FEA Simulation - Is this Way of Contacts for Bolted Connections right?

[andyleven]

Hello everyone,

I have an asssembly with some parts that are bolted together.

I make the faces of contact of the two parts to have sliding/no separation contacts and the faces of the holes (that normally should be a bolt there) to be bonded. Please see the attached file for better understanding.

Is this way of contacts right? I get some "strange" results from the simulation and I am wondering if they are right... 

Should I use bolt pre-tension?

I am looking forward to hearing from you.

Thank you in advance,

Andreas

kelly.young has embedded your images for clarity.

[Xun.Zhang]

Hi Andreas,

Before answer this question, could you explain a bit more for the words "strange result"? or what's your expectation compared with this result?

If you can provide a sample data here so that forum experts can help you out.

Thanks!

[andyleven]

Hi @Xun.Zhang,

Thank you for your response. I really appreciate it!

I am attaching two photos from the results I get. 

From the results it is shown that for the load i have applied the part will have a Factor Of Safety below 1 (0,41) and also it has a displacement of about 5mm.

However, i have tested this in reality and it hadn't got such displacement and also it hadn't passed to the plastic zone.

I am looking forward to hearing from you.

Thank you in advance,

Andreas

kelly.young has embedded your images for clarity.

[Xun.Zhang]

Hello Andreas,

Thanks for the clarification!

One more question, what is the "reality" means? Do you mean you have prototype a piece of sample and do the test in the lab?

Simulation result is more like a intention, it's not something accuracy, so please realize that it was a result for your reference and try to replace material and increase/decrease thickness in design stage to avoid late change.

In your case, the result looks reasonable since it's a simulating ideally without any other impact factors but in the reality, there are always existed other impact factors.

Hope it helps!

[johnsonshiue]

Hi Andreas,

I don't do FEA analysis regularly but I know the basics. Please bear with me. Could you tell me why you apply safety factor less than 1? Wouldn't it weaken the structural integrity?

Many thanks!

[Cris-Ideas]

Hi,

same question as Xun.Zhang what is the "reality" test you did exactly?

Also as far as I can tell from pictures of the results you posted I really do not see anything unusual or strange in them. Deformation is smooths and continuous,  so contacts you applied obviously work, stress is also something that you could expect for such defined simulation.

So if you have any concerns regarding correctness of the results you have to provide much more data and more comprehensive description of basis for your concerns.

Cris.

[andyleven]

Hi,

Firts of all i would like to thank all of you for trying to help me.

@Xun.Zhang , Yes I have that prototype in the lab and tested and it doesn't have such deformation or any signs of having gone to plastic zone.

@johnsonshiue , I don't work with safety factor below 1. This was an experiment to test inventor software for its result accuracy. The really strange thing is that with changing also the load to half in the simulation, I get safety factor very close to the previous one (0,55 instead of 0,4),  while i was expecting something enough greater!

@Cris-Ideas , you are right about the things that you mentioned. But after the test i was completed confused! I was expecting according to FEA a great deformation and even the part to have cracked, but none of these happened. 

Does anyone know if there is a need of bolt pretension at FEA to show me accurate results? Or the bonded contact is enough?

I'm looking forward to hearing from you about your thoughts and suggestions.

Again many thanks for your help,

Andreas.

[Cris-Ideas]

Hi,

I would be happy to assist you.

I do design a lot of structures and run FEM analysis in inventor.

But in any case results obtained form FEM analysis are only theoretical numbers and need interpretation.

So before trying to go with pretension bolting (this is possible in Inventor but very time consuming). I would start with finding possible causes of discrepancies between your simulation and test.

If you are interested in doing that please provide essential information on how your test was performed and what exactly are the results.

- how exactly is your test construction assembled, dimensions,  support, material .....

- any pictures

- how do you do measurements for the monitored values

- how is the load applied

- did you do any test to verify material properties

- your complete inventor model

Cris.

[andyleven]

Hello,

Thank you very much for your willing  to help! I really appreciate it!

Unfortunately I cannot give you details about the tests and also the 3d models....

However I believe that it would be very helpful for me if you can tell me what contacts you will put (between the parts, the bolt, the nut etc) to that simple assembly of bolted connection. 

Also will you prefer to do the FEA with the bolt inside or exclude the bolt from the study and use some other contacts and which?

