How to use the pipeline postprocessing

About the development of the FEM module/workbench.

Moderator: bernd

User avatar
HarryvL
Posts: 941
Joined: Sat Jan 06, 2018 7:38 pm

Re: How to use the pipeline postprocessing

Postby HarryvL » Wed May 09, 2018 9:13 pm

EDIT: Incorrect post deleted
Last edited by HarryvL on Fri May 11, 2018 5:01 pm, edited 1 time in total.
thschrader
Posts: 1380
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: How to use the pipeline postprocessing

Postby thschrader » Thu May 10, 2018 2:19 pm

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
model.JPG (73.39 KiB) Viewed 298 times
threshold_filter.JPG
threshold_filter.JPG (65.31 KiB) Viewed 298 times
slice_filter.JPG
slice_filter.JPG (79.78 KiB) Viewed 298 times
with_one_rebar.JPG
with_one_rebar.JPG (112.14 KiB) Viewed 298 times
User avatar
bernd
Posts: 7289
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: How to use the pipeline postprocessing

Postby bernd » 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?
thschrader
Posts: 1380
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: How to use the pipeline postprocessing

Postby thschrader » Thu May 10, 2018 5:41 pm

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
pcae1.JPG (39.45 KiB) Viewed 285 times
pcae2.JPG
pcae2.JPG (39.96 KiB) Viewed 285 times
pcae3.JPG
pcae3.JPG (14.77 KiB) Viewed 285 times
User avatar
HarryvL
Posts: 941
Joined: Sat Jan 06, 2018 7:38 pm

Re: How to use the pipeline postprocessing

Postby HarryvL » Wed May 16, 2018 4:31 am

... 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
Pre_Stressed_Beam_Deformation.png (289.37 KiB) Viewed 233 times
-
Pre_Stressed_Beam_Deformation_VM.png
Pre_Stressed_Beam_Deformation_VM.png (54.69 KiB) Viewed 233 times

Of course you can play with the temperature to simulate any pre-stress (Sig_prestress = Alpha * Delta_Temperature * E_steel)
User avatar
HarryvL
Posts: 941
Joined: Sat Jan 06, 2018 7:38 pm

Re: How to use the pipeline postprocessing

Postby HarryvL » Wed May 16, 2018 4:44 am

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
PSB_x_section.png (277.19 KiB) Viewed 229 times
User avatar
HarryvL
Posts: 941
Joined: Sat Jan 06, 2018 7:38 pm

Re: How to use the pipeline postprocessing

Postby HarryvL » Wed May 16, 2018 4:50 am

By the way, I didn't apply any other loads (e.g. gravity) to the beam for now.
User avatar
bernd
Posts: 7289
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: How to use the pipeline postprocessing

Postby bernd » Wed May 16, 2018 7:59 am

thschrader wrote:
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. :shock:
User avatar
HarryvL
Posts: 941
Joined: Sat Jan 06, 2018 7:38 pm

Re: How to use the pipeline postprocessing

Postby HarryvL » Wed May 16, 2018 8:32 am

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. ;)
thschrader
Posts: 1380
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: How to use the pipeline postprocessing

Postby thschrader » Wed May 16, 2018 7:04 pm

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
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?
stress_field.JPG
stress_field.JPG (36.46 KiB) Viewed 191 times