About the development of the FEM module/workbench.

Moderator: bernd

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

OS: Windows 10
Word size of OS: 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: 1992
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

You have to modify you're input file of calculix.
you need at least add the *AMPLITUDE parameter.
I'm not sure what type of analysis you need. just start with *STATIC and try out..
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

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

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

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: 1992
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

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

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: 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
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
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
0.2: CalculiX done!
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
Jee-Bee
Posts: 1992
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

Can you add you're inp file? with out it we can't see what you changed...
flachyjoe
Posts: 673
Joined: Sat Mar 31, 2012 12:00 pm
Location: Limoges, France

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 -
"Puisqu’on ne peut changer la direction du vent, il faut apprendre à orienter les voiles." Anonyme
HarryvL
Posts: 1071
Joined: Sat Jan 06, 2018 7:38 pm
Location: Netherlands

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
0., 5.

*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
``````
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