cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Simulating a Thread with a constraint

SOLVED
Highlighted
Newbie

Simulating a Thread with a constraint

Hi,

I am doing a simple pressure analysis on a pipe that is threaded on both ends. In the drawing, the thread is not modelled, it is only shown as a block. For my analysis, I am not considering the thread as a failure point, only as a constraint.

I am fully constraining the part on the surface of the "block" of threads with a surface region that has no displacement in any direction. I am getting a stress concentration on the edge of the surface region.

I have two questions:

1. Is it possible to exclude the edge of the surface region in the results so I can ignore the constraint? It holds the part fine, but I don't want to show this area as a failure. Currently I am ignoring any high stress in this area, but I would rather not have it show up

2. Is there a better way to simulate threads in a simple fashion so that stress concentrations do not appear? I do not want to model the threads to apply this constraint, but I believe the issue is that I am limiting axial movment on a surface. Because the surface has no shoulder, it is difficult to model and singularities will happen.

The picture below shows the stress concentrations I'm talking about. Any help would be appreciated in constraining my part to get more accurate results. Thank you.

-Andrew

Stress concentrations.PNG

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Simulating a Thread with a constraint

I know the way I am fully constraining it right now is not the best way, but I was not sure how else to simulate threads holding the part in place on both ends.

The best way to tackle this problem is to think of the idealized kinematics of the design assuming there is no friction. A threaded mechanical joint prevents on-axis translation, while everything else is technically free to move.The problem is that, for a finite element model, you need to constrain the system to prevent rigid body motion. This is where using springs and links or symmetry comes into place.

When I say that I'm ignoring the high stress areas, I mean that if I get a high stress concentration, I will ignore those results. They still happen, but when I present my results I classify them as outliers.

That's OK, just be sure that the stress concentration is due to modeling conditions and that you use an Isolate for Exclusion mesh control with some insulating elements. Singular elements can pollute the stress results you want to simulate if they're not handled properly.

I am performing the FEA to prove hand (and by hand I mean excel) burst/collapse formulas. The hand calculations are not able to account for cutouts, and this is where the FEA can provide more accurate information about whether a part can withstand a pressure or not.

Collapse or burst? Are we talking about a mechanical instability here (like buckling)?

Also keep in mind how load transmission can effect the results near the threads. Again, whether or not this is a problem depends on the design and where you want results. The image below shows two 3D models with and without threads and using a weighted-link with a zero-length spring, and a 2D axisymmetric model with contact.

Comparison.png

View solution in original post

5 REPLIES 5

Re: Simulating a Thread with a constraint

For my analysis, I am not considering the thread as a failure point, only as a constraint. I am fully constraining the part on the surface of the "block" of threads with a surface region that has no displacement in any direction.

It's hard to say if this is OK; it depends on what results you're after and at what locations. You also need to consider if the constraint will add stiffness to your model that isn't present in the real system. Can you provide more information?

1. Is it possible to exclude the edge of the surface region in the results so I can ignore the constraint? It holds the part fine, but I don't want to show this area as a failure. Currently I am ignoring any high stress in this area, but I would rather not have it show up

When you say you're ignoring the high-stress areas, do you mean you're using an Isolate for Exclusion mesh control? Anyway, you can't exclude the singular elements from the post-processor view. The only work around would be to create a volume region that contains all the singular elements, and then in the post-processor define what to show based off of volumes and select everything by the singular volumes. However, you'll then have volume regions missing from your post-processor's view.

2. Is there a better way to simulate threads in a simple fashion so that stress concentrations do not appear? I do not want to model the threads to apply this constraint, but I believe the issue is that I am limiting axial movment on a surface. Because the surface has no shoulder, it is difficult to model and singularities will happen.

You could replace the constraint with weighted-link, a zero-length spring element, and a point constraint; this will resolve the singularities that are currently present in your model. You'll need to define a stiffness matrix for the zero-length spring element, which you'll want to give a large stiffness value (but not too large; keep is 6 or so orders of magnitude greater than the stiffness of your material). You can also define your spring's stiffness matrix such that you will limit axial movement, but allow radial and angular movement.

Also, depending on your design, you might be able to take advantage of symmetry. It looks like you're using half-symmetry (based on what I see); if the geometry and loads are right, you could very well use 3D axisymmetry or even 2D axisymmetry.

