Discussion Groups

## Simulation Mechanical and Multiphysics

Contributor
Posts: 19
Registered: ‎09-09-2013

# Suspect FEA results

266 Views, 1 Replies
01-30-2014 01:26 PM

Forum,

Material (Color):

• W12x96 A992 (Purple)
• W6x25 A992 (Orange)
• W8x31 A992 (Light Blue)
• W6x9 A992 (light grey)
• 0.375 in. THK A36 plate

I am having a problem with an analysis I can't seem to figure out.  When I ran the FEA last week, I was only get deflections of 1.5 - 5 inches.  After adding in additional W6x9 beam supports depicted in grey beneath the 0.375" A36 plate steel and running the FEA again, I get over 10" of deflection (See FEA below).

The picture below is how the subassembly comes into SimMech when pushed from Fusion

I sectioned the plate in Fusion; the section of A36 plate in bright yellow and orange in the pictures shows where the surface pressure of -5.0 psi of water having a total weight of 131,000 lbs for the volume above this area section and surface temperature of 195 deg F were applied

I fixed (x,y,z) the W12x96 in all directions on the bottom of each in this partial assembly to represent them actually resting on level and reinforced ground.  I also employed gravity in the -Y direction to account for the weight of the partial structure.

The W8x31 and W6x9 are supposed to be supporting the 0.375" thick A36 plate.  What I see as a problem after the analysis is completed is that there is over 1.5 - 10" + deflection in the plate but virtually no deflection (0.000547 in.) in the cross beams.

• 176 in. x 148.25 in. = 26092 in^2   (181.194 ft^2)     AREA UNDER LOAD
• 181.194 ft^2 x 11.5 ft (height of the water in that volume space) =  2083.74 ft^3   VOLUME OF WATER
• 2083.74 ft^3 x 62.4 lb/ft^3 = 130,025 lbs      WEIGHT OF WATER IN THAT AREA/VOLUME
• 130,025 lbs / 26092 in^2  = 4.983 lb/in^2 (psi)   WEIGHT LOAD PER IN.^2 OF WATER IN THAT AREA/VOLUME

Now given that there is an automatically assumed bonding between parts in contact, I can't understand why there is no deflection showing for the beams.  Should I be ignoring gravity since the weight is already accounted for in material and element definition?

Thank you in advance.  If it'll help diagnose, I've included the NotePad results of the latest run which had one (1) WARNING:

Autodesk (R) Simulation Static Stress with Linear Material Models
Version 2014.01.00.0025-W64/X64 26-Jul-2013

-------------------------------------------------
DATE: JANUARY 30, 2014
TIME: 01:54 PM
INPUT MODEL: C:\FEA\XXXXXXX_FLOOR_FEA.ds_data\1\ds

PROGRAM VERSION: 201401000025
alg-win-x64.dll VERSION: 201401000025
agsdb_ar-win-x64.dll VERSION: 201401000025
algconfig-win-x64.dll VERSION: 201401000025
solvercallback-win-x64.dll VERSION: 201401000025
amgsolve.exe VERSION:    360000000

-------------------------------------------------

**** Model Unit System Settings:
--------------------------------------------
Unit System              : English (in)
Force                    : lbf
Length                   : in
Time                     : s
Temperature (Absolute)   : deg F (R)
Thermal Energy           : in*lbf
Voltage                  : V
Current                  : A
Electrical Resistance    : ohm
Mass                     : lbf*s^2/in
--------------------------------------------

1**** CONTROL INFORMATION

number of node points          (NUMNP)   =        402582
number of element types        (NELTYP)  =            22
number of load cases           (LL)      =             1
number of frequencies          (NF)      =             0
analysis type code             (NDYN)    =             0
equations per block            (KEQB)    =             0
bandwidth minimization flag    (MINBND)  =            -1
gravitational constant         (GRAV)    =    3.8640E+02
number of equations            (NEQ)     =       2272386

