# Lateral-torsional buckling

**URL:** <https://calculix.discourse.group/t/lateral-torsional-buckling/697>\
**Category:** Uncategorized\
**Created:** [August 25, 2021, 9:27am UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697 "2021-08-25T09:27:02Z")\
**Posts on this page:** 14\
**Page:** 1

<div class="post-metadata">

**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\
**Post date:** [August 25, 2021, 9:27am UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/1 "2021-08-25T09:27:02Z")

</div>

Hi,

I’m trying to analyze a cantilever beam with a narrow rectangular cross-section subjected to lateral-torsional buckling. The beam is fixed at one end and the top edge of the opposite end has a rigid body constraint applied. The reference point for this constraint is located in the middle of this edge and concentrated force is applied to it:

 ![bar](https://global.discourse-cdn.com/free1/uploads/calculix/original/1X/ffba6d257f5236cc62db0694573f020ef4b5e2bf.png)  
This approach works fine in Abaqus but I can’t make it run successfully in CalculiX. I don’t get any specific errors, there are just on results.

Do you know what could be wrong here and how I should proceed with this simulation in CalculiX ?

---

<div class="post-metadata">

**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\
**Post date:** [August 25, 2021, 10:35am UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/2 "2021-08-25T10:35:27Z")

</div>

Hello,

a local single load could be a problem sometimes.  
maybe you change with self weight,  
\*DLOAD and \*DENSITY

or you use the area instead one single point  
\*RIGID BODY

If you need some example with lateral torsional buckling, let me know.

wbr

---

<div class="post-metadata">

**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\
**Post date:** [August 25, 2021, 10:45am UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/3 "2021-08-25T10:45:12Z")

</div>

beam-3D.fbd

PNT P001 -50 -50 0  
SETA P001 p P001  
SWEP P001 L001 tra 100  
SETA L001 l L001  
SWEP L001 A001 tra 0 100 0  
SETA A001 s A001  
COMP A001 d  
SWEP A001 B001 tra 0 0 1000 20  
#DIV all mult 10  
ELTY all HE20  
MESH all  
SEND all abq  
SEND A001 abq nam  
prnt se  
view elem

beam-3D.inp

\*INCLUDE, INPUT=all.msh  
\*INCLUDE, INPUT=A001.nam

\*MATERIAL, Name=steel  
\*ELASTIC  
210000,0.3  
\*DENSITY  
7.86E-9

\*SOLID SECTION, Elset=Eall, Material=steel

\*STEP

\*\*\*STATIC  
\*BUCKLE  
4

\*BOUNDARY  
NA001,1,3,0

\*DLOAD  
Eall,P4,1

\*NODE FILE, OUTPUT=3D  
U,

\*EL FILE  
S,

\*NODE PRINT,NSET=NA001,totals=only  
RF

\*END STEP

 ![image](https://global.discourse-cdn.com/free1/uploads/calculix/original/1X/3063d924779dca4a22d8ee98cfad9e5e6ac5ece0.png)

---

<div class="post-metadata">

**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\
**Post date:** [August 25, 2021, 10:57am UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/4 "2021-08-25T10:57:10Z")

</div>

Thank you very much for your reply. The thing is that I want to model it in such a way that I can verify the results using analytical solution. And that solution assumes force acting only on the top edge of the beam. But maybe load applied to some narrow surface split from the top face of the beam will work in this case, I will definitely give it a try and let you know if it helped.

Regardless of the approach that I will use for this problem, I also wonder why the results can’t be obtained when load is applied via rigid body constraint only to the edge. Is that some kind of a bug in ccx ?

