General Mechanical

General Mechanical

An error occurred inside the SOLVER module: general error (Reccurent problem)

    • GGM
      Subscriber

      Hi,

      I know this is a recurrent problem. But I check all the previous posts and could not work it out!

      I am using Ansys 2020R2, Student License, static structural analysis. I try to run and receive the following message "An error occurred inside the SOLVER module: general error".

      No "file.err" or " solve.out" found to give me any clue on how to troubleshoot it!!!!

      I can run other similar projects, but not this specifically (see project enclosed). This might rule out any license or computer problem, I guess.

    • Ashish Khemka
      Ansys Employee
      nnI cannot look into the file but do you find the same issue if you try to create a new model from scratch?.Regards,nAshish Khemkan
    • GGM
      Subscriber
      Hi Ashish,nI created this model from scratch (material, geometry, mesh, BC, contact, loading). Do you thing this error means the file is corrupted and therefore I should start from scratch all over?nRegards,nGGMnn
    • GGM
      Subscriber
      Hi,I just started from scratch all over again. But the same error message appears:An error occurred inside the SOLVER module:general error.nnI do not know what to do? Can any one share with me any hint????.Regards,nGGMn
    • Gary Stofan
      Ansys Employee
      In Mechanical, Select Solution, then Tools (Tab) -> Write Input file. nWrite the input file to any convenient location, then open in a text editor.n=======================n/com,*********** Create Contact Bonded - half_adhesive_U To half_adhesive_L ***********n/com,      Real Constant Set For Above Contact Is 16 & 15 n*set,tid,16n*set,cid,15nr,tidnr,cidnnldiag,cont,iter      ! print out contact info each equilibrium iterationn/noprn/goprn=======================nNote that the input is cut off just after contact pair Bonded - half_adhesive_U To half_adhesive_L.nThis can happen if the contact pair has no elements. This can happen if the mesh is defeatured. We see it often with any sort of knife-edge contacts.nIn your case, the contact pair seem it is just not defined properly in some manner. If I suppress the above contact, the solve starts.n
    • peteroznewman
      Subscriber
      nI'm not an expert at CZM, but you made a few mistakes.nYou wanted to do a 2D Plane Strain model, which is okay, but you did not set the Analysis Type to 2D on the Geometry cell in Workbench.nYou cannot simply edit this value and change it to 2D. You must do that before you attach the geometry to the Model cell. Start a fresh model and do that.nYou have a Fracture branch with a Contact Debonding item pointing to a Bonded Contact region which is okay.nThe problem is you have selected the Faces of the 2D bodies to be Bonded. You should have selected the Edges. In your model, that didn't work because the Analysis Type was set to 3D.nAnother problem is you have selected No Separation contact to connect the half adhesive to the flexible and rigid adherends. You should have used Bonded Contact.nI made those repairs, but your geometry is too large to run in the Student license. The attached file has 127k nodes, while the student license is 32k nodes. Just cut 3/4 of the length off the beam and you will make it. Also, you could make the rigid parts have behavior of Rigid, then they won't need to be meshed except on one edge. Replace the Fixed Support with a Remote Displacement .nn
Viewing 5 reply threads
  • You must be logged in to reply to this topic.