How to Create a Custom Tube and Pipe Style in Inventor

Why Create a Custom Pipe Style?

Autodesk Inventor's Tube and Pipe module comes with many built-in piping styles covering common standards (ASME, DIN, ISO, JIS). But when your design requires a non-standard pipe specification — custom wall thicknesses, unusual sizes, or proprietary fittings — you need to build a pipe style from scratch.

A complete rigid pipe style requires four components: a Pipe, a Coupling, a 90-degree Elbow, and a 45-degree Elbow. Each is built as a parametric iPart (a single part file containing a table of size variations), then published into a custom pipe style that Inventor's routing tools can use.

This guide walks through the full process. If you need custom tube fabrication for your piping projects, check out our tube machining services.

Overview

1. Create the 90-degree Elbow solid and turn it into an iPart
2. Create the 45-degree Elbow by modifying the 90-degree
3. Create the Coupling solid and iPart
4. Create the Pipe component and iPart
5. Publish all components into a new Pipe Style
6. Use the style in your tube and pipe assemblies

Each component is built with User Parameters that control the geometry, so the iPart table can drive different sizes from a single part file.

Step 1: Create the 90-Degree Elbow

Build the Solid

1. Create a new Standard (mm) part file
2. Set the material via File > iProperties > Physical (e.g. PVC-Piping, Steel)
3. Make all Origin Planes, Axes, and Centre Point visible
4. Create a 2D Sketch on the XY Plane
5. Draw two concentric circles at the centre point — the outer circle is the pipe OD (e.g. 100mm diameter), the inner circle defines the bore (e.g. 90mm for 10mm wall thickness)
6. Add a construction centreline parallel to and above the X Axis at the revolve distance (e.g. 200mm from centre)
7. Finish the sketch and create a 90-degree Revolve of the annular area between the two circles, using the centreline as the revolution axis

This creates the basic elbow shape — a quarter-turn of hollow pipe.

1. Switch OFF visibility of Origin Planes, Axes, and Centre Point
2. Before the next steps, go to Tools > Application Options > Sketch tab and ensure "Autoproject edges for sketch creation and edit" is ticked. This automatically projects face edges when you sketch on a face
3. Create a 2D Sketch on the front elbow face — it will automatically pick up the inner and outer circles
4. Finish the sketch, then Extrude the ring profile outward by 20mm — this creates the connection stub
5. Repeat for the top face — sketch on it and extrude 20mm outward
6. Save the file (e.g. "90 degree Elbow.ipt")

Add User Parameters

Open the Parameters dialog (Manage > Parameters) and add these User Parameters:

Now link each parameter to the geometry:

• Sketch outer circle diameter → OD
• Sketch inner circle → OD - WallThk (derived)
• Centreline offset → RevDist
• Revolve angle → RevAngle
• Both extrusion distances → ElbowExt

Tip: To see which parameters are assigned where, go to Sketch > Options > Document Settings and set Modelling Dimension Display to "Display as expression".

Turn It into an iPart

1. Go to Manage > Author > Create iPart
2. In the iPart Author dialog, add rows for each pipe size:

1. Remove the Part Number column from the Properties tab
2. Set the OD column as Key > 1 (right-click the column header) so Inventor selects the right size automatically
3. Click OK

Excel editing tip: Right-click the Table in the browser and select "Edit via Spreadsheet". This opens Excel where you can fill values much faster. Use CONCATENATE formulas for member names, e.g.: =CONCATENATE("90 degree Elbow ",B2," dia")

1. Back in Inventor, activate each table row one at a time and verify the geometry updates correctly
2. Save the file

Step 2: Create the 45-Degree Elbow

You don't need to start from scratch — the 45-degree elbow is a copy of the 90-degree:

1. SaveAs the 90-degree elbow file with a new name (e.g. "45 degree Elbow.ipt")
2. Right-click the Table in the browser and select "Edit via Spreadsheet"
3. In Excel, change all RevAngle values from 90 to 45, and update the member names accordingly
4. Save and close Excel
5. Back in Inventor, activate each size row and verify the geometry — the revolve angle should now be 45 degrees
6. Save and close the file

The parametric model handles everything because the revolve angle is driven by the RevAngle parameter.

Step 3: Create the Coupling

Build the Solid

1. Create a new Standard (mm) part file, set the material
2. Sketch on XY Plane: two concentric circles (OD and OD minus wall thickness)
3. Extrude the ring symmetrically by the coupling gap distance (e.g. 20mm symmetric = 40mm total length)
4. Create a second sketch on the XY Plane with a larger circle (OD + coupling thickness for the flange)
5. Extrude this outer ring symmetrically by the total coupling length (CoupLength + CoupGap)
6. Hide Origin geometry and save (e.g. "Coupling.ipt")

Add User Parameters and iPart

Link parameters to geometry, then create the iPart table with matching OD sizes. Set OD as Key > 1. Verify all sizes.

Step 4: Create the Pipe Component

1. Create a new Standard (mm) part file
2. Sketch on XY Plane: two concentric circles (OD and OD minus wall thickness)
3. Extrude the ring to a nominal length (e.g. 500mm) — the actual routing length is set by Inventor when placed

User Parameters

Create the iPart table with matching OD sizes. Set OD as Key > 1.

Step 5: Publish the Components

Each component needs publishing so Inventor's Tube and Pipe module recognises it:

1. Open the 90-degree elbow iPart
2. Go to Manage > Publish Component
3. In the Pipe Fitting Authoring dialog:

- Set Connection 1: select the end face, set as "Fitting to Pipe" type

- Set Connection 2: select the other end face, same type

- Verify the engagement length matches your ElbowExt parameter

1. Save

Repeat for the 45-degree elbow, coupling, and pipe (pipe connections use "Pipe" type rather than "Fitting to Pipe").

Step 6: Create the Pipe Style

1. In a Tube and Pipe assembly, open the Pipe Style editor
2. Create a new style and name it
3. Under Components, add your four published iParts (Pipe, Coupling, Elbow 90, Elbow 45)
4. Set up the diameter table with your available OD sizes
5. Save the style

Your custom pipe style is now available for routing. When you draw pipe runs, Inventor automatically inserts the correct-size fittings.

Tips

• Consistent sizing — use the same OD values across all four components so they mate correctly
• Excel for iPart editing — much faster than the Inventor table editor for many size rows
• Test every size — activate every iPart row to verify geometry before publishing
• Shared storage — store custom styles on a network drive so your team can access them
• Backup source files — keep the original iParts. To add sizes later, edit the source and re-publish

Related Resources

For physical tube fabrication, we offer tube machining services including CNC turning, threading, coning, and welding of stainless steel tube.

More CAD guides:

• How to Prepare DXF Files for Laser Cutting
• How to Design for Sheet Metal
• Convert 3D Scan to STEP in Fusion 360
• K-Factor Explained — understanding bend allowances

Need parts manufactured? Upload your STEP or DXF to our instant quoting tool for immediate pricing. Get a quote →