---

<div class="post-metadata">

**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\
**Post date:** [August 25, 2021, 11:25am UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/5 "2021-08-25T11:25:46Z")

</div>

If i work with buckling modes in ccx,  
i use ccx only in ST, not in MT.  
all my examples are working with analytical solutions.  
Somtimes the user is the bug.

wbr

---

<div class="post-metadata">

**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\
**Post date:** [August 25, 2021, 12:01pm UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/6 "2021-08-25T12:01:32Z")

</div>

It doesn’t run on a single cpu as well but it’s good to know that parallel processing may not be a good idea for linear buckling analyses. Can you share some more tips regarding this type of simulations in CalculiX ? For example, which types of elements, loads and constraints (rigid body, coupling) to use and which to avoid. Do you get good agreement with analytical values ? So far all linear buckling simulations that I performed in CalculiX (even the one with a simple column fixed at one end and subjected to axial compression) predicted critical loads with rather small accuracy when compared with analytical values. Mesh refinement didn’t help as well. Maybe you could share some additional examples of buckling analyses ?

I tried with load applied to small surface separated from the top face of the beam and the simulation was completed but the results were completely incorrect.

Sure, normally I would suspect my fault first but in this case settings are the same as in other software (Abaqus, Fusion 360) where the analysis works. That’s the only reason why I thought that it might be a bug in CalculiX.

P.S. In buckling simulations I sometimes get some strange local buckling instead of a global buckling mode for selected meshes. It’s probably caused by small defects in tetrahedral meshes generated by Netgen, right ?

---

<div class="post-metadata">

**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\
**Post date:** [August 25, 2021, 8:11pm UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/7 "2021-08-25T20:11:10Z")

</div>

I have done buckling modes with I-Profile, U-Profile and C-Profile.  
All of them are working with lateral-, torsional and lateral torsional buckling.  
They work with solid but also possible with shell elements.

But there is a problem, that LTB is working with solid elements  
only  
if you use \*COUPLING with \*DISTRIBUTING, see examples.

For solid elements with LTB:

\*SOLID ELEMENTS  
\*Hexahedra (cube) (linear)  
\*ST  
\*COUPLING \*DISTRIBUTING

I have posted these issue (problem) years ago, but there was no response.  
I prefer to work with \*rigid body by nonlinear calc. with predeformation and nonlinear material.

---

<div class="post-metadata">

**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\
**Post date:** [August 25, 2021, 8:12pm UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/8 "2021-08-25T20:12:45Z")

</div>

I-profile\_solid.fbd

## lateral torsional buckling

## I-profile with solid elements

valu h 448  
valu b 400  
valu tw 12  
valu tf 24  
valu tp 24  
valu \_length 11000  
valu factor 0.5  
valu -factor -0.5  
valu bstern \* b factor  
valu -bstern \* b -factor  
valu hstern \* h factor  
valu -hstern \* h -factor  
valu twstern \* tw factor  
valu -twstern \* tw -factor  
valu d - hstern tf  
valu tp2 / tp factor  
valu lengthnetto - \_length tp2  
valu length1 - \_length tp  
valu aoeb 220  
valu aoew 4  
valu aoef 4  
valu aoet 0.25

pnt D001 0 -twstern 0  
pnt D002 d -twstern 0  
pnt D003 d twstern 0  
pnt D004 0 twstern 0  
pnt D005 hstern -twstern 0  
pnt D006 hstern twstern 0  
pnt D007 d -bstern 0  
pnt D008 hstern -bstern 0  
pnt D009 hstern bstern 0  
pnt D010 d bstern 0

line L001 D001 D002 aoew  
line L002 D002 D003  
line L003 D003 D004 aoew  
line L004 D004 D001

line L005 D002 D005  
line L006 D005 D006  
line L007 D006 D003

line L008 D002 D007 aoef  
line L009 D007 D008  
line L010 D008 D005 aoef

line L011 D006 D009 aoef  
line L012 D009 D010  
line L013 D010 D003 aoef

gsur A001 + BLEND + L001 + L002 + L003 + L004  
gsur A002 + BLEND + L005 + L006 + L007 - L002  
gsur A003 + BLEND + L008 + L009 + L010 - L005  
gsur A004 + BLEND + L011 + L012 + L013 - L007

