I’m working with ccx.2.20 and use ccx_static.
why is for default solver pastix chosen and not spooles like the previous version?
can i change these?
how can i choose spooles as solver if i make *BUCKLING calculation?
*STEP
*BUCKLE
4
I have a problem with cantilever beam and *COUPLING *DISTRIBUTING,
these is not working with pastix 2.20.
is there a possibility to get ccx_2.12 for win?
wbr dichtstoff
I think that it’s because PaStiX is much faster than Spooles and the issues with natural frequency calculations reported in the past should be solved now. However, I’m also somewhat skeptical about this decision.
Try with *BUCKLE, SOLVER=SPOOLES
The oldest version that I’ve found on the official website is 2.13: http://www.dhondt.de/calculix_2.13_4win.zip
ok,
i have checked all versions.
cantilever beam,fixed with
*COUPLING,REF NODE=24863,SURFACE=Ssbound_01,CONSTRAINT NAME=CN1
*DISTRIBUTING
1,1
2,2
3,3
4,4
5,5
6,6
is working with spooles and pastix until version 2.18.4win
result buckling mode with spooles 1.78939
result buckling mode with pastix 2.166570
with 2.19.4win and 2.20.win not working with spooles neither with pastix
or have the input command changed?
wbr
Hi dichtstoff,
¿Could you share your beam BC , material `properties and dimesions?
Maybe we can also check other compilations.
Thanks
i do simplified as
*DISTRIBUTING
1,6
and it seems to be working.
makes no change of the result,
still not working with ccx_2.19.4win and ccx_2.204win
formulation HAS changed: CalculiX: New features in Version 2.20 of CalculiX
I think all versions changes should be available in the documentation. I copied that page from old version from the wayback machine but I think Dhondt should make all available in his website
the problem exist with ccx_2.19.4wind and ccx_2.20.4win
here is an example: it works with ccx_2.18.4win
*NODE, NSET=Nall
1,5.000000000000e-001,-5.000000000000e-001,0.000000000000e+000
2,0.000000000000e+000,-5.000000000000e-001,0.000000000000e+000
3,0.000000000000e+000,-5.000000000000e-001,2.000000000000e+000
4,5.000000000000e-001,-5.000000000000e-001,2.000000000000e+000
5,5.000000000000e-001,0.000000000000e+000,0.000000000000e+000
6,0.000000000000e+000,0.000000000000e+000,0.000000000000e+000
7,0.000000000000e+000,0.000000000000e+000,2.000000000000e+000
8,5.000000000000e-001,0.000000000000e+000,2.000000000000e+000
9,0.000000000000e+000,-5.000000000000e-001,4.000000000000e+000
10,5.000000000000e-001,-5.000000000000e-001,4.000000000000e+000
11,0.000000000000e+000,0.000000000000e+000,4.000000000000e+000
12,5.000000000000e-001,0.000000000000e+000,4.000000000000e+000
13,0.000000000000e+000,-5.000000000000e-001,6.000000000000e+000
14,5.000000000000e-001,-5.000000000000e-001,6.000000000000e+000
15,0.000000000000e+000,0.000000000000e+000,6.000000000000e+000
16,5.000000000000e-001,0.000000000000e+000,6.000000000000e+000
17,0.000000000000e+000,-5.000000000000e-001,8.000000000000e+000
18,5.000000000000e-001,-5.000000000000e-001,8.000000000000e+000
19,0.000000000000e+000,0.000000000000e+000,8.000000000000e+000
20,5.000000000000e-001,0.000000000000e+000,8.000000000000e+000
21,5.000000000000e-001,5.000000000000e-001,0.000000000000e+000
22,0.000000000000e+000,5.000000000000e-001,0.000000000000e+000
23,0.000000000000e+000,5.000000000000e-001,2.000000000000e+000
24,5.000000000000e-001,5.000000000000e-001,2.000000000000e+000
25,0.000000000000e+000,5.000000000000e-001,4.000000000000e+000
26,5.000000000000e-001,5.000000000000e-001,4.000000000000e+000
27,0.000000000000e+000,5.000000000000e-001,6.000000000000e+000
28,5.000000000000e-001,5.000000000000e-001,6.000000000000e+000
29,0.000000000000e+000,5.000000000000e-001,8.000000000000e+000
30,5.000000000000e-001,5.000000000000e-001,8.000000000000e+000
31,-5.000000000000e-001,-5.000000000000e-001,0.000000000000e+000
32,-5.000000000000e-001,-5.000000000000e-001,2.000000000000e+000
33,-5.000000000000e-001,0.000000000000e+000,0.000000000000e+000
34,-5.000000000000e-001,0.000000000000e+000,2.000000000000e+000
35,-5.000000000000e-001,-5.000000000000e-001,4.000000000000e+000
36,-5.000000000000e-001,0.000000000000e+000,4.000000000000e+000
37,-5.000000000000e-001,-5.000000000000e-001,6.000000000000e+000
38,-5.000000000000e-001,0.000000000000e+000,6.000000000000e+000
39,-5.000000000000e-001,-5.000000000000e-001,8.000000000000e+000
40,-5.000000000000e-001,0.000000000000e+000,8.000000000000e+000
41,-5.000000000000e-001,5.000000000000e-001,0.000000000000e+000
42,-5.000000000000e-001,5.000000000000e-001,2.000000000000e+000
43,-5.000000000000e-001,5.000000000000e-001,4.000000000000e+000
44,-5.000000000000e-001,5.000000000000e-001,6.000000000000e+000
45,-5.000000000000e-001,5.000000000000e-001,8.000000000000e+000
*ELEMENT, TYPE=C3D8, ELSET=Eall
1, 1, 2, 3, 4, 5, 6, 7, 8
2, 4, 3, 9, 10, 8, 7, 11, 12
3, 10, 9, 13, 14, 12, 11, 15, 16
4, 14, 13, 17, 18, 16, 15, 19, 20
