have a beam go all the way through the plate but due to some modelling mistake the beam stops a few mm from the plate edge, thus the warning will help identify that issue. Also, having a partially split plate can create some improper mesh elements if the plate is not properly split at the end of the beam/feature edge.

Increase the quality of mesh or modelling will solve this warning. If the analysis can run and plate is not your interest, partially split plate warning can be ignored to the certain extent (with user’s consent).

Back to top

Plate Code Check for corrugated bulkhead

Version: All from 8.0

This knowledge article is to provide tutorial of plate code check (yield and buckling) for corrugated bulkhead. Please find attached tutorial document, and example model. GeniE journal file is also attached.

Please be noted that GeniE 8.4 version with dual assembly option has been used. If using old version, like GeniE 7.x version, there could be problem.

Back to top

Problems with graphic display such as wrong colors or slow response

Version: All

If you are experiencing problems with the graphic display in GeniE you may try turning hardware acceleration on/off.

The switch for hardware acceleration is found in the GeniE menu:

View > Options... > General tab > Hardware acceleration.

Press the X icon to switch on/off

See also the FAQ: Performance problem on ATI MOBILITY RADEON X600 for adjusting the amount of hardware acceleration

Back to top

Programe association on .gni files.

To the unset the GeniE programe version on the .gni file the following has to be done.

"Start---Run," type in "regedit"  and try deleting .gni file associations from the "Registry Editor."

Make sure you delete all the file associations.

Back to top

Results in truss elements

Truss members are a somewhat special beam member in Sesam. Truss members can be analysed as part of a normal linear structural analysis or as part of a tension-compression analysis (e.g. if the truss members have been set to tension- or compression-only). While they are beam members, the results are shown slightly different compared to normal (non-truss) beam members.

In GeniE's result presentation normal beams will only show forces. However, truss members will not show the forces in GeniE and Xtract, but stresses. As such, if you want to view the results of the truss members, you will need to inspect the stress along the member. You are able to inspect the truss member results via the Results view in GeniE or via Xtract. The truss axial stresses are available via G-STRESS > sigxx. The force can then be easily computed using the cross-sectional area of the member.

No code check is available for truss members.

Back to top

Version: All

Support rigid links should not be created by copy rotation operation, because then the dependent and independent nodes will get different coordinate system orientations. You can verify the local coordinate sytems by labelling them for the support rigid link (and any relevant support curves).

Unless the use is intended, this will give wrong results in analysis.

The differences between summed loads and reaction forces for the translational DOFs reported at the end of the Sestra.lis file should be small numbers typicall in the range 1.e-5 or less. If the independent and dependent point's coordinate systems are misaligned, the values are typically 1.e-1 or larger.

Back to top

Version: To 6.3-06

If spring stiffness is defined for any DOF in a rigid support link, it will not work properly. The spring will not take any reaction force.

Back to top

Sesam Compartments with Dipole elements

How to create a compartment model including dipole elements in GeniE, and use them in HydroD?

Please see the document which is found in the attached zip file , together with model files.

Notice that there is also a tutorial in HydroD 6.2 and later versions on how to use dipole elements in the panel model and compartments for Wadam analyses, available from the Help menu.

Back to top

Stresses in General Beam cross-section

Version: All

Its not possible to display Beam stresses through Beam Results diagram and Report in GeniE. User can see stresses in General Cross-section using Xtract.

Back to top

Staad Pro import to GeniE

To convert Staad model to GeniE, you need to use Staad2Sesam application:

This application will convert Staad file to .js file and user can import the .js file into GeniE.

Below is the link to Staad2Sesam software: https://sesam.dnv.com/download/windows/staad2sesam_1201_inst_win.zip

Back to top

What plate code checks are available and what are the differences between them? (GENIE/PLATEWORK/NAUTICUS HULL/PULS)

Plate buckling analysis and code checks are available in both GeniE, Nauticus Hull, PULS and Platework as described herein.

Sesam GeniE is used for FE analysis of offshore structures (Sesam) and ships (Nauticus Hull).

Plate code checks according to the following ship rule sets are integrated in GeniE:

  • DNV GL 1A ship and Offshore rules
  • CSR BC&OT
  • CSR Bulk
  • CSR Tank

DNV GL 1A ship rules and CSR BC&OT (harmonized) came into force 2015/2016, replacing DNV 1A1, CSR Bulk and CSR Tank rules. DNV GL Offshore rules came into force January 2019.

Tutorials for cargo hold analysis and code checks according to CSR BC&OT and DNV GL Offshore are available in the customer portal, search for cargo hold analysis. For tutorial according to DNV GL 1A ship rules rules, please contact software support.

PULS (Panel Ultimate Limit State) is a plate buckling analysis code used in CSR Tank and DNV-RP-C201 Part 2 (offshore). PULS integrated in GeniE can be used for offshore structures to check longitudinal structure according to DNV-RP-C201 Part 2 and some transverse structure according to DNV 1A1 ship class. This should be discussed with offshore class prior to usage. In this case some defaults in the CSR Tank plate code check in GeniE must be modified. More information is found in the Sesam training course SE-23 FPSO global strength and spectral fatigue analysis.

Furthermore, PULS is available in Nauticus Hull (ship structures) in three other ways:

  • PULS Excel standalone spreadsheet, effective for parameter studies
  • PULS AV (Advanced viewer) standalone program offering functionality for better understanding and optimization wrt buckling capacity of the plated structure
  • PULS in classic Nauticus Hull up to Jan 2018 (v18.15) Section Scantlings for hull girder capacity in the ULS check according to Offshore Standard DNVGL-OS-C102 (Ch.2 Sec.4.3).

See also separate FAQ "The four variants of PULS" about how these variants are licensed and installed.

