How to Address "Terminal Error, FEM2ESH#" Decoding Error Messages

[PipePakPat]

In the ideal world, there are no errors of difficulties.  In reality, some users experience unexpected problems.  I have provided a list of a specific type of error message class titled "Terminal Error: FEM2ESH#", which relates to the process of decoding the pre-processor model into the finite element model used for analysis.  Although this list does not provide all error messages, it does provide those that appeared within the last 10 years.

For the following “Terminal Error” messages, the following error message format is use:

            Terminal Error: FEM2ESH#n, decoding_module#pn

Where:

• “n” represents the “FEM2ESH” decoder error message number
• “decoding_module” represents an undetermined subset of error message which can be either “item” or “FEMAPI” in the following examples
• “pn” represents the part number for which the error references.  This part number can be zero or any other part that exists in the model.

It can be assumed that the possible Terminal Errors can range between 1 and the maximum number provided in the list below, which is 130, and could perhaps exceed this number.  All of the potential error messages are not known.  This is a list of terminal error messages experienced by product support over the past 10 years along with details of the assumed meaning of each message and the proposed solution(s).

Terminal Error: FEM2ESH#19

Terminal Error: FEM2ESH#34

Terminal Error: FEM2ESH#38

Terminal Error: FEM2ESH#54

Terminal Error: FEM2ESH#55

Terminal Error: FEM2ESH#59

Terminal Error: FEM2ESH#63

Terminal Error: FEM2ESH#77

Terminal Error: FEM2ESH#82

Terminal Error: FEM2ESH#86

Terminal Error: FEM2ESH#108

Terminal Error: FEM2ESH#110

Terminal Error: FEM2ESH#130

Terminal Error: FEM2ESH#142

Error Message: Terminal Error: FEM2ESH#19, item#1

Decoding Processor: FEM2ESH                        Error Number: 19

Decoding Module: item                                     Part Number: 1

Error Description and Proposed Solution:

User had a zero length line. Global snap fixed issue.

Error Message: Terminal Error: FEM2ESH#34, FEMAPI#0

Decoding Processor: FEM2ESH                        Error Number: 34

Decoding Module: FEMAPI                               Part Number: 0

Error Description and Proposed Solution:

Problem related to v20 software release and occurred for a short period (weeks).  This has since been addressed and should not occur (nor should any error I imagine).  The problem is the presence of an Accupak.Egroup(-1)... entry in the model.dbf file.  Removing this entry from the model.dbf file makes the model check correctly, and is the immediate solution to the customer's issue.

Error Message: Terminal Error: FEM2ESH#38, FEMAPI#1

Decoding Processor: FEM2ESH                        Error Number: 38

Decoding Module: FEMAPI                               Part Number: 1

Error Description and Proposed Solution:

Line-based meshing found no element: a manually built or imported part as lines that do not make any brick (missing interior lines?)  These mean that you defined your part as Brick elements, but actually you only have a surface defined, (plate element), there is not enough vertices to form a brick elements.  One solution is to define the element type appropriately for the existing geometry lines.  Perhaps the part should be defined as plate, beam or truss elements?  If the surface mesh exists, but no internal elements, right-click on the part and choose to generate solid mesh.

Error Message: Terminal Error: FEM2ESH#42, FEMAPI#0

Decoding Processor: FEM2ESH                        Error Number: 42

Decoding Module: FEMAPI                               Part Number: 0

Error Description and Proposed Solution:

FEM_FILE_NOT_OPENED.  This can occur on computers where there are file access problems.  Perhaps a file backup service is locking a file, or only specific drives have user access.  Check with the IT person to grant permission for read/write access to all required drives and TEMP folders.

Error Message: Terminal Error: FEM2ESH#54, FEMAPI#29

Decoding Processor: FEM2ESH                        Error Number: 54

Decoding Module: FEMAPI                               Part Number: 29

Error Description and Proposed Solution:

FEM_ERROR_PART_TYPE_UNKNOWN.  Changing the element type from Tet to Brick eliminated error.  This can occur if the FEA Editor is not in sync with the design scenario’s ds.mod directory’s database.  This can occur due to unusual problems with the FEM file which may have since been corrected, or if the model resides across a network and either the model’s path is too long or there may be some unknown file access problem.  If the recommendation above does not address the issue, save the model to the workstation’s “C:\Test\” directory, which you will create for this specific puprpose J

Error Message: Terminal Error: FEM2ESH#55, FEMAPI#0

Decoding Processor: FEM2ESH                        Error Number: 55

Decoding Module: FEMAPI                               Part Number: 0

Error Description and Proposed Solution:

FEM_ERROR_ACTIVE_PART_HAS_NO_ELEMENT this occurs if the element definition has not be defined for the named part.  This can occur if the model resides across the netword instead of on the workstation, or for some versions of software when more than one part is selected, then the Element Defintion is defined for that group of selected parts.  This problem occurred as a result of a software defect which should no longer be an issue.