seta ldiv2 L002 L004 L005 L006 L007 L009 L012  
div ldiv2 mult aoet

seta ldivtw L001 L003 L014 L017  
seta ldivtf L008 L010 L011 L013

seta sketch1 s all  
swep sketch1 volume1 tra 0 0 \_length aoeb

copy all beam mir x

merg p all  
merg l all  
merg s all

elty all HE8  
mesh all

#### RIGID BODY

seta rigidbody\_01 p D001  
seta rigidbody\_02 p D00D  
copy rigidbody\_01 refnode\_01 tra 0 twstern  
copy refnode\_01 rotnode\_01 tra  
copy rigidbody\_02 refnode\_02 tra 0 -twstern  
copy refnode\_02 rotnode\_02 tra  
seta refrotnode se refnode\_01 rotnode\_01  
seta refrotnode se refnode\_02 rotnode\_02  
setr all se refrotnode

#### RIGID BODY

seta sbound\_01 s A001 A002 A003 A004  
seta sbound\_01 s A00M A00N A00O A00P  
comp sbound\_01 down  
comp sbound\_01 down

seta sbound\_02 s A005 A006 A007 A008  
seta sbound\_02 s A00Q A00R A00S A00T  
comp sbound\_02 down  
comp sbound\_02 down

send all abq  
send refrotnode abq  
send sbound\_01 abq nam  
send sbound\_02 abq nam  
send sbound\_01 abq sur  
send sbound\_02 abq sur  
send refnode\_01 abq nam  
send refnode\_02 abq nam  
send rotnode\_01 abq nam  
send rotnode\_02 abq nam

prnt se  
plot e all  
view elem  
plot n sbound\_01 b  
plus n sbound\_02 y  
plus na refnode1 m  
plus na rotnode2 m

---

<div class="post-metadata">

**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\
**Post date:** [August 25, 2021, 8:13pm UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/9 "2021-08-25T20:13:56Z")

</div>

I-profile\_cd.inp

\*\*\*\* proof of lateral buckling by nonlinear geometric calculation  
\*\*\*\* example: TUHH STAHLBUA III BEULEN, TORSION, BIEGEDRILLKNICKEN p.33-37  
\*\*\*\* [Stahlbau III](https://www.yumpu.com/de/document/view/3436719/stahlbau-iii)

\*HEADING  
Model: ltb\_I-profile\_cd

\*\*\*\* centric pressure:  
\*\*\*\* lateral buckling: 4.385,0 ccx: 4.405,0  
\*\*\*\* lateral buckling: 15.877,0 ccx: 15.186,0  
\*\*\*\* torsional buckling: 10.427,0 ccx: 10.258,0  
\*\*\*\* bending moment:  
\*\*\*\* lateral torsional buckling: 1.502,0 ccx: 1.504,0

\*INCLUDE, INPUT=all.msh  
\*INCLUDE, INPUT=refrotnode.msh  
\*INCLUDE, INPUT=sbound\_01.nam  
\*INCLUDE, INPUT=sbound\_02.nam  
\*INCLUDE, INPUT=sbound\_01.sur  
\*INCLUDE, INPUT=sbound\_02.sur  
\*INCLUDE, INPUT=refnode\_01.nam  
\*INCLUDE, INPUT=refnode\_02.nam  
\*INCLUDE, INPUT=rotnode\_01.nam  
\*INCLUDE, INPUT=rotnode\_02.nam

\*COUPLING,REF NODE=11935,SURFACE=Ssbound\_01,CONSTRAINT NAME=CN1  
\*DISTRIBUTING  
1,1  
2,2  
3,3  
4,4  
5,5  
6,6

\*COUPLING,REF NODE=11937,SURFACE=Ssbound\_02,CONSTRAINT NAME=CN2  
\*DISTRIBUTING  
1,6

\*MATERIAL, Name=steel

\*ELASTIC  
210000,0.3

\*DENSITY  
7.86E-9

\*SOLID SECTION, Elset=Eall, Material=steel

\*STEP

\*BUCKLE  
8

\*BOUNDARY  
Nrefnode\_01,1,3,0  
Nrefnode\_01,6,6,0  
Nrefnode\_02,1,2,0  
Nrefnode\_02,6,6,0

