An error occurred inside the SOLVER module: general error

SmileyniallSmileyniall Member Posts: 2

Hi, I am currently in last stages of my thesis and hant difficulty with getting a solution. I had the program working with a much simpliar model but I wasnt getting realistic action at the joints. so I tried to add aspects that would simulate this more realistically. Excpet now when i go to solve the problem I get an "An error occurred inside the SOLVER module: general error" message and im not sure where to find to find why the error is ocuring. I was only ealier today The program would get to 90% then nothing would happen beyond that. Now after changing the mesh I only goes to about 30% without progressing. I was wondering if anyone is able to help me get a solution for the problem testing the racking resistance of the structre. here is a sample the problem i am working on.

Thanks,

Niall

«1

Comments

  • SmileyniallSmileyniall Posts: 21Member

    The other error I am recieving is "At least one contact pair has no elements in it. This may be due to mesh defeaturing. Please modify defeaturing settings which are accessible on the mesh object. This may also result from default trim tolerance of the respective contact or refine the mesh. You may aselect the offending pair(s) via RMB on this warning in the messages window. Alternately, set the variable" contactAllowEmpty to 1 in irder to ignore this error and allow the solution to proceed." I have tried to follow these instructions but havent been able to find he solution mentioned anywhere.

  • peteroznewmanpeteroznewman Posts: 11,378Member

    @Smileyniall

    Yes, "At least one contact pair has no elements in it" error is difficult to find the offending contact pair. I have struggled with that but ultimately figured it out with some help.

    In your post with the zip file, you have put only the .wbpj file which is useless without the accompanying _files folder of the same name. Use File, Archive to create a .wbpz file which holds both and can be directly attached to posts.

  • SmileyniallSmileyniall Posts: 21Member

    @peteroznewman Thanks for getting back to me, Sorry i didnt know the best way to upload the files as ive only been using the program for the last few months. I've attached the required format now.


  • SmileyniallSmileyniall Posts: 21Member

    Just realised the previous file needed to be repaired and how to repair


  • peteroznewmanpeteroznewman Posts: 11,378Member

    @Smileyniall

    This model has a timber material defined using an Orthotropic Elasticity where the high stiffness direction is defined along X.

    The high stiffness direction in timber is along the grain, and a long beam has the grain running along the length of the beam. Below is the image of the timber frame. The Header/Footer Rails are oriented along the X axis, so the orthotropic properties are appropriate for those two beams, but the five studs are along the Y axis but nothing has been done to align the material coordinate system to have the high stiffness along that axis. This model is simulating the grain running across the thickness of the stud which is wrong.

    I wasn't getting realistic action at the joints.

    I recommend you delete the nails and the holes in the footings and studs and replace them with an actual joint, such as a Revolute Joint. In the image below, you can see that I have arranged the Z axis of rotation to be aligned along the right edge at the bottom of the stud. Put the revolute axis at the left edge at the top of the stud. This will create the correct hinge points for the joint action you want as the frame is put under the shear load.

    If you take this approach, you can delete all the contact between the studs and the footer/header rails.

    When you delete all the holes from the studs and footer/header, the mesh will improve.

    Make sure that every solid body has at least two elements through the thickness, such as the Load Plate shown below.

    A better Idea is to delete the Load Plate and just push on the end face of the Header Rail. You can use a Remote Force to position the center of force to the location where the center of the Load Plate used to be.

  • SmileyniallSmileyniall Posts: 21Member

    @peteroznewman  thanks I forgot to add a orintation for the studs I have changed that now. Ive also removed the holes and nails I had a freeling they might be complicating the mesh and solution. Am I to replace all the holes/nail with a revolute joint in each connection? I have done this and now I seem to be getting some more errors I cant see where I have gone wrong and have struggled to rectify this today



  • peteroznewmanpeteroznewman Posts: 11,378Member
    edited March 27

    @Smileyniall

    In SpaceClaim, use Split Body to split the Header and Footer rails at each stud. Go from this

    to this

    Open the Header/Footer component, go to the Workbench tab and click the Share button to make sure the mesh connects across these new faces. Use those faces on the Revolute Joint. Note that on the header, I split it on the left side if the stud, while on the footer, I will split it on the right side of the stud.

