Contact formulation for beam with bolted joints, using shell elements

  • 203 Views
  • Last Post 28 April 2020
Aren posted this 26 April 2020

Hi all, newcomer to the forums here with a bolt joining problem. 

 

I am trying to model a beam, split across the middle, joined with a top and bottom plate and 4 bolts through it. Geometry as seen in figure 1. 



Figure 1: Full Geometry of Experiment

Figure 1 : Full geometry of experimental model

I've made a 3D and 2D model and I am now making a model which models the beam and plates with shell elements and the bolts as full 3D. However, I've ran into some issues with establishing contact. 

I would like to establish a frictional/frictionless contact between the bolt and the holes of the middle beams (the bolts are bonded to the top and bottom clamps and that works just fine) and also I would like to establish a frictional/frictionless contact between the end faces of the beams. 

 

Figure 2: Bonded connection with top and bottom of bolts

Figure 2: Bonded connection for top and bottom of bolts with top and bottom clamps respectively

Figure 3: Frictionless connection of mid-bolts to beam halves

Figure 3: Frictionless connection of mid-bolts to beam halves

Figure 4: Frictionless connection between plate halves

Figure 4: Frictionless contact between beam halves


My connections so far are pictured in figures 2-4 and the resulting issues displacement in a modal analysis is pictured in figure 5 and 6. 

Figure 5: Clipping issue of bolt holes not interacting with bolts

Figure 5: Bolts not interacting with bolt holes

Figure 6: Beam halves clipping through each other

Figure 6: Beam halves clipping through each other

As seen, the problem is any other contact aside from "Bonded" between the bolts and the two beam halves results in invalid results (see figure 5) additionally the two beam halves clip through each other (figure 6). 

How would I go about establishing effective frictionless contact between bolts - bolt holes and between the ends of the beams, in such a way it also allows pretension further down the line? Bearing in mind the beams are made of shells and are not solid. 

Attached is my project archive, SGBJM Modal contains the model as seen above. 

Order By: Standard | Newest | Votes
Aren posted this 27 April 2020

UPDATE:

I've resolved the frictionless contact between solid bolts and surface edges by using an offset.

 

Still having trouble with the two end to end surface bodies not contacting.

peteroznewman posted this 27 April 2020

Let me thank you for a very clear and detailed post!  I wish everyone would put in that kind of effort.

In Figure 3, you had a clearance between the bolt shaft and the hole edge, which you resolved by using an offset.
Instead of contact between the body of the bolt and the face of the beam, I would recommend contact between the face of the bolt and the edge of the hole.

Offset has worked because the contact is probably now closed, where before it was open.  If the load on the beams was axial force along the length of the beams, a slightly more accurate model would take up the clearance in CAD before running the solution. That means the bolt shaft is tangent to one side of the hole in the beam and tangent to the opposite side of the hole in the plate. As you do this for all bolts, the plates will move over by the diametral clearance and one beam will move over by twice that. Now all the contacts will be closed without needing an offset.  The improvement in accuracy is the contact zone of the bolt to the hole edge will be smaller and make the stress a little higher. If it is an in-plane side load, then the bolts on the tension side of the beam go one way and the bolts on the compression side of the beam go the other way.

In Figure 4, try selecting the edges of the midsurface of the beams, rather than the faces. I don't know that this will work for sure. Another approach is to increase the gap between the beams so there is always a gap and there is never any contact. The load is always going through the bolts.

Final comment is to use Friction between the plates and the beams and add a Bolt Pretension load to the four bolts.  Change Analysis Settings to use a 2 step solution. In step 1, the bolt pretension force is applied and the load on the beam is 0.  In step 2, the bolt changes to Lock and the load on the beam is applied.  In this way, you don't need any contact between the bolt shaft and the hole. The loads are completely supported by the friction force of the plates to the beams.

Aren posted this 27 April 2020

peteroznewman - thank you for the reply! 

I have changed the contacts to how you have suggested, it has worked for the bolt - bolt hole contact however, the left beam-right beam faces still pass through each other unfortunately. 

Also I have ran into another issue while using the model in a transient structural analysis:

I have applied a pretension to the bolts, however the bolts do not seem to be transferring the tension to the surfaces they are bonded to. Figure 1 shows the pretension formulation, figure 2 shows the contact of bolt to surface and figure 3 shows the equivalent stress results

Figure 1: Pretension formulation

Figure 2: Contact formulation, bonded bolt edge to surface hole edge

Figure 3: Results during a tap test represented in transient structural

 

The tension doesn't seem to be passed on to the surfaces, which is a critical part of this model, but I can't think how to change the contacts to get them to behave. 

The point of the project is to study the non-linear effects of the joint beam in free vibration for different tensions of bolts, so being able to effectively apply bolt tension and have the correct forces transfer to the top and bottom plate (clamping them tighter against the middle beam and increasing the stiffness of the system) is crucial. 

peteroznewman posted this 27 April 2020

I recommend a hybrid model.  Take each solid beam and cut it about 1 plate width away from the edge of the plate. Keep the plates and beam segments touching the plates as solids, create midsurfaces for the long ends of each beam.  Use bonded contact between the edge of the beam midsurface and the cut face of the beam.  Now the plate to beam bolted joint is all solid.  Use four elements through the thickness (minimum of two elements if you must reduce node count) to get good resolution of the through thickness behavior.

