Display principal stresses
Moderator: bernd
Forum rules
and Helpful information for the FEM forum
and Helpful information for the FEM forum
Re: Display principal stresses
Very value input Stefan. It is the way to go IMHO. The graphical output will even look better, similar to the picture in the first post.
-
- Posts: 108
- Joined: Wed Sep 12, 2018 1:31 pm
Re: Display principal stresses
Very interesting, I will need it sometime...
kudos.
kudos.
Re: Display principal stresses
AFAIK, Paraview offers three methods for reducing glyph density
Mode 2 and 3 are only dropping glyphs, there is no interpolation or other maths
BTW, because of ordered mesh numbering, necessary for optimized solving, there is no major difference in visualization between mode 2 and mode 3.
Perhaps not worth the effort.
Mode 2 and 3 are only dropping glyphs, there is no interpolation or other maths
BTW, because of ordered mesh numbering, necessary for optimized solving, there is no major difference in visualization between mode 2 and mode 3.
Perhaps not worth the effort.
-
- Posts: 108
- Joined: Wed Sep 12, 2018 1:31 pm
Re: Display principal stresses
Hello,
I have a doubt regarding the stresses and their posterior calculation like principal stresses....
Taking a row vector from calculix .frd and .dat files...
Are the indexes of stress values sorted in the same manner?
I check that in the .dat file the stress for each element integration point is indexing in the following manner:
So if we include the values in the stress tensor, it is in the following way:
S=[sxx sxy sxz
sxy syy syz
sxz syz szz]
Using numbers as index...
S=[1 4 5
4 2 6
5 6 3]
However, the .frd file shows that:
This means that the stress tensor values for nodes is:
S=[1 4 6
4 2 5
6 5 3]?
To sum up, are sxz and syz components exchanged?
Best regards,
I have a doubt regarding the stresses and their posterior calculation like principal stresses....
Taking a row vector from calculix .frd and .dat files...
Are the indexes of stress values sorted in the same manner?
I check that in the .dat file the stress for each element integration point is indexing in the following manner:
Code: Select all
stresses (elem, integ.pnt.,sxx,syy,szz,sxy,sxz,syz)
S=[sxx sxy sxz
sxy syy syz
sxz syz szz]
Using numbers as index...
S=[1 4 5
4 2 6
5 6 3]
However, the .frd file shows that:
Code: Select all
-5 SXX 1 4 1 1
-5 SYY 1 4 2 2
-5 SZZ 1 4 3 3
-5 SXY 1 4 1 2
-5 SYZ 1 4 2 3
-5 SZX 1 4 3 1
S=[1 4 6
4 2 5
6 5 3]?
To sum up, are sxz and syz components exchanged?
Best regards,
Re: Display principal stresses
I think you are right that components are written in a different order.
I don't exactly recall where it was discussed, if somewhere on this forum or on the ccx mailing list.
-
- Posts: 108
- Joined: Wed Sep 12, 2018 1:31 pm
Re: Display principal stresses
Re: Display principal stresses
It was discussed in this topic, see a few posts back:
https://forum.freecadweb.org/viewtopic. ... 10#p240408
https://forum.freecadweb.org/viewtopic. ... 10#p240408
-
- Posts: 108
- Joined: Wed Sep 12, 2018 1:31 pm
Re: Display principal stresses
Response from cxx mailing group https://groups.yahoo.com/neo/groups/cal ... ages/15199, I copy and paste it.
I don't know about .dat but I'll confirm that the .frd has the YZ component as the 5th component. I just ran a model with known shear stress and it appeared in the 5th position. It shouldn't matter though because you should use the ICIND1 and ICIND2 values to identify the component rather than the order.
Be careful when postprocessing .frd and .dat files...
-
- Posts: 108
- Joined: Wed Sep 12, 2018 1:31 pm
Re: Display principal stresses
Thumbs up!HarryvL wrote: ↑Sat Dec 22, 2018 9:44 pm It was discussed in this topic, see a few posts back:
https://forum.freecadweb.org/viewtopic. ... 10#p240408
-
- Posts: 108
- Joined: Wed Sep 12, 2018 1:31 pm
Re: Display principal stresses
Hello,
My last confirmation regarding stresses. I make a simple test: inital conditions pure stress (500 MPa - SXY direction) in element 51.
I check the values in NODE 1 from element 51:
# Stress FRD file
-0.5532 7.2032 76.1790 -4.4374 -279.1010 -15.9312
# Stress DAT file
-0.5532 7.2032 76.1790 -4.4374 -15.9312 -279.1007
Sxy and Sxz are in different order.
Best regards,
Ekaitz.
My last confirmation regarding stresses. I make a simple test: inital conditions pure stress (500 MPa - SXY direction) in element 51.
Code: Select all
#Element information
El=[46, 9, 3, 8, 6
47, 5, 3, 6, 4
48, 3, 4, 8, 6
49, 7, 5, 6, 4
50, 5, 3, 4, 2
51, 3, 2, 1, 4]
# From FRD file:
NodeS=[[b]-5.53205E-01 7.20325E+00 7.61790E+01 -4.43743E+00 -2.79101E+02 -1.59312E+01[/b]
1.45933E+01 1.11598E+01 8.20929E+01 9.95657E+00 -2.91087E+01 -2.00360E+01
5.04025E+00 -9.63229E-01 1.54117E+00 1.13816E+00 -1.38002E+00 -3.10907E+00
-2.67077E+00 -1.59571E-01 -1.99464E-02 2.53921E-01 5.64170E-02 -8.97747E-02
-1.78328E-01 -1.56922E+00 1.64284E+00 2.19851E+00 8.63545E+01 4.65185E+00
-7.29664E+00 -5.57991E+00 -4.10465E+01 -4.97829E+00 1.45544E+01 1.00180E+01
-2.52012E+01 4.81615E+00 -7.70584E+00 -5.69080E+00 6.90009E+00 1.55453E+01;
5.44095E-01 -1.24779E+00 -4.05538E+01 -1.07905E+00 1.00185E+01 9.87834E-01
1.33538E+01 7.97857E-01 9.97321E-02 -1.26961E+00 -2.82085E-01 4.48874E-01]
# From DAT file:
ElementS=[1.335383E+01 7.978568E-01 9.973210E-02 -1.269606E+00 4.488735E-01 -2.820850E-01
-5.073507E+00 -2.464022E+01 -7.537246E+01 -1.206424E+01 2.255105E+01 3.128036E+01
-1.226564E+01 -3.293428E+00 -8.120725E+01 -8.885034E-01 1.526795E+00 2.031913E+01
-2.520123E+01 4.816147E+00 -7.705843E+00 -5.690797E+00 1.554534E+01 6.900095E+00
2.973975E+01 1.511639E+01 8.800681E+01 2.435058E+01 -2.414085E+01 2.208832E+02
[b]-5.532049E-01 7.203245E+00 7.617900E+01 -4.437433E+00 -1.593121E+01 -2.791007E+02][/b]
# Stress FRD file
-0.5532 7.2032 76.1790 -4.4374 -279.1010 -15.9312
# Stress DAT file
-0.5532 7.2032 76.1790 -4.4374 -15.9312 -279.1007
Sxy and Sxz are in different order.
Best regards,
Ekaitz.