2.10 vs 2.19 on Windows

I have been using 2.10 on Windows (the bConverged package) and for several test cases get a good correlation between calculix and another tool I have available. When I replace the v2.10 ccx.exe with ccx_static.exe from the 2.19 package I no longer get that good correlation. Am I missing something? Thanks.

Can you say more about these test cases ? What kind of analyses and which type of elements do they involve ? Could share some simplified example showing this behavior ?

I am analysing power poles usually using 5 beam elements to model a tapered solid cylinder. I have pasted an example input file below. Using v2.10 I get displacement at pole tip (node 1) of 365mm. Using a different (linear) method for comparison gives 363mm. Using v2.19 with the same inp file gives 341.

*HEADING
model term_pole
created 25/07/2022 7:10:41 PM

*NODE, NSET=pole_pole1
1,0,0,9700
2,0,0,8730
3,0,0,7760
4,0,0,6790
5,0,0,5820
6,0,0,4850
7,0,0,3880
8,0,0,2910
9,0,0,1940
10,0,0,970
11,0,0,0

*ELEMENT,TYPE=B32, ELSET=EL_pole_pole1
1,1,2,3
2,3,4,5
3,5,6,7
4,7,8,9
5,9,10,11

*DISTRIBUTING COUPLING,ELSET=LOAD1
1,1
*ELSET,ELSET=LOAD1
6
*ELEMENT,TYPE=DCOUP3D
6,12
*NODE
12,0,0,0

*BOUNDARY
11,1,6
*MATERIAL,NAME=material_pole1
*ELASTIC
16500,0.3
*BEAM SECTION,ELSET=EL_pole_pole1,MATERIAL=material_pole1,SECTION=CIRC
300,300
1,0,0
*NODAL THICKNESS
1,240,240
2,248,248
3,256,256
4,264,264
5,272,272
6,280,280
7,288,288
8,296,296
9,304,304
10,312,312
11,320,320

*STEP,NLGEOM
*STATIC
*CLOAD
12,1,7600
12,2,0
*NODE PRINT,NSET=pole_pole1
U
*EL PRINT,ELSET=EL_pole_pole1
S
*NODE FILE
U
*END STEP

right, it seems the latest versions has some problems, definition of non-prismatic beams with *nodal thickness did not working as expected. still using old sectional dimensions, solver did not overwrites.

but, i will try to look up further in other model cases.

I submitted this input file in all the ccx versions currently available for download for Windows. Here are the results (displacement in x direction for node 1):

  • ccx 2.15 - 2.19: 341.43 mm
  • ccx 2.14: 354.48 mm
  • ccx 2.13: 364.66 mm
1 Like

I tried running the same inp file using 2.19 but deleting the *NODAL THICKNESS section and it gives 341. That does appear as if the thicknesses are being ignored.

hi,

i think i found a problem causes, latest version had little bit different at input deck format. you need to add definition at the end of beam section input, please see attachment.

if it’s not defined, the solver not to do overwrites and still using old previous sectional dimension.

best,

1 Like

Thank you. That has solved the problem. I see it says to add that parameter in the ccx 2.19 manual. I didn’t check the new manual.

It now gives the result of 354.48, consistent with Calc_em’s reported result from 2.14.

I am trying to understand the capabilities and limits of ccx vs other calculation methods. Any feedback would be appreciated. The inp file listed in an earlier post is similar to what is used to generate these results, pretty basic.

This is a chart showing deflection against applied load. The 2 ccx versions (2.10 and 2.19) give slightly different results, and both are lower than an external linear method. The deflections for this model are in the linear range.

  1. Why are the 2 ccx versions giving different results?
  2. What is the significance of the different between ccx and the external method?

regarding to discrepancy between of both version, it may due to method or formulation changes in distribution of nodal loads from beam element to 3d expanded element.

you need to do comparison with truly solid element, testing another cases also may help (e.g rectangle section, distributed loads, gravity, curved, modal analysis)

as i understand, 1D beam element use an assumption and approximation for tapered/curved beams . CalculiX use expanded element (solid) which can lead to better results when the model been set up properly. although some differentiation may occurs due knot existence at intersection, node loads and support.

for me, the advantages in uniformity of contact and plasticity may need to considering to judgment element type chosen also.

