Bolt load value during analysis 1

[Staszkinson]

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

 

[n3l3]

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

 

[Staszkinson]

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.

 

[TGS4]

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.

 

[TGS4]

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

 

[akabarten]

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

 

[Staszkinson]

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?

 

[akabarten]

Hi,

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

 

[n3l3]

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

 

[Staszkinson]

Hello,

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?

...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!

 

[n3l3]

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-6.11-Overview.pdf)

3) with that tool you'll be able to see the forces and moments in your bolt section.

good luck
n3l3