Diagnostics for Creo Ansys Simulation
While working on a simulation study, you can check the model, the status of a study, the mesh, and results using different tools provided in the software. Use the following tools to get more information about existing or potential issues and how to resolve them:
• Notification Center—Information about failed objects on opening the application.
• Review Geometry—Review geometry and connectivity in a model before meshing or running a study.
• Simulation Study Check—Runs preprocessor diagnostics.
• Process Manager—Monitor the mesh generation and study run.
Notification Center
On opening Creo Ansys Simulation you get a notification about failed simulation objects. Failed simulation objects can be viewed in the Notification Center and you can then make corrections to the model geometry or simulation objects as required. Failed simulation objects also display a failed status in the Simulation Tree.
 |
A failed object does not prevent mesh generation or a simulation study run unless it is the only load or constraint in the study that is a failed object.
|
For example, if a feature that you delete or suppress in Creo Parametric has a load applied to it in Creo Ansys Simulation, then you see a regeneration error in the Notification Center, and the object displays a failed status in the Simulation Tree.
Study Check
After you define a study and simulation inputs, click > > 
Study Check to run a preprocessor check before running the study.
Study Check to run a preprocessor check before running the study.The study check is also automatically run when you run a simulation study. You can use the configuration option creo_ansys_study_check_show to define when study check results are to be displayed. By default, the study check results are displayed if there are issues in the model that result in a warning message when you try to run a simulation study. The study check reports the following information:
• Lists all simulation objects that are defined in the model.
• Provides a status on each object in the model as follows:
◦ 
—Object is valid.
—Object is valid.◦ 
—Warning message indicates missing object or object that could have a potential issue and affect your results but does not prevent the simulation study from running. Click More info to view the log file and correct the object.
—Warning message indicates missing object or object that could have a potential issue and affect your results but does not prevent the simulation study from running. Click More info to view the log file and correct the object.◦ 
—Error message indicates missing, invalid or faulty object. Click More info to view the log file and correct the object. The study (or mesh generation) cannot run until errors are fixed.
—Error message indicates missing, invalid or faulty object. Click More info to view the log file and correct the object. The study (or mesh generation) cannot run until errors are fixed.The following table lists the errors and warning message that are reported by the study check.
Object | Error Message | Warning Message | Simulation Study | Suggested Solution |
|---|---|---|---|---|
Geometry | Your model does not have any valid geometry defined. | Some models do not have any valid geometry defined and will be ignored. Only applicable to assemblies. | Structural Modal Thermal | Redefine model. |
Material | Some models do not have a valid material assigned. (In the case of assemblies.) Your model does not have a valid material assigned. (In the case of parts) Some bodies in your model do not have a valid material assigned. (multi-body part) | Structural Modal Thermal | Assign valid materials to your model. Click More info to view the diagnostics log file that lists the bodies, parts or assemblies that do not have material assignments. | |
Structural Constraints | Your model does not have any constraints defined. (applicable for a model that has no constraints, no springs and no joints) | Your model does not have any constraints defined. (no constraints, but at least one spring or joint) | Structural Modal | Define constraints for the study. |
Structural Loads | Your model does not have any loads defined. | Structural | Define suitable loads for the model. | |
Boundary Conditions | Your model does not have any boundary conditions defined. | Thermal Studies | Define suitable boundary conditions for the model. | |
Contacts | Your model does not have any contacts defined. | Structural Modal Thermal | Define contacts if required. | |
Shell Compression | Some objects in your model have become invalid, preventing the analysis from running. | Shell Compression has modified some objects in your model, in a way that might affect the quality of the results. | Structural Modal | Click More info for details and take appropriate action. |
Other | Some objects in your model are invalid or defined in a way that might affect the quality of results. | Some objects in your model are invalid or defined in a way that prevents the simulation from running. | Structural Modal Thermal | Click More info for details and take appropriate action. |
For the error or warning messages in the Other category if you click More info you get details about the issue. The following table lists the issues that could result in incorrect results.
