How to use the pipeline postprocessing
Moderator: bernd
Forum rules
and Helpful information for the FEM forum
and Helpful information for the FEM forum
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.
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: How to use the pipeline postprocessing
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...
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?
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: How to use the pipeline postprocessing
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.
Re: How to use the pipeline postprocessing
... and how about some pre-stressed concrete simulations by using temperature contraction of the steel:
and here the results
-
Of course you can play with the temperature to simulate any pre-stress (Sig_prestress = Alpha * Delta_Temperature * E_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
-
Of course you can play with the temperature to simulate any pre-stress (Sig_prestress = Alpha * Delta_Temperature * E_steel)
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:
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.
Re: How to use the pipeline postprocessing
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.thschrader wrote: ↑Sat Nov 02, 1974 4:10 amMy 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.
BTW wow 9000 antennas.
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.
-
- Veteran
- Posts: 3129
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: How to use the pipeline postprocessing
@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
from ETH-Zürich about this design method. The design they do is a mix of static relevant
parameters (of course) and a intuitive visual method to place the reinforcment in the structure.
And here comes FreeCAD: lets take the numerical linear-elastic analysis of a concrete structure
as a first step. Have a look at the picture. Emil Mörsch had the basic idea. So: if I can visualize
the 3D-"stress-flow" through the body, I am free to define stress fields. In FC, you can add
with boolean-fragments an additional body (the estimated stress field) to the concrete structure
and trigger up the E-modulus. Then re-run the FEM-calculation. In paraview, you can integrate the
stresses to forces for getting the reinforcement. At a first glance, mixing mathematics/statics
with an intuitive approach looks crazy, but thats the idea.
@Harry:
Cool idea to "freeze" the reinforcement for prestressing. Do you know some filter techniques for paraview
to get the stuff I was talking above?