Structural Solvers and Results

Combining results from different loading conditions in Stofat

As of today, there is no possibility to combine results from different runs inside Stofat (for instance 80% operation 20% transit). This issue has been adressed previously and is listed as a development task.

There are two general workarounds for the issue, and neither of them is particularly simple. The first way is to combine the loadfiles (L#.FEM) in a small utility program called Waloco before running Sestra. However, the wave data in the S#.FEM files also has to been considered, which may not be so straightforward. This may also be problematic since Stofat has some model size limitations, and you may very well end up splitting up the runs either way since the model becomes too big. The second way would be to write scripts (Excel VBA/Phyton or similar) to manually combine text output vtf files with fatigue results from the different runs. This is perhaps not so straightforward and most likely very time consuming and prone to errors.

Back to top

Eigenvalue Analysis

When you have a superelement model and you move from static to dynamic (eigenvalue or forced response) analysis then the Master-Slave reduction technique is in effect used instead of the superelement technique which strictly speaking is for static analysis only.

When taking a superelement model created for static analysis into a dynamic analysis you have two options:

  • Master-Slave reduction technique
  • Component Mode Synthesis technique

The Master-Slave reduction technique involves that: All 1st level superelements should be assembled into a 2nd level superelement rather than having more superelement levels (if such is the case in the static analysis). Additional supernodes must be defined for the 1st level superelements. These additional supernodes should be spread out over the superelement, denser where high dynamic energy is expected (i.e. big mass or big motion). For these additional supernodes only the 3 translational d.o.f.s need be defined as super as the rotations dont contribute much to the dynamic energy. Select stiff points (major and some minor joints?) as additional supernodes and not points along beams. A disadvantage with the Master-Slave reduction technique is that you have to change the 1st level superelements.

The Component Mode Synthesis technique involves that eigenvalue analyses are performed for each 1st level superelement and a selected number of mode shapes for each superelement contribute as generalized d.o.f.s to the dynamic analysis. A disadvantage with this technique is that the mode shapes in general represent axial motion in inadequately (the mode shapes are predominantly transverse motion). This means that axial forces are poorly described which is bad for fatigue analysis and also earthquake 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

Framework: Error message in wind fatigue analysis

Question: What may make Framework issue the following message in a wind fatigue analysis? Warning from GRES73 called by GWRSTL: Reference outside pointer table Record identifier: BELOAD1

What Framework does: For a model containing a flare boom and a part of the deck, if non-zero air drag coefficients Cdy and Cdz are applied on flare boom beams and zero Cdy and Cdz are applied to deck beams, Wajac will only apply wind loads on beams with non-zero Cdy and Cdz. When the result file R1.SIN is imported into Framework, Framework will stop to read in loads when a beam without any wind loads is found, and the above message will be issued. However, the analysis will continue in the absence of other wind load cases and results will be reported. The calculated results are incorrect.

Solution: All FE elements included in a wind fatigue analysis must have non-zero wind loads applied on them. If wind loads on some elements are not desired, very small air drag coefficients, such as Cdy = 0.001 and Cdz = 0.001, can be applied to deck beams and flare boom support beams to make Framework read in wind loads correctly and generate the correct analysis results.

Back to top

How to export pictures from Framework, Profast, Stofat, Postresp

Update November 2017: As Office has been more restrictive to Postscript due to a security vulnerability in EPS please try this workaround:

  • select "Microsoft print to PDF" or a similar PDF printer driver as default printer on your computer
  • inside Postresp set the Plot to Format Windows-printers
  • When you Plot the image, this will be saved in a pdf file

Please note that the file will not be properly saved until you close Postresp. It was possible to import CGM files directly into MS Office in the past. However, a Windows update rendered MS Office uncapable of recognizing this file format.

In order to export pictures from the software it is recommended to export as Postscript format and change the file extension from .ps to .eps.

Then it is possible to import into MS Office.

Back to top

How to generate a PDF file for a plot from Framework, Profast, Stofat, Postresp

How to generate a PDF file for a plot from Framework, Profast, Stofat, Postresp? User can follow the below steps to create a PDF file for a Framework plot.

After a desired plot displayed on the screen, on Set tab select Plot and then choose Postscript Click Apply or OK to save the selection. Click Plot, the file with the defined name, such as FrameworkActivity1.PS, is created in the analysis folder. Now exit Framework. In the analysis folder, double click the generated postscript file FrameworkActivity1.PS to open Acrobat, click YES to generate the PDF file.

See also the for details.

Back to top

How to set up load case numbering for Submod

Any local loads in the local model (submodel) has to use exactly the same load case numbers as in the global model, i.e. a 1:1 mapping.

Submod will fetch the displacements from the global model, and put these on to the local model for each load case in the global model. If these do not match the local loads, the displacements from the global model will not either match the local loads, thus giving wrong results.

This means that dummy, empty, load cases may need to be created to make sure that the wanted load cases match. Alternatively, in GeniE, the "FEM load case" number may be changed.

And, it is not possible to add more load cases into the local model, as these will end up with zero displacements (=fixed) on the boundary of the submodel.

Back to top

The 'modal earthquake excitation forces' (or 'modal participation factors' or 'modal load factors') are computed using formula B.353 in the Sestra manual where the a_j are vectors of dimension six. The sum of squares of the elements of the a_j can be compared to the relevant numbers in the sum of masses reported in the Sestra print file.

When Master-Slave reduction is used the sum of masses of the top level (the complete model) as reported in the Sestra print file is the sum of masses of the first level superelements. However, the a_j factors are computed using the reduced top level mass matrix, i.e. the M_ii matrix in formula B.353. M_ii is the same as M_red of equation B.268. Thus the ratio of the sum of squares of a_j to the sum of the masses will not necessarily approach 1 from below when increasing number of eigenvalues, i.e. it may be larger than one.

Rather than making any change to the current computation of modal load factors and sum of masses we will, hopefully within this year, implement computation of modal load factors for the 'implicitly restarted Lanczos method' (EIGA command). Using this very efficient eigenvalue solver we believe the use of the Master-Slave technique will no longer be necessary. Or if you still have superelements you can define many more or all degrees of freedom as super in which case the deviation from 1 of the said ratio will be reduced significantly.

Back to top

Pile self-weight in Splice

Below is the information that how Pile Self-Weight is handled in Splice.

  1. The self weights of the pile wall and the soil plug or fluid inside the pile are calculated by Pilgen from the given geometry and unit weights.
  2. The axial forces acting upon the pile are:
  • Axial force at pile top
  • Given axial forces at any nodes
  • Self weight of pile steel and soil plug
  1. The sum of these forces must be balanced by:
  • Side friction (t-z)
  • Tip resistance (q-z)
  1. Splice assumes that the pile is plugged. For a coring pile, the user must therefore manually calculate the equivalent closed pile tip resistance.
  2. If self weights of pile steel and soil plug are to be included in the Splice model, some care is needed when specifying the ultimate tip resistance, q.ult. The user must decide if total or submerged pile unit weights are to be used. For a pile tip in clay, the ultimate unit tip resistance is normally taken as 9xSu. However, if pile self weights are included, the q.ult value should also include the weight of the overburden, i.e. q.ult = 9xSu+Gamma x Z. Gamma is either total or submerged unit weight, depend on which the user selected for the pile weights.
  3. For a pile tipped in sand, the API/ISO main text method finds q.ult as:
 q.ult = Nq x Sigz' < q.limit

Since Nq becomes 1.0 for a sand friction angle of zero, the Gamma x Z contribution to the tip stress is already included.

  1. Based upon the above, the expression for capacity in compression should be:

Comp. Cap = Soil res. - pile wall weight - soil plug weight

Normal practice is believed to be to drop the soil plug weight, assuming that this is balanced by the outside overburden. If the above reasoning is accepted, that practice is slightly non-conservative for a pile tipped in sand.

Because of this uncertainty/inconsistence, Splice rev.4 and rev.5 manuals state that "For simplicity, self weight of pile steel and soil plug have been neglected".

  1. Weight of pile steel and soil plug always act together, so Splice has no possibility of printing the two individual contributions.
  2. The gravity loading GZ has a fixed value, independent of compressive or tensile loading of the pile.

Back to top

Postresp, Stofat, Framework: Read jnl file

A JNL command file cannot be read from within Postresp (or Stofat, Framework) when it is located in a folder using blanks (spaces) in the name or path. Workaround: copy the file to another folder, e.g.

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

Rule Check (All from 16.0): Fatigue calculations (CN 30.7): Wrong Relative deflections from FEA

When performing Fatigue life checks in Cross Section Analyses, relative displacements that have been calculated in a FEA analysis in GeniE can be directly imported.