5, 5, 6, 7, 8, 21, 22, 23, 24
6, 8, 7, 11, 12, 24, 23, 25, 26
7, 12, 11, 15, 16, 26, 25, 27, 28
8, 16, 15, 19, 20, 28, 27, 29, 30
9, 2, 31, 32, 3, 6, 33, 34, 7
10, 3, 32, 35, 9, 7, 34, 36, 11
11, 9, 35, 37, 13, 11, 36, 38, 15
12, 13, 37, 39, 17, 15, 38, 40, 19
13, 6, 33, 34, 7, 22, 41, 42, 23
14, 7, 34, 36, 11, 23, 42, 43, 25
15, 11, 36, 38, 15, 25, 43, 44, 27
16, 15, 38, 40, 19, 27, 44, 45, 29
*NODE, NSET=Nrefrotnode
46,0.000000000000e+000,0.000000000000e+000,0.000000000000e+000
47,0.000000000000e+000,0.000000000000e+000,0.000000000000e+000
** Names based on refnode_01
*NSET,NSET=Nrefnode_01
46,
** Names based on rotnode_01
*NSET,NSET=Nrotnode_01
47,
** Surfaces based on sbound_01
*SURFACE, NAME=Ssbound_01
1, S3
9, S3
5, S3
13, S3
*COUPLING, REF NODE=46, SURFACE=Ssbound_01, CONSTRAINT NAME=CN1
*DISTRIBUTING
1,1
2,2
3,3
4,4
5,5
6,6
*MATERIAL, Name=steel
*ELASTIC
210000, 0.3
*DENSITY
7.86E-9
*SOLID SECTION, Elset=Eall, Material=steel
*STEP
*STATIC, SOLVER=SPOOLES
*BOUNDARY
Nrefnode_01,1,6,0
*DLOAD
Eall,GRAV,9810,0,1,0
*NODE FILE
U
*EL FILE
S
*END STEP
this can not be use anymore for the latest versions. restraint boundary conditions required different approach or methods using dcoup3d element and mean rotations.
That’s what I meant, formulation has changed several times. Check the manual, also v2.19 changed: CalculiX: New features in Version 2.19 of CalculiX
ok,
perfekt, than it is clear. maybe i’ll miss command *DISTRIBUTING with *BOUNDARY
it is in the manual ccx 2.19.
i want to have to control the boundaries with translation and rotation.
So there are now only two possibilities left:
loosing *DISTRIBUTING with *BOUNDARY is a big lost for me.
is there no possibility to preserve the command!?
thnx to all for your help
wbr
Hi ,
First to say is that *COUPLING with *DISTRIBUTING is not even responding with my compilation. It is a CalculiX Version 2.19 + PARDISO with out of core capabilities.
Despite this, we have other options. I have set up the beam with an interesting trick shown in page 3 CTICM LTBeam – Report on Validation Tests July 2002
“Beam elements (BEAM 4) are used at support locations and point load locations in order to stiffen the cross-section and to avoid local buckling effects.”
I’m using a line 2 beam with E=21000 GPa not to exceed the numerical safety boundary on Calculix. Load is directly applied to the node.
Lateral torsion buckling with that set up and without any use of coupling is giving me agreement which is better at some point than the LTB software.
hello,
cantilever beam ist not the problem,
you get the result with *Boundary fixed, or *RIGID BODY,
the challenge is with a beam and two supports.
I started first with shell elements and did the same like you did,
(without knowing these with the beam as support)
i added for the line for web beam elements like dummy rigid, but not in the flange
these work fine for shell elements, for I-Profile but also for U- or C-Profiles.
you get similar results, if you use *RIGID BODY connected with the web
but not so close like beam and shell elements or solid and *COUPLING with *DISTRIBUTING.
here is one example with solids and the results are ok for me, with *COUPLING with *DISTRIBUTING
why not using it!? it is working with solid elements!?
the ulterior motive is, that you can use the buckling mode for pre-deformation for
non-linear calc.
*SHELL SECTION,ELSET=Eflange,MATERIAL=steel
24
*SHELL SECTION,ELSET=Eweb,MATERIAL=steel
12
*BEAM SECTION,ELSET=Eebeam,MATERIAL=steel,SECTION=RECT
500,500
here is a link for download, with solid elements
if you like, you can get also with shell elements
I think your boundary conditions have to be as detailed as your structure’s model. If you model the beam with shells or solids you need to introduce more realistic boundary condition like in this example from Kraska (4 points bending test of sandwich beam with plasticity): CalculiX-Examples/NonLinear/Sandwichtest at master · calculix/CalculiX-Examples · GitHub
why should i use such a complex structure / calculation if i could use a very simple?
Hi and thanks both for your comments,
I will try
It is not working to me.
You can do this with shells too if you previously request the result as OUTPUT=2D. Then transfering displcements from solution to the nodes works as the number of nodes is the same.
-I did it with shells because the Validation file and ANSYS comparison is made with shells in LTBeam Software. I’m using 6400 S4 elements similar to the pdf.
-Shells are lighter and easy to mesh than solids.I prefere if possible.
-The beam trick is new and seems to work fine for me.
-Rigid body doesn’t work well with pure shells .
I also liked your idea of gravity and play with density. Tested but it is not so accurate.
I agree. In this case i tried to follow the same set up as in the pdf for better comparison.
