Table of Detected Return Codes | ||
| ||
Priority Levels
There are three priority levels for return codes.
| Level | Meaning |
|---|---|
| (1) | Priority One Return Code: cleaning action may lead to data deletion |
| (2) | Priority Two Return Code: cleaning action may lead to data modification (without deletion) |
| (3) | Priority Three Return Code: unimportant error, cleaning action with minor impact on data |
| (*) | The rule is not executed on a document coming from a PDM system (ENOVIAVPM, ENOVIA LCA) |
Detected Return Codes
The return codes that can be detected are listed in a dedicated table along with explanations about the action performed by the CheckRepresentation batch.
| Error | Domain | Symptom (user view) | Technical Problem | CheckRep Operation | After CheckRep Execution |
|---|---|---|---|---|---|
| AGG_1 (1) | Aggregation | Aggregated object does not know its aggregating object | Aggregated object does not know its aggregating object | Deletes aggregation | None |
| AGG_2 (2) | Aggregation | Ghost links, undeletable view, Copy Paste failure, etc. | Corruption of an aggregation link between two objects (reciprocity broken). An aggregated object does not know its aggregating object | Updates aggregation link | No more ghost links, the view is removed, works,
etc. Document needs to be updated |
| BOL_0 (2) | Part Design | Visualization problems due to Boolean between Solid body (old) and hybrid body (new) | Boolean operation between solid body (old) and hybrid body (new) | Moves operand body under the part | Specification tree changes because operand body has been moved from Boolean to part |
| BOL_1 (2) | Part Design | Visualization problems due to Boolean between two hybrid (new) bodies | Boolean operation between two hybrid (new) bodies with operand body not aggregated to the Boolean feature, however displayed under it, leads to visualization problems | Moves operand body under the part | Specification tree changes because operand body has been moved from Boolean to part |
| BOL_2 (2) | Part Design | Solid body containing a Boolean feature is not processed when Part to Part data filtering is done. Then, the geometry associated to the Boolean feature is not visible in the 3D area | Scope of the Boolean feature is missing because the geometry of the Boolean feature is not seen in the 3D area | Deactivates then re-activates the Boolean feature. This creates the scope of the Boolean feature | Geometry associated to the Boolean feature is visible in the 3D
area. Document needs to be updated |
| BST_1 (3) | Mechanical Modeler | External user cannot see CAA features created with a previous version | When startup catalog for CAA features is not present, features cannot be displayed | Declares object's backup startup class | External user can see CAA features |
| CAT_0 (2) | Specs Modeler | A core dump may occur when accessing some data | A Catalog Manager does not point to a catalog document | Removes the link to the document that is not a catalog | No more core dump when accessing data |
| CPF_0 (3) | Part Design | Size of a part is abnormally huge comparatively to the number of elements | Unreferenced BREP features in Part Design features | Deletes unreferenced BREP features | Model size is reduced |
| CRV_0 (2) | Sketcher Modeler | Curves created outside the Sketcher workbench with no endpoints | Resulting geometry associated to the sketch is not consistent | Adds required endpoints | Sketches are seen as not up-to-date. Document needs to be updated |
| CRV_1 (3) | Sketcher Modeler | Update result is wrong because the update propagation is wrong. Some features are not impacted by geometries modifications, e.g. Output features | Attributes of several features are set to sp_NEUTRAL instead of sp_IN | Sets quality of curves attributes to sp_IN | No impact, except when cleaned geometries are published by outputs
features. Document needs to be updated |
| CST_2 (2) | Sketcher Modeler | CPU loop or problem with the activation/ deactivation of a constraint | Bad quality of constraints attribute | Changes quality of attribute | Document needs to be updated. Constraint can be used again |
