Modeling Bolts in Shear
Modeling Bolts in Shear
(OP)
The attached file contains a project with two simulations. The first models a bolt uses frictional contact exclusively to restrain its motion. The second uses the same geometry and replaces the contact that would be between the shaft of the bolt and the clearance hole with a revolute joint. The difference in the two simulations is significant. The first captures the fact that the two plates are going to slide with respect to each other and eventually begin applying a shearing load to the shaft of the bolt. The second does not capture this behavior and makes it seem that the two plates will not slide with respect to each other.
My question is whether this is an inescapable result of the nature of a revolute joint, or if there is a way to capture the sliding behavior of the two plates with a revolute joint. Furthermore, if the applied load is more than 3702 lbs (which is what I have it set at currently), the plates come into contact with the bolt, the simulation takes far longer, and warnings and errors are thrown when it does finally finish.
In a small and simple simulation like this, it isn't that big of a deal, but in a larger simulation, these issues can make the model run for much longer than I have time to let it run. Furthermore, when the simulation does finally finish, it will often tell me that it didn't converge and the results can't be trusted. Is there a better way to model a bolt like this that is at risk of being sheared off?
My question is whether this is an inescapable result of the nature of a revolute joint, or if there is a way to capture the sliding behavior of the two plates with a revolute joint. Furthermore, if the applied load is more than 3702 lbs (which is what I have it set at currently), the plates come into contact with the bolt, the simulation takes far longer, and warnings and errors are thrown when it does finally finish.
In a small and simple simulation like this, it isn't that big of a deal, but in a larger simulation, these issues can make the model run for much longer than I have time to let it run. Furthermore, when the simulation does finally finish, it will often tell me that it didn't converge and the results can't be trusted. Is there a better way to model a bolt like this that is at risk of being sheared off?





RE: Modeling Bolts in Shear
https://www.sharcnet.ca/Software/Ansys/16.2.3/en-u...
Edit: apparently radial gap joint is supported only by rigid dynamics solver.
In my opinion the first model using frictional contacts is a correct way to model
a bolted connection. I would expect the convergence to be slow if there is a lot
of sliding between the surfaces.
RE: Modeling Bolts in Shear
RE: Modeling Bolts in Shear
is one example of stresses in bolt after pretensioning (no external loading yet). In this model both the bolt head and nut are connected to plates
using bonded contacts. Between plates are frictional contacts. I have not modelled contact between shaft and plates.
https://imgur.com/a/7iid7 (scale used in this picture is about 200, this is why it seems that surfaces are penetrating quite a bit)
RE: Modeling Bolts in Shear
Any idea what might be causing this to happen? Here's the settings for the contact connection there:
And here's the surfaces in contact:
I'm not sure whether that's enough information for you to be able to help at all, but any you might be able to provide would be greatly appreciated. At this point, I'm at a complete loss for where to look for problems. It's not at all clear to me how ANSYS could end up generating these results.
Edit: All materials are generic structural steel.
RE: Modeling Bolts in Shear
status, pressure etc of contacts in the model before analysis (under connections) and post-analysis
(under solution).
RE: Modeling Bolts in Shear
There was no numerical scale on your plot. Was the displacement small?
I'm not sure if this replicates your setup. (Note that Ansys Auto Scale is at 6400x magnification below, making it look weird):
The original geometry was a simple cylinder in block with no interference but the hole diameter is the same as the cylinder diameter (10mm):
The reason, as I understand, is because the mesh is not exactly coincident. From the end view, the mesh has tiny interference:
Once the mesh is lined up properly, the interference is negligible:
Best regards,
Jason
RE: Modeling Bolts in Shear
RE: Modeling Bolts in Shear
This is at 1X scale. Note that these results are not converged because the simulation crashes before it will finish. Ultimately, the only way I've found to get the simulation to run without crashing is to use joints to represent these interfaces rather than frictional contact. This problem is though that apparently joints are only valid if you can accurately assume that the joint won't fail in reality.
RE: Modeling Bolts in Shear
something in the model that is causing non-convergence. Have you already plotted
Newton-Raphson residuals?
http://www.padtinc.com/blog/the-focus/overcoming-c...