Re: Simulating a Thread with a constraint

Andrew,

If you constrain the thread you will overstiffen and the rotation about theta (cylindrical csys z-axis along the cylinder axis) will reduce.

This will push the high stresses along to somewhere else; more work has to be done in the structure elsewhere. i.e. 'bulging' under pressure should begin along the thread otherwise the answers are wrong and you will find that the stresses in any undercut are even bigger.

Also, if the threaded cap is loaded there will be a bursting force due to the angle of the thread. This radial load cannot be ignored. (butress threads attempt to mitigate this issue).

Weighted links can help but do not cause the bursting load. You could apply an estimate of the radial load I suppose.

For speed there are compromises each with criticisms. We tend to model 3 turns of thread at start-middle-end, simple triangles, keep the cap simple, use contact, assume pressure leaks into the first 2 turns.

Regards

Charles

Re: Simulating a Thread with a constraint

Shaun,

Thank you for the response.

As for looking at the part and ignoring the thread as a failure point, my company uses a separate thread calculator to determine when the thread would fail. This is why I am not considering it as a failure point. I will also be the first to admit that I am not the best with FEA and I try and keep things as simple as possible. If things get complicated, I do not trust myself to get accurate results. The part shown here is more or less a basic cylinder. As far as my constraint adding stiffness to the part elsewhere, I agree, that is something that I want to avoid. I know the way I am fully constraining it right now is not the best way, but I was not sure how else to simulate threads holding the part in place on both ends.

When I say that I'm ignoring the high stress areas, I mean that if I get a high stress concentration, I will ignore those results. They still happen, but when I present my results I classify them as outliers. I know this is not the failure point that I am analyzing, I am looking at the thin wall sections of the part. I am performing the FEA to prove hand (and by hand I mean excel) burst/collapse formulas. The hand calculations are not able to account for cutouts, and this is where the FEA can provide more accurate information about whether a part can withstand a pressure or not. Again, I am trying to keep it as simple as possible. I would rather not remove entire volume regions from the end result picture.

Because my model is a cylinder, i can use symmetry. I am currently using half symmetry.

I will experiment with weighted links to see if i can remove the singularities. I will also experiment with having only axial constrained and allowing radial/theta movement. Thanks for the help.

-Andrew

Re: Simulating a Thread with a constraint

I know the way I am fully constraining it right now is not the best way, but I was not sure how else to simulate threads holding the part in place on both ends.

The best way to tackle this problem is to think of the idealized kinematics of the design assuming there is no friction. A threaded mechanical joint prevents on-axis translation, while everything else is technically free to move.The problem is that, for a finite element model, you need to constrain the system to prevent rigid body motion. This is where using springs and links or symmetry comes into place.

When I say that I'm ignoring the high stress areas, I mean that if I get a high stress concentration, I will ignore those results. They still happen, but when I present my results I classify them as outliers.

That's OK, just be sure that the stress concentration is due to modeling conditions and that you use an Isolate for Exclusion mesh control with some insulating elements. Singular elements can pollute the stress results you want to simulate if they're not handled properly.

I am performing the FEA to prove hand (and by hand I mean excel) burst/collapse formulas. The hand calculations are not able to account for cutouts, and this is where the FEA can provide more accurate information about whether a part can withstand a pressure or not.

Collapse or burst? Are we talking about a mechanical instability here (like buckling)?

Also keep in mind how load transmission can effect the results near the threads. Again, whether or not this is a problem depends on the design and where you want results. The image below shows two 3D models with and without threads and using a weighted-link with a zero-length spring, and a 2D axisymmetric model with contact.

Comparison.png

View solution in original post

Re: Simulating a Thread with a constraint

Thank you, this was helpful.

Your picture simulation is exactly what I'm looking for. A weighted link seems to be the best option.

To answer a few of your questions, no I am not considering buckling. We do the hand calcs for this to see if its close. Most of the components I work with are short enough where this is not an issue. If it is close with the hand calculations, we then need to confirm with FEA.

Most of the components I work with have burst as the failure mode, but his specific instance collapse was also under question.

Going forward I will plan on using exclusion to prevent singularities from altering my results and simulating threads with weighted links. Thanks for the help!

-Andrew

Announcements