\*\*\*\*BUCKLING  
\*CLOAD

\*\*\*\*CENTRIC PRESSURE  
\*\*Nrefnode\_02,3,-1000  
\*\*\*\*CENTRIC PRESSURE

\*\*\*\*BENDING MOMENT  
Nrefnode\_01,5, 1000000  
Nrefnode\_02,5,-1000000  
\*\*\*\*BENDING MOMENT

\*NODE PRINT,NSET=Nsbound\_01,totals=only  
RF

\*NODE PRINT,NSET=Nsbound\_02,totals=only  
RF

\*NODE PRINT,NSET=Nrefnode\_01,totals=only  
RF

\*NODE PRINT,NSET=Nrefnode\_02,totals=only  
RF

\*NODE PRINT,NSET=Nrotnode\_01,totals=only  
RF

\*NODE PRINT,NSET=Nrotnode\_02,totals=only  
RF

\*NODE FILE  
U

\*EL FILE  
S

\*END STEP

I-profile\_rb.inp

\*\*\*\* proof of lateral buckling by nonlinear geometric calculation  
\*\*\*\* example: TUHH STAHLBUA III BEULEN, TORSION, BIEGEDRILLKNICKEN p.33-37  
\*\*\*\* [Stahlbau III](https://www.yumpu.com/de/document/view/3436719/stahlbau-iii)

\*HEADING  
Model: ltb\_I-profile\_rb

\*\*\*\* centric pressure:  
\*\*\*\* lateral buckling: 4.385,0 ccx: 4.381,0  
\*\*\*\* lateral buckling: 15.877,0 ccx: 15.224,0  
\*\*\*\* torsional buckling: 10.427,0 ccx: -,-  
\*\*\*\* bending moment:  
\*\*\*\* lateral torsional buckling: 1.502,0 ccx: 2.479,0

\*INCLUDE, INPUT=all.msh  
\*INCLUDE, INPUT=refrotnode.msh  
\*INCLUDE, INPUT=sbound\_01.nam  
\*INCLUDE, INPUT=sbound\_02.nam  
\*INCLUDE, INPUT=refnode\_01.nam  
\*INCLUDE, INPUT=refnode\_02.nam  
\*INCLUDE, INPUT=rotnode\_01.nam  
\*INCLUDE, INPUT=rotnode\_02.nam

\*RIGID BODY,NSET=Nsbound\_01,REF NODE=11935,ROT NODE=11936  
\*RIGID BODY,NSET=Nsbound\_02,REF NODE=11937,ROT NODE=11938

\*MATERIAL, Name=steel

\*ELASTIC  
210000,0.3

\*DENSITY  
7.86E-9

\*SOLID SECTION, Elset=Eall, Material=steel

\*STEP

\*BUCKLE  
6

\*BOUNDARY  
Nrefnode\_01,1,3,0  
Nrotnode\_01,3,3,0  
Nrefnode\_02,1,2,0  
Nrotnode\_02,3,3,0

\*\*\*\*BUCKLING  
\*CLOAD

\*\*\*\*CENTRIC PRESSURE  
\*\*Nrefnode\_02,3,-1000  
\*\*\*\*CENTRIC PRESSURE

\*\*\*\*BENDING MOMENT  
Nrotnode\_01,2, 1000000  
Nrotnode\_02,2,-1000000  
\*\*\*\*BENDING MOMENT

\*NODE PRINT,NSET=Nsbound\_01,totals=only  
RF

\*NODE PRINT,NSET=Nsbound\_02,totals=only  
RF

\*NODE PRINT,NSET=Nrefnode\_01,totals=only  
RF

\*NODE PRINT,NSET=Nrefnode\_02,totals=only  
RF

\*NODE PRINT,NSET=Nrotnode\_01,totals=only  
RF

\*NODE PRINT,NSET=Nrotnode\_02,totals=only  
RF

\*NODE FILE  
U

\*EL FILE  
S

\*END STEP

I-profile\_ck.inp

\*\*\*\* proof of lateral buckling by nonlinear geometric calculation  
\*\*\*\* example: TUHH STAHLBUA III BEULEN, TORSION, BIEGEDRILLKNICKEN p.33-37  
\*\*\*\* [Stahlbau III](https://www.yumpu.com/de/document/view/3436719/stahlbau-iii)

