## How to use the pipeline postprocessing

About the development of the FEM module/workbench.

Moderator: bernd

HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: How to use the pipeline postprocessing

EDIT: Incorrect post deleted
Last edited by HarryvL on Fri May 11, 2018 5:01 pm, edited 1 time in total.
Posts: 1622
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: How to use the pipeline postprocessing

bernd wrote:
Tue May 08, 2018 6:57 pm
I really would like to do this, but I have never seen some practical workflow for day by day usage on simple geometry like the one you posted.
I did a calculation on a simple beam (2500x150x200 mm, loading 100 kN)
Step 1:
Calculation without reinforcement. Export the results to vtk. In paraview use the "threshold" filter
to make the lower tension zone visible. Use "slice"-filter, then "intergrate variables". You get the
resulting Fx-force from the integrated Sxx-stress. In this case 232 kN, wich gives 5 cm^2 reinforcement
for steel with fy=460 MPa.

step 2:
Calculation with one rebar 5 cm^2. You can see that the rebar acts like a "stress-concentrator".
In needed 90 min fore the whole process. With my commercial software you need ten min...
So, for a simple structure like this the workflow is to complicated, but for a more complex structure
this could be a way. I will try this with the concrete-culvert from above. Long weekend...
model.JPG (73.39 KiB) Viewed 502 times
threshold_filter.JPG (65.31 KiB) Viewed 502 times
slice_filter.JPG (79.78 KiB) Viewed 502 times
with_one_rebar.JPG (112.14 KiB) Viewed 502 times
bernd
Posts: 9829
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

### Re: How to use the pipeline postprocessing

do you have commercial software for volume elements FEM or do you mean 10 min with comercial software with beam or shell element analysis?
Posts: 1622
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: How to use the pipeline postprocessing

bernd wrote:
Thu May 10, 2018 5:05 pm
do you have commercial software for volume elements FEM or do you mean 10 min with comercial software with beam or shell element analysis?
No, I have no commercial 3d-FEM volume-element software. Thats why I love FC.
I use software from pcae (www.pcae.de). I do 99% of my calculations with a 3D-beam program
from pcae called 4H-FRAP. In the last 25 years I have calculated more than 9000 antenna-structures
with this program. For these "middle-sized" problems the program is absolutely fast.
pcae sells only 2d-shell/plate solutions (for calculating walls/blankets).
About the ten minutes: pcae has some toolboxes for concrete/wood/steel design.
If I know the maxM (which in this case is easy to calculate "by hand"), I give in the
maxM and get the reinforcement. Thats what i have done in this case.
My opinion: there must be a possibility to set the paraview filters in correct order to get a good
estimation of the reinforcement from the FC-FEM calculation.
pcae1.JPG (39.45 KiB) Viewed 489 times
pcae2.JPG (39.96 KiB) Viewed 489 times
pcae3.JPG (14.77 KiB) Viewed 489 times
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: How to use the pipeline postprocessing

... and how about some pre-stressed concrete simulations by using temperature contraction of the steel:

Code: Select all

``````**Steel thermal expansion coefficient chosen relaistically
*MATERIAL, NAME=SolidMaterial
*ELASTIC
210000, 0.300
*EXPANSION, ZERO=273.
12.0E-06
**Concrete thermal expansion coefficient artificially set at 0.0
*MATERIAL, NAME=SolidMaterial001
*ELASTIC
32000, 0.170
*EXPANSION, ZERO=273.
0.0E-06

*INITIAL CONDITIONS,TYPE=TEMPERATURE
Nall,300.
.........
**Temperature dropped by 50 degrees to shrink steel (concrete coefficient=0.0)
*STEP
*STATIC
*TEMPERATURE
Nall, 250.
``````

and here the results

Pre_Stressed_Beam_Deformation.png (289.37 KiB) Viewed 437 times
-
Pre_Stressed_Beam_Deformation_VM.png (54.69 KiB) Viewed 437 times

Of course you can play with the temperature to simulate any pre-stress (Sig_prestress = Alpha * Delta_Temperature * E_steel)
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: How to use the pipeline postprocessing

If the concrete was infinitely stiff then the temperature reduction would cause a 12E-6 * 50 * 210000 = 126 MPa pre-stress in the steel. However, because the concrete compresses slightly, the effective pre-stress achieved is only 93 MPa:

PSB_x_section.png (277.19 KiB) Viewed 433 times
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: How to use the pipeline postprocessing

By the way, I didn't apply any other loads (e.g. gravity) to the beam for now.
bernd
Posts: 9829
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

### Re: How to use the pipeline postprocessing

Sat Nov 02, 1974 4:10 am
My opinion: there must be a possibility to set the paraview filters in correct order to get a good
estimation of the reinforcement from the FC-FEM calculation.
I do not know of any commercial software nor of a paper which covers such a design method. This was the reason I started with FreeCAD FEM development. But up to know I could not find an workflow to get reasonable results.

BTW wow 9000 antennas.
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

### Re: How to use the pipeline postprocessing

I have an idea on how to do this and am currently studying paraview programmable filters to create an example. Rather show by example than by theory.
Posts: 1622
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

### Re: How to use the pipeline postprocessing

bernd wrote:
Wed May 16, 2018 7:59 am
But up to know I could not find an workflow to get reasonable results.
@Bernd:
The workflow to design concrete structures with stress fields gives reasonable results.
But the workflow is to complicated for daily work "under fire". I have read some papers