Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - Femap Forum
- Which bolt model should be more reasonable?

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-05-2016 03:41 PM

In the model to the right, the component in the middle is fastened to the side c-channel with 3 bolts on each side. Load is added on the pin hole on the middle piece. so there is large moment on the middle component, I have to size the thickness of the middle conponent and bolt size.

I am considering 3 method to model the system:

1. Use plate element for the middle surface of all the components, then use beam and rigid element rb2(TX, TY, TZ constrainted only) to simulate the bolt joint.

2. Use solid model for all components except bot/nut, then use beam and rigid element to simulate bolt joint, and the rigid element is constrainted to the surface node of the solid model.

3. Use solid model for all components, bolts and nuts.

The first method is fast. I can get the axial force in max combined stress in the bolt. it is unknown for the stress in contact area between the bolt head and middle component.

If I use second method, the edge of the bolt head is high stress spot, the middle component will yield at nodes of rb2.

If I used the third method, I found much higher stress on bolt shank.

I want know what you guys usually do to analyse this type of joint?

Which method is more reliable in the mothods above?

I would appreciate your help if you can put some comments.

Anderson

9 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-05-2016 04:39 PM

Hi Anderson,

From my experience, I have found that it is better to extract loads from FE models and then use the loads to size the bolt.

If I was analyzing the model, I would first do a quick hand calc to get an idea of the stresses that I am expecting. I would treat the problem as a beam supported at two ends with 60% of the load at one reacted at one end and 40% at the other.

Thereafter, if this is a fail-safe structure, I would make sure that two or maybe one bolt can carry the load.

I would choose option 1 extract the shear force and bending moment at the beam elements and do a classical hand calculation.

However, if you are interested in knowing the bearing stress distribution and contact stresses then then go with option 3.

I hope this helps.

Regards,

Saptarshi

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-06-2016 07:01 AM

Following waht Abderosn said:

- bolt using rbe2 (free rotation) and getting the forces to dimsension the bolt size. With this model also you can check the overall stiffness and displacements. You can add that if the bolt goes in compression, bolt joint does not work.

- if you are interested in the stresses on the bolt area, then solid elements, contact, prestress . Rbe2 is not valid as it is like a "singularity "

Have a look to http://server2.docfoc.com/uploads/Z2015/12/22/nLEF

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-12-2016 11:39 AM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-17-2016 08:25 AM

Using RBE2 you have only 2 options. Or you fixed the rotations or leave free. The first one you add more stiffness than it may be . The second less. For the displacements you may be more conservative if you leave free the rotations. When you want a detail of behavior you should use 3d contact+preload

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-17-2016 02:52 PM

Anderson,

To calculate the bolts, I would use a modify version of #1. I would changed the CBeam to a CBush with only translational stiffnesses. The bolt should not take bending unless you have separation of the interfaces. The joint itself should take it.

We usually extract the load than use a spreadsheet to calculate the joint stiffness vs the bolt stifness and only use the portion of the load that goes into the bolt for further calculation. Using all the load will results in a mor conservative approach.

You can find more information within he NASA technical spec 5020.

For the plates, I would do as Jon suggested.

Frédéric

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-19-2016 03:23 PM

In this case, the load is at Y-Z plane and 45 degree to X-Y plane, If I do the quick hand calculation, Should I just average the moment and shear force to these 6 bolts, then use this load to do hand calculation?

By using option 1, I can export the load on each bolt (I use one beam element to simulate one bolt shank). I can obtain moment, shear force, axial force and torsional torque for each bolt, then should I used all these load to do a classical hand calculation? In you reply, it seems you only mention "extracting shear force and bending moment".

If I go with option 3, the hole size is 1/16" larger than the bolt. When I define connection, the inner surface of hole and the outer surface of bolt should be defined as contact? If yes, at the end of the calculation, these two surface will contact. and if there is pretention in the bolts, then they maybe contact. Am I saying correctly?

Thank you!

Anderson

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-19-2016 03:41 PM

Hi, Jon,

Thanks for you sharing.

As you said, the option 2 is not feasible method. we should either go 1 or 3.

In option 1, can I use the combined stress of the beam element, which is exported from the FEA result, to dimension the bolt? If I use hand calculation, I should use the result when the bolt is under preload?

Thank you!

Anderson

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-20-2016 06:50 AM

Hi,

I will try to answer shortly. If the preload is the appropriate the loading that undergoes the bolt joint is : preload+percentage of the external load. This percentage depends on the bolt/flanges stiffness. As the preload normally is 80% of the yield and this percentage of the external loads is 10-15% (with the right sizing of the flanges), the bolt should be ok.

Steps that I do:

- Size the bolt under external load. For example as you said
- With this size calculate the preload
- Preload>external load
- Run the analysis (preload+external) and check the loading in the bolt and the joint separation
- If the load=preload / joint separation is 0, means design ok. Bolt undergoes only axial (no moments or low as the joint is not opening )

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

10-20-2016 08:32 AM

Hi Anderson,

Follow this procedure to size the bolt:

Determine the axial load on the bolt due to preload.

For the shear loads, calculate the magnitude of the loads. Ps = sqrt(Fsx^2+Fsy^2)

For the bending moments, calculate the magnitude of the moments. Mb = sqrt(Mbx^2+Mby^2)

If the torque is negligible, ignore it. If it a simple pinned joint, there should not be any torque unless you account for friction effects or some anti rotation feature.

Ideally, the section where you have the max bending moment, the shear force should be 0; however for conservatism it is often better to use the max shear force and max bending moment at a single section along with the axial load to size the bolt/ pin.

Once you have determined the loads, get the stress ratios. (R = Calculated Stress / Material Allowable)

So you need to calculate Ra (Axial), Rs (Shear) and Rb (Bending). Depending upon whether you are doing your analysis with limit loads or ultimate loads you need to use either limit or ultimate material allowables. (Material Tensile Strength and Material Shear Strength is widely available; for Material Bending Strength depending upon the application you can either use FTU/ FTY or FBU/ FBY)

After you have calculated the stress ratios, use an interaction formula (ref: Bruhn C4.26) to determine your margin of safety. A positive MS value of 0 is the most optimized design for the given set of loads.

MS = {1/ (Ra + sqrt (Rb^2+Rs^2))}-1

Regarding your second question, why is thehole size larger than the bolt. If you have bushings, then you have to include them to get a correct representation of the stress distribution.

Regards,

Saptarshi

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc