## steel structure joint, end plate

Jee-Bee
Posts: 2145
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

### Re: steel structure joint, end plate

HarryvL wrote:
Fri Nov 02, 2018 7:07 pm
I ran your example. It took 20 minutes to run. The output object reports a maximum von Mises stress of 292MPa and a maximum equivalent plastic strain (PEEQ) of 0.0091. Clearly these are not consistent with your input values, where at a PEEQ of 0.02 the stress should be 240 MPa. This is because of the extrapolation of stress and strain values to the nodes.

The DAT file is too big to load into my spreadsheet tool, but I am pretty sure that a bit of Python wizardry will show that the von Mises stress in the Gauss (integration) points (to be calculated from the formula below) is perfectly in line with the PEEQ (saved to file) in the same point.

Screenshot from 2018-11-02 20-04-04.png
I have to learn some stuff interesting!!
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: steel structure joint, end plate

Jee-Bee wrote:
Fri Nov 02, 2018 8:10 pm
I have to learn some stuff interesting!!
@Jee-Bee most of it is explained here:

and here:

and here:

but I also promised to do a tutorial, which I never did
Jee-Bee
Posts: 2145
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

### Re: steel structure joint, end plate

thanks i'll check them out
Posts: 1906
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: steel structure joint, end plate

Hi Bernd,
I checked the flange with my commercial software.
At Q=20 kN, M=46 kNm, M20 10.9 bolts I get a
utilization of 99% (without safety-factors for loading).
Thomas
report.pdf
Posts: 1906
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: steel structure joint, end plate

UR_ provided a nice flange-model (contact-analysis).
Maybe you can use this as a basis for your problem.
Attachments
rivlet-stripped.FCStd
fandaL
Posts: 382
Joined: Thu Jul 24, 2014 8:29 am

### Re: steel structure joint, end plate

HarryvL wrote:
Fri Nov 02, 2018 7:07 pm
The DAT file is too big to load into my spreadsheet tool, but I am pretty sure that a bit of Python wizardry will show that the von Mises stress in the Gauss (integration) points (to be calculated from the formula below) is perfectly in line with the PEEQ (saved to file) in the same point.
Hi,
If you would use it, I can extract the code from my scripts to convert von Mises stress from dat file to vtk format. It should not take much time.
Posts: 1906
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: steel structure joint, end plate

my two cent:
loading 230 kN at top/bottom of IPE-200, gives M=46 kNm
stresses at corner/web of IPE a little too high (plastifies out )
bolts are ok ==> M20 10.9
endplate_ts.FCStd
deformation.JPG (141.16 KiB) Viewed 730 times
stress_max_principal.JPG (86.68 KiB) Viewed 730 times
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: steel structure joint, end plate

fandaL wrote:
Sat Nov 03, 2018 10:32 am
HarryvL wrote:
Fri Nov 02, 2018 7:07 pm
The DAT file is too big to load into my spreadsheet tool, but I am pretty sure that a bit of Python wizardry will show that the von Mises stress in the Gauss (integration) points (to be calculated from the formula below) is perfectly in line with the PEEQ (saved to file) in the same point.
Hi,
If you would use it, I can extract the code from my scripts to convert von Mises stress from dat file to vtk format. It should not take much time.
Thanks @fandaL. It would be interesting to see what Paraview does with stresses at integration points. But I suspect it will also extrapolate to and average over nodes to create continuity across element edges. So this will give similar inaccuracies as the ones induces in CCX by interpolation and averaging. I will do some reading before you put in much effort.
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: steel structure joint, end plate

Sat Nov 03, 2018 11:22 am

stresses at corner/web of IPE a little too high (plastifies out )
Hi Thomas. Did you do an linear elastic analysis or a non-linear elastoplastic analysis? In a linear elastic analysis you will get unrealistic stress concentrations at sharp corners. That's the paradox I talked about: "The finer the mesh, the higher the stress" In a non-linear analysis the von Mises stress should not exceed the stress strain curve you have given as input. It it does, it is due to extrapolation and averaging of the results in integration points to nodes. I would never reject the design of a statically loaded detail becuase of local stress concentration. Buckling and fatigue is of course a different matter.
fandaL
Posts: 382
Joined: Thu Jul 24, 2014 8:29 am

### Re: steel structure joint, end plate

HarryvL wrote:
Sat Nov 03, 2018 12:00 pm
fandaL wrote:
Sat Nov 03, 2018 10:32 am
HarryvL wrote:
Fri Nov 02, 2018 7:07 pm
The DAT file is too big to load into my spreadsheet tool, but I am pretty sure that a bit of Python wizardry will show that the von Mises stress in the Gauss (integration) points (to be calculated from the formula below) is perfectly in line with the PEEQ (saved to file) in the same point.
Hi,
If you would use it, I can extract the code from my scripts to convert von Mises stress from dat file to vtk format. It should not take much time.
Thanks @fandaL. It would be interesting to see what Paraview does with stresses at integration points. But I suspect it will also extrapolate to and average over nodes to create continuity across element edges. So this will give similar inaccuracies as the ones induces in CCX by interpolation and averaging. I will do some reading before you put in much effort.
I have not found a way how to save integration point values to the vtk legacy format (I'm afraid that for displaying each integration point, one would need some other file format). I use integration point stresses and strain energy density values and average them over the element or take maximal value of von Mises stress for optimization purposes. I can export them to the vtk file and display in Paraview as one color on whole element.