| CST_3 (1) | Sketcher Modeler | Some Sketcher constraints are wrongly displayed or ignored during update | Value of a constraint attribute is lost | Deletes constraint | Document needs to be updated. The constraint can be used again |
| DAC_4 (2) | Drafting Annotation | A Roughness symbol is reversed when changing the standard through Page Setup. Roughness has an orientation link on the extension line (with interruption) of a dimension. | The orientation link on the extension line of a dimension with interruption could not be correctly built in previous releases before V5R14. In this case, the orientation link can return a wrong orientation direction. Thus, the roughness orientation on dimension is wrong. | Restores a correct orientation link | Roughness symbol is reversed and a possibly missing extension line is created |
| DAF_0 (3) | Drafting Annotation | The area fill is an empty space | The area fill not associated to any geometrical elements | Deletes the area fill | The area fill has disappeared |
| DAF_1 (3) | Drafting Annotation | The area fill cannot be selected | The area fill is not aggregated | Deletes the area fill | The area fill has disappeared |
| DAF_3 (3) | Drafting Annotation | Drawing contains some Area Fills that the user cannot see (only by using the Search function) | Area Fill without pattern | Deletes the area fill | The area fill has disappeared |
| DAO_2 (2) | Drafting Feature | Extension line is not visible (or not correctly) when creating extension line for roughness | View scale was badly taken into account for associative position on dimensions extension line (overrun). Extension line for roughness creation was not using the good length of dimension extension line (overrun) | View scale is taken into account for associative position dimensions extension line (overrun) | Extension line for roughness is now correctly visible |
| DCT_2 (1) | Drafting | Ghost links when running the File > SendTo command | Some features in CATDrwCont should have a father but are actually not aggregated anywhere: these corrupted/useless features are not visualized but can have links to external documents | Deletes non-aggregated feature | No more ghost link when running the File > SendTo command |
| DCT_4 (3) | Drafting | Error panel when opening the document saying that a used font is not available, although this font is not used by any annotation | A DrwMappingTable feature keeps a reference to a no more used font | Reference to the font is removed from the document | No more error panel when opening the document |
| DCT_5 (2) | Drafting Annotation | Impossible to use new fonts on dimensions inside the document | Internal font list is full | Removes unused fonts from the list and adds space in the list if needed | New fonts can be used and existing annotation now use the right font |
| DDI_4 (2) | Drafting | Dimension attribute is not valuated | Dimension display does not match dimension properties | Updates dimension properties | Dimension value does not go any more on the dimension line after view update |
| DDI_11 (2) | Drafting | Dimension text does not use the right font | Link from font and dimension visualization has been lost through undo/redo operation | Dimension visualization is rebuilt | Correct fonts are used for dimension visualization |
| DDU_2 (1) | Drafting | Ghost link on a Drawing document leads to the detection of the problem | Feature (which leads to the ghost link) is set under DrwCont instead of being aggregated under a view | Deletes axis lines, center lines, or thread that are directly under DrwCont container | No more ghost links when running the File > SendTo command |
| DFM_0 (2) | Drafting | When opening a document which was created with a previous version, the format of some sheets are flipped | Check/Clean DrwFormats whose width should not be strictly greater
than height.
Indeed, in documents with post R14 embedded standard, every
DrwFormat's characteristics should be width >= height.
