AnsweredAssumed Answered

How to Simulate a Threaded Joint in Shear?

Question asked by John Willett on Apr 23, 2015
Latest reply on Apr 24, 2015 by Jared Conway

Like • Show 0 Likes0
Comment • 12

I have an application for a threaded rod separating two plates that are sheared relative to one another. The image below shows a test jig in which the threaded rod is simulated by a smooth rod "bonded" (as opposed actually threaded) into equal-diameter holes in the two blocks:

Here's a blow-up (for a particular mesh-control density) of the bottom joint, where the maximum stress exceeds the 20,000 psi yield strength of the steel:

I observe that the high-stress coverage decreases in area and increases in magnitude, apparently without limit, as mesh density is increased near the right-angle corner. I'm not trained as an engineer, but I understand that this behavior is typical of "re-entrant edges," where the theoretical stress can be unbounded. I have also modeled this configuration with fillets and observed that the stress converges nicely. Unfortunately my application does not permit a fillet or other stress-relieving feature around the actual joints.

So my questions are:

1) What is the most realistic way to simulated such a threaded joint?

2) How can one establish a practical failure criterion in order to choose bolt diameter, etc? -- John Willett

No one else has this question

Outcomes

12 Replies

Jim Riddell Apr 23, 2015 2:51 PM
Mark Correct
Correct Answer
First - I'd model the rod for such a study with the root diameter of the thread. That way it is more easily compared to a hand calculation.

Second - If your FEA shows stress higher than the yield value it just means that there would be some plastic (permanent) deformation expected in that area. If it goes over the UTS for the material then it would break IRL.

Failure criteria depend heavily on the application. How safe do you want it to be?
Like • Show 2 Likes2
Actions
- John Willett @ Jim Riddell on Apr 23, 2015 3:12 PM
  Mark Correct
  Correct Answer
  James -- Thanks for your prompt response.
  
  >>I'd model the rod for such a study with the root diameter of the thread.<<
  
  I actually used the so-called tensile area diameter -- only slightly larger than the root.
  
  >>Second - If your FEA shows stress higher than the yield value it just means that there would be some plastic (permanent) deformation expected in that area. If it goes over the UTS for the material then it would break IRL.<<
  
  I presume permanent deformation cannot be accepted, since one of these threaded joints must be adjustable. I don't know what the UTS means...
  
  My main quandary is, given the non-convergence of maximum stress in the simulation, do I have to assume that the part will deform and/or fail? (After all, screw joints of this type are commonly used.) Or is there a better way of modeling such a joint that gives a more realistic answer? -- John Willett
  Like • Show 0 Likes0
  Actions
Chris Michalski Apr 23, 2015 3:19 PM
Mark Correct
Correct Answer
In actuality you aren't in shear. The 2 cubes would have to be touching to shear the bolt, you have a bending load.
It may be worth trying a non-penetration contact between the bolts and blocks to allow them to separate like they truly would when the bolt begins to bend (the threads will prevent it from moving axially, but nothing will prevent it from the centerline shifting sideways as it bends).
(UTS that James mentioned is Ultimate Tensile Strength)
Like • Show 2 Likes2
Actions
- Jim Riddell @ Chris Michalski on Apr 23, 2015 3:29 PM
  Mark Correct
  Correct Answer
  I like @Chris Michalski 's idea but would restrain both ends axially so they couldn't 'pull out' of the nut/plate. He's also correct pointing out that you have bending going on here so, by rights, you have some tensile loading, bending and shear (due to the geometry of the threads). The tensile load area you describe is for an axial load only and is probably not appropriate in a shearing situation.
  Like • Show 2 Likes2
  Actions
  - John Willett @ Jim Riddell on Apr 23, 2015 9:02 PM
    Mark Correct
    Correct Answer
    Sounds like you're getting me closer to a realistic model.
    
    I've heard the no-penetration idea before (as Chris suggests), but I never understood how that accounted for thread engagement along the entire contact length. Indeed, no-penetration contact does reduce the maximum stress (see image below, noting the very different stress scale and the subsidence of the top end of the bolt), though I'm not completely sure why, since even in bonded contact the block can distort and allow the bolt axis to tilt a little.
    Maybe its because of eliminating the tensile part of the stress in the bolt? Maybe friction needs to be introduced to compensate for the vertical sliding of the bolt?
    
    Even with the ends of the "bolt" restrained flush with the outside faces of the blocks (as James suggests), say with roller/sliders, the bolt will still pull out somewhat from the inside faces of the blocks, which seems inconsistent with a full-length threaded joint. What am I missing here?
    
    A shrink fit might also be considered, with friction specified between the shrink-fitted faces, but what degree of interference should be used and what friction would be appropriate? I feel like I'm shooting in the dark here. I was hoping there was some standard practice for such joints... -- John Willett
    Like • Show 0 Likes0
    Actions
    - Mike Pogue @ John Willett on Apr 24, 2015 12:13 AM
      Mark Correct
      Correct Answer
      Hi John,
      
      You are asking some smart questions here. You will not be able to reproduce the stress state at the threaded interface using a finite element model, as you are observing. This would be a pretty sophisticated FEA project, and one that I would probably not try to tackle.
      
      The standard way to model a bolted joint is to model it as a bond or a spring (depending on the required detail), then to extract the resultant forces and conduct a bolted joint hand calculation from that. This doesn't help you, because this is not a bolted joint; this is something entirely new.
      
