Proper way of extracting component and bolt forces in an assembly

[humbleninja]

I need to do a shock analysis on an assembly that can be simplified into a fixed plate with tapped holes, and a cantilevered beam with a flange bolted to the plate. My objective is to find stresses in the bolts and the beam. I am using ANSYS Mechanical to solve this problem. The system is setup as Static Structural (preload bolts) -> Modal -> Response Spectrum.

My question mainly revolves around contacts. In the past, we have setup two models - one with bolts, and one without. The philosophy behind this is that the model without bolts would have a bonded contact between the entirety of the plate and cantilevered beam's flange and be used to find stresses in the beam. The other model has bolts, and has frictionless contact between the plate and beam flange, which would result in the highest stresses in the bolts.

My questions are as follows:

1. Is it appropriate to use two different models to solve for stresses in the beam and bolts? Or can we use one model?
2. Is it appropriate to first solve the frictionless model with bolts to confirm that there is no gapping between the plate and beam flange? If there is gapping, then the bonded model is no longer valid, correct?

 

[SWComposites]

If you are gapping the joint you do not have a good joint design. Either increase fastener torque, or add bolts, or something.

You can use either one or two models, just have to consider the limitations of each. Both are an approximation to reality.

 

[humbleninja]

If you are gapping the joint you do not have a good joint design. Either increase fastener torque, or add bolts, or something.

You can use either one or two models, just have to consider the limitations of each. Both are an approximation to reality.

Thanks for the reply. I agree that a gapped joint is a bad design, but I should confirm that right?

I would ideally use only one model to save time and work, but I think the only option to do that is to use a frictional contact. I think this is the most accurate way of representing the contact, but my thought was frictionless contact is more conservative when solving for bolt stresses. Thoughts there?

 

[SWComposites]

are you going to model the bolts with solid elements?
or are you modelling the bolts with bars/springs/etc?
are you going to attempt to model the fastener preload? which is quite difficult.
there have been many thousands of aerospace fastened joints analyzed with FE models with simple fastener connections to shell element nodes without any contact elements, where fastener loads are extracted and then fastener shear stress, sheet bearing stress, etc are calculated outside the FEM.
what exactly are you modelling and why do you need the complexity of contact elements?

 

[GVDR]

Hello, since you are interested in stresses in the bolt from a shock response, you should consider a realistic approach in terms of geometry and loading.
My take is you should do a pre-stress analysis to assess the contact areas around the bolt first, and ensure the head and nuts connections are representative enough.
This information will help you assess the amplitude or shock g levels your structure can take before the static pre-stress and loading do not hold. Passed this threshold, you will need to go transient to understand the deformations.

Hope this helps!

 

[humbleninja]

are you going to model the bolts with solid elements?
or are you modelling the bolts with bars/springs/etc?
are you going to attempt to model the fastener preload? which is quite difficult.
there have been many thousands of aerospace fastened joints analyzed with FE models with simple fastener connections to shell element nodes without any contact elements, where fastener loads are extracted and then fastener shear stress, sheet bearing stress, etc are calculated outside the FEM.
what exactly are you modelling and why do you need the complexity of contact elements?

I am modeling with solid elements because this is a relatively small assembly and I want maximum accuracy. Preload is included. I haven't heard the term contact elements before - when I say contacts, I would categorize them as boundary conditions in ANSYS. A bonded contact between two interfaces doesn't allow for penetration, sliding, or separation, whereas a frictionless contact allows for sliding and separation, but not penetration. I need to define some form of contact between every part or they would be free to penetrate.

 

[humbleninja]

Hello, since you are interested in stresses in the bolt from a shock response, you should consider a realistic approach in terms of geometry and loading.
My take is you should do a pre-stress analysis to assess the contact areas around the bolt first, and ensure the head and nuts connections are representative enough.
This information will help you assess the amplitude or shock g levels your structure can take before the static pre-stress and loading do not hold. Passed this threshold, you will need to go transient to understand the deformations.

Hope this helps!

I might not be on the same page as you, but I was thinking I need to apply the shock load to assess first to see if my assumptions of preload and contact hold. Then I solve the model with fasteners, and the model without fasteners.

 

[btrueblood]

One problem is that the actual joint can slip at the bolt interfaces, and this slip dissipates some of the shock energy via friction, which lowers the response. If your design cannot tolerate this slip (usually measurable in micro-inches or less) then a fastener might not be the correct design for attachment.

But the sequence should be - model the bonded condition first and assess stresses and determine if bolt preloads may be exceeded. Do the frictionless model only as a worst case check, since real world the joint has friction, which allows the fasteners to share more of the load and dissipate the shock.

Real world ends up you have to run the test to see if the shock response of the actual parts is anywhere near the simulation.

 

[humbleninja]

One problem is that the actual joint can slip at the bolt interfaces, and this slip dissipates some of the shock energy via friction, which lowers the response. If your design cannot tolerate this slip (usually measurable in micro-inches or less) then a fastener might not be the correct design for attachment.

But the sequence should be - model the bonded condition first and assess stresses and determine if bolt preloads may be exceeded. Do the frictionless model only as a worst case check, since real world the joint has friction, which allows the fasteners to share more of the load and dissipate the shock.

Real world ends up you have to run the test to see if the shock response of the actual parts is anywhere near the simulation.

So you think modeling with frictionless contact is too conservative to assess if there is any separation and to calculate margins on bolt strength? My concern is that modeling everything as bonded is too unconservative. I'm much less concerned about gapping because this is a very stiff joint, so I'm more interested in the bolt margins of safety. In a bonded condition, I would assume that the bolt stresses would be much lower than in the frictionless contact model, so that's not an accurate way of assessing margins.

 

[rb1957]

what happens if this fails ? do people die ?? if you have to redesign will that cost $B ??

what sort of loads is your model predicting ? high margins ? low margins (close to failure) ??

is it Really important to be super accurate in this ?

is it very difficult to set up a test ? A test would be considered to be much more reliable than a FEM with lots of bells and whistles ...

 

[SWComposites]

If you are modelling the bolts with solid elements, well, to be frank, that is gross overkill and its not going to be accurate anyway. All it does is make for a very complicated model and will generate lot and lots of output for which you won't know what to do with. What are you going to do when the model shows a very local hot spot on the bolt?

Show us a picture of the model.

And suggest running a simple static load case to check out the model before doing the dynamic shock analysis.

Is this for a real part on a actual flight vehicle? or a student / research project?