General Mechanical

General Mechanical

An error occurred inside the SOLVER module: general error

    • Smileyniall
      Subscriber

      Please help me to fix this error.

      I have build a model in inventor, then I convert it to file which has "Step" tail. Most of subject in model this plate. So I used Mid surface tool in Space claim to create face model. Next to, I used Ansys workbench to mesh and mesh connect.

      I try to test my model in Modal, It appear error: "An error occurred inside the solver module: General error".

      Can you explain why appear this error and how to fixed it.

      Thank you for your support.

    • Smileyniall
      Subscriber
      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.n
    • peteroznewman
      Subscriber
      ArraynYes, 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.nIn 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.n
    • Smileyniall
      Subscriber
      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. nn
    • Smileyniall
      Subscriber
      Just realised the previous file needed to be repaired and how to repair nn
    • peteroznewman
      Subscriber
      nThis model has a timber material defined using an Orthotropic Elasticity where the high stiffness direction is defined along X.nThe 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. nI wasn't getting realistic action at the joints.nI 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.nIf you take this approach, you can delete all the contact between the studs and the footer/header rails.nWhen you delete all the holes from the studs and footer/header, the mesh will improve.nMake sure that every solid body has at least two elements through the thickness, such as the Load Plate shown below.nA 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.n
    • Smileyniall
      Subscriber
        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 todaynnn
    • peteroznewman
      Subscriber
      nIn SpaceClaim, use Split Body to split the Header and Footer rails at each stud. Go from thisnto thisnOpen 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.nChange all the hemp panels from Frictionless to Frictional with a 0.2 COF.tnIt 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.n
    • Smileyniall
      Subscriber
      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? nI 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.nThanks againnn
    • peteroznewman
      Subscriber
      nI 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 2.1nIt seems you have attached an old file.n
    • Smileyniall
      Subscriber
      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 againnn
    • peteroznewman
      Subscriber
      nYes, you need to change the Analysis Settings and turn on Large Deflection.nYou 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.nChange the Analysis Settings as shown below.n
    • Smileyniall
      Subscriber
      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.ot sure if ive done something incorrectly. nn
    • Smileyniall
      Subscriber
      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? nn
    • peteroznewman
      Subscriber
      nYou 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.nThe solver issues many warnings and most of them can be safely ignored.nWhat 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.n
    • Smileyniall
      Subscriber
      Hi I cant find the force convergence plot, when i run the solution it starts then after a minute I get this warning nThe 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 nn
    • peteroznewman
      Subscriber
      n
    • Smileyniall
      Subscriber
      ok thanks for that tried t find out online where to access itnn
    • peteroznewman
      Subscriber
      nUnder Analysis Settings, turn on Auto Time Stepping.nChange the initial substeps to 100, minimum substeps to 10 and maximum substeps to 1000.nUnder Solution Information, type 3 for Newton Raphson Residuals.nThen Solve.n
    • Smileyniall
      Subscriber
      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 needednn
    • peteroznewman
      Subscriber
      nPlease reply with an image of the Analysis Settings for Step 1. nWhat number did you use for Initial Substeps? The graph is informing you to use a number 8 times larger.nPlease reply with an image of the Anaysis Settings for Step 2.nThat should have an Initial Substeps value similar to Step 1.nn
    • Smileyniall
      Subscriber
      Sorry about the delay I've been having issues with my remote desktop and accessing Ansys on it. I have managed to down load it onto my pc there and I only changed the subset setting for step one, I didnt realised I ad to do them all seperatly. Hopefully I be able to run the program soon on the remote desktop and will let you know if it is successfulnn
    • Smileyniall
      Subscriber
      Hey I've ran it again after finally getting back online and the getting the MPC message again. and it also stopped at 178nn
    • peteroznewman
      Subscriber
      nThere were 3 converged substeps, you should look at those. Reply with an image of the last converged substep for Total Deformation. Is it behaving the way you expect?nThere are 3 Newton Raphson Residual Force plots, you should look at those, they are under the Solution Information folder. Look at the location of the maximum. Do all three plots show the same location? Reply with an image of the elements around the N-R-R maximum. This generally indicates where you need to make a change. The change could be to soften the contact, or it could be to use smaller elements. Show us the plot.n
    • Smileyniall
      Subscriber
      I can't seem to find any reults for steps 2 and 3 only step 1n
    • peteroznewman
      Subscriber
      nCorrect, you got 3 converged substeps in step1.nWere you going to show me the plots of N-R Residual and the last converged substep?n
    • Smileyniall
      Subscriber
      Sorry been running a solution for over 24 hours now. Realised the top and bottom rails were off by .2mm and fixed that woudl that have been an issuue? The program is currently on step 810 furthest point it has gotten to in a while. I have gotten a warning saying Two or more remote boundray conditions are sharing a common face, edge, or vertex. This behaviour can cause soler to over constraint and is not recommended, please check results carefully. you may select offending object and/or geomerty via RMB on this warning in the messages window. would this have anything to do with how long it is taking to solve?n
    • Smileyniall
      Subscriber
      n
    • peteroznewman
      Subscriber
      nThis is working properly. Let it continue to run. There may be things to try to reduce the waiting time, but mostly you want to get to the full solution.n
    • Smileyniall
      Subscriber
      The solution failed at 1336 the deformation has a large hole in the second infill, not sure why it just happened for this one, As the others seem to be un effected. nn
    • peteroznewman
      Subscriber
      nDon't look at the Unconverged step. Look at the last converged substep.nUnder Solution Information, show the Time Increment Plot.nUnder Analysis Settings, show the Step Controls. What is the Minimum and Maximum Substeps?.
    • Smileyniall
      Subscriber
      The max and min subsets are the same for all stepsnn
Viewing 31 reply threads
  • You must be logged in to reply to this topic.