      I propose this analysis:
      
      1. Remove the blocks from your model
      2. Restrain the top and bottom of the bolt to its plane.
      3. Fix the bottom of the bolt.
      4. Apply your force to the top of the bolt.
      5. Extract the moment (which is the bending torque) from the reaction at the bottom fixture in inch*lbf.
      6. Assume the moment is reacted at the centroid of the thread shear area. You can calculate this analytically, but since you have SolidWorks, I would not do that. I would model a half an annulus with an ID of the minor diameter and an OD of the outer diameter and find the center of mass (see below)
      7. Divide the moment by the distance in inches from the center to the centroid. This gives you a tensile force in lbf.
      8. Calculate the thread shear area (http://www.engineersedge.com/thread_strength/thread_bolt_stress.htm ) for the internal and external threads. Assume that about 5 threads are engaged, regardless of actual thread engagement.
      9. Divide the tensile force from 7 by each of the areas from 8. This gives you stress in psi.
      10. Compare each stress from 9 to the yield stresses of the bolt and the blocks, respectively. You want the yield stress to be higher, obviously, probably by a factor of 2 or 3--to account for the fact that I made all of this up, but also to account for the fact that I wouldn't guess this analysis is accurate to better than about 50%.
      
      Note that in this analysis, it's conservative to use the nominal diameter of the bolt, because that increases the moment. Constraining the top surface to a plane is also conservative.
      Like • Show 1 Like1
      Actions
      - Mike Pogue @ Mike Pogue on Apr 24, 2015 2:19 AM
        Mark Correct
        Correct Answer
        Well, been thinking about this, and the above only accounts for the shear in the thread (it was a mistake to compare shear to yield stress, but I will fix it).
        
        You actually need to look at the von Mises stress, which means you need to account for the bearing stress. In fact, depending on the bolt size, the bearing stress may be dominant. To get the von Mises stress:
        
        1. Calculate the bearing area. This is half the thread engagement length times the nominal diameter times .875. The .875 is to account for the .125P lack of engagement at the root (see below). The area is in in^2. You can ignore the shape of the threads, because it is the projected area that matters in bearing.
        2. Take the moment from 5 in the FEA above and assume that it is reacted at the centroid of a triangle with a vertex at the center of the thread engagement. Then the force from this moment is 3*F*L/(4*Te), where L is the distance between blocks, F is the force on the whole system, And Te is the thread engagement length. This is the average force from the moment.
        3. Add the force from 2 to the force you place on the blocks to get the average force.
        4. Divide the force from 3 by the bearing area from 1 to get the average stress in psi.
        5. Assume the stress falls off linearly with thread engagement. Then the peak stress is 2x the average stress.
        6. Take the shear stress from my last post and call it tau. Take the max bearing stress from 5 and call it sigx. The von Mises stress is (from memory, please check this) sqrt(sigx^2 + 3*tau^2)
        
        Compare the von Mises to the yield stress., including an appropriate safety factor.
        
        I think the takeaway is that you need to test this.
        
        Edited
        Like • Show 1 Like1
        Actions
      - Mike Pogue @ Mike Pogue on Apr 24, 2015 1:33 AM
        Mark Correct
        Correct Answer
        Side note:
        To simulate this stress state in FEA without doing a dissertation on it, you'd probably create split faces 114 degrees wide on both the bolt and the tapped hole, front and back, and bond them together. This only works if they have the same Young's modulus, otherwise you introduce a discontinuity at the bond. You can remove the discontinuity by plotting the stress leading up to the bond and doing a linear extrapolation to the bond point. This result should be roughly comparable to the above hybrid FEA/ hand calc.
        Like • Show 1 Like1
        Actions
        John Willett @ Mike Pogue on Apr 24, 2015 8:34 AM
        Mark Correct
        Correct Answer
        Mike and James -- Thanks much for the deep analysis of my problem. I have visitors over the weekend so won't be able to seriously consider your thoughts until Sunday or Monday. Best Regards -- John Willett
        Like • Show 0 Likes0
        Actions
    - Jim Riddell @ John Willett on Apr 24, 2015 6:04 AM
      Mark Correct
      Correct Answer
      John, in actuality the ends of the threaded rod will not pull away from the outside planes of the plates. Due to the uneven loading along the axis, the bolt/rod will stretch within the threaded area unevenly. Bolt theory indicates that only the first three threads carry the bulk of a properly designed fastened connection in any case. (Visual inspection of any failure bears this out; they all break at the connection plane, no matter the loading condition.)
      
      As Mike suggests below, you are treading into dissertation waters here. This is no job for as simple an FEA software as SW.
      Like • Show 1 Like1
      Actions
      - Mike Pogue @ Jim Riddell on Apr 24, 2015 9:34 AM
        Mark Correct
        Correct Answer
        Yeah. He needs to test it.
        Like • Show 0 Likes0
        Actions
      - Jared Conway @ Jim Riddell on Apr 24, 2015 6:52 PM
        Mark Correct
        Correct Answer
        i wouldn't single out SW
        
        this is a hard virtual test period
        Like • Show 0 Likes0
        Actions

How to Simulate a Threaded Joint in Shear?

Outcomes

Related Content

Recommended Content