×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

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

Jobs

Bolt load value during analysis

Bolt load value during analysis

Bolt load value during analysis

(OP)
Hello,
Is it possible to obtain loads in bolts(solid model) at some steps of my analysis? How Can I do that?

Should I convert stresses to force? Or maybe there is another, easier way?

Thanks

RE: Bolt load value during analysis

Hi, i dont know if you model it like a beam/truss but may be this can help:


In beam/truss elements you can check out the SF (section force) variable.
SF1 should be the one you need, while SF2 and SF3 would show a value of zero.
If you cannot see the SF variable in the results viewer is because you have to select it previously in the field ouput requests.

cheers

RE: Bolt load value during analysis

(OP)
Thank You,
It's sounds good for beam/truss elements. I'm sure that it works properly.
Unfortunatly my bolt is made of solid elements(C3D8R) and SF field output request is not available in this case.

RE: Bolt load value during analysis

You need the SF to perform a "free body cut". That will give you a sum of the forces across a cut (such as a cross-section of a 3D-Solid bolt). If you don't have it available, then you need to re-run the analysis adding that field output request to your set of requests.

RE: Bolt load value during analysis

Correction to my previous posting - you need NFORC to perform the "Free Body Cut".

RE: Bolt load value during analysis

Hi,

In Abaqus/Explicit you can ask for integrated output.
See 4.1.3 Output to the output database, Integrated output in Abaqus/Explicit.

Regards,
Bartosz

RE: Bolt load value during analysis

(OP)
I use Abaqus/Standard Bartku :)

Could You explain why sum of the NFORC values in direction of loading IS NOT equal to the pressure loading * area?

Let's consider simple column made of solid elements. It's fixed and the bottom and loaded by a tensile pressure at the top of the column. I have made a few analysis with different mesh size. The pressure was always 1e10^6 N/m^2.
The sum of NFORC values(in the loading direction) for all nodes in cross-sections has different values for different mesh size and it's not equal to total pressure * loaded area.

What is wrong in my method?




RE: Bolt load value during analysis

Hi,

Quote:

I use Abaqus/Standard
In this case you can use section output.
4.1.2 Output to the data and results files, Section output from Abaqus/Standard

Disadvantage is that the output cannot be save into *.odb file.

Regards,
Bartosz

RE: Bolt load value during analysis

Hi,

when doing a "view cut" and showing the resultant force you can chack out the sum of forces in the cut direction, of that what you display at that moment, if you eliminate a piece in the display manager, then values in its elements are not accounted.

may be this tool can help you to check the results.

(if the problem persists with different results with different meshing sizes, rememeber that you should tend to a solution as you do your mesh smaller, so it could be that you have a coarse mesh?)


cheers
n3l3

RE: Bolt load value during analysis

(OP)
Hello,

Quote (n3l3)

when doing a "view cut" and showing the resultant force you can chack out the sum of forces in the cut direction, of that what you display at that moment, if you eliminate a piece in the display manager, then values in its elements are not accounted.

I'm not sure if I understand your method correctly.
Take a look at the attached screenshot if you can.
1) I cut the bold at the middle of bolt shank.
2) I picked up all of nodes in this cross section
3) I got data(NFORC2 - parallel direction to the 'y' axis in global coord system) from field output
4) Sum NFORC2 values from 3)

Is it ok?

Quote (n3l3)

...if you eliminate a piece in the display manager, then values in its elements are not accounted.
Can You explain that in other words?

Thanks!

RE: Bolt load value during analysis

Hi, cannot see that picture, you can upload it to this website.

Why dont you try this:
0)You don´t have to choose nodes or whatever. Just ask for NFORC's in the field output
1)in the visaulization module just plot only the bolt part
2) cut the bolt with a Free Body Cut (page 7 of this presentation http://www.simulia.com/download/rum11/UK/Abaqus-6....)
3) with that tool you'll be able to see the forces and moments in your bolt section.

good luck
n3l3

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!


Resources