Error Message: Terminal Error: FEM2ESH#59, FEMAPI#12

Decoding Processor: FEM2ESH                        Error Number: 59

Decoding Module: FEMAPI                               Part Number: 12

Error Description and Proposed Solution:

FEM_ERROR_NO_1D_ELEMENT this occurs if there are no lines in the named part, or if there is a problem in the database for this part.  To verify if lines exist for this part, examine the surfaces in the model tree, if no surfaces exist, then delete the part from the model tree.  If surface and lines do exist, then copy select all lines in that part, right-click and choose to duplicate to a new part number, then copy the element type, definition and material from the original part to the new part.  Also, it may be possible to change the surface number of the existing lines, then change them back to clear the defect in the database.

Error Message: Terminal Error: FEM2ESH#63, FEMAPI#0

Decoding Processor: FEM2ESH                        Error Number: 63

Decoding Module: FEMAPI                               Part Number: 0

Error Description and Proposed Solution:

NO_3D_ELEMENT this can occur if the solid mesh does not exist for originally surface meshed parts.  Normally the solid mesh is generated at the time of analysis, but if one deactivates parts, then surface meshes other parts, then reactivates all parts, only those parts surface meshed last will have the flag set to generate the solid mesh.  Right-click on the problem parts and choose to generate solid mesh, or re-surface mesh the entire model at one time.

Error Message: Terminal Error: FEM2ESH#64

Decoding Processor: FEM2ESH                        Error Number: 64

Decoding Module: FEMAPI                               Part Number: 0

Error Description and Proposed Solution:

FEM_ERROR_3D_ELEMENT_NODE_OVER_BOUND this issue was resolved by regenerating the mesh on the model.

Error Message: Terminal Error: FEM2ESH#77, FEMAPI#0

Decoding Processor: FEM2ESH                        Error Number: 77

Decoding Module: FEMAPI                               Part Number: 0

Error Description and Proposed Solution:

FEM_ERROR_CONTACT_END_UNUSED_NODE this really relates to FEM2ESH#34 which demonstrates the inability to write to the DBF file.  Use the solution for #34.

Error Message: Terminal Error: FEM2ESH#82, item#1

Decoding Processor: FEM2ESH                        Error Number: 82

Decoding Module: item                                     Part Number: 1

Error Description and Proposed Solution:

FEM_ERROR_OBTAIN_OBJECT, A multi-body part was created in Inventor such that one part was defined as four separate volumes.  This created a problem when generating the solid mesh, which can only operate on a single volume per part number.

Error Message: Terminal Error: FEM2ESH#86, item#2

Decoding Processor: FEM2ESH                        Error Number: 86

Decoding Module: item                                     Part Number: 2

Error Description and Proposed Solution:

DCX_ERROR, found problem in line based meshing. This may have related to large number of elements and surface contact.  The model size was reduced and the problem no longer occurred, or the customer used the 64-bit version of the software to solve the issue.

Error Message: Terminal Error: FEM2ESH#108, FEMAPI#1

Decoding Processor: FEM2ESH                        Error Number: 108

Decoding Module: FEMAPI                               Part Number: 1

Error Description and Proposed Solution:

Define the thickness after mid-plane meshing a part.

Error Message: Terminal Error: FEM2ESH#110

Decoding Processor: FEM2ESH                        Error Number: 110

Decoding Module: FEMAPI                               Part Number: 52

Error Description and Proposed Solution:

FEM2ESH_ERROR_UNDER_DEFINED_ELEMENT_PROPERTIES: complete in element screen or switch to part-based 52.  Plate or Shell elements with surface based properties defined in the Element Definition screen may not have been properly defined, such that thickness values may be zero for some entries.  The solution is to define thickness for each surface, or switch to part based properties and define one thickness for all surfaces of that part.

Error Message: Terminal Error: FEM2ESH#130, FEMAPI#1

Decoding Processor: FEM2ESH                        Error Number: 130

Decoding Module: FEMAPI                               Part Number: 1

Error Description and Proposed Solution:

FEM2ESH_FEM_UNSUPPORTED_MESH_FORMAT, possible unknown element format in FEM (imported ?) Or the 1st element of the part has already distorted.  The mesh was generated in Altair Hypermesh as a NASTRAN file and imported to Algor. Algor read the CTETRA element type as degenerate brick instead of a tetrahedral which has a different node numbering format when stored into the Algor (Sim Mech) database.  This issue has since been addressed and should no longer occur.

Error Message: Terminal Error: FEM2ESH#142

Decoding Processor: FEM2ESH                        Error Number: 142

Decoding Module: FEMAPI                               Part Number: 1

Error Description and Proposed Solution:

FEM2ESH_FAIL_SOLVE_FOR_EQUIVALENT_FORCE, Accessing the Element Definition screen and choosing “OK” for each beam element part in the model may address this issue.

[anne.mellier-luguya · Accepted solution]

thanks for the solution