General Mechanical

General Mechanical

large deflection results problem

    • msnadeem
      Subscriber

      Dear connections,


      Facing problem regarding Large deflection results in the model, figure pdf file attached in this message. Also when trying to check results using ''true scale'', unrealistic results of deformation are been observed. Please can anyone let me know what's wrong with the results? what could be the reason of such results and how can it be corrected ?

    • Sandeep Medikonda
      Ansys Employee

      Some recommendations:



      • Solve it with large deflection turned on. Use more sub-steps if needed.

      • Use EREX,NO. See this discussion.

    • msnadeem
      Subscriber

      Dear Sandeep sir,


      I have also tried before by keeping Large deflection ''ON'' in analysis settings and also ''EREX,NO, but the solution never got complete even after about 3-4 hours or neither the solution failed. Also, I got ''contact status has experienced an abrupt change'' message during the solving period, since the model is a die holder assembled with two different components as you can see in pdf file attached, on applying torque, the assembly components might slide little(my assumptions) even after fully assembled, and I kept the sliding assembled parts contact as ''No seperation'' or Do I need to keep all contacts ''bonded'' only ? I am doing something wrong with contacts ?   

    • msnadeem
      Subscriber

      Dear Sandeep sir,


      Could you please help me in solving this model, I will attach the stp file and ansys file for you, I can learn and rectify my problem once you will be able to solve it, I have already invested a lot of days behind it, Can you help me out please?


      Looking forward to hearing from you.


      Thank you!!


      Best regards


      Nadeem

    • peteroznewman
      Subscriber

      Dear Nadeem,


      ANSYS staff are not permitted to download attachments, so Sandeep will not be able open your stp file or archive. Sandeep and other ANSYS staff can help by replying to what you put in your replies, including when you insert images into the post directly using the button. No one from ANSYS has seen the images in the pdf attached to your first post.


      There are a few members, like me, who are not  ANSYS staff and will download and look at your ANSYS .wbpz Archive file.  Check the box to Include Imported files and the stp file should come with the archive.

    • msnadeem
      Subscriber

      Dear sir,


      I am really grateful to you, please help me in solving the problem dear sir. I have attached the file in this message with necessary requirements which you have described.


      Looking forward to hearing from you.


      Kind regards


      Nadeem 

    • msnadeem
      Subscriber

       


      Dear sir,


      I forgot to mention one thing regarding Ansys archive file, please check the results of Group B- Static structural. Group A results are incomplete due to incomplete model and is not part of our discussion.


      Thank you!! Looking forward to hearing from you.


      Regards


      Nadeem

    • peteroznewman
      Subscriber

      I made a change under Analysis Settings, turn Large Deflection On and set the Auto Time Stepping On and request 10 Initial Substeps. That created an error...


      *** ERROR ***                           CP =      86.971   TIME= 17:04:04
       Element 32575 (type = 12, SOLID187) (and maybe other elements)
      has become highly distorted.  Excessive distortion of elements is usually a symptom indicating the need
      for corrective action elsewhere. 

      You can see which element this is by copying the Element ID and creating a Named Selection in the worksheet, but the easy way is to click on Solution Information and in the Details window, type a 1 in the field for Identify Element Violations. Now you get a Named Selection automatically created for you under the Solution Information folder.



      The bonded contact to the Handles is deforming the elements. You need smaller elements around these holes.

    • peteroznewman
      Subscriber

      You have a warning message about your mesh quality.



      It would be wise to fix the mesh to address this problem before proceeding. It is the pin that the small gear sits on. Just add a sizing control to that body of 1 mm to fix that.


      You have a lot of parts in your model. Please describe what question you want the model to answer. There may be some simplifications that can be made that won't affect the answer you want the model to provide, but could greatly reduce the model complexity and make it much easier and faster to converge on a solution.

    • msnadeem
      Subscriber

      Dear sir,


      Thanks a lot for rectifying my problems, I am currently working on it as described by you. Will get back to you soon.


      Kind regards


      Nadeem 

    • peteroznewman
      Subscriber

      I suppressed all parts except for: Die, Fixed Part, Moving Part and two Handles.


      I suppressed the No Separation contacts since each Part on the die was already bonded to the die, so it seemed redundant to have that also.


      I also picked all the edges on the center of the Die to apply the Moment to avoid excessive pressure on the four edges you had selected.


      I set the Analysis settings to have 200 Initial Substeps.


      I increased the mesh density around the holes the handles went in by using Contact Sizing of 1 mm element size.


      I let it solve for 2.75 hours on 12 cores out to 52% of the total Moment you specified, which is 300 N.m


      The website is broken now and will not allow images to be inserted or attachments to be attached.


      The die has rotated almost 40 degrees and the handles are bending a lot. It seems to me that the Moment you have specified is much too large.  How did you come up with that number?

    • msnadeem
      Subscriber

      Dear sir,


      Currently I am pursuing Internship in Denmark. This square die is used for cutting big threads for large bars in various mechanical industries, The value I used is correct or may lie between ''285 N-m to 310 N-m'' standard value range from company's catalogue (Because the torque can't be constant all the time during operation), but I used 300 N-m (assumptions).


