Ansys Products

Ansys Products

Discuss installation & licensing of our Ansys Teaching and Research products

Bolt pretension and contacts

    • Saketh Bharadwaj Kopparthy


      I have a questions related to 2 topics.
      1. geometry selection for bolt pretension
      2. deleting the contacts

      Geometry selection for bolt pretension: What is the difference between selecting a surface and selecting a 3D body for applying bolt pretension? In my model, when I try to apply pretension on the screw shank surface, the selection is not accepted. I had to create a new coordinate system for the "shank surface" and apply pretension on the 3D screw body with newly created coordinate system.

      The screw here is a an anchor screw. So the shank surface has been split to two parts. The bottom part was later considered as bonded contact and the remaning screw shank just stays inside the concrete block and the coordinate system was created for this remaining screw shank. Is this the reason for me to not able to select the surface?

      Deleting the contacts: In continuation to setup explained above, the contact between remaining screw shank (part that is not bonded) and the surrounding concrete is getting tricky to handle. Since it an anchor screw, the contact area is assumed to be minimal with small friction coefficient. If I consider frictional contact and run the simulation, I have convergence problems. The case runs for around 2hrs on my laptop (8GB RAM, i5-4th gen) and the convergence is never reached. But if I ignore this contact by deleting it altogether (screw and concrete are still touching each other but contact is not modelled) the case converges. 

      Can someone tell if this is the correct approach?

      Thanks in advance.

    • mjmiddle
      Ansys Employee


      Assuming you are selecting the face of a solid and not a surface body, the difference is that for any geometry other than a solid (face/beam edge) it will detect a direction for the bolt and split at the middle of the entity while the APDL solution runs. For a face selection, the face needs to be cylindrical type, so that it can detect an axial direction for the bolt. You may have a spline type face, rather than cylindrical if it doesn’t accept the selection. A cylindrical face type will show that in the “Selection Information” and at the bottom when you select it:

      If you select a body(ies) it can’t automatically determine the direction for the bolt. That is why you need to select a coordinate system when selecting a body. It also uses the origin as the split location.

      Convergence problems are an entirely different issue, and contact problems are common. But many issues can cause convergence problems, and it will be hard to diagnose such a thing in a forum without the workbench project. Is it transient or static structural? Transient can have chattering of the contact where it bounces between contact and no-contact and so uses small time step which takes a long time to run, and has convergence problems. Static analysis often has rigid body motion issue if contact is not recognized. If it converges even one subtep, you can look at a partial solution to see what’s happening. Try a very small initial time step to get a first substep convergence. If you can’t get a first subtep convergence, put a non-zero integer Newton Rhapson residual value (such as last 3 iteration residuals) in the “Solution Information” to see where problems are worst. You can also insert contact tracker under the “Solution Information” to look at number of nodes contacting and many other items. Try inserting a “Contact tool” under the Connections branch, Evaluate the “Initial information” to see if the contact is initially touching. Setting a lower contact normal stiffness factor, such as 0.1 or 0.01 often helps convergence, except where press-fit is being modeled. And try setting the “update stiffness” to “each iteratiion” or the aggressive setting. You may need to increase the pinball radius. The “adjust to touch” on the contact can help a lot for convergence if contact are meant to be in initial contact. Convergence problems can be caused by anything in the model. Geometry problems such as initial penetration of the bolt and hole body will be an issue. Mesh that is too coarse to reasonably model the curvature of the bolt is a problem too, maybe a minimum of 6 elements around the bolt shank curvature. Contacts work best with similar mesh size on contact and target sides also. Materials can also cause convergence problems although I would guess that is not the issue here.


    • Saketh Bharadwaj Kopparthy

      Hello @mjmiddle

      Thank you very much for the detailed information. I have some follow up questions. Below is further information about my case and I finally listed my questions in the end. Thanks in advance for your patience.

      I created the geometry in Spaceclaim and imported it for the analysis. You are correct. The surface selection shows "face" instead of "Cylinder". How do I fix this? And is it logical to expect that the results will not differ by large extent after changing this. The screw geometry was just created using "pull" command in space claim. I do not understand why it takes as surface instead of cylinder.

      I am doing a static structural analysis. I am trying to model stresses in screws, concrete block and deformation in rectangular pipe as shown in below image. 

      A concrete block with dimensions 400mm*400mm*150mm is the base. On top of this concrete block, a steel flange of thickness 20mm is placed. A rectangular pipe is placed on top of the steel flange. The steel flange is attached to concrete block using M12 Anchor screws. 20kN force is applied on patch surface of the rectangular pipe. The displacement of a point on the rectangular pipe at distance of 110mm from the steel flange is to be validated against the experiments.