Issue | Error or Warning Message | Additional Information |
|---|---|---|
Quilt referenced without a shell. | Warning: Some objects in your model reference quilts that do not have shells defined and will be ignored. | Assign shells to quilt surfaces if you do not want to have those surfaces ignored by the analysis. |
Curve referenced without a beam. | Warning: Some objects in your model reference curves that do not have beams defined and will be ignored. | Assign beams to curves if you do not want to have those curves ignored. |
A constraint or load is defined on a vertex. | Warning: Some constraints or loads in your model reference vertices. This may lead to singularities in results. | Review loads and constraints that are defined on vertices and redefine or delete as required. |
Multiple Loads on a single vertex. | Warning: Your model contains multiple loads applied to the same vertices. These are not supported in CAS. You may want to redefine or delete the loads. | |
Failed objects. | Warning: Some objects in your model are failed and will be ignored. Please check the Notification Center for more details. | |
Mass without a gravity or acceleration load. | Warning: There are no gravity/acceleration loads applied to your top model. All mass objects will be ignored. | This is only applicable only to structural loads. |
Non Zero Displacement Constraint | Warning: Modal analyses always assume an unloaded model. All non-zero displacements will be ignored. | This warning is displayed for modal analyses that have non-zero displacement constraints defined. |
Path to the study results folder is invalid. | Error: The path to the result folder is invalid. The path should not include Unicode characters and can have a maximum length of 248 characters only. The folder is set in Creo settings or via the configuration option creo_ansys_run_folder |
When there are issues related to shell compression, the Creo Ansys Study Check dialog box shows a generic message indicating an issue with shell compression.
When you click More Info you could see one or more of the following errors or warnings in the log file.
Condition/Type of Error or Warning | Error or Warning Message | Additional Information. |
|---|---|---|
Shell compression standard conflict error | Error: After shell compression the following objects in your model are referencing the same shell surfaces, edges or vertices . Edit the definition of objects or shell pairs, or delete some of them. | |
Shell compression standard duplicity error | Error: Some objects in your model reference either both sides, opposing edges, or opposing vertices of the same shell pairs. This causes ambiguity during shell compression and may lead to lower quality results. Edit the definition of the objects or shell pairs, or delete some of them. | |
Shell compression standard rotation warning | Warning: Some objects in your model reference the side (thickness) surface of a shell pair. After shell compression they may not constrain some rotations and may lead to lower quality results. You may want to either edit the definition of the objects or the shell pairs or delete some of them. | |
Mixed geometry within the same body | Warning: After shell compression, some solids and shell pairs contained in the same bodies became disconnected. Split the bodies to contain either solids or shell pairs but not both, and define bonded contacts between them. | |
Dissimilar Objects referencing opposing surfaces or edges of a shell pair | Warning: After shell compression some objects in your model are referencing the same shell surfaces or edges. Edit the definition of objects or shell pairs, or delete some of them. | Dissimilar objects that produce a conflict when referencing the same solid geometry will also create a conflict upon compression, if referencing opposing surfaces or edges of a shell pair |
Objects referencing surfaces of shell pair and solid geometry | Warning: Some objects in your model reference mixed geometry types after shell compression. These are not supported in Creo Ansys Simulation and will cause solver errors. Edit the definition of either the objects or the shell pairs or delete some of them. | Shell compression can result in some objects referencing mixed geometry. This is not supported by Creo Ansys Simulation |
Similar objects referencing opposing vertices of shell surfaces, or thickness edges | Some load directions in your model reference compressed edges and are lost. Edit the definition of either the loads or the shell pairs or delete some of them. | Any of the vertices of the opposing surfaces can have objects (Loads, constraints, etc.) defined on them individually. The short edges (thickness-wise) may also be references for such objects. On compression opposing vertices and the edges connecting them will become a single shell vertex. |
Error: Ball Joints—Some ball joints in your model reference vertices of shell pairs. After shell compression they may not constrain movements as intended, leading to lower quality results. You may want to check the model and edit the definition of the joints or the shell pairs or delete some of them | ||
Error: Planar Joints—The following planar joints in your model, that reference the thickness edges of shell pairs became invalid after shell compression. Edit the definition of the joints or shell pairs or delete some of them | This error is seen if both references of a planar joint are compressed. | |
