Tutorial Video Link

Importing and Assembly

Importing SolidWorks to NX

• The easiest way to import is to save a SolidWorks file as .stp and import that into NX, this avoids additional work on mating and assembly. NX will create a .prt file that contains all the parts. (More info on the NX tutorials page)
• Otherwise, work from .SLDPRT SolidWorks part files, each will become an NX part (this is what the video tutorial covers)
• SolidWorks parts to NX parts: Select “Open” from NX homepage, navigate to and open a SolidWorks part, may edit if needed (”Applications” → “Modeling”), then “Save As” (now as NX .prt file)
• Repeat to import all SolidWorks Parts

Assembly

• Create Assembly: Select “New” from NX homepage, select “Model” tab, select “Assembly”, choose save settings (same directory as parts), select “OK”
• The first part import will be through a pop-up menu after opening, this menu can be accessed again by selecting “Assemblies” → “Add Component” (right click on the ribbon if the “Assemblies” menu tab is not shown to show it)
• Importing parts: Select folder icon to navigate and pick component, choose number of component if needed, select “OK”
• On the left, the topmost menu is the “Assembly Navigator” with the parts shown, here you can “Unpack” groups of parts (when you import multiple of the same part, they group)
• Assembly Constraints: Use constraints to correctly place/orient parts, and restrict their degrees of freedom
  • Touch align: Select faces to align, this is the easiest way to match parts in relationship to other parts, it may over constrain but this is okay right now
  • Distance: Set exact distances between components, measure in SolidWorks model then enter that measurement
  • Center: 2 to 2 to select two sides of part to be centered and two sides of part centering on
  • Concentric: Select edge of hole (for example, for a screw), and the threaded rod to concentrically mate, then mate bottom of rod and inside of hole
  • Align and Lock: For example, locking threaded rod into hole to avoid rotation
• Freely move and rotate parts: Select “Assemblies” → “Move Component”
• In the “Assembly Navigator” menu there is a place to see all constraints, here you can easily remove them if needed.

Checking Constraints

• CHECK: Axis alignment between SolidWorks and NX, match orientation of axis and proper rotation of components
• CHECK: under constrained components, in the “Assembly Navigator” menu right click on a part, select “Show Degrees of Freedom” (see text at the bottom of the page and/or red arrows through part), add constraints to eliminate these DOF, F5 to clear arrows
  • It is okay to over-constrain components at this point

Meshing

Beginning the Mesh and Mesh Settings