    Change all the hemp panels from Frictionless to Frictional with a 0.2 COF.t

    It will be better to make this a 2-step analysis. In step 1, apply the 5000 N to the top of the frame and keep that on during step 2. Make the shear force 0 in step 1 and apply that in step 2.

  • SmileyniallSmileyniall Posts: 21Member

    @peteroznewman thank you for the help, I have Split the top and bottom headers and I was wondering do I just need to select just one face from each split when adding the joint?

    I have also ran the program and it has fainly given me a result. the deflection is much larger than expected. I was wondering is there a given stiffness with the joints or do I need to apply one? I am also being told the boundry box is too small and that I should turn on Large deflections in more than one warning.

    Thanks again


  • peteroznewmanpeteroznewman Posts: 11,378Member

    @Smileyniall

    I was expecting you to upload a file named Hemp-lime 2.3.wbpz since the last one was 2.2 and the one before that was 2.1

    It seems you have attached an old file.

  • SmileyniallSmileyniall Posts: 21Member

    @peteroznewman I saved over an old one that wasnt working so I just checked there and 2.1 is the most uptodate version I have but ther was a problem with the material file so heres an updated version again


  • peteroznewmanpeteroznewman Posts: 11,378Member

    @Smileyniall

    Yes, you need to change the Analysis Settings and turn on Large Deflection.

    You can delete all the Bonded Contact. It is unnecessary because the Share button in SpaceClaim connected the mesh along the top and bottom rails that were split.

    Change the Analysis Settings as shown below.

  • SmileyniallSmileyniall Posts: 21Member
    edited March 28

    I have done the following and now i get a mesage saying one or more MPC contat region or remote boundary condition may have conflicts.... Im also geting an error message saying that the solver was unable to converge on a solution.

    not sure if ive done something incorrectly.


  • SmileyniallSmileyniall Posts: 21Member

    @peteroznewman hey any idea what the offending pairs might been spent the day trying to resolve it but havnt been able to get ride of the warning about the MPc contact regions?


  • peteroznewmanpeteroznewman Posts: 11,378Member

    @Smileyniall

    You are using ANSYS 2020 R2 on an Academic Research License. I only have access to the Student license for that version. There are 261,244 nodes in your model but the Student limit is 32,000 nodes, so I can't solve. I have a full license for ANSYS 2020 R1.

    The solver issues many warnings and most of them can be safely ignored.

    What is important is the Force Convergence plot of Solution Output. This shows how the solver is progressing at ramping on the load. Please reply with an image of that plot. The corrective action is usually to add more substeps.

  • SmileyniallSmileyniall Posts: 21Member

    @peteroznewman Hi I cant find the force convergence plot, when i run the solution it starts then after a minute I get this warning

    The program then stays at (1%) solving mathematical model/(1%) preparing mathematical mmodel.. before stopping after around 20/30 minutes without any solition and three more warnings


  • SmileyniallSmileyniall Posts: 21Member

    ok thanks for that tried t find out online where to access it


  • peteroznewmanpeteroznewman Posts: 11,378Member

    @Smileyniall

    Under Analysis Settings, turn on Auto Time Stepping.

    Change the initial substeps to 100, minimum substeps to 10 and maximum substeps to 1000.

    Under Solution Information, type 3 for Newton Raphson Residuals.

    Then Solve.

  • SmileyniallSmileyniall Posts: 21Member

    @peteroznewman I tried solving it twice and the first time it failed at 178 and this time it failed at 330 tried to look up the trouble shooting but struggled to find what i needed


  • peteroznewmanpeteroznewman Posts: 11,378Member

    @Smileyniall

    Please reply with an image of the Analysis Settings for Step 1.

    What number did you use for Initial Substeps? The graph is informing you to use a number 8 times larger.

    Please reply with an image of the Anaysis Settings for Step 2.

    That should have an Initial Substeps value similar to Step 1.

Sign In or Register to comment.