FEM - Tubular Connection with Shell Elements

Show off your FreeCAD projects here!
User avatar
HarryvL
Posts: 1010
Joined: Sat Jan 06, 2018 7:38 pm

FEM - Tubular Connection with Shell Elements

Postby HarryvL » Wed Feb 14, 2018 10:08 pm

Hi all,

I would like to share an analysis of a steel tubular connection, like you could find in a major truss span of a bridge or roof. Of particular note is that (thanks to the great selection of tools and workbenches in FreeCAD) it only took me 1 hour or so to model and complete this whole analysis.

The dimensions are fictitious, but credible, i.e.: the horizontal tube has a diameter of 500mm and wall thickness of 10mm, whereas the diagonal braces have a diameter of 250mm and a wall thickness of 10mm. The diagonal loads are 1MN each.

The first picture shows the 4 solids used to create the tubulars and the region for mesh refinement

KBR3_Solids.png
KBR3_Solids.png (279.12 KiB) Viewed 3081 times

Next, the BooleanFragments of the combined solids are downgraded to faces in the Draft workbench, after which the model can be cleaned up by removing unwanted faces and stitched together with "Join Connect Objects" in the part workbench

KBR3_Faces.png
KBR3_Faces.png (263.24 KiB) Viewed 3081 times

This can be meshed in FEM work bench and the region where the braces meet the horizontal can be refined by creating a mesh region.

KBR3_Mesh.png
KBR3_Mesh.png (390.59 KiB) Viewed 3081 times

The results show the local deformation of the horizontal tube (scaled by a factor 50) and the high stresses the braces induce. This would be the starting point for designing local reinforcement of the node.

KBR3_Def_Mis_1.png
KBR3_Def_Mis_1.png (431.16 KiB) Viewed 3081 times

Finally a glossy Paraview picture of the same result

KBR3_Def_Mis_2.png
KBR3_Def_Mis_2.png (128.99 KiB) Viewed 3081 times

In my view FreeCAD is a great tool to quickly asses conceptual designs.
Last edited by HarryvL on Thu Feb 15, 2018 7:33 am, edited 3 times in total.
thschrader
Posts: 1394
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: FEM - Tubular Connection with Shell Elements

Postby thschrader » Thu Feb 15, 2018 12:06 am

Harry, nice work.
How can I see the deformed shape in paraview?
When i select displ, I get the colours, but not
a deformed shape... :?
User avatar
HarryvL
Posts: 1010
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM - Tubular Connection with Shell Elements

Postby HarryvL » Thu Feb 15, 2018 2:34 am

Hi Thomas. In Paraview you need to create a Warp filter and scale the displacements. In this example I applied a scale factor of 50. Harry
User avatar
bernd
Posts: 7757
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: FEM - Tubular Connection with Shell Elements

Postby bernd » Thu Feb 15, 2018 11:57 am

Yeah cool example of FEM workbench, harry :)
User avatar
bernd
Posts: 7757
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: FEM - Tubular Connection with Shell Elements

Postby bernd » Fri Feb 16, 2018 6:46 am

I gave done similar tests on structural beam connections. The problem I have is when is the connection no more ok. In such an analysis you get poits of yielding quit early (on minor loads) This mostly due to singularity because of sharp edges. Means the connection is still ok. But at some point it is no more ok because than there are really yielding areas. The question is how to distinguish brtween both.

Hopefully you got my point harry and thomas?!

bernd
User avatar
HarryvL
Posts: 1010
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM - Tubular Connection with Shell Elements

Postby HarryvL » Fri Feb 16, 2018 9:07 am

Hi Bernd, the answer is "it depends":

1) If the joint is statically loaded (self weight dominates and cyclic loading is therefore insignificant) AND it is made of ductile material like structural steel (so it doesn't crack like glass or wrought iron when exceeding a limit stress) AND other lighter loaded regions have remaining capacity to carry further load increase, then stress concentrations don't matter too much. The load at which first yielding occurs is in that case a lower bound for the actual failure load.
2) If one or more of the above three conditions are not satisfied then you may be in trouble and need to pay close attention to the peak stresses.