Currently this import does not work correctly, and the displacements are wrongly interpreted. This option should therefore not be used.

However it is possible to specify relative deflections manually. This method is described in the attached document.

Please see the attached document.

Back to top

Sestra (All version from 10.0): Not Enough total memory or Unable to allocate sufficient memory message

Below are example of Sestra error message found in Sestra.mlg file, regarding insufficient memory issue. Example 1 : Not enough total (physical + swap) memory for in-core factorization (required memory is 4221 Mb; available total memory is 841 Mb). If running a static analysis with multiple load cases, reduce the number of load cases to store in memory at the same time. Otherwise, exit other processes and/or increase the size of swap memory and then restart Sestra.

Example 2 : Sestra was unable to allocate sufficient memory. This error typically occurs when handling many load cases at the same time, especially for models with many elements. Consider whether your analysis can be run with low memory options (SOLV command) or split into multiple analyses; or consider increasing the virtual memory on your system. Peak memory usage (physical / total): 27410 Mb / 84270Mb. For remedies for this issue,

Workaround 1-1 : Add SOLV card in Sestra.inp with TMEM=1 (available from 10.7 version) This enables low memory model. Sestra uses a smaller memory footprint at a modest reduction in performance. For example, Sestra caches only n (instead of all) load vectors at the same time

Workaround 1-2: Add SOLV card in Sestra.inp with both TMEM=1, and NUMLC (NUMLC is available from 10.2 version) When using TMEM, devalue NUMLC=1 or static, and NUMLC=100 for dynamic time-domain analysis. Try smaller value, less than 100 for dynamic analysis.

Workaround 1-3: Add SOLV card in Sestra.inp with FORCE=1 & OOC=1 (available from 10.2) Default values are FORCE=0 & OOC=0, which is using in-core (in physical memory factorization). This enables Out-of-core (utilizing the HDD) for matrix factorization, which requires less memory, but slow performance.

Workaround 2. Increasing paging files in windows setting. For detail information for SOLV command, please refer Sestra UM and below is one from Sestra 10.16 version.

Sestra 10.16 (released 05 Apr 2022) has been improved for performance of import of load interface files in low-memory model, and for memory footprint for static and dynamic analyses with long load histories, so its recommended to always use latest version of Sestra, especially for such cases. Also, make sure that the computer has plenty free hard drive space left for temp files and paging files; normally, the free hard drive space shall be well over 300Gb.

Back to top

Sestra (All Versions): Analysis with supernodes on the highest level is not possible

Running an analysis for a model including piles results in the following error indicated in Sestra.lis:

*** INPUT ERROR ***
Analysis with supernodes on the highest level is not possible unless saving is specified.

The procedure to solve this issue is outlined in the attached FAQ document. Please see the attached document

Back to top

Sestra (All Versions): How to obtain modal participation factors in Sestra

Runing Sestra from batch file or Sesam Manager: This is achieved by setting the MOLO parameter on the CMAS command to Sestra equal to 1. Note that the Implicitly Restarted Lanczos method cannot be used for this and the Lanczos method should be used instead.

To see the results, you need to open the results SIN file in Framework. Then, simply click Print > Modal Mass. You can then select the mode shapes for which you want the participation factors (e.g. include all). Next you click Apply, which will show you the resulting modal load factors in x, y and z per mode shape.

Using GeniE 7.2-07 or later:

You can get the modal participation factors directly from the report (FEM Results > FEM Modal Mass Factors) after running an eigenvalue analysis (except Implicitly Restarted Lanczos method).

Using GeniE 7.1-12 or older:

You can follow the attached FAQ document for the procedure. Please see the attached document.

Back to top

Sestra (All Versions): Base Shear from earthquake analysis

There is no direct way of printing the base shear from earthquake analysis at the moment. However, there is a bit of lengthy procedure for it.

To start from scratch, follow these steps:

  • Run a static Sestra analysis with gravity loading.
  • Run an eigenvalue analysis in Sestra with MOLO on CMAS set to 1 and results file format set to formatted.
  • Merge two results file in Prepost on the merged results file the gravity load is results case 1 under run 1, the mode shapes are stored under run 2.
  • Run Framework earthquake analysis, in the SELECT command where type of modal combination is chosen select displacements as output. In the RUN command give a name for the run, say QUAKE.
  • The earthquake run in Framework establishes a result case taking the name of the run, i.e. QUAKE.
  • Use PRINT DISPLACEMENTS to print displacements for all joints for result case QUAKE. You then get a table over displacements for the earthquake.