\*HEADING  
Model: ltb\_I-profile\_ck

\*\*\*\* centric pressure:  
\*\*\*\* lateral buckling: 4.385,0 ccx: 4.381,0  
\*\*\*\* lateral buckling: 15.877,0 ccx: 15.224,0  
\*\*\*\* torsional buckling: 10.427,0 ccx: -,-  
\*\*\*\* bending moment:  
\*\*\*\* lateral torsional buckling: 1.502,0 ccx: 2.479,0

\*INCLUDE, INPUT=all.msh  
\*INCLUDE, INPUT=refrotnode.msh  
\*INCLUDE, INPUT=sbound\_01.nam  
\*INCLUDE, INPUT=sbound\_02.nam  
\*INCLUDE, INPUT=sbound\_01.sur  
\*INCLUDE, INPUT=sbound\_02.sur  
\*INCLUDE, INPUT=refnode\_01.nam  
\*INCLUDE, INPUT=refnode\_02.nam  
\*INCLUDE, INPUT=rotnode\_01.nam  
\*INCLUDE, INPUT=rotnode\_02.nam

\*COUPLING,REF NODE=11935,SURFACE=Ssbound\_01,CONSTRAINT NAME=CN1  
\*KINEMATIC  
1,3  
1,3

\*COUPLING,REF NODE=11937,SURFACE=Ssbound\_02,CONSTRAINT NAME=CN2  
\*KINEMATIC  
1,3  
1,3

\*MATERIAL, Name=steel

\*ELASTIC  
210000,0.3

\*DENSITY  
7.86E-9

\*SOLID SECTION, Elset=Eall, Material=steel

\*STEP

\*BUCKLE  
8

\*BOUNDARY  
Nrefnode\_01,1,3,0  
Nrefnode\_01,6,6,0  
Nrefnode\_02,1,2,0  
Nrefnode\_02,6,6,0

\*\*\*\*BUCKLING  
\*CLOAD

\*\*\*\*CENTRIC PRESSURE  
\*\*Nrefnode\_02,3,-1000  
\*\*\*\*CENTRIC PRESSURE

\*\*\*\*BENDING MOMENT  
Nrefnode\_01,5, 1000000  
Nrefnode\_02,5,-1000000  
\*\*\*\*BENDING MOMENT

\*NODE PRINT,NSET=Nsbound\_01,totals=only  
RF

\*NODE PRINT,NSET=Nsbound\_02,totals=only  
RF

\*NODE PRINT,NSET=Nrefnode\_01,totals=only  
RF

\*NODE PRINT,NSET=Nrefnode\_02,totals=only  
RF

\*NODE PRINT,NSET=Nrotnode\_01,totals=only  
RF

\*NODE PRINT,NSET=Nrotnode\_02,totals=only  
RF

\*NODE FILE  
U

\*EL FILE  
S

\*END STEP

---

<div class="post-metadata">

**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\
**Post date:** [August 25, 2021, 9:01pm UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/10 "2021-08-25T21:01:00Z")

</div>

Thank you very much, I finally managed to obtain good results for my LTB model using this approach with narrow surface separated from the top of the beam. And I used rigid body constraint to apply load so apparently it can help in some cases. The preprocessor that I use doesn’t have coupling constraints and I would have to define them manually. But it’s good to know that they work well in LBA.

However, there’s still that issue with some local buckling showing up instead of global buckling modes. It happens when I prepare and run the analysis with identical settings (including meshing parameters) a few times. I suspect that this is caused by the fact that the tetrahedral mesh from Netgen is not identical each time and there are some small differences in nodal coordinates that form something like imperfections. Have you encountered this issue in your studies ? Or do you not use this kind of mesh ?