DrwFormats that can be cleaned must match the following criteria
(otherwise they are ignored):
Note: the code which produced such corrupted DrwFormat has been fixed |
Cleaning such corrupted DrwFormats involves the following
operations:
|
Corrupted formats of the sheet are flipped back to normal |
| DOC_6 (3) | Specs Modeler | Document cannot be stored in ENOVIAVPM | Applicative container with no stream in the document | Creaties an empty stream for this applicative container | Document can be stored in ENOVIAVPM |
| DRF_0 (3) | Part Design | When deleting the draft, some related data are left in the document | Data model inconsistency | Removes Usur Features from Geometrical Set to PartBody under Draft feature | Data model inconsistency is now solved for this draft feature. If
deleting the draft the life cycle management will be better. Document needs to be updated |
| DRF_1 (3) | Part Design | When creating a new draft feature, the geometry selected to define the pulling direction is inconsistent with the pulling direction vector | Inconsistency between the vector and the selected object in the definition of default values | Resets default pulling direction in object and vector | Default draft pulling direction is changed. The next created draft will use this new default pulling direction |
| DTE_2 (2) | Drafting | 1. Text with position link to another text is not up-to-date
after canceling text edition of reference 2. Text leader with Positional Link with a 2D Line is pointed to other element |
1. Associative position with text as reference was not updated
after canceling text edition 2. Text leader with Positional Link with a 2D Line was not updated |
Updates position link to get the correct position | Position of text or leader is moved to the right location |
| DVM_0 (2) | Drafting | Error when saving a Drawing | Useless view makeup detected | Deletes useless view makeup | Drawing is correctly saved. Reduces the size of the document |
| DWR_0 (3) | Drafting | No visibility | Useless relation has been detected: either the in or the out of the relation is not valuated | Deletes useless DrwRelation | No impact. Document size is reduced |
| DWS_0 (2) | Drafting | Impossible to select a view (not allowed), Grid disappears, or impossible to activate Drafting workbench | Internal value which determines the order of the views is not correctly set | Internal value correctly set: the order of the views is correct | View can be selected |
| DWS_1 (1) | Drafting | No visibility | Corrupted sheet has been detected: either it has not the minimum required views (background and main view), or it is not under the drawing | Deletes corrupted sheet | No impact. Document size is reduced |
| DWV_0 (1) | Drafting | No visibility | One or several rules for a view in the drawing is not respected:
1. A view must have a parent 2. A view of type Pure_sketch must not have a sheet as its parent 3. A view which is not of type Pure_sketch must have a sheet as its parent |
Deletes view | Drawing is correctly saved. Document size is reduced |
| DWV_4 (3) | Drafting | Axis elements of the sketch support associated with a view that has been put in the No Show space before V5R14 cannot be visualized in the Show space anymore | Sketch support is in the No Show space | Puts sketch support in Show Space and puts its axis elements in No Show space | Sketch support axis elements can be seen in the Show space (provided that the user puts them in it) |
| DWV_6 (3) | Drafting | File size for Drawing or Part containing some 2DLayoutData is unexpectedly important | Update mechanism has been corrected in V5R14 to avoid the creation of the Geometrical result of Drafting/2DLayout Views and 2D Component references. When correction has been performed, no corrective action has been done to manage former level models that had been updated with a software level that was creating some useless geometrical results | Useless geometrical results are removed from CGM container data. This data can represent MB of file size | Document size is reduced |
| FGM_1 (3) | Geometric Modeler | Part size is abnormally huge comparatively to the number of elements. Some vertices have unnecessary geometric data (linked curves/surfaces and some surfaces are over-defined (unnecessarily extrapolated)) | Some vertices have unnecessary geometric data (linked curves/surfaces). Some surfaces are over defined (unnecessarily extrapolated) | Removes unnecessary geometric data. Warning: 1. If you update the part, this error may re-appear again (after the cleaning rule). 2. If un-extrapolated elements are finally extrapolated, the shape of extrapolation can be different from the original one: the extrapolated part of the element has been "cleaned", and extrapolation can be different, depending on the algorithm that generates it |
Removing of unnecessary geometric data, the part is the same but smaller |