Now you have to assign these displacements as prescribed displacements to your model in GeniE. You may have the print of nodal coordinates of your model so you have to either use excel or some other editor to generate all these commands for inserting the supports for creating prescribe displacements.

Typically, you need to create a loadcase, insert support point at the required joints(nodes), changing the boundary conditions to Prescribed in it and then you insert prescribed displacement as a load.

Create a new analysis now and run a static analysis in Sestra of this model. Assuming that the model has spring-to-ground elements connecting it to the sea floor the Sestra analysis will give a sum of reaction forces being the base shear and overturning moment you seek. Note that you cannot use the Multifront solver for this case. The reason for this is that this solver cannot handle a model with absolutely no free degrees of freedom.

The analysis will in fact only consist of a retracking (finding internal forces) since all displacments are known. Switch to the Supermatrix solver by removing the SOLM command.

Back to top

If you are having larger differences in between summed loads and reaction forces, run analysis using 2nd order elements.

Back to top

If you are using Rigid support link in the model for dynamic analysis then it may end up with an error. It may work in Superlement technique in a way that beam end node (master node) has to be represented as super node.

Back to top

Sestra (All Versions): Hinges with 2nd order elements

End moments will not be zero if you use hinge properties for 2nd order elements.

Back to top

Sestra (All Versions): How to combine load cases with Rotation Fields

Load cases with different Rotation Fields can only be combined in GeniE if the Smart Load Combination option is On.

However, for some analyses the Smart Load Combination option must be off. In this case Sestra will not accept the load combination created by GeniE, because it has several BNACCLO cards for each node.

This can be overcome by creating the load combination in the Sestra input file itself using the cards SLCO, LCOM and optionally SCAL (if load factors are to be defined).

Back to top

Sestra (All Versions): Printing springs reaction forces

If you want to print reaction forces in spring supports then you may need to use CPRI card in Sestra input file. Please check for the proper entries in the Sestra user manual.

Back to top

Sestra (All Versions): Retracking one single sueprelement in heirarchy

If you want to retrack results for one superelement in the heirarchy then RETR card may look as follows, RETR 2. 2. 0. 0. 2. 1.

For further explanation, please see the user manual.

Back to top

Sestra (All) - DOFs fixed in Presel will not print out reaction forces

If a DOF is defined originally as super and changed into fixed inside Presel, the corresponding reaction force will not be printed out by Sestra in the .lis file or in the results files. Therefore, results presentation in GeniE or Xtract will not print reaction forces for this DOF. This force can be computed from the shear forces in the beam. Alternatively, defining this DOF as fixed originally will provide the reaction forces.

Back to top

Sestra (Since version 8.5-01): How to avoid basic errors in tension/compression analysis

  1. Make sure all tension/compression concept elements are not divided into many FEM elements. 1 concept tension/compression beam should only consist of 1 FEM beam element.
    Expected error: TensionCompressionDriver.log will display:
    No truss elements have been assigned the Tension only or the Compression only beam type property - no analysis has been run.
  2. Don't use 2nd order elements for analysis.
    Expected error: TensionCompressionDriver.log will display:
    No truss elements have been assigned the Tension only or the Compression only beam type property - no analysis has been run.
  3. All load cases have to contain loading.
    Expected error: TensionCompressionDriver.log will display: Direct Accesss file TC_520131104_100759_R2.SIN was not found at DNVS.Sesam.SifFramework.IO.SifStreamFactory.OpenDirectAccess(String path, Boolean readOnly) at DNVS.Sesam.TensionCompression.Driver.Program.RunThroughResultFilesAndMerge(String masterSinFile, Dictionary`2 slaveFiles) at DNVS.Sesam.TensionCompression.Driver.Program.MergeTheResultFiles() at DNVS.Sesam.TensionCompression.Driver.Program.Main(String args) SIN file was not created for the specific load case, that does not contain any loading.
  4. Included load cases needs to have the highest FEM load case numbers. Analysis will be Terminated. No file will be created.

Back to top

Sestra 10 unexpected error message DNVS MoFa

During analysis of Sestra 10 program, sometimes it will report kind of error message starting with DNVS::MoFa . When this happens, it means an unexpected error occurs during analysis and together with model files, this error message should be reported to DNV support for further assistance.

