Expand IntroductionIntroduction
Expand AdministrationAdministration
Expand User InterfaceUser Interface
Expand SOLIDWORKS FundamentalsSOLIDWORKS Fundamentals
Expand Moving from 2D to 3DMoving from 2D to 3D
Expand AssembliesAssemblies
Expand CircuitWorksCircuitWorks
Expand ConfigurationsConfigurations
Expand SOLIDWORKS CostingSOLIDWORKS Costing
Expand Design CheckerDesign Checker
Expand Design Studies in SOLIDWORKSDesign Studies in SOLIDWORKS
Expand Detailing and DrawingsDetailing and Drawings
Expand DFMXpressDFMXpress
Expand DriveWorksXpressDriveWorksXpress
Expand FloXpressFloXpress
Expand SLDXML Data ExchangeSLDXML Data Exchange
Expand Import and ExportImport and Export
Expand Model DisplayModel Display
Expand Mold DesignMold Design
Expand Motion StudiesMotion Studies
Expand Parts and FeaturesParts and Features
Collapse RoutingRouting
Expand Sheet MetalSheet Metal
Expand SimulationSimulation
Expand SimulationXpressSimulationXpress
Expand SketchingSketching
Expand Sustainability ProductsSustainability Products
Expand SOLIDWORKS MBDSOLIDWORKS MBD
Expand SOLIDWORKS UtilitiesSOLIDWORKS Utilities
Expand TolerancingTolerancing
Expand TolAnalystTolAnalyst
Expand ToolboxToolbox
Expand WeldmentsWeldments
Expand Workgroup PDMWorkgroup PDM
Expand TroubleshootingTroubleshooting
Glossary
Hide Table of Contents

Geometry Requirements - Tube Section

The following items are required for a component to be used as a Tube Section in SOLIDWORKS Routing.

Names of routing sketches and dimensions are case sensitive.

Pipe Sketch

  • A front-oriented sketch named PipeSketch
  • Two concentric circles, centered at the origin of the sketch, with dimensions named:
    • InnerDiameter@PipeSketch
    • OuterDiameter@PipeSketch
  • The inner circle must be defined as For construction
To avoid errors in the sweep feature when creating tube routes, the tube thickness should be no greater than 0.25 times the outer diameter. (That is, make the outer diameter no more than twice the inner diameter.)

Example:
pipesketch.gif

Sweep-path sketch

  • In a 3D sketch, a line normal to the PipeSketch
  • A concentric relation between the endpoint of the line and the centerpoint of the circles

Example:
tube_sweep_path.gif

Feature

A Sweep FM_sweep_feature.gif using:
  • PipeSketch for Profile
  • The 3Dsketch for Path
  • The Thin Feature option to set the wall thickness

Example:
pipepart_no_dimension.gif

Filter Sketch

  • A sketch named FilterSketch
  • A circle with a dimension named NominalDiameter@FilterSketch

Example:
filtersketch.gif



Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Geometry Requirements - Tube Section
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:

x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: SOLIDWORKS 2015 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.

0.20.26