1 Like

since you’re using dcoup3d element to attach nodal loads, i’m figure out another cause of discrepancy.

circular beam expanded to eight side polygonal shape, i checked with qdis command in CGX 2.19. the area will be smaller about 11% compared to actual, flexure and torsional stiffness also.

quadratic beam element type (reduced or not), large deformation theory and activated, shear deformation also can be another causes.

btw. i’m interested to test non-prismatic beam, but for rectangular section (due to analytical reference document available). long (slender) and short (stocky), using beam, shell and solid element to seen further about discrepancy.

This is another model I am having trouble with. It gives a result when run using 2.10 but using 2.19 the output says convergence at the end but doesn’t give meaningful output in the dat file and gives a message “*ERROR: max. # of increments reached”. It is almost the same as the earlier model but with addition of a truss representing a guy/stay wire from the pole to the ground. I checked the manual for 2.19 and the only item of note was the NODAL THICKNESS issue we discussed before. Any thoughts? Thanks.

*NODE,NSET=Nall
1,0,0,0
2,0,1000,0
3,0,2000,0
4,0,3000,0
5,0,4000,0
6,0,5000,0
7,0,6000,0
8,0,7000,0
9,0,8000,0
10,0,9000,0

12,-7000,0,0

*NODE,nset=poletip
11,0,10000,0
*ELEMENT,TYPE=B32,ELSET=Eall
1,1,2,3
2,3,4,5
3,5,6,7
4,7,8,9
5,9,10,11

** stay wire
*ELEMENT,TYPE=T3D2,ELSET=Stay1
6,10,12
*SOLID SECTION,MATERIAL=Steel_staywire,ELSET=Stay1
** cross section in mm2
42

*BOUNDARY
1,1,6
12,1,3

*MATERIAL,NAME=S2_pole
*ELASTIC
** class S2 timber pole
14000,.37

*MATERIAL,NAME=Steel_staywire
*ELASTIC
** steel
200000,.3
** *NO COMPRESSION

*BEAM SECTION,ELSET=Eall,MATERIAL=S2_pole,SECTION=CIRC,NODAL THICKNESS
** diameter in mm
300.,300.
1.d0,1.d0,0.d0

*NODAL THICKNESS
1,300,300
2,290,290
3,280,280
4,270,270
5,260,260
6,250,250
7,240,240
8,230,230
9,220,220
10,210,210
11,200,200
*STEP,NLGEOM
**STEP
*STATIC
*CLOAD
** load on a node in N
**10kN along line
11,1,10000

** to dat file
** el print at the integration pts
** PRINT request has to have set name

*EL PRINT,elset=Eall
S
*NODE PRINT,NSET=Nall
**RF: Reaction force and moment components
U
RF
*NODE PRINT,NSET=poletip
**RF: Reaction force and moment components
U

** to frd file
** el file at nodes

*NODE File,NSET=Nall
U
RF
*END STEP

in versions 2.19 a 3D output shown all zero values of deflection. but it’s not a problem when requested as 2D output

need a try to the latest versions (v2.20) is this problem exist.

*edited (about convergence issue of truss element in large deformation analysis)

as in my previous test of truss element, without additional rotational restraint along the axis member it will be generate spurious movement around (unrestrained rigid body movement)

you may try using beam with end release, separated nodes with zero length and connected by equation.

using B31R for truss like element may another option for the problems.

Thanks for your comments on this. I have done more tests and the results I get using 2.10 are consistent with results using other methods but the outcomes from 2.19 and 2.20 are either quite different or lead to errors. I don’t know much about FEA or Calculix but there seem to be some changes in later versions. I think I just stick to using 2.10.