Back to top

Sestra error during retracking

The reason seems to be your definition of pin-joints. In your file Sestra-1.mnt the following message was written:

Record is already established. IDGR:BELFIX

This means that you have duplicated some definitions of flexible- or pin-joints in beams. The reason for this problem is probably that you have included the 'load' defining the 'Pin Joints' in more than one load case that you are writing to the T-file (in 'Analysis').

In Patran-Pre the 'Pin-Joints' are load case dependent, since Patran generally also shall be able to model nonlinear models. And in nonlinear analyses there may be different definition of 'Pin-Joints' in each load case. In the linear FEM analyses like Sestra, however, the stiffness matrix is equal for all load cases. Since the 'Pin-Joints' are modifying the stiffness matrix, it must be the same for all load cases.

Generally one may say that the boundary conditions and similar input (supernodes, MPC etc.) shall only be included in one of the load cases that are written to the T-file. Patran-Pre is usually able to not make any doublets for the boundary conditions, but it is not as clever for the 'Pin-Joints'. The solution should be to remove the Pin-joint 'load' from all but one load case.

Back to top

Sestra: invalid map<K, T> key error message

This is an unexpected error in Sestra, so there is little or no detailed description to document. One possible reason that can cause this mapping error is normally due to the lack of system memory. Please try the below steps and see if it can make the analysis to run:

  1. Turn off use of Sestra 10. This will make the program uses Sestra 8.8 for the analysis. The analysis time will be longer, but no memory issue and the error message (if any) will be clearer. In some cases, the error message will point out where the structure is not connected that could cause the mapping to fail.
  2. Try to run the analysis with a computer with larger RAM memory and available hard drive space.
  3. Increase the Windows paging file size (to the order of 64Gb), make sure plenty of hard drive space will be available during the analysis.
  4. Also try to add a SOLV command in the Sestra input file when running Sestra 10. This command will allow the program to process less load cases per time into memory and set NUMLC = 10% of all load cases. This will reduce the usage of memory during the analysis. If none of the above works, please:
  5. Send us the analysis model files and we will try to replicate the issue.
  6. Let us know the computer configuration (especially the RAM memory amount and Paging file size settings).

Back to top

Sestra: Increase eigen solver convergence by specifying maximum number of iterations

Increase eigen solver convergence by specifying maximum number of iterations. Sometimes, for dynamically not sound models, Sestra program may report an error message says the converged eigenvalue number is less than user required, as following,

ERROR Execution failed!

Eigensolver did not converge to within the desired tolerance. Maximum number of iterations reached. Only 37 eigenvalues converged to within specified tolerance 1e-07 (50 eigenvalues are requested). When this error occurs, increase the maximum number from the default 10 to 50 of Lanczos iterations will often get the problem solved, as following,

PS. Notice that COMM needs to be removed for Sestra to read the EIGA command. All commands are described in the Sestra user manual.

Back to top

Sestra: Unable to find Sestra (32bit or 64 bit) in GeniE

Some users may experience this Warning!:

Unable to find Sestra (32bit or 64 bit) on location as defined in DNVS_ApplicationVersions.xml or on location Sesam_HOME in Sesam.INI

Could not read default version installation information for application Sestra from DNVS_ApplicationVersions.xml.

This problem should be resolved by installing Application Version Manager.

If you continue to get an error after this, first please ensure you have installed the latest version of Sestra.

Then, open GeniE, select File -> Set External applications and click Browse. Find the folder where Sestra is installed on your PC (typically it is located in C:\Program Files (x86)\DNVS\Sestra V8.4-04\bin) and select Sestra.exe.

Back to top

Sestra: Tri Criterion

GeniE reports on elements that does not satisfy these criteria. It prints a warning message indicating element number and associated face, as well as the failing value. Sestra will not accept those elements and the analysis will not finish successfully.

For Triangles: 100*A - L 2 < 0 Where A is area, L is length of Longest edge

For Rectangles: 25*C - D < 0 Where C is the shortest diagnonal, D is the longest diagonal

Back to top

Splice (All Versions): Pile head local forces mis-match

The following warning is shown in Splice.lis:

PILE HEAD LOCAL FORCES MIS-MATCH

There are multiple causes that may result in this error and hence multiple solutions:

  1. If not done already, setting the pile to be infinite below a certain z-coordinate may solve this issue. This can be done via Edit > Properties > Pile Characteristics > Edit. The pile boundary condition can then be changed. The pile will still be analysed correctly in the axial direction. Only the torsional and lateral solutions are determined by assuming the pile to have an infinite length.
  2. Alternatively, you may have defined very thin soil (sub)layers (e.g. 0.1 m thick (sub)layers when the pile to be analysed has a diameter of 2 m) or very thick soil (sub)layers. Removing these thin (sub)layers or adding more (sub)layers may be an additional step necessary to remove the warning in Splice.

