Learning Forum

[MishaBME]

Hi, I am having a problem with Static Structural's last step ( solution) in ANSYS 18.1.

The error is -

"An unknown error occurred during solution check the solver output on the solution information object for possible causes."

I have tried to solve the problem in many ways but it did not work. Could you please help me out to solve this error? 

Here, the file of solver information is attached.

 

[peteroznewman]

 *** ERROR ***                           CP =   83804.156   TIME= 17:42:52

The value of UY at node 16247060 is 8.736429281+134.  It is greater

than the current limit of 1000000 (which can be reset on the NCNV

command).  This generally indicates rigid body motion as a result of

an unconstrained model.  Verify that your model is properly

constrained.



*** ERROR ***                           CP =   83804.156   TIME= 17:42:52

*** MESSAGE CONTINUATION ---- DIAGNOSTIC INFORMATION ***

If one or more parts of the model are held together only by contact

verify that the contact surfaces are closed.  Also make sure that

there are constraints (or friction) in the sliding direction even if

no load is applied in that direction.  You can use the CNCHECK command

to check the initial contact status in the SOLUTION module.             

The model is unconstrained in the Y direction. Please reply with an image of the geometry and the loads and supports. Describe how contact is connecting the parts.

[MishaBME]

 I chose the vertebra body as target and the disc was chosen as a contact. Because the young's modulus of a vertebra is larger than the disc's young's modulus. 

Here, the details of the contacts are given in the photo.

 

When I initialize the contact tool all the results of information had the orange color legend. 

 

Here is the photo of my model. 

 

I chose the disc of Lumbar 5 as fixed support.

 

 

And the force was given on atlas. ( -20 N force was applied in the y-direction).

Here the details of force are given. 

 

 

[peteroznewman]

In Workbench, drag and drop a Modal analysis onto the Model cell of the Static Structural analysis.

In Mechanical, drag the Fixed Support and drop it into the Modal branch of the Outline.  Solve the Modal analysis.  Show the Tabular Data of the first six modes. Are they close to zero?  The deformed shape helps you figure out if any bodies in your model are not connected.

[MishaBME]

Hi, I had run the model but it took a lot of time. At first, I tried to run the model with the engineering data which was created by me. But there came an error. 

" Vertebral contains invalid property".

Then I changed the engineering data. I used stainless steel in my model to check the Modal analysis of the fixed support. And it was completed but there were an error and a warring, This time it also took more than 24 hours. 

The warring is -

"During this solution, the elapsed time exceeded the CPU time by an excessive margin. Often this indicates either a lack of physical memory (RAM) required to efficiently handle this simulation or it indicates a particularly slow hard drive configuration. This simulation can be elected to run faster on identical hardware if additional RAM or a faster hard drive configuration Is made available. For more details, please see the ANSYS Performance Guide which is part of the ANSYS help system."

And the error is the same one.  

"An unknown error occurred during solution check the solver output on the solution information object for possible causes."

 

I do not understand how to solve this problem. When I am trying to attach any file, the website is showing an internal error. I can not even upload any photos to show you regarding this problem.  Please, guide me. 

[peteroznewman]

I had the same problem attaching files and inserting images yesterday and reported that to the administrator for the site. It should be fixed soon.

Under the Solution Information folder, you can click on Solution Output and the text in the Graphics window is searchable with a Ctrl-F. Look for ERROR. You can copy and paste the text around that work into your reply.

[MishaBME]

 I looked for Error. And I found it in two places.

Here, the first error is--

*****  ANSYS SOLVE    COMMAND  *****

 

 *** WARNING ***                         CP =     123.391   TIME= 118:25

 Element shape checking is currently inactive.  Issue SHPP,ON or         

 SHPP,WARN to reactivate, if desired.                                    

 

 *** NOTE ***                            CP =     207.672   TIME= 119:11

 The model data was checked and warning messages were found.             

  Please review output or errors file ( F:ANsys COmmunitywhole         

 spine_final_trial_2_ProjectScratchScr53E8file0.err ) for these       

 warning messages.  

This is the second error--

 

***** ROUTINE COMPLETED *****  CP =     69205.547

PRINTOUT RESUMED BY /GOP

*GET  _WALLDONE  FROM  ACTI  ITEM=TIME WALL  VALUE=  14.1011111    

PARAMETER _PREPTIME =     86.00000000    

PARAMETER _SOLVTIME =     8861.000000    

PARAMETER _POSTTIME =     1.000000000    

PARAMETER _TOTALTIM =     8948.000000    

EXIT ANSYS WITHOUT SAVING DATABASE

NUMBER OF WARNING MESSAGES ENCOUNTERED=          1

NUMBER OF ERROR   MESSAGES ENCOUNTERED=          0

 

[peteroznewman]

It looks like there are no errors. If you show some lines at the end of the convergence reports, that will show how the solver finished converging.