| FIL_0 (2) | Part Design | During edition of fillet an error "Internal error in mechanical modeler" is displayed | Support of some PointOnEdges (used to define radius for variable fillet) belongs to a ribbon other than the one to which the PointOnEdge itself belongs. Hence, when the support edge is removed (de-selection from user Interface), the corresponding PointOnEdge is not removed. This PointOnEdge then remains without support and gives an error "Internal error in mechanical modeler" when we try to access its support | Moves the PointOnEdge (FilletRadius object containing it) to the appropriate ribbon | Some objects (the fillet concerned and its impacted features) are
seen non-updated. Document needs to be updated |
| FMP_4 (2) | Part Design | Functional feature using a "to-shell" length does not correct the shell | Wrong shape is referenced by the feature | Changes reference to the correct shape | Part is red (not up-to-date). Document needs to be updated |
| FMP_5 (2) | Part Design | Feature does not update | "Ignore update" flag is incorrectly set | Clears the "Ignore update" flag | Part is red (not up-to-date). Document needs to be updated |
| FMP_6 (2) | Part Design | Functional feature using body thickness for its wall value does not update when body thickness is changed | Incorrect parameter is referenced by the feature | Changes reference is to the correct parameter | Part is red (not up to date). Document needs to be updated |
| FMP_7 (2) | Part Design | "Shellable" feature does not change "wall" direction when the part's shell properties wall direction (inward/outward) are changed | Incorrect parameter is referenced by the feature | Changes reference is to the correct parameter | Part is red (not up to date). Document needs to be updated |
| FMP_8 (2) | Part Design | Functional modifier is trying to modify the features of another part | Modifiers target list contains the features of another part | Removes the targets of the list that are not in the same functional body | Part is red (not up to date). Document needs to be updated |
| FMP_9 (2) | Functional Molded Part | Unable to update part using force update and part is corrupt | Shell property feature which is mandatory for wall based features is missing | Creates missing shell property feature with zero wall thickness | Shell property feature is created in the part. On update, part gets updated and build is OK |
| GSD_0 (3) | Generative Shape Design | Sometimes the user can only see invalid "Parent/Children" or impact analyses | An object is aggregated under "Component" attribute but it is never used elsewhere | Suppresses useless object | Visually no impact, better "Parent/Children" or impact analyses, reduces the size of the document |
| GSD_1 (1) | Generative Shape Design | Reference planes have datum mask on their icon and must have been moved with the compass | Reference planes are turned into datum or flagged as contextual features | Resets datum and\or contextual flags to 0. If a reference plane has been moved, a new one is created and added at the place of the moved reference plane. The moved reference place is renamed with the "moved by cleaner" to its alias | Icon of the reference plane has not the datum mask any more. A reference plane is removed and a new reference plane is created |
| GSD_2 (2) | Generative Shape Design | When updating a part containing axis systems created before V5R12SP2, orientation is inverted for some of them | Axis system algorithm was modified without versioning. When updating the axis system, which was built using old algorithm, its orientation might change since it now uses the new algorithm | Axis system attribute has been modified so that it maintains the same orientation with new algorithm | Update the axis system. Axis system orientation is not inverted.
Axis System and dependent features seen not up-to-date. Document needs to be updated |
| HIE_8 (2) | Specs Modeler | None in V5, as other links are expected between the two documents so , , behave as expected | Some links are created as external links during the creation of a local reference, links that should be within the local reference's structure | Offending links are re-routed within the local reference's structure (internal links) | None in V5. Document needs to be updated |
| HOL_0 (1) | Part Design | Rule created on V5R17 on the Hole's Activity parameter does not work correctly | In V5R17 for the Hole feature, there are 3 Activity parameters visible to the user among which 1 is valid and 2 are invalid. If the rule is set on invalid Activity parameter, such rule would not work | Rule set on the invalid activity parameter of the Hole is copied and set on the valid Activity parameter. The rule set on invalid Activity parameter is then deleted | A new rule would be seen under the Relation Set which would be same
as the old rule. Update would be required on the data after which
the rule would correctly work. Document needs to be updated |
| IGS_0 (3) | Sketcher | Use edges created when constraints are created, then when deleting these constraints, use edges that are not deleted and are therefore unnecessary (severity 3 since V5R9SP3) | Use edges that are not deleted when associated constraints are deleted. Unused elements (phantom operators) stay in the document | Deletes unused elements | Document needs to be updated. Document is the same but smaller |
