## steel structure joint, end plate

fandaL
Posts: 382
Joined: Thu Jul 24, 2014 8:29 am

### Re: steel structure joint, end plate

HarryvL wrote:
Sat Nov 03, 2018 8:23 pm
Exporting the maximum values for SigvM and PEEQ as a constant value for the element would be good. But no nodal averaging over adjacent elements should be applied.
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: steel structure joint, end plate

fandaL wrote:
Sun Nov 04, 2018 7:11 pm
HarryvL wrote:
Sat Nov 03, 2018 8:23 pm
Exporting the maximum values for SigvM and PEEQ as a constant value for the element would be good. But no nodal averaging over adjacent elements should be applied.
To demonstrate the difference between values in nodes and integration points, respectively, I analysed the problem of a 400x200x10mm plate with a 100mm diameter hole under 130MPa uniform tension.

As the theoretical stress concentration factor for this case is 4.312, the plate at the cross-section of the hole will show significant local yielding, while the average stress at that cross section is "only" 260MPa, which is lower than the assumed ultimate yield strength of 360MPa (see further).

I made use of double symmetry to cut down on the number of elements:

Plate_with_Hole_Mesh.png (42.55 KiB) Viewed 523 times

The material properties are taken as follows:

Code: Select all

``````Sig_yield = 235MPa @ Eps_plastic = 0.00

Sig_yield_2 = 238.4MPa @ Eps_plastic = 0.02

Sig_yield_ult = 360MPa @ Eps_plastic = 0.20
``````

An elasto-plastic analysis gives the following nodal values for von Mises stress and equivalent plastic strain (PEEQ):

Plate_with_Hole_vMises_1.png (317.75 KiB) Viewed 523 times

Plate_with_Hole_PEEQ_1.png (285.7 KiB) Viewed 523 times

The necking of the plate at the cross section of the hole is clearly visible. The equivalent plastic strain is very high and could well lead to cracking and rupture of the plate.

As the stress and strain distribution around the hole is relatively smooth, the extrapolation of stress and strain from integration points to nodes is quite accurate. In fact, the deviation from the specified stress-strain curve is only 0.063%. In hindside therefore not a very convincing example of inaccuracies introduced by extrapolation. However, inspection of stresses in the integration points will show that even higher accuracy can be achieved.

The following Paraview plot for maximum PEEQ and SigvM per element is created with the help of @fandaL's Python script:

vMises_PEEQ.png (81.82 KiB) Viewed 523 times

The maximum values of stress and strain thus obtained are in near-perfect allignment, showing 0.00075% error compared to the input values.

Although the practical improvement in accuracy is negligible for this example, in cases of more extreme stress concentration, like the ones analysed by Bernd and Thomas and the ones I quoted in earlier posts, the improvement is crucial for getting sensible results and making judgements about the acceptability of designs.

I would like to encourage others to give fandaL's script a try and see how it helps understanding stress and strain results.
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: steel structure joint, end plate

bernd wrote:
Fri Nov 02, 2018 4:21 pm
We had a disscussion about calculation of an enplate of steel beam cantilever which ist with bolts at work. The beam on the plate is a is a IPE 200. The plat itself is 30 mm thick. I just said let's do it with volume elements and nonlinear in FreeCAD.

The problem:
The yield point is 235 N/mm2, max sigma should be 223 N/mm2 according national standard, but it is impossible. If the steel starts to yield by 235 the max sigma is above 235. The picture shows any sigma above 240 N/mm2

How about the fixes. Is the fix wron and it should be on top of the plate for the tension bolt hole and on bottom of the plate for the pressure bolt hole.

cheers bernd
I decided to rerun this example on my Windows machine (which is faster and reduces the time to run this from 20 minutes to 4) and also use @fandaL's script to show the difference between nodal and integration point stresses.

The problem I now have is that I cannot reproduce the excessive stress values:

Screenshot (2).png (410 KiB) Viewed 435 times
Screenshot (3).png (474.48 KiB) Viewed 435 times
vMises.png (111.93 KiB) Viewed 435 times

Maximum nodal value is 67 MPa and maximum Integration Point value is 59MPa. Anyway, what it does show is how inaccurate nodal stress values can be.

OS: Windows 10
Word size of OS: 64-bit