RE: Modeling Bolts in Shear
With a little more effort, I'm sure you can get your frictional interface to work. Here's a recorded webinar by Simutech.
There are different trade-offs to using joints instead of friction interface. If you must have preload, slip etc, frictional interface is the way to go. I have seen people extract forces from simpler bolt model representation (e.g. contacts, beam element). Those forces are then plugged into a spreadsheet. If it's a concern, a more detailed frictional interface model is created.
Kind regards,
Jason
RE: Modeling Bolts in Shear
Clearly, whatever settings I have for contact between these two parts is not effective at enforcing contact between them. These are the settings I'm using:
Note that the diameter of the pin is 0.25in smaller than the diameter of the sleeve, which is why I set the radius of the pinball region to 0.13in.
Any suggestions as to what settings I have wrong would be greatly appreciated. I feel like I'm shooting in the dark here.
RE: Modeling Bolts in Shear
What was the error message?
How does the force convergence plot look like?
Does your Contact Tool>Status plot show the friction contact as "Far"?
Kind regards,
Jason
RE: Modeling Bolts in Shear
CODE -->
Here's the force convergence:
Here's what the contact tool status plot shows:
For comparison, when I do the same simulation with joints representing the contact (i.e. in a simulation not getting these crazy results), this is the results of the contact status plot:
RE: Modeling Bolts in Shear
Some suggestions:
1. Would it be possible to apply a temporary displacement 'support' on a small section of the 'red part' to avoid rigid body motion, apply your bolt preload, lock it, then remove the temporary support in the next time step? This should help keep the model from flying.
2. I noticed the red part has a thin face that is 'Near' (Yellow circle in this picture). Could you modify the geometry such that it is line-to-line to the contacting part?
Kind regards,
Jason
RE: Modeling Bolts in Shear
This is a cover for the end of an HVAC chiller, and what I'm modeling is the hinge that allows the cover to be opened so the chiller's tubes can be cleaned. The large square plate in the model is the end of the chiller to which the hinge gets bolted to. If you want to compare it to the hinge on a door, the large square plate is the door jam. The bolts referenced earlier attach the "jam side" of the hinge to the plate. At this point (potentially because you've helped me fix the problems with them), they don't seem to be causing an issue. What is happening however, is that the contact connections between the "hinge pin" and the "door side" of the hinge aren't being enforced properly and as a result the "door" and the "door side" of the hinge can go flying off.
The point of all that is the only thing preventing the behavior seen here from happening in reality is the contact between the "hinge pin" and the sleeve of the "door side" of the hinge that the "hinge pin" goes into. This is relevant to the conversation about the bolts in contact because when I define a revolute joint between the "hinge pin" and the sleeve, everything stays together just fine, but when I define a contact connection between the two surfaces, they fly apart. I think the issue is that initially there is a 1/8 in clearance all the way around the pin, which means that ANSYS ignores the contact at the start of the simulation and never reconsiders it later. This is what I was trying to prevent by setting the radius of the pinball region to 0.13 in (shown in the screenshot of the frictional contact settings above), but evidently that either doesn't do what I though it did or I didn't set it correctly.
RE: Modeling Bolts in Shear
Other suggestions:
1. Increase the pinball radius (say... 1 inch).
2. In geometry, move the door such that pin and sleeve are touching near where they are expected to.
Kind regards,
Jason
RE: Modeling Bolts in Shear
Now, to be clear, the solution has obviously not converged. Here's the force convergence plot:
Here are the error/warning messages I'm getting:
CODE -->
The reported error "An internal solution magnitude limit was exceeded" is quite strange to me. The node number is on the other side of the model and is not even close to being loaded in any significant way, so I'm not sure how a limit of any kind could be exceeded in any way.
RE: Modeling Bolts in Shear
In addition to previous suggestions...
1. Increase your initial substeps to a bigger number (e.g. 100) for the second load step.
2. Apply displacement control to make sure contacts are engaged before swapping it with gravitational load in the following step.
Kind regards,
Jason
RE: Modeling Bolts in Shear
It will inform you if there are gaps between contacting surfaces.
RE: Modeling Bolts in Shear
Thanks so much to both of you for all your help! I've definitely learned a lot!