| KWE_1 (1) | Knowledge | No visible symptom | Knowledge objects are not aggregated | If these objects are not pointed, they are removed. If it is a parameter that is pointed, it is added to the parameter set. If it is a relation that is pointed, it is added to the relation set | No visibility |
| LIF_1 (1) | Mechanical Modeler | Size of part abnormally huge comparatively to the number of elements or, some mechanical features are absent from the specification tree although detected in some commands | Unused elements (geometrical feature) are present or used elements should appear in the specification tree | Deletes unused elements. Some used elements (such as GSD features, geometrical sets and part bodies) are regenerated properly under the part in the specification tree | Part is the same but smaller. Used GSD features, geometrical sets and part bodies are all visible in the specification tree |
| LIF_3 (3) | Mechanical Modeler | No visibility except the size of the Product document (constraints deletion cases) | Unused elements (mechanical constraints) are present | Deletes unused elements | Document is the same but smaller |
| LIF_5 (3) | Mechanical Modeler | Ghost links displayed during SendTo or Save in ENOVIA | After deletion of some elements in part or product, links are kept in selection set | Deletes unused elements | No more ghost links |
| LPR_1 (1) | Drafting | When deleting a specific profile, other Profile2DL objects are impacted, and seen as not up-to-date. If automatic update is selected in , the update error panel is triggered with the error "Unable to evaluate the profile. No profile definition found in the layout view" | An internal structure definition for Profile2DL is shared by many Profile2DL objects, instead of being unique for one Profile2DL. When a Profile2DL is deleted, it deletes its internal definition, and deletes it for all Profile2DLs sharing this definition. The remaining Profile2DLs cannot access their internal structure, and cannot be rebuilt afterwards | Two corrections exist depending on the geometrical result of the
Profile2DL:
|
All profiles that shared the same internal structure definition are
either isolated or deleted. It means that all children of these
profiles are impacted by CheckRepresentation execution.
Document needs to be updated |
| MFG_0 (1) | Manufacturing | No visibility except abnormal size of Process document | Unused machining feature is not deleted (activities cases) | Deletes unused machining feature | Document is the same but smaller |
| MFG_1 (1) | Manufacturing | No visibility except abnormal size of Process document | Unused pattern definition is not deleted (pattern cases) | Deletes unused pattern definition | Document is the same but smaller |
| MFG_3 (1) | Manufacturing | No visibility except abnormal size of Process document | Toolpath not referenced by an activity is not deleted | Deletes the unused toolpath | Document is the same but smaller |
| MFT_1 (1) | Mechanical Modeler | When a solid is deactivated, the previous solid's result is damaged | Inactive feature storing the result of the previous feature | Reconstruction of the internal result when possible | Document needs to be updated |
| MGN_6 (1) | Mechanical Modeler | Size of a part on disk is abnormally huge | Useless Mechanical modeler data | Removes useless data | Model size is reduced |
| MGN_7 (2) | Mechanical Modeler | Some cells of Datum feature cannot be selected. Copy/Paste operation aborts | Cells cannot be selected because they have no naming | Adds a naming to the cells | All cells can be selected, and other features may be applied.
Document needs to be updated |
| MGN_9 (1) | Mechanical Modeler | Some existing cleaning rules (LIF_1) are too generic and delete data, and there is no easy way to repair them | Problem should occur only when the user creates publication in the part on non aggregated BRep features by using a batch. If geometry is changed, publications are not put to non updated status and features using them are not updated | Deletes invalid BRep features and re-plug the publication on equivalent BrepAccess. In some particular case, error may be returned as 'Non fixable'. Then a detailed comment explain to end user how to clean manually its data | Existing cleaning rules LIF_1 will no longer appear in these cases, publications will be pointing correct geometry, and update/no update status will work correctly |
| MGN_12 (3) | Mechanical Modeler | Size of the document is too big | Some Brep features pointing geometry with big history even if correct are really big | Compresses these Brep features to minimize the size | Brep feature and part need to be updated. Document needs to be updated |
