FEM - Dynamic Loads?

About the development of the FEM module/workbench.

Moderator: bernd

JensElmo
Posts: 11
Joined: Fri Feb 16, 2018 9:16 am

FEM - Dynamic Loads?

Postby JensElmo » Fri May 18, 2018 8:29 am

I have a project where I have essentially a mechanical hammer hitting object with a down force of 160kN in a percussion rate of 32 Hz.
I am not able to find out how in the FEM module to apply a dynamic load, if that is even possible in FreeCAD.
So I was hoping somebody could help me, or direct me to a tutorial about dynamic loads.




FreeCAD Info
OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.13387 (Git)
Build type: Release
Branch: master
Hash: c5f4079252b11e3c54cd603be7d3697fa9f9d922
Python version: 2.7.14
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.1.0
Locale: Danish/Denmark (da_DK)
Jee-Bee
Posts: 1262
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

Re: FEM - Dynamic Loads?

Postby Jee-Bee » Fri May 18, 2018 11:33 am

You have to modify you're input file of calculix.
you need at least add the *AMPLITUDE parameter.
see for a bit more information http://www.feacluster.com/CalculiX/ccx_ ... de202.html
I'm not sure what type of analysis you need. just start with *STATIC and try out..
User avatar
HarryvL
Posts: 539
Joined: Sat Jan 06, 2018 7:38 pm
Location: Denmark

Re: FEM - Dynamic Loads?

Postby HarryvL » Fri May 18, 2018 1:57 pm

@Jee-Bee, the simplest analysis type that captures steady state dynamic response is "Steady State Dynamic Analysis, as I use and describe here:

https://forum.freecadweb.org/viewtopic. ... 50#p232309

However this assumes a sinusoidal periodic load. If you have a different periodic load then you would need Fourier analysis to write this as a sum of periodic loads. I believe there is an option for that too in CCX. However, I would first try to use the simplest option (above) and see if you can make that work.
User avatar
HarryvL
Posts: 539
Joined: Sat Jan 06, 2018 7:38 pm
Location: Denmark

Re: FEM - Dynamic Loads?

Postby HarryvL » Fri May 18, 2018 2:05 pm

I just checked the manual. CCX can indeed decompose a general periodic load into sinusoidal (harmonic) components using Fourier transform. The only additional thing you need to do (in addition to what I describe above and in my bridge post) is to add HARMONIC=NO to the *STEADY STATE DYNAMICS card and describe one period of the load in the *AMPLITUDE card. It will produce similar results as in my post, so please take care with the post processing. I would be interested to see your results.
Jee-Bee
Posts: 1262
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

Re: FEM - Dynamic Loads?

Postby Jee-Bee » Fri May 18, 2018 3:12 pm

Sorry @HarryvL i just read sometimes parts of of the CCX documentations but it takes time to gain some experience
JensElmo
Posts: 11
Joined: Fri Feb 16, 2018 9:16 am

Re: FEM - Dynamic Loads?

Postby JensElmo » Mon May 28, 2018 8:31 am

Sorry I am late replying, have been ill.

I am relativly new to FreeCad and have no experience in Python, so i have possible misunderstood the post on Steady State Dynamic Analysis. So would like to check if I understood it correctly.

What I understood and did was make a simple part to test on before moving on to my actual part.
Then on my simple test part I set up a FEM study ( Chose material, Contraints, Force and Mesh) , Then ran the solver and edited the file to replace the 'Static Step' with the 'Steady State Dynamics Step' you wrote in the bridge thread.

It gives an error message : "*ERROR in steadystate: cannot open eigenvalue file for reading", but still says that it is done and opening results but never does.
(See below for complete message)

