Request for help with Analysis and Constraints

[thschrader]

...
The one area I struggled with was introducing the mesh regions _ I just couldn't figure out how to get them into the analysis tree??
...

Put all parts in a Compound, with Part-wb "Make Compound" (BooleanFragments Mode=CompSolid!)
Generate the basic mesh.
Select mesh in modell tree, press refinement button.
In refinement-dialog, select the region to refine (line, face or solid).
Remesh body.
You can define more than one refinement-zone.

mesh_refine1.JPG (127.29 KiB) Viewed 1465 times

mesh_refine2.JPG (115.28 KiB) Viewed 1465 times

[thschrader]

...
Nevertheless I didn't like the look of those "hot-spots" in the top corners of the tube pockets and felt I could alleviate them by introducing curves into the pocket corners and chamfers to the top edges of the brick.
...

Rounding the corners in the tube opening doesnt help, still excessive stress
in the corner (10 kN loading). The color-plot is cut of at 235 MPa, peak-stress is 1700 MPa, red zones.
A linear-elastic analysis gives the result, that your part breaks. Which is not true.
Your part is a good example why @harryvl recommends a plastic analysis with
max plastic strain as design parameter.

peak_stress_vMises.JPG (25.52 KiB) Viewed 1446 times

[thschrader]

Plastic analysis with Steel S235 sigma/strain curve.
max sigma v.Mises now 283 MPa, max equivalent plastic strain 1% < 5% ==> ok.
Convergence is poor, ccx needs 1000 seconds

Converter_10kN_plastic.FCStd

(77.3 KiB) Downloaded 33 times

[Laurie Hartley]

@thschrader thanks yet again for your three posts Thomas. Subjects for further investigation next week;

Mesh regions
Plastic strain and
convergence?

I will try to reproduce your latest file after I have downloaded it and examined it.

I must admit I was surprised the curves made little difference which just goes to show you are never too old to learn

Nevertheless going by your numbers this design is more than adequate for what I have in mind.

[Laurie Hartley]

@thschrader Thomas I was able to take a quick look at your file today - it looked a bit strange when I opened it? See screenshot. Did you change the pocket size or has something happened during transit?

Nevertheless I was able to run the mesh and calculix successfully - it took about 6000 seconds.

[thschrader]

Did you change the pocket size or has something happened during transit?

I shortened the tube/block length to reduce FEM-cell count.

Nevertheless I was able to run the mesh and calculix successfully - it took about 6000 seconds.

6000 sec is definitely too long. Strange.
I will have a look at it.

[thschrader]

Reduced model size, changed mesh-refinement.
Runtime now 250 sec plastic analysis on intel i5 cpu.
I played with different yield-curves (S235 and S460).
There is no relevant difference in runtime.

Result:
S235 PEEQ=2,4% < 5
S460 PEEQ=1,4% < 5
PEEQ=equivalent plastic strain.
No need to use high grade steel and waste money.

test-files:

stress_elastic.FCStd

(101.26 KiB) Downloaded 33 times

stress_plastic.FCStd

(101.66 KiB) Downloaded 34 times

[Laurie Hartley]

Reduced model size, changed mesh-refinement.
Runtime now 250 sec plastic analysis on intel i5 cpu.

Your results are encouraging.
I tried to reproduce your model from scratch - obviously unsuccessful. I was warned - see screenshot. It produce a mesh after about 600 seconds and the CPU running at about 80% capacity (AMD Ryzen 7 3700)
Can you see where I have gone wrong please?

[HarryvL]

Result:
S235 PEEQ=2,4% < 5
S460 PEEQ=1,4% < 5
PEEQ=equivalent plastic strain.
No need to use high grade steel and waste money.

A few comments:

1) If the load is cyclic (repeated loading/unloading) then it becomes important to also consider stress itself and apply a Miner-type failure criterion.
2) High grade steel is actually more brittle and therefore not only a waste of money, but also more prone to ductile cracking/failure.
3) The 5% limit strain is just a rule of thumb and under high triaxial tension it may be non-conservative. It is therefore better to use the latest FreeCAD version and let it calculate the critical strain ratio. I ran the analysis and find a critical strain ratio of 0.591, which is lower than 1, but still quite high. However, considering the safety factor of 1.5 perhaps acceptable for STATIC loading:

Screenshot from 2022-10-20 11-56-21.png (162.19 KiB) Viewed 1096 times

[thschrader]

...
Can you see where I have gone wrong please?

You must upgrade the Boolean-Fragments to a Compound.
This works with part-wb (button or Part/Compound/Make Compound)
Be sure that the Boolean-Fragment Mode is "CompSolid".
After that, you must re-attach the mesh to the compound, otherwise the meshing-error remains.
Re-attach force and fixings to compound too.

Or: use a simple part-fusion body

compound.JPG (40.3 KiB) Viewed 1061 times