| MIR_0 (2) | Part Design | When updating a corrupted mirror feature, an error with message " One or several features of the list have been deleted. Data is no longer consistent. You must delete the transformation feature." is displayed | One or many reference elements kept in Generative Tool for mirroring are lost | Reference elements kept in Generative Tool are created again | Document needs to be updated |
| MMR_0 (1) | Mechanical Modeler | Severe global malfunctionings in the part | At least one of the part's reference planes (xy, yz, zx) is damaged or missing | Part's reference planes (xy, yz, zx) are regenerated or repaired | Document needs to be updated |
| MMV_1 (3) | Mechanical Modeler | Visualization of a part is black | Invalid graphic property on the part | Deletes invalid property | Part is correctly visualized |
| MMV_2 (3) | Mechanical Modeler | Visualization of previously dressed-up geometry (used in Free Style workbench) can be wrong: the dress-up can still be visualized after removal. This problem can only occur for documents created before V5R10 | In some cases, dress-up properties could be duplicated, so that one property remained even after removal | Restores correct dress-up properties | Correct visualization, corresponding to the dress-up properties |
| MMV_3 (3) | Mechanical Modeler | If multi-viewer infrastructure is available on the part body (e.g. in SheetMetal workbenches), wrong view names appear in Views and Add view dialog boxes of the contextual menu. These view names appear in addition to the correct ones (i.e. 3D View and Flat View) | This problem can only happen for Part documents created in V5R10. On that level, wrong attribute values were streamed on the part body | Deletes wrong attribute names | Both multi-viewer windows contain only the correct view names |
| MTR_0 (2) | Mechanical Modeler | Generated drafting view is not complete: some elements are missing compared with the 3D visualization of the part | Wrong plug of attribute from the mechanical body to its last solid | Correctly resets attribute | Document needs to be updated |
| MTR_2 (2) | Mechanical Modeler | Visualization and/or update errors among solids | Wrong plug between solids | Correctly re-plugs solids | Document needs to be updated |
| OLE_0 (2) | Drafting | No visibility | DrwOLE object points to a startup not located in the same CATDrawing | OLE startup will be imported into the same drawing as the DrwOLE object if necessary. The DrwOLE object will then point to the right OLE startup | No visibility |
| PAT_0 (1) | Part Design | Document cannot be updated. Error obtained when update is called on part having user pattern, which has redundant instances in its Generic Tool | If user pattern has user defined feature as one of its item to pattern and if there are any redundant instances of features to pattern in Generic Tool of the pattern object, the model is corrupted | Redundant instances in Generic Tool of user pattern are deleted | Instances available in Generic Tool of user pattern are correct.
Document can be updated. Document needs to be updated |
| PAT_2 (2) | Part Design | If you select the edge/face of an instance of circular pattern (made of user pattern), the edge/face of another instance of circular pattern will be also selected | Generic naming of instances of circular pattern was incorrect because of a confusion point in the user pattern. The confusion point was not ignored during the naming of instances of user pattern | Confusion point is now ignored during the naming of instances of user pattern. It leads to the correct naming of instances of circular pattern | Each instance of circular pattern can be selected individually. Document needs to be updated |
| PIC_0 (3) | Drafting | Drawing picture disappears after a copy/paste | Non aggregated picture | Deletes non aggregated Drawing picture | Document is smaller |
| PIC_1 (2) | Drafting | When opening Drawing, reframe on is infinite | Some pictures have been created with a position set to a very huge value (value>float max value) | Modifies picture position value (set at 0;0) and moves to No Show space | New position set on picture to have a correct reframe on when opening Drawing |
| SCS_0 (2) | Sketcher | Sketch solving result is not stable. Geometries can move when the sketch is edited | Some geometrical constraints do not have Help parameter. This parameter is used by constraint solver to help solving the sketch | Adds missing Help parameter to sketcher constraint | Solving result is stable. When editing a sketch, geometries do not
move. Document needs to be updated |
| SHM_0 (2) | SheetMetal | Some SheetMetal objects cannot be deactivated | Information managing the activity is missing on some SheetMetal objects | Adds information. The activity will be at Yes after the operation | Activity is at Yes. Document needs to be updated |
| SHM_2 (2) | SheetMetal | Some functionality like CutOut, Hole, etc. fail if they are created on the part | Failure occurs during unfolding transaction because all cylindrical transformations are not correctly defined | Restores invalid cylindrical transformation to a valid one | Failing functionality can be applied successfully. Document needs to be updated |