Does your bolt look like a hand held dumbell weight?  Two big cylinders for the head and nut and one small cylinder for the shank? If so, don't apply bolt pretension to the Body of the bolt, apply it to the face of the shank. Make sure there are at least two elements along the bolt shank, otherwise the bolt pretension can't be properly applied. It is better if there are four elements along the bolt shank.

Since you are studying vibration, can you assume that there is never a gross slip of the joint where the bolt shank makes contact with the edge of the hole? That way you don't care about the contact between the ends of the beams or the bolt shanks to the hole cylinders.

I updated my previous post while you were online, so you might reread it in case you missed the update.

Aren posted this 27 April 2020

Thank you for the update - the first post was from a Modal analysis, which was purely to get a rough idea for the mode shapes, which is why I wasn't modelling friction or bolt pretension seeing as it is a linear analysis. 

I'd ideally like to make this model work, modelling both plates and beams as surfaces, as I am trying to pursue a similar model to P.J.Gray and C.T. McCarthy's Global Bolted Joint Model. In the model (pictured figure 1 below) both beams are modelled as surfaces, the bolts are modelled as beam elements with a rigid surface, my one modification to the model is to use a full solid 3D model for the bolt, but omit modelling the head, nut and washers. 

Figure 1: P.J. Gray and C.T. McCarthy Global Bolted Joint Model 

My aim is to use this model to compare to a full 3D model and a 2D model and discuss the differences, which is why I'm so adamant on using this particular type of model. 

To address your other questions:

  • I have applied the bolt pretension along the face of the shank, with 2 elements along it but I'll increase to 4
  • I cannot assume a non-gross slip, during my experiment I tested bolt torques from 5Nm to 0.02Nm, effectively a loose bolt, where the bolt shank would be contacting the hole edge, I'd ideally like to represent this with my model. 

 

(Figure 1 from "A global bolted joint model for finite element analysis of load distributions in multi-bolt composite joints" by P.J. Gray, C.T. McCarthy)

peteroznewman posted this 27 April 2020

You can certainly have the model be just shell and beam elements.  ANSYS can create a remote point at the center of the hole in the plate. It could be scoped to the hole edge or a small annular face. The behavior of the remote point can be set to Rigid. Create a line body in SpaceClaim or DesignModeler from the center of the hole in the top plate to  the center of the hole in the bottom plate. That line body can be meshed with beam elements and the end points can be supported by the remote points. It is feasible to have contact between the line body and the edge of the hole in the midsurface body representing the long beams.  With beam elements, you only need two elements along the length of the shank in order to assign Bolt Pretension load.

The only item I am not sure about is the problem you show in Figure 6, which is the reason why I recommended solid elements for the joint.

Another idea is to put a spring element between the vertex of each beam corner to cross the gap between the vertices. Use a Command Object to add some APDL commands to convert this spring element from the default COMBIN14 to a COMBIN40 which has a GAP capability.  You can assign a spring rate to the COMBIN40 that matches the stiffness of the corner of that beam.  Read this discussion for more information.

Aren posted this 27 April 2020

Modelling the problem as shell and beam elements would be ideal, the only reason I'm using solid bolts in my model is because previously I couldn't get the contacts to work for a shell and beam model. 

Could you please go into more detail on how I would go about that? Especially:

  • How would I create the remote point and set it to Rigid, would that be in SpaceClaim or in the Model?
  • How would I go about meshing a line body with beam elements? I have no experience in selecting a type of element for a body. 
  • How would I establish the contact between the beam element and edge of the hole? Would that require using an offset and an appropriate pinball radius or some other means?

Apologies, I realise that is a lot to answer, thank you for all the help up till now!

As for the other problem, from figure 6, it is a secondary issue. It would be good to have it work properly but my scope doesn't require looking at side loads, being able to model vibration normal to the beam surface accurately, robustly and efficiently is good enough for this model. But I will certainly give it a go, it's just not a priority. 

peteroznewman posted this 28 April 2020

I will make a video on how to create a bolted joint using shell elements to go along with the two videos I have already made. I can use the archive you attached in an earlier post.

Aren posted this 28 April 2020

That would be much appreciated, I'll also have a look over your current videos.

For myself, I need to be able to have this model working before the weekend for a report I'm writing, but if the video would be available tomorrow that would give me plenty of time. Feel free to make use of the archive files, it's not a confidential component in any way.

Also thank you for your help again, I've been working on 3D solid, 2D and shell models for this project for over a month and I thought I was almost done, before my shell model refused to cooperate.

peteroznewman posted this 28 April 2020

I can't open your Archive because you used a Module I don't have on this Student license.

Please clear the mesh and see if that archive allows the model to open.

As a backup, also export the geometry.
If you open it in SpaceClaim, you can save the .scdoc file and attach just the geometry.

Aren posted this 28 April 2020

The ICEM mesh is an old mesh I was trying but ultimately ended up not using. I've since deleted the component from the files, here is the new archive hopefully it'll work now. 

Attached Files

peteroznewman posted this 28 April 2020

Here is the new video. Thanks for the geometry.

Close