Actually, you are applying a pressure (not a force) to a surface of the model (not an edge, although it is fair to call it an edge of the mesh). I prefer to think in terms of the model in order to make the terminology compatible with the 3D geometry that is really being analyzed. (A nodal force applied to a single node of the mesh is treated as applied to an edge of the model. This would be equivalent to selecting an edge of a 3D CAD model and applying an edge force.)
Only nodal type loads in a 2D axisymmetric analysis need to be divided by 2pi because the magnitude over a full revolution is different than the magnitude over 1 radian. The magnitude of a pressure is the same whether it is the full revolution, 1 radian, or any other portion. This is also true when using symmetry in a 3D CAD model. You would apply the same pressure magnitude regardless of the portion modeled (1/4 symmetry, 1/8 symmetry, etc), but you would divide the total force applied to an edge by 4 or 8, respectively.
I presume the "failure" that you refered to is the abnormal results. The analysis you provided runs and gives results, so there is no reason that the processor would give any messages. (True, the processor could detect that the displacement is much larger than the size of the model and likely indicates an error with the setup, but the software is not programmed to do that.) The wireframe arc on the bottom of part 2 is not split so that it a duplicate of part 3, so the mesh does not match between parts 2 and 3. Since they do not match, the parts are free to move independently of each other. Please fix the wireframe directly in Simulation. Now that the DXF geometry is in Simulation, I suggest that you not worry about fixing the DXF file.
After fixing the geometry to get common edges between adjacent parts, the next issue that you will encounter is that some of the nodes are off by a very small amount. (That's the problem with math and computers: 2+2 doesn't necessarily equal 4!). The nodes along the centerline of the model were creating an error during the analysis, probably because some were a very small negative value. (Transforming a coordinate from the DXF file that is almost 0 in the XY plane to the YZ plane in Simulation results in a non-zero coordinate.) You can select the vertices along the centerline, right-click, and choose "Project". That is hort for "projection", not "project" as in "my project inclues performing an analysis". You can then project (move) these nodes to Y=0 so that they are on the theoretical centerline of the model.
Good luck.
. In my first post I was asking if force is to be divided but before I got the answer I decided to go with a pressure as this dosen't have to be "scaled". So not being sure if force has to be put for 2Pi or 1rad pressure was the safe choice.
![Autodesk Design & Make Report](https://forums.autodesk.com/t5/image/serverpage/image-id/1350519iCB55845EBFC43016/image-size/large?v=v2&px=999" "Autodesk Design & Make Report")