For more information, see the GeniE User Manual Volume II, section 3.5.2 (Structure-Pile-Soil Modelling) and 3.5.3 (Structure-Pile-Soil Analysis).

Back to top

Splice error message on displacement

Question: What does 10 pile cmn. Diameters mean? What is cmn specifically?

Answer: This is typical non-convergence error for Splice program. The program calculates the displacements from pile tip to pile head, and if the differences in each node does not satisfy the convergence requirement, the program will adjust the pile tip displacement and iterates again. The displacement printed in the error is just the value at final step and does not hold any real/physical meaning. To overcome this convergence issue, try:

Increase soil sublayers. This will add more soil layers. Define Properties > Pile Characteristic, to change "pile boundary condition" from "pile tip is free" to "the pile is assumed to be infinitely long beneath z= and assign it to the piles.

The cmn does not have any meaning in the printed output. This was a misprint in Splice listing files (identified as BUG 354472) and will be corrected in future version.

Back to top

Stofat: How is Stofat calculating stresses for fatigue calculation

Stofat is based on the documentation in DNV Class Note 30.7 and DNV RP-C203. We recommend looking up these documents, in addition to the Stofat user manual.

In Stofat, the stresses are extrapolated from the user defined interpolation points to the hotspot, as given in the RP-C203 section 4.3.1, fig. 4-3.

Stofat will first interpolate the component stresses from the element stress points to the two user defined interpolation points. Next, the component stresses are extrapolated from the interpolation points to the hotspot, where the principal stresses are calculated.

The principal stresses are used together with the wave spectra to calculate the respons spectra. Spectral moments are computed from the respons spectra. The stress ranges used in the fatigue calculation are computed based on the spectral moments.

Stofat is not using equation 4.3.1 (in RP-C203) directly, but will use the principal stresses together with the 'Weld normal line' method, as shown in fig. 2-3 and 2-4 in the RP, to sort out the principal stresses parallel to a weld. When the main principal stress is within the sector defined by the weld normal line, it will be used. If the main principal stress is outside this sector, the damage is set to 0.

Back to top

Stofat: Is there a thickness correction in solid elements

No. The thickness correction is only done for 2D shell elements, not for 3D solid elements.

To do this for solid elements is too complex. The need of a thickness correction is not that important when using solid elements anyway. These elements may be used as a number of elements through the plate thickness, capable of describing the stress variation a lot better than the shell elements.

The thickness correction is used to adjust for a different stress variation through the plate thickness for thin plates as opposed to thick plates. This may influence the calculated damage. If solid elements are used with just one element through the plate thickness, a correction may still be needed. This can be included as a stress concentration factor (SCF).

Back to top

Stofat: Long term fatigue calculations and Weibull distribution

CURRENTLY FOR INTERNAL USE ONLY.

Stofat may include calculation of Weibull parameters. It shold however be noted that the Weibull distribution is NOT used in the fatigue computation in Stofat. The long term distribution is taken from the scatter diagram and the long term probabilities for the wave directions. The total damage is a summation over all part damages calculated from the short term response for each sea state (cell) in the scatter diagram. Appendix C3 i the Stofat user manual explains the procedure, ending with "The damage is then summed over all sea states and over all wave directions." The DNV Class

Note 30.7 is also a very useful document, serving as a background for the calculations in Stofat.

This means that if you print all the part damages, the total damage can be calculated by summing these in e.g. Excel.

The Weibull distribution is an additional benefit from Stofat. The Weibull parameters may be calculated by Stofat, and printed, to be used if a user wants to do a simplified long term calculation. In such a case, a Weibull distribution may be assumed instead of using the detailed scatter diagram etc. This simplified method is not part of Stofat, but is exaplined in the Class Note 30.7, section 4.3.

Back to top

Stofat: What is the exceedence probability levels

The commands DEFINE SHELL-FATIGUE-CONSTANTS EXCEEDENCE-PROBABILITY-LEVELS or DEFINE FATIGUE-RESULTS-DUMP EXCEEDENCE-PROBABILITY in Stofat are more or less doing the same thing, which is to define the number of stress exceedence levels that are to be included in the dump file from a certain fatigue run. The default amount of levels are set to 11, but this may be changed if neccesary.

