steel structure joint, end plate

Show off your FreeCAD projects here!
User avatar
ppemawm
Posts: 745
Joined: Fri May 17, 2013 3:54 pm
Location: Manhattan New York

Re: steel structure joint, end plate

Postby ppemawm » Sat Nov 03, 2018 2:01 pm

thschrader wrote:
Sat Nov 03, 2018 11:22 am
bolts are ok ==> M20 10.9
[/quote

How did you handle the preload in the bolts? Just curious how others deal with this in FEA.
"It is a poor workman who blames his tools..." ;)
thschrader
Posts: 1905
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: steel structure joint, end plate

Postby thschrader » Sat Nov 03, 2018 2:11 pm

HarryvL wrote:
Sat Nov 03, 2018 12:31 pm
Hi Thomas. Did you do an linear elastic analysis or a non-linear elastoplastic analysis?
@Harry: only linear elastic as a first start.
@Bernd: is the flange attached to a column? Or another flange/beam?
Thomas
flange_column.JPG
flange_column.JPG (27.43 KiB) Viewed 799 times
thschrader
Posts: 1905
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: steel structure joint, end plate

Postby thschrader » Sat Nov 03, 2018 2:14 pm

ppemawm wrote:
Sat Nov 03, 2018 2:01 pm
How did you handle the preload in the bolts? Just curious how others deal with this in FEA.
No prestressing of the bolts. It is only a first model. I will think about that.
Harry has used "cooling" of rebars to simulate prestressing of concrete beams.
thschrader
Posts: 1905
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: steel structure joint, end plate

Postby thschrader » Sat Nov 03, 2018 2:17 pm

ppemawm wrote:
Sat Nov 03, 2018 2:01 pm
How did you handle the preload in the bolts? Just curious how others deal with this in FEA.
No prestressing of the bolts. It is only a first model. I will think about that.
Harry has used "cooling" of rebars to simulate prestressing of concrete beams.
EDIT:
Btw: the external momentum of a prestressed bolted flange does not raising the force in the bolts (only a very little...)
User avatar
ppemawm
Posts: 745
Joined: Fri May 17, 2013 3:54 pm
Location: Manhattan New York

Re: steel structure joint, end plate

Postby ppemawm » Sat Nov 03, 2018 2:48 pm

thschrader wrote:
Sat Nov 03, 2018 2:17 pm
Harry has used "cooling" of rebars to simulate prestressing of concrete beams.
Ah, OK. That is how I have been doing it.
thschrader wrote:
Sat Nov 03, 2018 2:17 pm
Btw: the external momentum (moment?) of a prestressed bolted flange does not raising the force in the bolts (only a very little...)
Depends heavily upon the relative stiffness between the flange, gasket, and bolt. FEA is a way of accounting for that stiffness ratio if the bolts are preloaded in the model, especially if the bolts are in bending. Critically important for fatigue or cyclic loading.
"It is a poor workman who blames his tools..." ;)
User avatar
bernd
Posts: 10959
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: steel structure joint, end plate

Postby bernd » Sat Nov 03, 2018 7:51 pm

according to ickby vtk supports element data out of the box. Means it should be possible to show results in integration points in paraview. https://forum.freecadweb.org/viewtopic. ... 10#p260932
User avatar
bernd
Posts: 10959
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: steel structure joint, end plate

Postby bernd » Sat Nov 03, 2018 7:56 pm

wow lots of answers ... I have carefully read the other topics of harryvl. great stuff ...

The bolts are 8.8 M24 Staifix ancor and the cantilever beam should be on a concrete wall. Between plate an concrete is 20 mm special stiff insulation. But not at around the bolt. I may need to make a geometric model of all ...


Seams we somehow need to attract the integration point data for these plastic analysis. This is something FreeCAD is able to analyze but most structural analysis software not :D

bernd
User avatar
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

Re: steel structure joint, end plate

Postby HarryvL » Sat Nov 03, 2018 8:23 pm

fandaL wrote:
Sat Nov 03, 2018 1:59 pm
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.
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.

PS: it's just an inherent characteristic of the FEM that stresses and strains get evaluated at integration points. So any extrapolation to the other positions within the element (like nodes) and averaging over adjacent elements for the sake of getting pretty pictures will lead to confusing interpretation and inconsistency between stress and strain. 25 years ago I implemented a more accurate method for smoothing results (one originally proposed by Clough in the 60s); but even with that small inconcistencies remain.
User avatar
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

Re: steel structure joint, end plate

Postby HarryvL » Sat Nov 03, 2018 8:49 pm

Just a thought ... would it be possible/difficult to implement functionality where the user gets to see the smoothed, but inaccurate, results to identify area of high stress and strain and then when hovering the mouse over an element in that region gets to see tabulated values for the integration point results for that specific element? Even the 10 node quadratic tetrahedron (C3D10) only has 4 integration points, so that is not a massive amount of information.
UR_
Posts: 1197
Joined: Tue Jan 03, 2017 8:42 pm

Re: steel structure joint, end plate

Postby UR_ » Sun Nov 04, 2018 8:10 am

thschrader wrote:
Sat Nov 03, 2018 2:14 pm
No prestressing of the bolts. It is only a first model. I will think about that.
Harry has used "cooling" of rebars to simulate prestressing of concrete beams.
If you are using contact analysis already, one can simply achieve pretension (without *PRETENSION :( ) by design.
In this case you will have overlapping solids.
i.e. There is a gap between both plates (0,01 mm) and a "negative" gap between bolt's head and it's supporting plate (-0,3 mm)

ccx will solve this intrusion by applying as much strain as needed to accomplish the contact constraint.

FreeCAD 0.18-000097.png
FreeCAD 0.18-000097.png (191.34 KiB) Viewed 741 times

pretension_stripped.FCStd
(24.53 KiB) Downloaded 37 times

So no heating up to melting point is needed.
And therefore no firefighter needs to be present, while you are doing your calculations :lol:
Last edited by UR_ on Sun Nov 04, 2018 8:49 pm, edited 1 time in total.