      1. Frictional contact between concrete and steel flange 
      2. Frcitional contact between steel flange and bottom face of screw head
      3. No contact between screw shank and steel flange since the hole diameter is atleast 1mm bigger than the shank diameter
      4. Below is the image of anchor screw. The length of shank inside the concrete is 80mm. In real time, only the black part is in contact. So the surface of screw shank and the hole in concrete were split and the bottom 10mm was assigned as bonded contact (i.e., a simplified model)

      5. Remaining screw shank inside the concrete block (70mm) can be assumed as frictionless contact or frictional contact with small friction coefficient of 0.1.
      6. Bonded contact between steel flange and rectangular pipe.

      Boundary conditions:
      1. Bottom surface and sides of concrete block are fixed support
      2. A ramped load of 20kN force is applied in 11 steps on a surface as shown in the picture.

      3. Bolt pretension of 5kN on each bolt during first step and stays locked for all further steps

      Like you mentioned, I am already using the contact tool. The gap in contact tool show gap between concrete and the steel flange. But I see that this originates from the mesh in the contact region but not directly from the geometry itself. Here is the picture.

      I just ignored it proceeded further. The convergence was not reached and the newton raphson residuals showed some problems in the contact regions. So instead of modelling the contact between screw shank and concrete (point number 5 in the contacts list) I suppressed the contact and run the simulation. If I understand correctly, I am just not modelling the contact (assumption in point number 5). All other contact settings that you suggested were left default.

      In the Non-linear controls, the minimum reference value was changed to 5E-2 . The solution converged after 2 hours with this message "The time for solution exceeded 1 hour. A High Performance Computing (HPC) license will reduce your solution time. Consider using an HPC license or purchasing an HPC license from your Ansys Representative." The result is achieved and it is within expected range. 1mm in experiment and 0.968mm in simulation. But when I double the load, 40kN instead of 20kN, the displacment at point of interest is also doubled which does not match with the experiments. 12mm in experiment and 2mm in simulation. In experiments, the deformation is in plastic region but in simulation it is still in elastic region.

      So my questions are:
      1. How do I fix cylindrical face problem in the geometry? And is it logical to expect that the results will not differ by large extent?
      2. Is my assumption of completely suppressing the contact between screw shank and concrete is correct?
      3. Is there a particular way to model the plastic deformation or what am I missing in modelling this?

      If you need, I would be happy to share the archive file of the simulation case. This case was setup in ANSYS student version 23.


    • mjmiddle
      Ansys Employee
      1. In SpaceClaim, you probably pulled a curve/edge that was not circular, so the pulled surface was not cylindrical. You probably imported the model, or maybe the curve/edge you pulled was from a bolt thread that was not circular. You can draw a circle in sketch mode over the circle you intend to pull to a cylinder, or use "Repair > Simplify" to turn the near-cylindrical shape to actual cylinder defintion.
      2. I think you probably don't need the side contacts on the bolts to the concrete if the model is behaving as most real world models would when a plate is bolted tightly to concrete. These are usually bolted tight enough that the plate would not slide when forces occur, but only you know if that is something that you really think happens in the real model (or test show it). If the bolt pretension is not enough relative to the side force as a result of friction under the bolt head and the plate/concrete friction force, then there may be some shifting where bolt shank comes into contact with concrete hole.
      3. It's possible #2 above contributes a little to the total deformation at the 110mm point, but I would think material properties for transitioning to plastic deformation is most responsible. Have you defined a plastic (bilinear or multilinear) material property in the Engineering data? Have you turned on "Large deflection" in the Analysis Settings?"
    • mjmiddle
      Ansys Employee

      You should not need to raise the force convergence tolerance in this model. Make sure to use auto time stepping, and specify a smaller initial time step, maybe a smaller minimum time step too.

    • Saketh Bharadwaj Kopparthy

      1 I just noticed that I used pulled command for the rectangular bodies and for screws I used rotate command on the contour. I think this the reason for modeller to not recognise the surface as Cylindrical. I will change it.
      2. I agree with you. The plate is tightly bolted to concrete and the displacement of steel plate (considered at one corner) is only 0.23mm in experiment which suggests that the movement is tiny. But in simulation I got 0.8mm of displacement. I will check the friction and pre-tension values once again. 

      3. There are some videos on youtube posted in official ansys channel explaining the theory and model setup for accommodating plastic behaviour. I am going through further information available. I will get back to this thread and post further questions if I have any.

      Information you gave me is gold and I highly appreciate your help.

      Thank you.

Viewing 5 reply threads
  • You must be logged in to reply to this topic.