---

<div class="post-metadata">

**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\
**Post date:** [August 25, 2021, 9:27pm UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/11 "2021-08-25T21:27:08Z")

</div>

If i have a structure like beam with solid ( or shell)  
it is always better to use hexahedra elements,  
because with tetrahedron the beam could get to “stiffness”.  
you have to realy take care, if you use tetrahedron with beam properties.  
Try one beam with hex and one with tehtr, and the deflection is different.  
these has maybe also influence of your buckling modes.  
I have also tried to put in middle nodes with the mesh of netgen,  
to change from linear to higher order elements, but it had no influence.  
i like to work with ccx(, or salome or gmesh) to build your fem mesh.  
you can change quick elements and geometry and so on.  
at beginning it is wasting time, but with every example you can paste & copy.

here is link for download:

> **[Ihr persönlicher Freigabelink | GMX Cloud](https://c.gmx.net/@324820432001700943/oSWS-B9iQyG2GF0zvoLHGg)**
>
> Mit diesem Link erhalten Sie Zugriff auf die mit Ihnen geteilten Daten.

feel free to ask, but give back your knowledge to the community.

wbr

---

<div class="post-metadata">

**Author:** ![Calc\_em](https://avatars.discourse-cdn.com/v4/letter/c/43a26b/32.png) [@Calc\_em](https://calculix.discourse.group/u/Calc_em)\
**Post date:** [August 25, 2021, 9:39pm UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/12 "2021-08-25T21:39:43Z")

</div>

Thanks again. I really appreciate your support. And the examples that you share here will definitely help me gain experience with LBA in ccx.

The fact that tetrahedral elements overstiffen the model is one thing but I’m really surprised that their generation (at least with Netgen) can be inaccurate enough to cause such problems in buckling analyses. It happens so often that for some scenarios I get meaningless results more times than the correct ones.

---

<div class="post-metadata">

**Author:** ![vicmw](https://avatars.discourse-cdn.com/v4/letter/v/6de8d8/32.png) [@vicmw](https://calculix.discourse.group/u/vicmw)\
**Post date:** [August 26, 2021, 3:16am UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/13 "2021-08-26T03:16:07Z")

</div>

Regarding local buckling modes, some buggy version of CCX are around that cause that or what can look like that. To make sure:

- As Dichtstoff said, don’t use the multithreaded SPOOLES solver for buckling. It causes random errors in mode shapes and buckling factors.
- Check that it can find modes below a buckling factor of 1. They’re excluded in some versions.

Otherwise, if the modes are jumping around that much with re-meshing, it might be too mesh sensitive and in need of refinement. Or the local modes might be too close to the global modes so they switch places sometimes, which is not really wrong.

Tetrahedron elements have a bad reputation but they’re not qualitatively wrong, just less efficient so they require a finer mesh for similar accuracy. They are overstiff in bending but as you refine the mesh, bending of individual elements becomes less significant and the error should approach zero.

Here’s a mesh convergence study for lateral torsional buckling with 4 different elements shapes. Tet meshes generated with Netgen. You can see that 4-node tet is utterly useless but does seem to converge to the correct value. Just use 10-node tets instead.

 ![buckling_elements](https://global.discourse-cdn.com/free1/uploads/calculix/original/1X/5b5d9fcfd59ca50171001525d16a9567830fba5d.png)

---

<div class="post-metadata">

**Author:** ![dichtstoff](https://avatars.discourse-cdn.com/v4/letter/d/dec6dc/32.png) [@dichtstoff](https://calculix.discourse.group/u/dichtstoff)\
**Post date:** [August 26, 2021, 7:29am UTC](https://calculix.discourse.group/t/lateral-torsional-buckling/697/14 "2021-08-26T07:29:14Z")

</div>

The support has also an influence of the buckling modes!?  
how you see with the example?  
Only with \*COUPLING \*DISTRIBUTION you get exact results  
with \*RIGID BODY and \*COUPLING \*DISTRIBUTION seems to stiffness!?

how you get 10-node Tetrahedron elements with netgen?  
i always tried, but don’t get it! ☹  
thnx