[MishaBME]

Actually, I want to know that if there are no errors, it means all the contacts are perfectly done? And I could not get my results yet. Is it possible to get convergence reports? Actually, I understand the convergence report which is got under solution information like stress or strain. Right now, the results of stress and strain are not completed. So do I need to run the solution of the model in modal analysis? 

[peteroznewman]

 What kind of analysis was done?  If it was Static Structural, then the contacts are sufficient to compute a solution. I never use the word perfect to describe any model. All models are wrong but some are useful.

A modal solution will complete without errors even if the contacts are missing. The clue that the model is useless is if the first six natural frequencies are practically zero. This indicates a mistake in the contacts. You can find out which body is missing a contact by plotting the deformation. One body will have very large deformation relative to the body that is supported.

You don't look at stress and strain in a Modal analysis. Do that in a Static Structural model.

[MishaBME]

Yes, the model was done in static structural. But I got two natural frequencies, not six. Here is the data of frequencies -

 

  ***** FREQUENCIES FROM PCG LANCZOS ITERATION *****

MODE    FREQUENCY (HERTZ)      

 1     0.000000000000    

 2    0.4796555354550E-01

 

 *** NOTE ***                            CP =    2382.375   TIME= 13:48:13

 The file0.full has not been written.  If necessary, please use the      

 WRFULL command to generate the file0.full for any subsequent analysis   

 that requires it.                                                       

 

 *** NOTE ***                            CP =    2411.844   TIME= 13:59:29

 The .full file does not exist by user request.  Participation factor    

 calculations will be skipped.             

 

Could you kindly tell me why I am not getting the first six natural frequencies? Is it a problem with my engineering data or my model?  I did not get any errors. but I got a warning.  And one value is zero and the other one is 0.047 which is also close to zero.                            

[saifali]

Hi, Can you share the file?

 

s96aif@gmail.com

[peteroznewman]

Okay Misha, when you plot the Total Deformation from the Modal analysis, which part is moving the most?  That is the part whose contacts are not working.

[MishaBME]

Hi, Peteroznewman. there are two parts are moving fast and those parts are broken in Total deformation. These two parts are having contact problems and I can not solve that. I tried different ways in contact settings.

Here are the pictures. Could you please help me on how to solve this contact problem? 

[MishaBME]

Hi, saifali. I will publish the files after I have finished my research work.  

Thanks for your interest.

[peteroznewman]

The Pinball Radius is the critical parameter to change from Program Controlled to Radius, then you type in a radius that is large enough to span the gap.

Insert a Contact Tool under the Connections folder and Generate Initial Contact Status. Reply with a screen shot of the table of Status. You must see everything is closed. If it is Open, then you have problems.

[MishaBME]

I have changed the pinball radius. I gave 5 mm. The two parts are having problems, they are multiple and c5 which I have marked in the photos by red color. 

In initial contact status, it is seen that all the contact status is closed. 

[peteroznewman]

I can't see the contacts that you need to scroll down to see, but I assume you checked them.

For debug purposes, suppress all bodies except for the two that are misbehaving. Add a temporary Fixed support to one face of the bone.

Change the contact Formulation to MPC.  Submit that to a Modal analysis.

After it solves, the MPC contact elements are visible in the Graphics Window by clicking on the Solution Information folder.  You have to click the Graphics tab on the lower left corner of the graphics window because it flips over to the Worksheet tab when you pick the folder. Show a screen shot of that.

Then try larger pinball radius values, like 10 and 20 mm.

[MishaBME]

Hello Peter

Thanks a lot. I have finally solved my contact problem. 

But there is another problem in Engineering Data. Recently, I have started working on it. Actually, I need to give Power Law Plasticity value as engineering data for my model. In Static Structural, I could not find any properties in Toolbox. Could please tell me how can I find the properties in Static Structural or for plasticity which property should I use? 

[peteroznewman]

Hello Misha, please start a New Discussion for this new question and mark one of the posts above with Is Solution to mark this discussion as solved.

[TUSHAR Verma]

 ANYONE PLZ TELL ME HOW TO DEFINE CONTACT TO CONTACT TIEBREAK IN ANSYS INTERFACE LS DYNAWHERE IS THE OPTION PROVIDED?