Good Evening, I am trying to model an element composed of two parts linked by a bolt, where the bolt is the means of porpagation of the force among the two pieces, I am problably wrong in designing the model since the solver stops with no convergence at the first iteration. Since I am modelling these kind of parts ( see model in the link) is it possbile to have force values on the bolt in the world reference system or, even better, avoid to model bolts by adding “linkage” constraints on the model main surfaces without modelling a bolt. I am asking anyone help to figure out the last two aforementioned issues I am facing.
Model : https://wetransfer.com/downloads/b3c3f7ac6d887010c63cc27dbc5e8cd120230529203620/3b2505c46bb6a069dde589eac27c4d1920230529203634/a4b6d1
Thank you.
Best Regards.
Hello @Agazzotti.
When I try to run a frequency analysis to check for rigid body modes in your model, I get the following error:
*ERROR in e_c3d: nonpositive jacobian determinant
In too many elements. Check the image below.
Your model is pretty complicated. Too many contact interactions and too many solid elements… Consider simplifying the bolts to beams or even springs with proper coefficients to model axial and transverse response then connect the spring to the hole in the parts using coupling. I show a simple example below. The lateral L plates could be modeled as shells - with your current mesh density, you will probably not be able to properly simulate the bending that will occur under your actual loading. Contact is very tricky, I would avoid it if possible. I suppose the brick in your model is not the critical part, so consider using a coarse mesh there, or even substitute it for a RBE.
Best regards,
Lucas.
Of course, you can model the bolts as solids but you have to be very careful with connections. Use tie constraints or tied contact wherever nonlinear contact is not needed to avoid non-convergence (at the beginning you can tie everything to make sure that the rest of the model definiton is correct). Disable adjustment for selected pairs if you encounter issues with element distortion (like negative jacobian errors). But first you should refine the mesh (especially in the thickness direction). Also, avoid applying boundary conditions to surfaces involved in contact:
P.S. The analysis works if I just disable adjustment for contact between the bolt shank and the box. However, the aforementioned improvements should still be made.
Thank you I managed to make the model converge. I would also like to know where can I read contact forces(Fx,Fy, Fz) between the hole and the bolt since I need to verify
those values are within a range(?). I have a further curiosity for what concerns the ways I can model a bolt contact, is it possibile to add tie constraints to the corresponding hole faces( one belonging to one part and one beloging to the other part) whitout modelling the bolt itself(?), morover, I have seen on calulix that it seems possbile to model bolt contatct through a parametric interface (like the one in the attached file), can prepomax do something similar?
You can request the CF (total contact force) variable as history output.
A simplified approach to bolt modeling involves a beam element connected to the surfaces of joined parts via coupling/MPC constraint. It’s not supported in PrePoMax at the moment but you could definie it manually or just ignore the bolt and connect the cylindrical faces using rigid body constraint.