The stress concentrations you refer to are usually very localized and redistribution can easily take place. However for cyclic conditions (e.g. Offshore structures or slender masts subject to wind loading ... which I believe is Thomas' speciality) it becomes important to see if the stress concentrations are real or just an artifact of the mesh discretisation. I have had practical cases for offshore structure where they are real and then you need to adapt design (rounded edges etc) to prevent fatigue issues. But I have also had cases where it is just a matter of refining the mesh to get rid of them.

In the case I show here the peak stresses don't occur at isolated sharp corners and redistribution can take place, so in this case the approach is quite safe for design. I plan to do a follow-up of this case where I compare the solutions to design code (and show how the FEA in this case is far less conservative) and will analyze a few possible design solutions for strengthening the joint that could not be found by just looking at the code. All-in-all FreeCAD is a great design aid.

Hope this helps.

Harry
thschrader
Posts: 1394
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: FEM - Tubular Connection with Shell Elements

Postby thschrader » Fri Feb 16, 2018 2:03 pm

HarryvL wrote:
Fri Feb 16, 2018 9:07 am
I plan to do a follow-up of this case where I compare the solutions to design code (and show how the FEA in this case is far less conservative) and will analyze a few possible design solutions for strengthening the joint that could not be found by just looking at the code. All-in-all FreeCAD is a great design aid.
Interesting idea! Keep up the spirit :)
@bernd, your post above: what do you mean with " ..connection no more ok."
Is it damaged? Can you post a pic? (maybe new thread)
Thomas
User avatar
HarryvL
Posts: 1010
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM - Tubular Connection with Shell Elements

Postby HarryvL » Fri Feb 16, 2018 5:40 pm

bernd wrote:
Fri Feb 16, 2018 6:46 am

... This mostly due to singularity because of sharp edges. Means the connection is still ok. But at some point it is no more ok because than there are really yielding areas. The question is how to distinguish brtween both.

bernd
Further to my earlier response and specifically on the question of growing/spreading plastic zones:

That is where an elastic-plastic collapse analysis will give you the answer. The plasticity card in Calculix and some other programs allows you to push redundant structures beyond the point of first yielding. In areas where plasticity occurs, stresses in integration points remain on the yield surface, but the stress components in those points can still change due to movement of the stress state in a point along the yield surface or due to hardening (shift or expansion of the yield surface).

In fact, what I hope to get to with FreeCAD in the future is to analyze structural response from first yield to full plastic collapse. This is what I programmed 30 years ago in a program called Plaxis (see Google) and I am keen to get it done again in the FOSS environment. In addition to an elasto-plastic material model (as already available in CalculiX) it requires automatic scaling of load steps and arc length control (mixed load/displacement control) at limit points. This isn't too hard to program but requires full access to the code (which, having done most of my work in Fortran, I find very tough). PS: on the Calculix page Guido announced a long time ago that he is working on a Riks procedure (= arc length control), but I don't see that back in the code.

Sorry for the long response, but this is a main area of interest for me.
User avatar
HarryvL
Posts: 1010
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM - Tubular Connection with Shell Elements

Postby HarryvL » Sun Feb 18, 2018 9:03 pm

bernd wrote:
Fri Feb 16, 2018 6:46 am

... The question is how to distinguish brtween both.
Bernd,

Although the conclusion is the same, there is a much simpler answer to your question. Under static loading conditions, the plastic strain (and not the stress) determines when the material will fail. The stress-strain curve of the material will tell you what an acceptable plastic strain is (low for a brittle material and high for a ductile material). In a good design, the overall section will yield (and lead to large deflections of the structure) before any material point reaches its plastic strain limit and cracks.

Harry
User avatar
bernd
Posts: 7757
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: FEM - Tubular Connection with Shell Elements

Postby bernd » Tue Feb 20, 2018 4:17 pm

Plaxis, the geotechnical FEA software? We do have one licence here in the office. I am and FreeCAD is too involved to use our CAD software (Nemetschek) to create the geometry for Plaxis (Allplan --> IFC --> FreeCAD --> brep --> Plaxis) ... But that is another story ...

Thanks guys for all your value input in the regard of plasic design :D We may need to disscuss this further on examples.

BTW: FreeCAD FEM has plasic card of CalculiX implemented and can display plastic strain too.

Apart from a few examples I have never done real nonlinear plasic FEA design with concerning plasic stain. Most strucrual engineers normaly only do geometrical nonlinear design. The plasic design is done only with plasic structural steel resistance but not with nonlinear plasic fea analysis. At least here in my region.

Bernd