Below is an excerpt of a dumpfile (.pex) for a certain hotspot or element (294) with 15 exceedence levels (becomes 16 in reality since level 0 is included):

Stress range  
Exceedence probability
294 8 All 0 4.25488950E+06 1.94639291E-08
294 8 All 1 4.09540550E+06 6.57393002E-08
294 8 All 2 3.80287650E+06 5.52219262E-07
294 8 All 3 3.51034725E+06 3.98817792E-06
294 8 All 4 3.21781850E+06 2.47715889E-05
294 8 All 5 2.92528950E+06 1.32427696E-04
294 8 All 6 2.63276050E+06 6.09929557E-04
294 8 All 7 2.34023150E+06 2.42231088E-03
294 8 All 8 2.04770262E+06 8.29821639E-03
294 8 All 9 1.75517362E+06 2.45170034E-02
294 8 All 10 1.46264475E+06 6.24469407E-02
294 8 All 11 1.17011588E+06 1.37006059E-01
294 8 All 12 8.77586875E+05 2.57967234E-01
294 8 All 13 5.85057938E+05 4.12830949E-01
294 8 All 14 2.92528969E+05 5.52937984E-01
294 8 All 15 0.00000000E+00 6.10746741E-01

Notice the significant change in exceedence stress range probability between the levels. If both these commands are used, the command with the highest exccedence level will be the active one. Please also have a look at chapter 2.7 in the user manual for more info about the dump file, and also try the commands in Stofat to look at the actual results.

Back to top

Stofat: What is the number in the FILE TRANSFER command?

The number used in the FILE TRANSFER command is the superelement identification KEY number, not the superelement number. This KEY number is defined by the sequence of assembling superelements in Presel.

When running Stofat interactively, a table showing the connection between the superelement type number (T#.FEM) and the key number is displayed.

From the Prepost user manual:

A superelement identification key is simply an integer number in the range 1 to number of 1st level superelements, numbered from left to right in the superelement tree.

PREPOST will present a list showing the available superelements and their

corresponding keys.

Back to top

Submod (All Versions): Why does Submod say that it is not possible to find a node?

The following message may be written to the file Submod.mlg, and may happen when Submod is trying to match the defined boundary nodes in the submodel with the global model.

*** ERROR RETURN FROM XHZ230 *** ERROR FLAG =-100 NOT POSSIBLE TO FIND XI, ET AND ZE. VALUES NOT CONVERGING. XI,ET,ZE: 1.08290E+00 5.50330E-01 8.79095E-14 FOR POINT WITH COORDINATES X,Y AND Z: 2.36000E+01 -2.70000E+01 1.38000E+01 IF NODE IS FOUND LATER IN ANOTHER ELEMENT, DISREGARD THIS ERROR MESSAGE

The message is an early warning, saying that so far, searching in a specific element, Submod has not found the node in question. If you later find that all nodes are indeed matching, the execution should be okay:

   Number of matching coupling-nodes ........:    411
   Number of non-matching coupling-nodes .:        0

Of course, you should always check the deformation plot of the sub-model, for example in Xtract. The deformation on the boundary of the sub-model should match the deformation of the global model in the same area.

Back to top

To force Sestra10 run in Sesam Manager

To force the new Sestra 10 to run the new solver, a /dsf switch is required.

If running the analysis from Sesam Manager, then need to add the /dsf switch to the additional argument field,

Or if running the analysis from command prompt, then the /dsf switch should directly follow the Sestra.exe command,

Back to top

WindExtension (1.0-01): Limitation due to memory allocation in Sestra

Applies only to version 1.0-01 Use Sestra Version 8.4.5 or higher to avoid possible memory problems.

Back to top

WindExtension (2.0-662 from 1.0-01): Limitation due to memory allocation in Sestra

Applies from version 1.0-01 to version 2.0-662 Use Sestra Version 8.4.5 or higher to avoid possible memory problems.

Back to top

WindExtension (2.0-662): Splice does only support up to 5000 load cases

Applies only to version 2.0-662 If the simulation time multiplied by the time-step of the wave/wind combination exeeds 5000. (e.g. 600sec * 0.1sec > 50000), Splice will return with an error message.

Back to top