Code: Select all

0.0: Check dependencies...
0.1: Write completed.
0.0: CalculiX binary: C:/Program Files/FreeCAD_0.17.13387_x64_dev_win/bin/ccx.exe
0.0: Run CalculiX...
0.0: Starting CalculiX...
0.0: CalculiX is running...
0.2: CalculiX stopped.
0.2: ************************************************************ 
CalculiX Version 2.12, Copyright(C) 1998-2015 Guido Dhondt 
CalculiX comes with ABSOLUTELY NO WARRANTY. This is free 
software, and you are welcome to redistribute it under 
certain conditions, see gpl.htm 
************************************************************ 
You are using an executable made on Tue, Apr 4, 2017 11:04:04 PM 
The numbers below are estimated upper bounds 
number of: 
nodes: 1792 
elements: 1489 
one-dimensional elements: 0 
two-dimensional elements: 0 
integration points per element: 4 
degrees of freedom per node: 3 
layers per element: 1 
distributed facial loads: 0 
distributed volumetric loads: 0 
concentrated loads: 62 
single point constraints: 198 
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: 5 
terms in all sets: 6155 
materials: 1 
constants per material and temperature: 2 
temperature points per material: 1 
plastic data points per material: 0 
orientations: 0 
amplitudes: 2 
data points in all amplitudes: 2 
print requests: 2 
transformations: 0 
property cards: 0 
STEP 1 
Decascading the MPC's 
Determining the structure of the matrix: 
number of equations 
5178 
number of nonzero lower triangular matrix elements 
165792 
Composing the steady state response from the eigenmodes 
*ERROR in steadystate: cannot open eigenvalue file for reading
0.2: CalculiX done!
0.3: Loading result sets...
I have attached my test part, but that is just a basic part made to see if I could get it to work.
Attachments
Test - Dynamic.FCStd
(105.13 KiB) Downloaded 6 times
Jee-Bee
Posts: 1262
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

Re: FEM - Dynamic Loads?

Postby Jee-Bee » Mon May 28, 2018 8:52 am

Can you add you're inp file? with out it we can't see what you changed...
User avatar
flachyjoe
Posts: 539
Joined: Sat Mar 31, 2012 12:00 pm
Location: Limoges, France

Re: FEM - Dynamic Loads?

Postby flachyjoe » Mon May 28, 2018 9:36 am

Hi,
the *STEADY STATE DYNAMIC step need eigenmodes and eigenfrequencies calculation, these are gave by a *FREQUENCY, STORAGE=YES step.
See : http://web.mit.edu/calculix_v2.7/Calcul ... de244.html

For the Frequency step, same boundary conditions as for the steady state step are needed.
- Flachy Joe -
alias FFW @ irc.freenode.net #freecad et #freecad-fr
"Puisqu’on ne peut changer la direction du vent, il faut apprendre à orienter les voiles." Anonyme
User avatar
HarryvL
Posts: 539
Joined: Sat Jan 06, 2018 7:38 pm
Location: Denmark

Re: FEM - Dynamic Loads?

Postby HarryvL » Mon May 28, 2018 9:46 am

flachyjoe wrote:
Mon May 28, 2018 9:36 am
Hi,
the *STEADY STATE DYNAMIC step need eigenmodes and eigenfrequencies calculation, these are gave by a *FREQUENCY, STORAGE=YES step.
See : http://web.mit.edu/calculix_v2.7/Calcul ... de244.html

For the Frequency step, same boundary conditions as for the steady state step are needed.
Indeed, you need 2 steps, for example:

Code: Select all


** step 1

*STEP
*FREQUENCY, STORAGE=YES
10,0.0,1000000.0

** BOUNDARY cards

*NODE FILE, OUTPUT=2d
U
**EL FILE
**S, E

**NODE PRINT , NSET=Nall
**U
**EL PRINT , ELSET=Eall
**S

*END STEP

** step 2

*STEP
*STEADY STATE DYNAMICS
0., 5.

** CLOAD/DLOAD cards

*MODAL DAMPING
1,10,0.1

*NODE FILE, OUTPUT=2d
U
**EL FILE
**S, E

*NODE PRINT , NSET=Output
U
**EL PRINT , ELSET=Eall
**S

*END STEP
EDIT: no need for a DLOAD/CLOAD card in the first step.
Last edited by HarryvL on Mon May 28, 2018 10:34 am, edited 1 time in total.
JensElmo
Posts: 11
Joined: Fri Feb 16, 2018 9:16 am

Re: FEM - Dynamic Loads?

Postby JensElmo » Mon May 28, 2018 10:15 am

Jee-Bee wrote:
Mon May 28, 2018 8:52 am
Can you add you're inp file? with out it we can't see what you changed...
Oh, yes of course, the attachment wonøt let me attach an inp file, so i zipped it
Attachments
FEMMeshNetgen.zip
(57.74 KiB) Downloaded 8 times