Warning: Planar Joints—A shell compression standard rotation warning will be reported | This warning is issued if only one side of a planar joint is compressed. | |
Warning: General Joints—The following general joints in your model, reference the thickness edges of shell pairs and may have become invalid after shell compression. Check the model and edit the definition of the joints or the shell pairs, or delete some of them. | ||
Error: Your model contains multiple loads referencing opposing shell vertices or edges compressed to adjacent vertices that are also loaded. These are not supported in Creo Ansys Simulation and will be ignored. Edit the definition of either the loads or the shell pairs or delete some of them. | This error is issued for forces or moment on opposing vertices, or on a vertex and an adjacent thickness edge. | |
Error: Some objects in your model reference compressed edges and became invalid. Edit the definition of either the objects or the shell pairs or delete some of them | This error is issued if the force per unit length is defined on a thickness edge or you have a frictionless constraint defined on compressed thickness edges. | |
Warning: The model contains objects referencing shell thickness edges or vertices. Some of these are not supported in Creo Ansys Simulation and will be ignored. You may want to change their definition | This warning is issued for either of the following conditions: • Moment Reactions on thickness edges. • Results on thickness edges. | |
Same object referencing both the opposing vertices of a shell pair | Constraints—A shell compression standard duplicity error will be reported | |
Similar objects referencing opposing edges of shell pair surfaces | Warning: Some joints in your model reference the side (thickness) surfaces of shell pairs. After shell compression they may fail or not constrain movements as intended, leading to lower quality results. You may want to edit the definition of some joints or shell pairs or delete some of them | This warning is issued if multiple joints reference opposing edges of shell pair surfaces. |
Constraints: Shell compression standard conflict error is reported. | ||
Same object referencing both edges of a shell pair | Force or Moment load per unit length—A shell compression standard duplicity error is reported. Constraints—A shell compression standard duplicity error is reported. Mesh controls—A shell compression standard duplicity error is reported. | |
Similar objects referencing surface pairs | Constraints—Shell compression standard conflict error is reported. Mesh controls—Shell compression standard conflict error is reported. | Simulation objects may reference any of the opposing surfaces. On compression they need to be correctly applied to the resulting shell surfaces. |
The same object referencing both surfaces of a shell pair | Force/Moment load per unit area—A shell compression standard duplicity error is reported. Constraints—A shell compression standard duplicity error is reported. Mesh controls—A shell compression standard duplicity error is reported. | |
Objects referencing compressed side surfaces | Error: Some loads in your model reference the side surface of a shell pair. These loads become invalid after shell compression. You may want to edit the definition of the loads or shell pairs or delete some of them. | This warning is issued in the case of a force load per unit area that references side surfaces of a shell pair. |
Structural Contacts (bonded, no separation)—A shell compression standard rotation warning is reported. | ||
The model contains Bearing or Pressure loads applied to shell thickness. These loads are not supported in Creo Ansys Simulationand will be ignored. You may want to edit the definition of some loads or shell pairs or delete some of them. | Pressure or Bearing loads that reference side surfaces and result in edges on compression are not transferred to the solver. You need to edit or delete either the shell pairs or the loads. | |
Joints—A shell compression standard rotation warning is reported. | All joints except for fixed joints. |
You need to note the following points:
• When there are multiple shell pairs in a model, there maybe multiple failing shell pairs but Creo Ansys Simulation can report only one error at a time.
Hence you may have to fix the error for multiple shell pairs until the error is no longer reported.
• You may have to identify the problematic pair using a method of elimination or by looking for some cause for invalidity, like intersecting shells for example.
Process Manager
The Process Manager provides information about the mesh, study and results tasks running on the solver for a session. For a study that is in progress or running on the Ansys solver you can view the diagnostics file by clicking 
and then selecting 
Diagnostics to open the diagnostics file.
and then selecting Diagnostics to open the diagnostics file.The diagnostics file from the solver is a detailed log of the study run. Some experience with the Ansys solver might be required to interpret it.
For a meshing-only (mesh generation) process, when meshing completes, click Diagnostics to see the following information:
Diagnostics to see the following information:• Number of nodes generated.
• Number of meshing elements generated.