      I really don't understand why the handles are bending so much, the task is optimize the current die holders and reduce weight, since current designs are very heavy. What do you think about my thoughts? 


      Also, please attach archive file which you have worked on once the website works fine. Looking forward to hearing from you.


      Kind regards


      Nadeem

    • peteroznewman
      Subscriber

      Dear Nadeem,


      I did a quick model of just one of the handles and put half the moment at the end of that handle. There was very little deformation in the handle. There is something wrong with the original model solution quality. It might need non-default convergence criteria.


      Now I have the reduced model, but I inverted the boundary conditions. I made all the edges at the center of the die to be Fixed Support, and I put a 545 N force at the end of each handle, where 150 N.m / 0.275 m = 545 N.  One handle has +545 N and the other handle has -545 N both for the X coordinate.  We will see what that gives for a result in a few hours...

    • msnadeem
      Subscriber

      Dear sir,


      Thank you very much for cooperating and giving me time for this problem sir, can you please tell me how much deformation in ''mm'' did you get in the previous result where you said the die has bend 40 degree angle (approx.) ? I hope you got something around 700-850 mm deformation results ?


      It is possible to invert the boundary conditions for performing simulation, no problem. But the reason I fixed handles and applied moment on die sharp edges is because I considered the die holder to be analyzed for real and actual environmental conditions.


      Currently, I am also running the simulation, but the solution is unable to reach the solution because the time limit of processor is exceeding. Now waiting for 2nd try results.

    • peteroznewman
      Subscriber

       Dear Nadeem,


      Swapping the BCs did not help. An excessive, incorrect amount of deformation showed up in the solution.


      If I separate out just the handle, and compare a solid and beam model, both get the correct small amount of deformation.
      For a 275 mm long 16 mm diameter solid cylinder of stainless steel with a 545 N tip load, the tip deformation is 6 mm.


      This will take some more study to understand.  I think it will need a non-default treatment of the convergence criteria.


      Regards,
      Peter

    • msnadeem
      Subscriber

      Dear sir,


      I tried and the solution completed and the equivalent stresses seems to be fine to me but the deformation results are still unrealistic.


      Regarding Non-default treatment of convergence ? I don't know much about this process. How should I solve this issue dear sir? 


      Thank you !!


      Kind regards


      Nadeem

    • peteroznewman
      Subscriber

      I made a simplified version of your model and it gave the correct handle deformation as shown on the left.


      I need to review your model some more to determine what went wrong with it as shown on the right.



      The model has 349 N.m of Torque applied by 500 N at the end of 349 mm long handles.


      Attached is the 2019 R2 archive.

    • peteroznewman
      Subscriber

      Okay, here it is!  Element Quality.  Here is the Orthogonal Quality of the mesh with the incorrect deformation.



      If I go into SpaceClaim, and cut away the geometry that has these bad quality elements, I can get this mesh:



      Results



      An element with an orthogonal quality of 1E-7 destroys the entire solution.


      ANSYS 2019 R2 archive attached.

    • msnadeem
      Subscriber

      Dear sir,


      The threads were the real reason of improper mesh quality ? How did you find that mesh in the die was improper and had a lot of broken elements already. Was it in the solution information worksheet ? But now the results seems to be very nice. Thanks a lot dear sir, so glad to see the good results, but I am unable to open the files in Ansys 19.0 student version. which version do you use currently ?


      Looking forward to hearing from you.


      Nadeem

    • peteroznewman
      Subscriber

      Dear Nadeem,


      The elements are not broken, they just have a very, very, poor shape. It is possible to get good element shapes on the threads, it would just take a lot of elements and you wouldn't be able to solve it on the Student license. The workaround is to remove the threads so that you can get good element shapes without using a lot of elements.


      Poor element quality destroyed the numerical precision in the solution process. This is a known fact about FEA (and CFD) and is why there is a mesh quality section in the Mesh details so you can evaluate the element quality before you solve.  I should have checked this earlier, but I finally remembered to check it.


      I don't have ANSYS 19.0.  You should download and install ANSYS Student 2019 R2 using the button at the top of this page because there are many improvements to the software.


      Regards,
      Peter

    • msnadeem
      Subscriber

      Dear sir,


      Thanks a lot for helping me out. I have understood the problems in the geometry and mistakes I did in it. Will install new version. It was a big help from your side to me. Have a nice day.


      Kind regards


      Nadeem

    • Sandeep Medikonda
      Ansys Employee

      Nadeem, Peter has gone above and beyond to help you here....you can show your gratitude by marking (also liking) his response as an answer....

    • msnadeem
      Subscriber

      Dear sandeep sir,


      Yes definitely, I will write and give him all the points. I was checking the same option of mark in his comments. Thanks a ton . Have a nice day too. 

Viewing 22 reply threads
  • You must be logged in to reply to this topic.