Reviewing tabular data reports

Open the file Frame.rpt in a text editor. The contents of this file are shown below. Your node and element numbering may be different. Very small values may also be calculated differently, depending on your system.

Stress output:
Field Output Report

Source 1
---------

   ODB: Frame.odb
   Step: Apply load
   Frame: Increment      1: Step Time =   2.2200E-16

Loc 1 : Integration point values from source 1

Output sorted by column "Element Label".

Field Output reported at integration points for part: FRAME-1

         Element             Int           S.S11
           Label              Pt          @Loc 1
-------------------------------------------------
               1               1    -294.116E+06
               2               1     294.116E+06
               3               1    -294.116E+06
               4               1     147.058E+06
               5               1    -294.116E+06
               6               1     147.058E+06
               7               1     294.116E+06


  Minimum                           -294.116E+06
      At Element                               5

          Int Pt                               1
  Maximum                            294.116E+06
      At Element                               7

          Int Pt                               1
Displacement output:
Field Output Report

Source 1
---------

   ODB: Frame.odb
   Step: Apply load
   Frame: Increment      1: Step Time =   2.2200E-16

Loc 1 : Nodal values from source 1

Output sorted by column "Node Label".

Field Output reported at nodes for part: FRAME-1

            Node            U.U1            U.U2
           Label          @Loc 1          @Loc 1
-------------------------------------------------
               1     1.47058E-03    -2.54712E-03
               2    -46.3233E-12    -2.54712E-03
               3     735.291E-06    -4.66972E-03
               4             -0.         -5.E-33
               5     1.47058E-03         -5.E-33


  Minimum           -46.3233E-12    -4.66972E-03

         At Node               2               3
  Maximum            1.47058E-03         -5.E-33

         At Node               5               5
Reaction force output:
Field Output Report

Source 1
---------

   ODB: Frame.odb
   Step: Apply load
   Frame: Increment      1: Step Time =   2.2200E-16

Loc 1 : Nodal values from source 1

Output sorted by column "Node Label".

Field Output reported at nodes for part: FRAME-1

            Node          RF.RF1          RF.RF2
           Label          @Loc 1          @Loc 1
-------------------------------------------------
               1              0.              0.
               2              0.              0.
               3              0.              0.
               4     454.747E-15          5.E+03
               5              0.          5.E+03


  Minimum                     0.              0.
         At Node               5               3

  Maximum            454.747E-15          5.E+03
         At Node               4               5

           Total     454.747E-15         10.E+03

Are the nodal displacements and peak stresses in the individual members reasonable for this hoist and these applied loads?

It is always a good idea to check that the results of the simulation satisfy basic physical principles. In this case check that the external forces applied to the hoist and the reaction forces sum to zero in both the vertical and horizontal directions.

What nodes have vertical forces applied to them? What nodes have horizontal forces? Do the results from your simulation match those shown here?