Platework is focused towards the offshore industry and supports rules and regulations from the following authorities: API, DNV and NPD, covering the following types of checks: Plate yield and buckling checks, stiffener yield and buckling checks, girder yield and buckling checks. The methodology in Platework is based on DNV-RP-C201 Part 1. The last update to the code (major revision) was made in 2004 and the user interface has not been updated since the mid-90’s.

Platework references DNV: DNV Recommended Practice C201, 2004. API: Bulletin on Design of Flat Plate Structures, API Bulletin 2V (BUL 2V), First Edition, May 1, 1987. Recommended Practice for Planning, Designing and Constructing Tension Leg Platforms, API Recommended Practice 2T (RP 2T), First Edition, April 1, 1987. NPD: Regulations for structural design of load-bearing structures intended for exploration of petroleum resources, Norwegian Petroleum Directorate, 1984. Guidelines for design of steel structures, Norwegian Petroleum Directorate, 1989.

Back to top

Which shortcuts exist in GeniE?

Version: 6.6-08

In GeniE it is possible to use keyboard shortcuts. The following is an overview of the shortcuts available in GeniE.

Updates are shown in green.

File
Ctrl+N - New workspace Ctrl+O - Open workspace Ctrl+S - Save workspace
Edit
Ctrl+Z - Undo Ctrl+Y - Redo Ctrl+U - Set Undo mark Ctrl+T - Copy (with transform) Del - Delete
View
Alt+O – Options Alt + B – Changes background color from default to white
Tools
Alt+M – Turn activity monitor on with only meshing activity set to active Alt+D – Turn activity monitor on with current analysis set to active Alt+P - Presentation (of results in Results views) Alt+G - Beam result diagrams Alt+C - Customize
Help
F1 - Help
Model viewing
F2 - Rotate (with right mouse button) F3 - Zoom (with right mouse button) F4 - Pan (with right mouse button) Ctrl+Shift + RMB - Zoom rubber band (with right mouse button) Shift + RMB – Zoom to the cursor Ctrl+ RMB – Pan  model Alt + RMB – Rotate model Alt+Z - Fit to selection (new in GeniE V6.6-08) X + RMB – Rotate model around axis that is currently in vertical position C + RMB – Rotate camera Z + RMB – Rotate camera S + RMB – Set camera to see model in horizontal position F5 - ISO view F6 - View from X axis F7 - View from Y axis F8 - View from Z axis F9 - Fit (zoom in/out to fit model in screen) F10 - Spin model Alt+S - Show selection only Alt+Plus - Add selection (display together with other currently shown concepts) Alt+Minus - Remove selection (hide concepts) Alt+A - Show all Alt+Q - Show complement (of currently shown concepts)
Modelling
F11 - Snap perpendicular/tangential/plane/eccentric (select option via Toolbar button) ESC - cancel operations/go to selection mode

Back to top

Why and how to scale down basic load cases in a pile-soil analysis?

Version: All

Description: In GeniE you may need to scale down the basic load cases when performing a pile-soil analysis.

Explanation: In a non-linear pile-soil analysis only results for the load combinations are normally of interest. In real life, there will always be multiple loads simultaneously acting on a piled structure, e.g. a jacket. For example, a wave load will never occur alone, but will always be accompanied by a gravity load and most likely even more loads. These different loads exist in the different load cases in GeniE, while the combined simultaneous loading is applied using load combinations. With this in mind, imagine only a wave load acting on the structure, so without any other loads acting on the jacket. This will most likely give a large stress in the piles, and the loading may even be such that a tensile stress results in some piles. These loads will give trouble in the convergence of the pile-soil analysis and in certain cases the basic load cases may cause the whole analysis to stop. Even more, these kinds of loads do not exist as such in reality, as also e.g. gravity will act on the structure together with the wave. The load combinations will usually give no convergence issues in the pile-soil analysis, while the separate load cases may do so. Hence, to circumvent this problem, the basic load cases can be scaled down, e.g. by a factor 100, to make sure the pile-soil analysis converges and the analysis does not stop with a convergence error.

How to control it? You are able to change the behaviour of scaling the load cases in GeniE by setting the scaling factor. This is done using the command: GenieRules.Meshing.basicLCfactor = 0.01; 0.01 will scale down the basic load cases by a factor 100. A value of 1 will give no scaling of the basic load cases. Note that this may cause the issues mentioned above.

If you want to check which value is active at the moment, you can use:

*print(GenieRules.Meshing.basicLCfactor);*

Back to top

Why can my XML report not be opened in Excel?

Version: All

Symptoms:

When creating a report in GeniE and saving this as an ExcelXML, an error will show up in Excel when opening the report:

Problems came up in the following areas during load:Workbook Setting

Cause:

This is caused by a limitation in Excel combined with the report section names used by GeniE. The section names from the report in GeniE, preceded by the load case name, are being used to give the worksheets in Excel a name. However, the worksheet names in Excel have a maximum length. When this maximum length is surpassed, the name is cut off. As a result, some sheets may get the same name, because some GeniE result sections start with the same words:

Load Summary Conceptual
Load Summary Applied
Load Summary FEM Loads
Load Summary FEM Reactions
Load Summary FEM Differences
Load Details - Conceptual
Load Details - Applied

The effect of this is that Excel gives an error upon opening the XML.

Solution:

A workaround is to only include one of the sections at a time that are starting with the same words. One can then e.g. manually change the sheet name and copy the sheets into the same Excel document.

Shortening the load case names, which are used to preceed the worksheet name in Excel, may also help, but will in most cases not completely solve the problem, as some of the section names used in GeniE are simply too long to be displayed as a worksheet name in Excel.

Back to top