I am looking forward to hearing from you

Thank you in advance,

Andreas

kelly.young has embedded your image for clarity.

[Cris-Ideas · Accepted solution]

Hi,

it all depends what you want from your calculations.

Generally there is a problem with friction between plates you are practically unable to model.

So either you will have situation where force will go threw contact between plates or threw the bolt.

In case you are dealing with prestressed bolts you can split surface of the plate around bolt hole to limit contact between pates to some area that would be closer to modelling stress being transferred only close to the bolt where there are biggest compression coming from the bolt.

As for contacts if I am interested in analysis of connection I model bolts and depending on how stress can influence pieces I either split surface to accumulate stress or leave it as it is if stress in plates is not essential.

As for bolts and holes I usually use separation- non sliding contact as sliding or separation. But you must make sure there is no empty space between bolt and hole so I use additional hole patching parts in FEM analysis assembly.

Read this thread FEM stress analysis - disturbing results to see what happens when you don't.

As for nuts/washers/bolts I use bonded

As for nuts/ plates I use separation no sliding or shrink fit if prestressed bolts (model must be made with proper interference)

If prestressed bolts are in question I usually suppress bolt/plate contact and only "friction" between plates is active

For plat / plate I usually use separate no sliding contact to find is joint will open.

For joints with bolts with shear (witch I very really use) or pins I use no gap connection plate/pin and separation no sliding contact + I suppress plate/plate contacts.

If I am not interested in connection I just exclude all the bolts and simply go with bonded, there is no difference for global analysis.

Cris. 

[Frederick_Law]

Simulation is correct.

Area with low safety factor is where there is stress concentration.

Since you have 5000mm displacement, there is something wrong with your number.

How much load you're putting on the part?  Check your units.

[Cris-Ideas]

@Frederick_Lawhe has displacement of only 5mm.

@andyleven

What you show in your screen shot is that you have displacement of about 5mm.

But this displacement is not the save as vertical displacement.

From what I can see from screen you provided (with is not ideal form of result presentation) this part also has significant displacement from its plane.

You have not given us anything regarding your test so we are more guessing than anything else doing. But verify if displacement you read is the same as the one you measured.

Without more data I do not see anything I can do more to help you.

When I run simulations on my models I often get very high values of max stress (like few thousand MPa) but it is always the case to do result analysis and filter out values that come from numeric and meshing causes.

It is much faster than trying to fight it and force software to do "perfect" calculation.

Cris.

[Frederick_Law]

Usually we don't FEA bolt connections.  There are already enough studies and standards on their proper use.

Basically when parts are connected properly with bolt or rivet.  They're consider solid and non-movable, non-separable.

For your info.  When nut is torque onto the bolt, it result in a clamping force.  You can't apply torque in Inventor FEA and generate clamping force, I think (I've been point out to be wrong a few times already ).  You can fix the nut and apply force on the bolt to simulate bolted connection.  The nut should slide along the bolt.  Then you can load the sheet metal parts and see how they'll behave.  The sheet metal parts should again slide between themselves, bolt and nut.  You could do this to every nut and bolt on your assembly.

[Cris-Ideas]

---

@Frederick_Law wrote:
.
......You can't apply torque in Inventor FEA and generate clamping force....

---

Actually you can,

build your model with proper interface and apply "shrink fit contact" between washer and plate face

Than bolt acts exactly as torqued.

If force in the joint < clamping force => no separation

if force in the joint > clamping => separation and additional deformation and stress in the bolt.

Cris.

[andyleven]

Hello,

I really thank all of you for your help!!

Best regards,

Andreas

[LT.Rusty]

Another thing you might consider is doing the simulation on one piece at a time. This can be useful particularly if you have complex parts or there are complicating factors in the design.

With something like the picture you show in the first post, I wouldn't jump straight into doing FEA on the assembly. I'd start off with (for instance) just the horizontal part. I'd set up the constraints so that it's fixed wherever there's a bolt that attaches it to something, set the load as needed, and then run the simulation like that. Then I'd do the same for the vertical part. If things looked like they were working correctly, I'd then move on to trying the assembly, and see how the results look when the parts are put together.

[andyleven]

 Hello @LT.Rusty ,

Thank you very much! You are right about that!

Best regards,

Andreas