**** PRINT OF NODAL DATA SUPPRESSED
**** PRINT OF EQUATION NUMBERS SUPPRESSED
**** Part     1: plate (shell) elements
**** The maximum warp angle =  4.4733E+00 degrees
There are 130 quadrilateral elements over tolerance :  1.0000E-01
Total 1406 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part     2: plate (shell) elements
**** The maximum warp angle =  6.0707E+00 degrees
There are 493 quadrilateral elements over tolerance :  1.0000E-01
Total 1124 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part     3: plate (shell) elements
**** The maximum warp angle =  5.3709E+00 degrees
There are 233 quadrilateral elements over tolerance :  1.0000E-01
Total 1338 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part     4: plate (shell) elements
**** The maximum warp angle =  1.9915E+00 degrees
There are 189 quadrilateral elements over tolerance :  1.0000E-01
Total 106 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part     5: plate (shell) elements
**** The maximum warp angle =  4.4745E+00 degrees
There are 12 quadrilateral elements over tolerance :  1.0000E-01
Total 1922 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    26: plate (shell) elements
**** The maximum warp angle =  4.4068E+00 degrees
There are 35 quadrilateral elements over tolerance :  1.0000E-01
Total 50 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    27: plate (shell) elements
**** The maximum warp angle =  4.4041E+00 degrees
There are 19 quadrilateral elements over tolerance :  1.0000E-01
Total 46 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    34: plate (shell) elements
**** The maximum warp angle =  5.5276E+00 degrees
There are 408 quadrilateral elements over tolerance :  1.0000E-01
Total 572 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    35: plate (shell) elements
**** The maximum warp angle =  5.3552E+00 degrees
There are 519 quadrilateral elements over tolerance :  1.0000E-01
Total 350 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    36: plate (shell) elements
**** The maximum warp angle =  4.6745E+00 degrees
There are 518 quadrilateral elements over tolerance :  1.0000E-01
Total 348 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    37: plate (shell) elements
**** The maximum warp angle =  1.2695E+00 degrees
There are 243 quadrilateral elements over tolerance :  1.0000E-01
Total 94 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    38: plate (shell) elements
**** The maximum warp angle =  4.2532E+00 degrees
There are 246 quadrilateral elements over tolerance :  1.0000E-01
Total 100 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    51: plate (shell) elements
**** The maximum warp angle =  1.8545E+00 degrees
There are 1 quadrilateral elements over tolerance :  1.0000E-01
Total 2574 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    52: plate (shell) elements
**** The maximum warp angle =  5.3240E-07 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 2 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    53: plate (shell) elements
**** The maximum warp angle =  1.6084E-06 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 2 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    54: plate (shell) elements
**** The maximum warp angle =  1.3634E-10 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 8 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    55: plate (shell) elements
**** The maximum warp angle =  8.7709E-11 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 8 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    56: plate (shell) elements
**** The maximum warp angle =  1.6084E-06 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 2 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    57: plate (shell) elements
**** The maximum warp angle =  5.3240E-07 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 2 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    58: plate (shell) elements
**** The maximum warp angle =  5.3261E-07 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 2 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    59: plate (shell) elements
**** The maximum warp angle =  1.6085E-06 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 2 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Part    60: plate (shell) elements
**** The maximum warp angle =  1.4390E-10 degrees
There are 0 quadrilateral elements over tolerance :  1.0000E-01
Total 10 triangle elements.
**** PRINT OF TYPE-6 ELEMENT DATA SUPPRESSED
**** Hard disk file size information for processor:

Available hard disk space on current drive =1703585.625 megabytes
Gravity direction vector =  0.0000E+00 -1.0000E+00  0.0000E+00

load case     Pressure   Gravity  Displacement  Thermal  Electrical
---------    ---------- ---------- ---------- ---------- ----------

1         1.000E+00  1.000E+00  1.000E+00  0.000E+00  0.000E+00

Centrifugal force / angular acceleration

---------    ---------- ----------

1         0.000E+00  0.000E+00

**** Symbolic Assembly Using the Row-Hits Matrix Profile ...
**** Number of equations                 = 2272386
Estimated maximum bandwidth         = 287
Estimated triangle matrix nonzeroes = 120864045
Symbolically assembled nonzeros     = 62625075
**** Real Sparse Matrix Assembly ...

1**** STIFFNESS MATRIX PARAMETERS

minimum non-zero diagonal element =           1.0393E+02
maximum diagonal element          =           2.3255E+13
maximum/minimum                   =           2.2376E+11
average diagonal element          =           4.5301E+08

warning: max/min stiffness ratio =            2.2376E+11
maximum stiffness =  2.325452E+13 at eqn#204920, node=41818, DOF=Ty
minimum stiffness =  1.039269E+02 at eqn#2014558, node=359611, DOF=Rx

in the upper triangle:
number of entries in the profile    = 120864045
number of nonzeros                  = 43264318

**** Sparse Matrix Assembled

**** Invoking Parallel BCSLIB-EXT Sparse Solver...

BCSLIB-EXT solver memory status:
in-core memory requirement (MB) =         7399.58
minimum memory requirement (MB) =          642.16
user specified memory (MB) =        24422.05
available physical memory (MB) =        24422.05
available virtual memory (MB) =        87464.03
memory currently allocated (MB) =         7399.58
**** End Sparse Solver Solution

