Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Explain high stress spot in bolt joint with femap/NX Nastran

Explain high stress spot in bolt joint with femap/NX Nastran

Explain high stress spot in bolt joint with femap/NX Nastran

I have a 3 pieces assembly jointed by bolt. I use RB2 in Femap/Nx Nastran to simulate the bolt. Two side parts are fixed. One part is under the upper right load from the two free hole. After run the analysis, I get results shown in attached picture.

I can see the bolt squeezing the side piece. so there is high stress area. This high stress is much high than the yield strength 36ksi.

The results show is the max value of nodal stress. if I use average stress of elements, the high stress is down to 48.4kis from 66.6.

it is still higher than yield strength. In real case. we know it could be safe. but not 100% sure. and we also want safety of 2. Could anybody help me the interpret this case? Is the result correct?
I would appreciate if somebody could help me out.

RE: Explain high stress spot in bolt joint with femap/NX Nastran

Are you putting a preload on the bolt or just using the RBE2 to rigidly connect the 2 parts? If you're not using it for preload, is that really the best way, or should you define a bolt connection region? I am horribly inexperienced at Femap (just look at my other threads and you'll see), so maybe consider this a bump for your thread so that someone else will take a look tongue

RE: Explain high stress spot in bolt joint with femap/NX Nastran

it is simple reason: you can't evaluate stress where is connection to RBEs (or you can but results are very unrealisticdazed )
RBEs are rigid elements, their stiffness is unlimited therefore they cause artificial stress peaks.

Let me suggest how to proceed:

Ask a question: Do I really need to evaluate stress/strain result for the bolt connection?

if NO
- simple, because the goal of your task is something different that bolt itself. Of course, you can still f.e. check the stress for the bolt body, if the stress is still during the external loading still under Yield strength).
There are even some guidelines that say that you can evaluate stress f.e. regions that are 2 elements far from RBE2 legs, but this is too specific - depends on mesh density, structure, loading etc, not useful for general problem.

if YES
- than you should consider different bolt model, avoid RBE2's (even RBE3's). Very suitable is solid model with the bolt body and head (and nut if there is), and define a frictional contact between the bolt head and plate.
This is what I mean:

Hope it helps,


With best regards,
Dr. Jan Vojna
Lead Engineer Development

Siemens, s.r.o.

RE: Explain high stress spot in bolt joint with femap/NX Nastran

my 2c ... this is driving FEA down a deep mine shaft. there are lots of reasons why the FEM might be showing unrealistically high stresses local to load transfer points.

let the FEA tell you the load on the bolt, then use traditional hand calc to show the load is good.

another day in paradise, or is paradise one day closer ?

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close