Problem in running lpbf inp in calculix

1

I’m working on a laser powder-based simulation. I successfully ran the simulation in Abaqus and generated an .inp file. I then modified the .inp file to make it compatible with CalculiX. While I resolved all errors, my simulation still doesn’t start when I run CCX. I was solving a simple cube with a substrate. Below is the CCX log output, and I’ve also attached the .inp file. I would greatly appreciate any help in troubleshooting this issue. Looking forward to your responses!

CalculiX Version 2.12, Copyright(C) 1998-2015 Guido Dhondt
CalculiX comes with ABSOLUTELY NO WARRANTY. This is free
software, and you are welcome to redistribute it under
certain conditions, see gpl.htm

You are using an executable made on Tue, Apr 04, 2017 8:38:45 PM

The numbers below are estimated upper bounds

number of:

nodes: 72
elements: 24
one-dimensional elements: 0
two-dimensional elements: 0
integration points per element: 1
degrees of freedom per node: 3
layers per element: 1

distributed facial loads: 0
distributed volumetric loads: 0
concentrated loads: 0
single point constraints: 15
multiple point constraints: 1
terms in all multiple point constraints: 1
tie constraints: 1
dependent nodes tied by cyclic constraints: 0
dependent nodes in pre-tension constraints: 0

sets: 11
terms in all sets: 194

materials: 2
constants per material and temperature: 2
temperature points per material: 1
plastic data points per material: 0

orientations: 0
amplitudes: 6
data points in all amplitudes: 6
print requests: 0
transformations: 0
property cards: 0

STEP 1

Static analysis was selected

(Simulation stops after this, no further run)

2

You are using very old version of CalculiX, I would suggest switching to 2.22. I get this message from it:

 *ERROR in dsort: the number of values to be
        sorted is not positive:            0

Quite generic but I’ve noticed an issue in your input file (not attached here yet but it was attached in your duplicate post in another thread): *TEMPERATURE needs node sets while you are giving it elset names.

1 Like
3

Hi Calc_em, Thanks you very much for your insights. I have now assigned *TEMPERATURE to node sets. I installed newer version 2.22, but i getting this message which you pointed -
*ERROR in dsort: the number of values to be
sorted is not positive: 0

Could you please tell me what this means ? and how to solve it ?

4

Can you share the updated input file ?

5
6

https://drive.google.com/file/d/1KFITgRZMeMePJU-gH8N5HFJzDnFhLwY4/view?usp=drive_link

7

Hi Calc_em, I hope you’re doing well. I just wanted to follow up and check if you had a chance to look into the .inp file I shared. I’d really appreciate any insights you might have found. Thanks again for your help!

8

I can’t access that file. You have to set access to “Anyone with the link” and then copy the link and paste it here.

9
10

Remove the type=node parameter from *TEMPERATURE, this keyword doesn’t have such a parameter. Also, remove the in-line comments starting with exclamation mark. Comments should be placed in new lines and start with double asterisk. But even after fixing those issues, Abaqus indicates wrong element connectivity so you should check your definition of elements (it might be better to use a preprocessor for meshing).

11

I have generated a new simple cube inp of 2 layers from Abaqus now and tried to run with ccx222.exe. There is no error now thrown by ccx222.exe, but simulation is not progressing.
I have made following changes to inp to convert to ccx format. Refer to image.

abaqustoccxconversion
abaqustoccxconversion825×441 11.4 KB

Following is the log -

CalculiX Version 2.22, Copyright(C) 1998-2024 Guido Dhondt
CalculiX comes with ABSOLUTELY NO WARRANTY. This is free
software, and you are welcome to redistribute it under
certain conditions, see gpl.htm

You are using an executable made on Sun Aug 4 19:39:24 2024

The numbers below are estimated upper bounds

number of:

nodes: 27
elements: 8
one-dimensional elements: 0
two-dimensional elements: 0
integration points per element: 27
degrees of freedom per node: 3
layers per element: 1

distributed facial loads: 0
distributed volumetric loads: 0
concentrated loads: 0
single point constraints: 27
multiple point constraints: 1
terms in all multiple point constraints: 1
tie constraints: 0
dependent nodes tied by cyclic constraints: 0
dependent nodes in pre-tension constraints: 0

sets: 18
terms in all sets: 168

materials: 1
constants per material and temperature: 2
temperature points per material: 1
plastic data points per material: 1

orientations: 1
amplitudes: 3
data points in all amplitudes: 3
print requests: 0
transformations: 0
property cards: 0

STEP 1

*INFO reading *STEP: nonlinear geometric
effects are turned on

*INFO reading *DYNAMIC: for implicit calculations
the calculation of the internal energy
is activated.