Reaction Sums and Maxima for Load Case       1

Sum of applied forces
X-Force     Y-Force     Z-Force    X-Moment    Y-Moment    Z-Moment
-1.2714E-04 -1.6276E+05 -2.7695E-03  1.2899E-02  1.1758E-02  9.2720E-02

Sum of reactions
X-Force     Y-Force     Z-Force    X-Moment    Y-Moment    Z-Moment
8.0048E-05  4.7004E-04  7.4947E-06  2.7131E+04  9.6315E+01  1.4256E+05

Sum of residuals
X-Force     Y-Force     Z-Force    X-Moment    Y-Moment    Z-Moment
-4.7091E-05 -1.6276E+05 -2.7620E-03  2.7131E+04  9.6327E+01  1.4256E+05

Sum of unfixed direction residuals
X-Force     Y-Force     Z-Force    X-Moment    Y-Moment    Z-Moment
-1.6005E-05  1.4380E-04  4.8936E-05  1.8817E-06  1.8582E-06  5.3725E-07

Largest applied forces and moments
Node        Node        Node        Node        Node        Node
X-Force     Y-Force     Z-Force    X-Moment    Y-Moment    Z-Moment
26801      306072       19344       50150       62829       62829
-1.8079E-02 -7.8434E+01  1.1604E-02 -1.8536E-03  1.2322E-03  1.7259E-03

Largest nodal reactions
Node        Node        Node        Node        Node        Node
X-Force     Y-Force     Z-Force    X-Moment    Y-Moment    Z-Moment
122562       50959       50958       50959      122563      253224
-1.3406E+04 -3.1761E+03 -1.1810E+04  5.8549E+03  2.3227E+02  1.8166E+03

Largest nodal residuals
Node        Node        Node        Node        Node        Node
X-Force     Y-Force     Z-Force    X-Moment    Y-Moment    Z-Moment
122562       50959       50958       50959      122563      253224
-1.3406E+04 -3.1763E+03 -1.1810E+04  5.8549E+03  2.3227E+02  1.8166E+03

Largest unfixed direction residuals
Node        Node        Node        Node        Node        Node
X-Force     Y-Force     Z-Force    X-Moment    Y-Moment    Z-Moment
90501      103024       86954      103044       86954       90501
-7.2988E-06  4.8633E-05  4.3924E-05 -2.2595E-06  2.6675E-06  1.6831E-06

1**** TEMPORARY FILE STORAGE (MEGABYTES)
----------------------------------
UNIT NO.  7 :     17.337
UNIT NO.  8 :     18.429
UNIT NO.  9 :      0.000
UNIT NO. 10 :      0.000
UNIT NO. 11 :      0.000
UNIT NO. 12 :     17.337
UNIT NO. 13 :     17.378
UNIT NO. 14 :      0.000
UNIT NO. 15 :      0.000
UNIT NO. 17 :      0.000
UNIT NO. 50 :    423.170
UNIT NO. 51 :     56.031
UNIT NO. 52 :   1048.503
UNIT NO. 54 :      8.668
UNIT NO. 55 :    165.040
UNIT NO. 56 :    330.081
UNIT NO. 57 :    330.081
UNIT NO. 58 :      0.000
UNIT NO. 59 :      0.000

TOTAL       :   2432.054 Megabytes

*Expert Elite*
Posts: 575
Registered: ‎08-30-2012

# Re: Suspect FEA results

02-03-2014 07:10 AM in reply to: CPEProjE

Hi CPEProjE,

If the plate is deflecting but the beams are not, it is because the plate is not connected to the beams. One of these may be the problem:

1. The CAD model has a gap between the plate and the beams which is larger than the mesh matching tolerance, so the parts are not bonded. (Bonding only occurs in linear stress if the gap between parts is 0.)
2. The mesh type is wrong to get bonding to occur. For example, a midplane mesh would put the elements at the mid-thickness of each part, so the gap between the plate and beam would be 1/2*(plate thickness + flange thickness), and bonding will not occur with a gap.
3. The mesh type is wrong for the geometry. It looks like you started with a solid model but ended up with plate elements. If you chose the "plate/shell" type of mesh for a solid model, then you ended up with hollow shapes for each part. Search the documentation for the page titled "Model Mesh Settings" for examples of the three types of mesh (solid, midplane, plate/shell) on a CAD solid model.

Good Luck.

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

Simulation Mechanical user since Dec 1997