Slab and steel column with steel plate

[Zarda]

Hi,

I have some issues with my model in Freecad. I guess that I have done modelling process correctly. But it does not run it neither write inp-file.

I assume that problem is related to subtract and solid body or some thing else..

Could you please have a look on it?

Please click on following link in order to download freecad-model.

https://ufile.io/6xsa2

Regards

Zarda

[bernd]

Hi and welcome to the world of FreeCAD FEM.

- What is your FreeCAD version info? see https://forum.freecadweb.org/viewtopic.php?f=18&t=12212
- to post big FEM modells just clear the mesh. Right click on the mesh clear mesh will clear the mesh. You can than directly attach the file to the forum post.

input file writing runs smooth here. Takes just some time (less than 5 minutes here) CalculiX gives the following error lots of them:

Code: Select all

 *ERROR in calinput: no material was assigned
        to element        12236
 *ERROR in calinput: no material was assigned
        to element        12262

As a fast workaround I added another material object with no reference shape. Which means it will cover all elements without assigned material. With this your file runs. Means you missed to define a material for some part of your geometry. Attached the file with mesh cleared.

cheers bernd

BSP_bhb1.FCStd

(67.87 KiB) Downloaded 46 times

pic.jpg (203.13 KiB) Viewed 1945 times

[bernd]

What would you like to analyse with this model? What is your intention?

[Zarda]

Hi Bernd,

Tanks a lot for a quick reply. I do use Freecad version 17 on windows x64.

I am a structural engineer. This is a practical task, that I want to analyse to see concrete stress under a steel plate incasted into concrete slab. I want to realise the actual scenario. I found freecad a very useful and reliable software. anyway thanks for a try.

I realised my self, that some of geomtry is missing material assign. as I mentioned in my previous post, I doubt about cut functon to form my steel profil, which could properly give some errors. could you recommend a turorial or a video how to draw and make analyse for different material?

Regards

Zarda

[bernd]

try this FEM_Shear_of_a_Composite_Block

I would only define the reference shapes of one material either concrete or steel. If no reference shape is given the material uses all shapes without material for this material.

I'm structural engineer too I assumed you would like to know the real stress distribution under the steel plate. You fixed the plate under the concrete. Is this plate really fixed or is it able to move a mm This could may be make a difference, but I'm not sure.

You should try the vtk post processing filter in FreeCAD FEM. You can cut your model and filter only stress above or under some value and more useful stuff. Keep up posting your results, I'm interested too. I tried similar calculation some month ago but could at the end could just use a bigger and thicker plate at column bottom.

cheers bernd

[Zarda]

Hi,

Interesting

Yes I would look stress distribution under steel plate. I keep trying to perform a model with different materials. when ever my model runs I post the model and results.


Regards
Zarda

[Zarda]

Hi,

I figured out myself how to solve it and fixed 'no assign material' problem!

This model is solved as I desire it with multi materials ( Different materials). I would explain it below.

1- make your geometries as body.
2- Highlight bodies and convert them into Boolean fragments. ( Part >> Split >> Boolean fragments). Remember in property box change to compsolid
3- Highligt Boolean fragments convert to CompoundFilter. ( Part >> compound >> Compound Filter).
4- Highlight CompoundFilter and choose analysis.
5- Highlight CompoundFilter and choose FEM material for solid. Note : You need to repeat this for each solid element you have in model. in this model, There are a steel profile, a steel botton plate, 2 molded steel plates and concrete slab. so I have created and defined 5 individual materials.
6- Define you boundary and loads.
7- mesh and run model..... Enjoy your results.

Some interesting VTK post processing results from this model.

Deformation result

1vtk.PNG (70.84 KiB) Viewed 1761 times

Stress in steel profile, 160-200 MPa

2vtk.PNG (77.44 KiB) Viewed 1761 times

Stress in concrete slab under steel plate. 15-30 MPa

3vtk.PNG (85.48 KiB) Viewed 1761 times

Model file
https://ufile.io/x0rq4

Best regards
Zarda

[gnathan87]

Could I clarify if this is a bug, and if so, if there has been progress on a fix? I'm currently running into this issue with a two-material model on 0.17.13541. The "add a material object with no reference shape" solution removes the errors (and should be fine for my purposes), but seems like the wrong material could get assigned when the erroneous elements are in different parts, and it is inconvenient to have to keep checking the affected nodes manually.

OS: Debian GNU/Linux 8.11 (jessie)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13541 (Git) AppImage
Build type: None
Branch: releases/FreeCAD-0-17
Hash: 9948ee4f1570df9216862a79705afb367b2c6ffb
Python version: 2.7.6
Qt version: 4.8.6
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedKingdom (en_GB)

[bernd]

would you post an example file and give a better explanation what exactly your problem is!

[gnathan87]

Sure, it's exactly the same issue as Zarda was having above. I have attached a sample file, which contains a single tread from a staircase. The model uses a CompSolid BooleanFragments + Compound Filter. The BooleanFragments contains tread and riser objects, the tread being assigned wood and the riser steel. Gmsh works fine but solving with Calculix 2.11 gives rise to multiple errors such as:

*ERROR in calinput: no material was assigned
to element 16756
*ERROR in calinput: no material was assigned
to element 16759
*ERROR in calinput: no material was assigned
to element 16760
...

The errors do not appear if the cut object is removed (taking the holes out of the riser). However, the cut itself is not sufficient to produce the error; it is possible to add cylinders without any errors occuring, and the precise placement of the cylinders also seems makes a difference.

Furthermore, the problem elements do not only occur in the cut object. Where they appear depends on the mesh. Fully automatic grid generation results in all of the problem elements being in the riser:

highlightednodes_default.png (15.67 KiB) Viewed 1460 times

However, setting the maximum element size to (say) 100mm gives problem elements in both the tread and riser:

highlightednodes_100.png (25.17 KiB) Viewed 1460 times

Using a "default material" object does eliminate the errors, but this is clearly problematic if there are a problem elements in parts with different materials.