| SKS_2 (2) | Sketcher Modeler | O point, H and V vectors of the absolute axis of the sketch are missing in the specification tree and are not visualized | O point, H and V vectors of the absolute axis of the sketch are missing in the model | Recreates missing elements of the absolute axis of the sketch | O point, H and V vectors of the absolute axis of the sketch are in
the specification tree and in the 3D visualization. Document needs to be updated |
| SKT_0 (1) | Sketcher Modeler | Sketch absolute axis is seen as up-to-date, but there is no resulting associated geometry | Operations within the Sketcher cannot be performed properly | Marks non up-to-date absolute axis | Sketches are seen as not up-to-date. Document needs to be updated |
| SKT_27 (2) | Sketcher Modeler | Output features are badly aggregated | Output features are aggregated as brothers of the sketch they are from and not under the dedicated node in the sketch | Modifies the aggregation of such outputs. The outputs are replaced under the dedicated node under the sketch they belong to | |
| SMG_16 (2) | Sketcher | Updates of sketches must be performed many times to get sketches updated | Constraints re-impacted during the feature update | Corrects constraints update | Result of the update is correct. Sketches are seen as not
up-to-date. Document needs to be updated |
| SSS_1 (3) | Mechanical Modeler | Selective loading on documents having selection sets containing elements outside their scope can have unexpected behaviors. Ghost links can be generated between documents linked through selection sets that do not respect their scopes. Using on documents that have selection sets containing elements outside their scope can have unexpected behaviors. Using on documents that have selection sets containing elements outside their scope can have unexpected behaviors | Selection set contains elements that are outside its scope. It was created before selecting elements outside the scope of a selection set that was prohibited. It is recommended to delete the selection set and to create another one containing only elements within its scope. If you decide to keep the selection set as is, this might generate ghost links | Non fixable error. The message associated to the rule recommends you to delete the selection set and to create another one containing only elements within its scope |
Non fixable error. The message associated to the rule recommends you to delete the selection set and to create another one containing only elements within its scope |
| TER_0 (2) | Mechanical Design | Update status of the Technological Result node does not change when adding/modifying a feature in the body. The consequence is that the technological result information may be inconsistent with the body content | Output is not plugged to the last shape feature (or its ResultOut) of the tool in which it has been created | Re-plugs invalid Technological Result Output to the last shape feature (or its ResultOut) of the tool in which it has been created | Update status changes when adding/modifying a feature in the body.
Document needs to be updated to refresh Technological Result information |
| THD_0 (3) | Part Design | When running the File > Send To > Directory in a CATPart, a thread reference file is also sent whereas it should not. | Link between a design table and the standard reference file is not broken but it should be | Breaks the invalid link | sends the correct set of data |
| THD_1 (3) | Part Design | A relation has been defined on the Thread Description attribute of a Thread with an external parameter. Changing the value of the external parameter does not update the Thread Description through the relation, which creates an error in the Thread feature | Thread Description attribute of Thread is sp_NEUTRAL. This attribute is linked to an external parameter through a relation. Change in value of the external parameter does not lead to update of Thread Description through the relation before the update of the Thread feature. Hence, the Thread feature is in error | Thread Description attribute is made an sp_IN attribute, thus change in value of external parameter leads to the update of Thread Description through the relation, before the update of PartBody. This results in valid update of the Thread feature | Part needs to be saved because of the change in attribute quality |
| UPD_0 (2) | Specs Modeler | Update cycle on the object cannot be seen/edited | An object has been created which is a direct input of itself in terms of update | Unsets the link to itself (breaks the cyclic dependency) | Update should no longer fail due to the update cycle |
| UPD_2 (2) | Specs Modeler | Update status: propagation problem. Data which should be not up-to-date is shown as up-to-date | The update stamp limit has been reached (MinInt = -2147483647) and the last feature modification has not been detected by the update engine | Increments the update stamp of the feature | Document may need to be updated if impacted features are active and belong to an update graph of the document |