Dynamic analysis was selected

Nonlinear material laws are taken into account

Newton-Raphson iterative procedure is active

Nonlinear geometric effects are taken into account

INP is attached in this link -

Could you please help me understand why this issue might be occurring?
Also, if you’re available for external consultation over an online call, I’d be happy to formally propose a session with you, if that’s something you’d consider.

12

Hi Calc_em,
Hope you are doing well. I was able to run Abaqus inp into Calculix by making modifications mentioned in the table in previous reply and removing PickedSet6 from Step 1.

But I am getting unexpected result. Below are images for your reference.

image
image1330×474 131 KB

Abaqus INP link -

Our Calculix INP -

I have attached both the abaqus and calculix .inp files for reference. Could you please review them and help me resolve the issue?

13

Is there a reason why you are running this with implicit dynamics?

14

Hi, There is no specific reason, I have tried same with static, result is same.

15

I think this should work with latest ccx:

*Heading
 Test
*Node
  1,  0.,  5., 10.
  2,  0.,  5.,  0.
  3,  0.,  0.,  0.
  4,  0.,  0., 10.
  5, 10.,  5.,  0.
  6, 10.,  0.,  0.
  7, 10.,  0., 10.
  8, 10.,  5., 10.
  9, 10., 10., 10.
 10,  0., 10., 10.
 11, 10., 10.,  0.
 12,  0., 10.,  0.
 13,  0.,  5.,  5.
 14,  0.,  0.,  5.
 15, 10.,  5.,  5.
 16, 10.,  0.,  5.
 17,  5.,  0., 10.
 18,  5.,  5., 10.
 19,  5.,  0.,  0.
 20,  5.,  5.,  0.
 21,  5., 10., 10.
 22,  5., 10.,  0.
 23,  0., 10.,  5.
 24, 10., 10.,  5.
 25,  5.,  5.,  5.
 26,  5.,  0.,  5.
 27,  5., 10.,  5.
*Element, type=C3D8R
  1, 18, 25, 26, 17,  1, 13, 14,  4
  2, 25, 20, 19, 26, 13,  2,  3, 14
  3,  8, 15, 16,  7, 18, 25, 26, 17
  4, 15,  5,  6, 16, 25, 20, 19, 26
  5, 13, 25, 27, 23,  1, 18, 21, 10
  6, 25, 15, 24, 27, 18,  8,  9, 21
  7,  2, 20, 22, 12, 13, 25, 27, 23
  8, 20,  5, 11, 22, 25, 15, 24, 27
*NSET,  NSET=nSet_All, GENERATE
  1,  27,   1
*ELSET, ELSET=elSet_All, GENERATE
 1,  8,  1
*NSET,  NSET=nSet_L1
  1,  2,  3,  4,  5,  6,  7,  8, 
 13, 14, 15, 16, 17, 18, 19, 20,
 25, 26
*ELSET, ELSET=elSet_L1, GENERATE
 1,  4,  1
*NSET,  NSET=nSet_L2
  1,  2,  5,  8,  9, 10, 11, 12,
 13, 15, 18, 20, 21, 22, 23, 24,
 25, 27
*ELSET, ELSET=elSet_L2, GENERATE
 5,  8,  1
*NSET,  NSET=nSet_PickedSet4
  1,  2,  3,  4,  5,  6,  7,  8,
 13, 14, 15, 16, 17, 18, 19, 20,
 25, 26
*ELSET, ELSET=elSet_PickedSet4, GENERATE
 1,  4,  1
*NSET,  NSET=nSet_PickedSet5
  1,  2,  5,  8,  9, 10, 11, 12,
 13, 15, 18, 20, 21, 22, 23, 24,
 25, 27
*ELSET, ELSET=elSet_PickedSet5, GENERATE
 5,  8,  1
