Visualizing the model / Errors in node definition

Model setup
1

Hello everybody,

I’ve created an input file. I built the mesh - that is, the nodes and element definitions - myself. So there might be some errors in it (most likely node numbering for element definition). Is there a way to visually inspect the model without having to solve it?

My input actually consists of just one *NODE block and two *ELEMENT blocks. Here are the first few lines of each block:

*NODE, NSET=NALL
1,-5.0,-8.881784197001252e-16,15.0
2,-5.0,5.740251485476346,13.858192987669302
3,-5.0,10.606601717798213,10.606601717798213
4,-5.0,13.858192987669302,5.740251485476348
[....]
*ELEMENT, TYPE=C3D20, ELSET=RING
1,1,929,2529,881,16,1034,2724,926,932,2532,1037,883,928,2209,2727,
2728,4193,4305,2533,4929
2,881,2529,771,145,926,2724,876,160,2533,2534,2728,882,927,4305,2729,
880,4929,2257,775,4259
3,929,930,2530,2529,1034,1035,2725,2724,933,2535,1038,2532,2727,4193,2730,
2731,4194,4929,2536,4930

In any case: To get a visual representation of the model, I tried to solve it by applying a simple boundary condition to the first and last nodes, with displacement set to 0 in all directions.

*MATERIAL, name=steel
*ELASTIC
210000, 0.333
*SOLID SECTION, ELSET=RING, MATERIAL=steel
*STEP
*STATIC
*BOUNDARY
1, 1,3
5312, 1,3
*EL FILE
S
*NODE FILE
U
*END STEP

However, this output in a very strange error, claiming that my Node 1 is undefined (please compare the error below with the excerpt from the node 1 definition above).

You are using an executable made on Sa 28. Mär 15:07:44 CET 2026
 
The numbers below are estimated upper bounds 
 
  number of: 
 
   nodes:         5312 
   elements:         1104 
   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:            6 
   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:            3 
   terms in all sets:        11728 
 
   materials:            1 
   constants per material and temperature:            2 
   temperature points per material:            1 
   plastic data points per material:            0 
 
   orientations:            0 
   amplitudes:            1 
   data points in all amplitudes:            1 
   print requests:            0 
   transformations:            0 
   property cards:            0 
 
 *ERROR reading *NODE. Card image: 
        1,-5.0,-8.881784197001252E-16,15.0 
 
 
 STEP            1 
 
 *ERROR reading *BOUNDARY: 
        node            1  is not defined 
 *ERROR in calinput: at least one fatal 
        error message while reading the 
        input deck: CalculiX stops.

Which I find strange, because at the beginning, in the “number of” section, it lists that it found 5,312 nodes and 1,104 elements—exactly the same number I defined. And a little further down, it seems to have an issue with something in the node definition.

Could it be that I typed an incorrect end-of-line character, or some extra spaces, or something like that?

2

Sounds related to this discussion: Maximum number of characters in a .inp line
I cannot check myself at the moment - could you try reducing the decimals for node 1?

3

I guess it’s just this limitation of the number of decimals: Strange *CLOAD error

But it would be best if you could share the complete input deck to run some tests.

4

Thank you very much, that was exactly what I needed. I’ve now adjusted the file-generation so that the node coordinates are saved in the Python format “:16.9e.” It worked right away.

Does anyone have any advice regarding my first question: Is there a way to view the INP file without having to solve it?

5

Any preprocessor that supports the Abaqus .inp format will do it, e.g. cgx (CalculiX GraphiX).

6

Thank you very much. I’ve tried several times to load the .inp file using CGX, but I kept getting different error messages each time. On my third attempt, I found in the help section that there’s a -c flag. This allows the .inp file to be displayed.

1 Like
7

Sometimes you may also want to use the *NO ANALYSIS keyword to perform a quick check run. This allows you to look for errors and visualize 1D/2D element sections, among others.

1 Like
8

Thank you very much; I’ll give that a try. According to the help section, it also checks the Jacobi determinants, which can be extremely helpful if I accidentally have a twist in the indexing of the mid-nodes. That’s not always easy to spot from pure visuals.

9

cgx also has a viewing option “Show bad elements”, which checks the Jacobians.