Tips & Tricks – Pipework Assemblies

Looking for a quick and accurate way to control your pipework fabrications and assemblies? Try using a skeletal layout sketch. See the example below for a simple method to create pipework using Autodesk Inventor or SolidWorks.

  1. Create a layout sketch of the entire pipework assembly using 2D and/or 3D sketches. Use sketch points (SolidWorks) or work points (Inventor) to indicate locations of in-line features (e.g. flange joint).
  2. Save the layout sketch as a part file.
  3. Create a new assembly and insert the layout sketch part as the first part of the assembly. Make sure that the part and assembly origins are aligned.
  4. Add elbows, tees, flanges etc as required. Mate/constrain these parts to the sketch lines/points of the skeletal sketch
  5. Fill in the gaps with straight pipe sections. Mate/constrain the straight pieces to the skeletal sketch lines (concentric) and to the part at one of the ends (e.g. coincident with end face of elbow).
  6. Create any other pipe fabrications using the same method:
  7. Create a new assembly and insert the fabrications. There should be no need to add any mates/constraints because all fabrication origins should be aligned at the assembly origin by default (if necessary, use “ground and root” command (Inventor) to force the origins to align. For SolidWorks, add a coincident “mate” between the fabrication origin and assembly origin and check the “align axes” box).
  8. If the pipework includes some pipe pieces which are bent (rather than using welded elbows), then “derive” the skeletal sketch part into each bent pipe part and use the skeletal sketch lines to drive the pipe’s geometry.

The above method is fairly simple, yet can be applied to very complex pipework assemblies and manifolds.