*NSET,  NSET=nSet_PickedSet6, GENERATE
  1,  27,   1
*ELSET, ELSET=elSet_PickedSet6, GENERATE
 1,  8,  1
*NSET,  NSET=nSet_PickedSet7
  3,  4,  6,  7, 14, 16, 17, 19, 26
*ELSET, ELSET=elSet_PickedSet7, GENERATE
 1,  4,  1
*NSET,  NSET=nSet_PickedSet8
  1,  2,  3,  4,  5,  6,  7,  8, 
 13, 14, 15, 16, 17, 18, 19, 20,
 25, 26
*ELSET, ELSET=elSet_PickedSet8, GENERATE
 1,  4,  1
*NSET,  NSET=nSet_PickedSet9
  1,  2,  5,  8,  9, 10, 11, 12,
 13, 15, 18, 20, 21, 22, 23, 24,
 25, 27
*ELSET, ELSET=elSet_PickedSet9, GENERATE
 5,  8,  1
** -----------------------
*Orientation, name=Ori_1
1., 0., 0., 0., 1., 0.
 3, 0.
** -----------------------
*MATERIAL, NAME=in718
*DENSITY
 8.146E-09
*ELASTIC
 208000., 0.3
*EXPANSION, TYPE=ANISO
 -0.008,  0.018, -0.008,     0.,     0.,     0.
*PLASTIC
 1170.0, 0.0
 1170.5, 0.002
 1171.0, 0.1
** -----------------------
*SOLID SECTION, ELSET=elSet_PickedSet4, MATERIAL=in718, ORIENTATION=Ori_1
*SOLID SECTION, ELSET=elSet_PickedSet9, MATERIAL=in718
** -----------------------
*INITIAL CONDITIONS, TYPE=TEMPERATURE
nSet_PickedSet6, 0.0
** -----------------------Dummy Step---------------------------
*STEP, NLGEOM=YES
*STATIC, SOLVER=SPOOLES
 1.0, 1.0, 1.E-5, 1.0
*BOUNDARY
nSet_PickedSet7, 1, 3, 0.
*NODE OUTPUT, FREQUENCY=1
U, NT
*ELEMENT OUTPUT, FREQUENCY =1
S 
*NODE FILE
U
*END STEP
** -------------------STEP: Remove top + LayerAct-1 ------------
*STEP, NLGEOM=YES
*STATIC
 0.10, 1.0, 1.E-5, 0.1
*MODEL CHANGE, TYPE=ELEMENT, REMOVE
elSet_PickedSet5
*NODE OUTPUT, FREQUENCY=1
U, NT
*ELEMENT OUTPUT, FREQUENCY =1
S 
*NODE FILE
U
*END STEP
** -------------------STEP: Add Temperature on LayerAct-1 -----------
*STEP, NLGEOM=YES
*STATIC
 0.10, 1.0, 1.E-5, 0.1
*TEMPERATURE
nSet_PickedSet4, 1.
*NODE OUTPUT, FREQUENCY=1
U, NT
*ELEMENT OUTPUT, FREQUENCY =1
S 
*NODE FILE
U
*END STEP
** -------------------STEP: Add LayerAct-2 -----------
*STEP, NLGEOM=YES
*STATIC
 0.10, 1.0, 1.E-5, 0.1
*MODEL CHANGE, TYPE=ELEMENT, ADD=STRAIN FREE
elSet_PickedSet5
*NODE OUTPUT, FREQUENCY=1
U, NT
*ELEMENT OUTPUT, FREQUENCY =1
S 
*NODE FILE
U
*END STEP
** -------------------STEP: Add Temperature on LayerAct-2 -----------
*STEP, NLGEOM=YES
*STATIC
 0.10, 1.0, 1.E-5, 0.1
*TEMPERATURE
nSet_PickedSet5, 1.
*NODE OUTPUT, FREQUENCY=1
U, NT
*ELEMENT OUTPUT, FREQUENCY =1
S 
*NODE FILE
U
*END STEP
16

Hi jbr,
Thank you so much! It worked perfectly! I really appreciate your help and the time you took to look into this. Your support made a big difference—thanks again!

1 Like
18 
 *ERROR in checktemp: no final temperature
        defined in node           18
19

See this: Discrepancy in Results between ccx 2.13 and ccx 2.17 Versions - #4 by Calc_em