Compression Only

[Matej]

@ANYS

When the user define a Spring Stiffness of 1 N/mm how does Prepomax apply it?

If it is a point spring: for each selected node a spring with the given stiffness 1 N/mm is created.
If it is a surface spring: for each node, one spring is defined, and its stiffness is computed in such a way that the sum of all stiffness equals 1N/mm (parallel connection) and that the resulting stress field is constant. So different values of stiffness are applied on the main and mid-side nodes in dependence on the element interpolation functions. So if the user applies a load of 1 N to the component in the spring direction, the displacement of the component will be 1 mm.

@ANYS

Does it happens the same in Spring Support option N/mm?

Probably you are asking for the N/mm^3. The basic idea is the same but the resulting spring stiffness scales with the size of the surface. So if a surface of size 100 mm^2 is used and a displacement of 1 mm is computed, using a surface size of 50 mm^2 one would expect a displacement of 2 mm (if everything works as expected).

[ANYS]

EDITED: I have seen on the other post that you find the problem. I can wait for the next release before asking again.
Thanks.

[Gunnar]

@synt

@synt

Quadratic hexahedral solid element seems not working properly

versioin 1.5.5dev has fixed to this problem,

Can you please upload the pmx file? I wonder why I don’t get it running with 2nd order hexaeder…
Thanks

[synt]

unfortunately the file size is growing big, maybe you can start another ones without CAD imported, simple model as possible.

below another test case of frequency and buckling analysis by simple run, i’m not check further detail or verify the result.

*edited
even solvable, it seems gap element can not work well at this analysis type.

[Gunnar]

@Gunnar

It is noticeable that in the example convergence problems only occur when the lower plate is meshed with 2nd order hex-elements (4). Also the last model (5) with tied contact does not converge.

Okay, the problem is i used the default spring stiffness for all models (1 000 000 000 000 N/mm). With this value, the first 3 models converged, while for the 2nd order hex-models (C3D20), the stiffness needs to be much lower to converge → divided by 10 000 in this case = 100 000 000 N/mm.

Anyhow, tied contact seems to work better at higher stiffness than tie constrain - at least for this example.
While the stiffness of 100 000 000 N/mm worked for tied contact, i get an error with tie constain:

*ERROR: solution seems to diverge; please try
automatic incrementation; program stops
best solution and residuals are in the frd file

[synt]

@Gunnar

Okay, the problem is i used the default spring stiffness for all models (1 000 000 000 000 N/mm). With this value, the first 3 models converged, while for the 2nd order hex-models (C3D20), the stiffness needs to be much lower to converge → divided by 10 000 in this case = 100 000 000 N/mm.

i can not reproduce the problem, it’s solvable using default stiffness and quadratic hexahedral element.

[Gunnar]

Can you please test attached example?

test.zip (114.1 KB)

[synt]

@Gunnar

Can you please test attached example?

not a problem for my model, but i’ll look into attachment of input files.

*edited
not sure why but i guessed is it related to over-constraint condition on model, you can try to add more element layer trough thickness.

[Gunnar]

Here with 3 elements through thickness, makes no different. It only works when i reduce the default spring stiffness as written before

[synt]

that’s specific problem since my model with similarity in load and boundary condition is work.

maybe you can start new file and replicate my model in the same mesh density and feature of tie constraint and rigid body.

*edited
sorry, in previous file the size is large (maybe contains result)

piastra_solid_2moda.pmx (1.9 MB)

[Gunnar]

Thanks for your file, the reason your model converges is because you turned nonlinearities off. For compression only, it must be turned on:

@Matej

Then, in the step properties, the Nlgeom must be turned on (gap elements without the Nlgeom behave as spring elements, and such elements can be used for testing).

[synt]

It has not been notified in CalculiX documentation. Did it mean gap element separation is not working when NLgeom is turned off, it seems not Many case i tested shown different result of spring and gap, deflection and stress increased due to lost in tension spring or uplift occurs. However, i will check further in detail.

[Gunnar]

@Agazzotti

HI
I tried applying the constraint as suggested but the analysis fails.
I tried a further model by generating the horizontal and vertical plate from CAD as the only element so as not to define any constraints between the parts, even the static analysis fails. I can’t resolve the problem. I have always used ver. 1.5.5
piastra_solid_4.pmx (926.3 KB)

For your example you need to reduce the stiffness to 1 000 000 N/mm^2 or less.

Maybe the default value in prepomax should be reduced to make the simulation more stable in general? I just wonder why 1 000 000 000 000 N/mm is chosen as default, especially when even simple models barely converge.

[synt]

i’m still trying to understand how gap element is actually work in CalculiX, it mentions a nonlinear geometry need to be activated.

can it give explains from my simple test case below? both have the same model: left part using surface spring and right part using compression only.

when Nlgeom is turned off. both models should have identical in results, but actually are not. I’m thinking discrepancy due to uplift and lost of tension springs at edge end, probably i can be wrong.

[Matej]

@Gunnar

I just wonder why 1 000 000 000 000 N/mm is chosen as default, especially when even simple models barely converge.

This is the default value given in CalculiX documentation when using Gap elements.

[Matej]

What I found is that using Amplitude with very small angle helps. For the case of the shared file I used:

and got the result with the default gap stiffness:

[ANYS]

I have deactivate NL effects on my balance file used as validation. Due to it’s simplicity I think it can provide some light.

tip displacements result is like this.

Surface Spring NLGEOM / ON = -6.66 mm (Agrees with theoretical value)
Surface Spring NLGEOM / OFF = -6.66 mm (Agrees with theoretical value)

Compression Only Support NLGEOM / ON = -7.50 mm (Agrees with theoretical value)
Compression Only Support NLGEOM / OFF = -13.33 mm (Do not agree with theoretical value)

NLGEOM=OFF uses different Strain meassures.

[synt]

indeed, i’m also observing results of “Compression only” with NLgeom deactivated shown larger than activated. Something that make me lead to wrong interpretation is in behavior and result which similar and reasonable for my simple case above.

unfortunately, NLgeom need to be activated since it can not directly compare due to second order effect (membrane, flexure magnification) and probable in stability. Maybe i can try to ask the possibility in CalculiX forum to eliminate such condition.

[Matej]

Maybe adding a fake Contact card can introduce the nonlinear solution without Nlgeom?

[ANYS]

I think I have a better understanding of the Only Compression Support and it’s weeak points. This is my aproachand and how I have applied it to the file piastra_solid_4.pmx

Use Material Stiffnes as Starting Point *(x5- x50) to obtain the N/mm3 value

Material
E 210 Gpa
Coeficient 5
E= 210,000 [Mpa] N/mm3
Only Compression 1,050,000 N/mm3

Use Only Compression value x expected surface in contact to obtain the N/mm value. Inspect Result and extend as needed

Expected Surface in contact 625 mm2 (25*25 mm2)

Only Compression Stifness 6.6.E+08 N/mm

Avoid adding surfaces in traction inside the support definition to speed up the process.

The process is NLGEOM ON.

EDITED: With new Prepomax even faster. Total CalculiX Time: 0.751970

piastra_solid_4.pmx