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
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
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
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
RE: Bolt load value during analysis
RE: Bolt load value during analysis
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
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
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
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
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?
Can You explain that in other words?
Thanks!
RE: Bolt load value during analysis
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