Bolt pre-load applied after the applied loads?

[j.hancock01]

Hi, 

I'm running a few tests using the bolt connector tool in Fusion 360's simulation before I start using this in more complex models. I'm modelling a 1000mm long hollow steel tube (48mm ID, 70mm OD) with a bolt running through the middle. Firstly, a 45mm diameter bolt with an applied pre-load of 279477N, modeled using the connector tool. The cross-sectional area of the tube is 2039mm^2, so expected stress under pre-load is 137MPa,  screenshot below. End displacement was also as expected from hand calculation at 0.65mm. All looks great so far!

Next I took the case of the tube without the bolt but loaded by a force of 300000N applied at each end to put it into compression, Theoretical stress expected 147MPa, displacement 0.7mm. Fusion gave 135MPa stress, end displacement of about 0.66mm, see below, not exact but ok.

I then ran a case with both the pre-loaded bolt and the 300000N load. This gave stresses of 272MPa and end displacement of 1.3mm. This is a simple addition of the previous two cases which implies that the pre-load is calculated and applied after the application (and hence compression of the tube) by the externally applied load.

This is rather odd as the majority of cases the bolts on a connection will be tightened and the pre-load locked in and then the loads applied to the structure. This means that in these "real world" cases a compression load, such as that modeled above, will reduce the stretch of the bolt and hence reduce the applied pre-load. This should have reduced the stresses and the displacement from that given here. 

As the pre-load is actually applied after the forces I think that things like allowing a user defined "Elastic modulus" and "coefficient of thermal expansion" won't have any noticeable affect on the results. Indeed the whole "connector" option at the moment doesn't seem to do much more than apply a set of opposing forces equal to the pre-load to the bolt and nut locations. This would be an order of magnitude more useful and realistic if the pre-load was calculated (which basically represents tightening the bolts) before the structural loads are applied to the structure. 

Perhaps I'm missing something. Is there a way to get fusion to apply the pre-load (tighten the bolts on the joint) and then apply the externally applied loads as would be the case for the majority of situations with pre-loaded bolts? 

Thank you for your guidance in advance!

[James.Youmatz]

Hi @j.hancock01,

Thanks for posting and reporting this. Let me do some digging and chat with the simulation team and see what is going on here and if we can shed some more light around this topic.

[j.hancock01]

Thanks James, much appreciated.

I've seen some people suggest modelling the bolt with solid elements and using a contact with a "Penetration Surface Offset" between the bolt head and the contact surface to apply a pre-load to the bolt. I've tried this, I think a displacement of about 1.7mm would be enough so entered this as one of the contacts:

Unfortunately, this didn't seem to work in this case. I'm guessing the contact doesn't become active if the prescribed contact surfaces are already overlapping at the start of the analysis? The results had negligible stress and displacement:

Perhaps I've missed something with this technique?

Best wishes

Jon

[James.Youmatz]

Hi @j.hancock01,

Sorry about the delay in getting back to you.

I just wanted to let you know that we dug into this deeper and have found some issues with it as you have noticed. As of right now, I don't have too many specifics around it, but I do know that the development team is working on this and is working on a fix. 

Thanks again and as soon as I have an update I will let you know!

[j.hancock01]

Hi James,

Thank you for the update, I'm glad you and the team are looking into this, much appreciated. In case that anyone else has similar issues I've developed a partial workaround as follows. Feel free to check, any comments most welcome:

I'll show this with an example of a M45 steel bolt with a pre-load of 279477N used to compress a steel tube 1000mm long, 70mm OD, 48mm ID. An M45 bolt has a stress area of 1300mm^2, which gives and effective diameter of 40.684mm for modelling in the analysis - the actual OD of the bolt (including the threads) is about 45mm although I don't use this in the analysis. Young's modulus of steel = 210000 N/mm^2. It's a simple example to show how it works, I don't see any reason why the method shouldn't work with more complex structures with multiple bolts etc.

1) Apply the pre-load from the bolt(s) directly to the compression faces of the items taking the pre-load as a pair of opposing forces (each equal to the pre-load force). In the example case these are the ends of tube. I've not directly modeled the bolts at this stage.

2) Measure the displacement of the compression faces under the action of the pre-load force (0.6021mm in the example case, as shown above)

3) Determine the amount of force required to compress the bolt(s) the same amount as the displacement of the compression faces. This is the shortening of the bolt as the compression faces squash together under the action of the initial bolt pre-load. This can be achieved from using conventional theory:

Force to cause shortening = Young's modulus of the bolt x cross-sectional area of bolt x shortening of bolt / original free length of bolt (distance between inside face of bolt head and nut)

In the example case this is  = 210000 N/mm^2 x 1300mm^2 x 0.6021mm / 1000mm = 164373N

4) Explicitly model the bolts in the analysis of the joint, use a "separation" contact between the bolt & nut heads and the compression faces of the part being bolted together.

5) Apply a force to the inside face of the bolt head equal to the pre-load plus the force required to cause shortening (from step 3). Apply the same force in the opposite direction to the inside face of the nut:

This should lock the correct pre-load into the compression structure. When an externally applied force is applied to the structure it will be resisted by pre-load and the combined stiffness of the compression structure and the bolt as in the real world case. Note that the stresses in the bolt won't be correct as the pre-load has been locked into the bolt in compression rather than tension - better to work out the bolt forces/stresses with a hand calculation.

It's a bit of a pain to apply this work around and the bolt forces aren't right so it'll be great when you and the team have it fixed and we can use the built-in bolt tool!

On a similar but related issue, I think there's also an issue with the way contact friction is modeled so likely to be issues with analyzing the sliding of a bolted joint/connector at the moment. I've included my notes at the end of an existing post on this issue (see https://forums.autodesk.com/t5/fusion-360-design-validate/bolt-connection-simulation/m-p/7451617#M13...). Any assistance on these would be much appreciated by myself and I'm sure many other users. I already love fusion as a tool for the design and analysis of structures without bolted joints - get these fixed and it'll be even more fantastic!

Many thanks for your help.

Best wishes

Jon