This files explains the different steps that have to be performed to generate the input
files that are necessary for a 3D structural analysis, starting from existing input files
that have been previously defined for a 2D analysis
Step 1 : calculate the torsional stiffness in the section
We assume that the starting point is an input file created to calculate the temperatures,
say C2T.IN.
1. Copy the existing C2T.IN file and rename it in C2TOR.IN
2. In this new file, change the comment lines (optional)
3. In this new file, replace the commands
TEMPERAT
TETA
TINITIAL
MAKE.TEM
by the command
TORSION
0.9
20.0
4. In this new file, change the name of the file which will be created, for example, replace
"c2t.tem" by "c2tor.tor"
5. Delete all the FRONTIER and related commands (there is no fire curve applied here). The
SYMMETRY command now follows immediately the definition of the elements.
6. Delete the TIME …. ENDTIME commands (there is no need of time steps because the
calculation is done only once).
7. Use of symmetries
a. If the whole section is modelled (no symmetry is used), IT IS ABSOLUTELY
REQUIRED to fix the value of the solution to 0 in at least one node of the axis of
symmetry. If not, the torsional stiffness will be correctly evaluated, but the
warping function at all nodes will be offset by an arbitrary value and this will
create amazing results in torsion during the mechanical analysis.
b. YSYM cannot be used in a 3D problem. It means that, if the temperatures where
previously calculated using the YSYM command because the .TEM file was to be
used in a 2D mechanical analysis, it is now necessary to recalculate the
temperatures and to replace this YSYM command by a REALSYM command.
c. If one part of the section only is discretised and 1 or 2 REALSYM commands are
used, it is necessary to fix the value of the solution to 0 at all the nodes which are
on the axes of symmetry. If there is another axis of symmetry in the solution, but
this axis is not used in a REALSYM command, the values of the solution must also
be fixed to 0 on this axis. This is the example of a square section if ¼ of the
section is discretised, then the solution must also be fixed to 0 on the diagonal of
the square section.
8. In the MATERIAL command, you must enter the material mechanical properties for each
material (the same properties as the one you will use in the mechanical analysis. Don't
forget the Poison's ratio).
9. Run SAFIR with this new file. The CPU time is extremely short. The end of the .OUT file
looks like this:
G * Ip =
27259615.3846154
According to the principle of virtual works,
GJ = 0.919990E+08
EIw = 0.856407E+07
THE STIFFNESS MATRIX HAS BEEN TRIANGULARISED
1 TIMES.
GJ is the elastic torsional stiffness of the section at room temperature. In reality, this value
will decrease because of cracking even at room temperature (may-be not so much for a
column loaded in compression) and will decrease even further during the fire because of the
temperature increase and the subsequent decrease in material stiffness. it is not possible to
calculate this evolution as a function of time in SAFIR. Only a constant value can be entered.
The stiffness can, for instance, be divided by an arbitrary factor of 2. This has to be made in
the .TEM file. This means that the simulation is valid provided that torsion is not the may load
path. This is not so restrictive in most usual building elements. This would be restrictive in,
for example, a cantilever beam submitted to a pure torsion moment.
Step 2. Introduce the torsion properties in the .TEM file.
1) Open the .TEM file which had been created during the temperature analysis and open the
new file which has been created during this torsion analysis, "c2tor.tor" in this case. They
look very similar (the number of fibres, NFIBERBEAM, must be the same in the 2 files),
with the difference that the value of the warping function and of the torsional stiffness is
present in the torsion file.
2) From the .TOR file, copy the group of lines starting with
w
and finishing with
According to the principle of virtual works,
GJ = 0.919990E+08
3) Insert this group of lines in the .TEM file just before this line
HOT
The .TEM file is now ready to be used in a 3D mechanical analysis. If an YSYM
command was used when the file was to be used in a 2D calculation, the number of points
has now been multiplied by 2, and the information on torsion is now present in the file.
Step 3. Modify the IN file for the mechanical analysis.
1) Copy and rename the .IN file, for example C2M.IN into C3M.IN
2) If a first step, don't modify the NPTTOT value. SAFIR will later let you know to which
value it has to be increased. The same holds for LARGEUR11 and LARGEUR12.
3) Even if one single member, i.e. a beam or a column, is analysed, the number of nodes has
to be increased by 1, here from 21 to 22 (see section 4.2 of the user's manual to see why
this node is needed and how you can define the coordinates). In more complex structures,
it is possible that more additional nodes are needed.
4) NDIM goes from 2 to 3.
5) NDDLMAX goes from 3 to 7.
6) The nodes which had 3 DoF have now 7 DoF, see the FROM command.
7) Add a FROM command which says that the node(s) that you have added, see point 3, has 0
DoF.
8) The number of fibres has to be adapted in the NFIBERS command (probably multiply it
by 2 if you previously used an YSYM command in the thermal calculation).
9) The nodes which were previously present have to be given a third coordinate. In order to
have a traditional view with DIAMOND, it is preferable that the new co-ordinate be the Y
co-ordinate, see table below. Giving 0 to all these Y coordinates means no initial
imperfection in this direction.
2D
=>
3D
X
=>
X
-
=>
Y
Y
=>
Z
10) Give the coordinates to the node(s) that you have added, see point 3
11) Modify the BLOCK commands taking into account the new DoF's. they go in the order: X,
Y, Z, tetaX, tetaY, tetaZ, warping. Note that 1 line is needed for each blocked node, and 1
blank line at the end of the series.
12) Add the fourth node (the one that you have added) to every beam finite element.
13) Modify the loads in order to reflect the new DoF's. Note that DISTRBEAM have 3
components, pX, pY and pZ. NODELOAD have 6 components, FX, FY, FZ, MX, MY,
MZ.
Step 4 : run SAFIR
You may have to adapt some values for the dimensions of the arrays, but SAFIR will let you
know. When using Diamond, don't forget to use the TOOL-ViewPoint Tool.
">
