ANSYS Bolted Connection Questions

[FullMetalBracket]

Hi all,

I've recently begun a new job doing stress analysis using ANSYS. I'm new to ANSYS and relatively new to the industry (a little over a year out of school). I have some questions regarding simulating bolted connections in ANSYS.

We are analyzing rather large structures composed of thousands of individual parts. Wether analyzing the dynamic response of the entire structure as a whole or doing a static analysis of a smaller sub-structure, almost every part is modeled using 2d shell elements in order to simplify the mesh and reduce computing time.

On top of this, bolted connections are simulated by one of two methods:

1. Adjacent nodes around circumference of holes are coupled between mating parts.

2. Holes are eliminated altogether and keypoints placed at the former hole centers are coupled.

This leads to innaccuracy and singularities in the region around the holes. Nodal forces are then extracted at each hole and used to calculate axial and shear stresses in the bolts. This leads me to ask several questions:

1. Does this method of simplification followed by 'hand' calculation lead to significant innaccuracies that I should be concerned about?

2. Using the first method to simulate the connection and summing the forces/moments about the hole center leads to Fx,Fy,Fz,Mx,My,Mz outputs (obviously). Assuming x to be the axial direction, Fx is used to calculate axial stress and Fy and Fz are used for shear stress. The moments are generally ignored. Does a large My or Mz value indicate that I should be concerned about prying forces in the bolts? I do not have a reference that indicates when prying forces are important and how to calculate them, nor was this ever covered in school.

Sorry for the long-winded question, hopefully some of you can provide some guidance and help me attain peace-of-mind.

Thank you.

 

[PriamEngineering]

Modelling multi bolted connections in detail can be extremely tedious. If you use element 179 in Ansys you till be able to extract more accurate bolt tensile loads…. but little else.
When faced with a big problem like yours I would do as you are currently doing. I usually delete the holes and then place a node at the centre of the filled in section. I extract all reactions from this point and use the rules of thumb that exist for tensile stress limits and shear loads.

If you are concerned about prying loads leading to one sided opening of the joint you can always create a submodel of the worst affected bolt in detail using solid geometry. I don’t normally do this if my rules of thumb point to no chance of failure.

For refrence invest in Bickfords ‘an introduction to the design and behaviour of bolted joints’ and VDI2230 (German standard)


Good luck

http://www.priamengineering.co.uk

 

[FullMetalBracket]

Thanks for the response!

Let me remove the focus from prying forces and instead focus on the accuracy of the axial/shear forces I'm extracting. I'll explain my concern using an example:

An angle bracket is modeled using 2d shell elements. The shorter arm of the angle is 3" in height and bolted to a rigid wall using 2 symmetrically placed holes (bolt axis = x-direction). The 8 nodes at each hole circumference are constrained in all DOF. No other constraints are applied along this face (no contact between the angle and the wall). The longer arm of the angle extends 10 inches out from the wall. A load of 500 lbf downwards (-y direction) is distributed along the nodes at the tip of the angle. Upon solution of the problem ansys yields:

Fx = -2.35
Fy = -250.31
Fx = -238.9376
Mx = 98.175
My = -68.621
Mz = -2505.041

If I blindly follow the process of ignoring the moment outputs and look only at the forces extracted, I would conclude that the tensile load in the bolt due to the applied force is only 2.35 lbs, when i know it should be MUCH larger. Obviously in this case, modeling the bolted connections in this way is not accurate. If I add a second set of holes under the original set, Fx gets much higher but I still have a significant Mz component.

How do I make up for this innacuracy without compromising the simplicity of the model? Is it possible? Any comments/suggestions are greatly appreciated!

 

[PriamEngineering]

If I have translated your problem correctly, you have a symmetrical joint and a symmetrical load, however you seem to have shear reactions in 2 planes. You have to understand why you are getting this before looking at anything else.

http://www.priamengineering.co.uk

 

[FullMetalBracket]

So sorry, I worded things wrong (or didn't explain at all...)! The forces/moments I gave are not the overall reaction sum of the system but the nodal forces applied on the nodes of only ONE of the holes, all summed about the hole center.

The opposing hole as an equal and opposite shear reaction in the Z direction. My apologies for the error, I hope this clarifies things.

 

[PriamEngineering]

Your confusion might be due to the fact that the bolts in your problem lie on the save plane (vertical height). Have a look at what happens when you move the position even slightly.
/prep7
et,1,93
r,1,1
mp,ex,1,30e6
mp,nuxy,1,0.3
k
k,2,,-1.5
k,3,,-3
k,4,10
k,5,,,-1.5
k,6,,,-3.5
k,7,,,-5
l,1,2
l,2,3
l,1,4
l,1,5
l,5,6
l,6,7
adrag,1,2,3,,,,4,5,6
amesh,all
nsel,s,loc,x,10
*get,nc,node,,count
f=500
f,all,fy,-f/nc
alls
/solu
d,31,all,0
d,150,all,0
solve
/post1
prrsol,

http://www.priamengineering.co.uk

 

[FullMetalBracket]

Thanks for taking the time to respond again and prepare the example, Priam.

Ofcourse I understand that two symmetrical holes on the same vertical plane relative to the downward applied force can't have an axial component (Fx=-2.35 is due to the mesh being slightly asymmetric). My point was that if extracting axial force components to calculate bolt tensile stress does not apply whatsoever in the example I gave, how can I trust to apply it to other situations?

Lets take the example you gave above. The results give one connection seeing a tensile force of 906.72 and the other seeing an opposing force of -906.72. This seems highly unrealistic. If you made your angle wider to space the holes out even more, you'd ofcourse get a similar result (equal and opposite tensile forces). In actual fact, logic tells us that both bolts will be subjected to tensile forces due to this loading. Once again, our constraints are providing us with unrealistic results. Without modeling the interection between the bolted face of the angle and the underlying surface, we are getting highly unrealistic and not necessarily conservative results.

I can't conclude that simply because I'm getting a significant axial reaction at one of the points that the forces extracted are accurate when applied to the real situation. On top of all this, depending how I constrain the holes (constrain the nodes at the hole circumference or fill the hole in and constrain the center node) I get DRASTICALLY different axial forces. I'm starting to wonder if modeling connections in this simplified manner can be trusted at all.

What are your thoughts?

 

[PriamEngineering]

Obviously in the example that I gave the boundary conditions are unrealistic. The bracket can rotate. If you constrain the nodes at the bottom of the bracket in the model in the bolt axial direction you will see a more realistic result.
As I said in my first reply… bolted joint analysis can be tedious. If you are concerned about tensile loads (as opposed to shear) then you might be best performing two analysis types. One for tensile loading (fill solid model) and one for shear loading (simplified shell model)

regards

http://www.priamengineering.co.uk