Routing To

Routing From

· Routing - Pipes and Tubes

· SolidWorks Routing

· Create a special type of sub-assembly that builds a path of pipes, tubes, or electrical cables between components

· Lessons:

· Pipe and Tube Routes

· Customizing a routing template

· Adding parts to the Routing Library

· Creating route paths by various automatic and manual methods

· Route Drawings

· Create a drawing for assembly

· Drawing includes

· Bill of materials

· Pipe length information

· Auto balloons

· Start Lesson

· Activate SolidWorks Routing add-in

· Click Tools, Add-Ins

· In Active Add-ins column

· Select SolidWorks Routing to activate it

· Click OK

· Customizing Routing Templates

· In Windows Explorer

· Hidden files and folders visible

· Default template location

· Options > File Locations

· Under Show folders select Document Templates

· Click OK

· Browse to template

· In Windows Explorer, browse to your default template location

· Default routing template: routeAssembly.asmdot, appears in the folder

· Close Windows Explorer

· Open routeAssembly.asmdot

· Save As MyRouteAssembly.ASMDOT

· Options

· In dialog box

· On Document Properties tab, select Units

· Under Unit system, select IPS (inch, pound, second)

· Click OK

· Specify that the folder is a template location

· Click Options

· In the dialog box

· Select File Locations

· Under Show folders for select Document Templates

· Click Add and browse to C:\MyRoutingTutorial

· Click OK to close Browse For Folder dialog box

· Click OK

· C:\MyRoutingTutorial is added to list of document template folders, and its contents are now available for selection in New SolidWorks Document dialog box

· Specify to use your custom template as default routing template

· In Options

· Routing > Routing File Locations

· On the File Locations tab, for Routing template, click (...)

· New SolidWorks Document dialog box appears

· It has a tab corresponding to folder you created (C:\MyRoutingTutorial)

· On the MyRoutingTutorial tab, select MyRouteAssembly

· Click OK

· Click OK again

· Custom routing template is now default routing template used when you create new route sub-assemblies

· Adding Parts to Routing Library

· In Task Pane:

· Click Design Library tab

· Browse to Design Library\routing\tubing

· The tubing folder contains sub-folders, such as flanges, tees, tubes

· At top of Task Pane click Create New Folder

· Type tutorial for folder name and press Enter

· Add tube - rubber.sldprt to tutorial folder

· At the top of the Task Pane, click Add to Library

· In the PropertyManager

· For Items to Add, select tube - rubber at the top of the flyout FeatureManager design tree

· Under Save To, make sure the tutorial folder is selected under Design Library folder

· Click OK

· The part is added to the Routing Library, and is available for selection when you create a route

· Close the part

· Starting a Route

· Add pipe and tube routes to an assembly

· Open Piping-Tubing.sldasm in ...\routing-pipes\Piping-Tubing.sldasm)

· Save the assembly as MySkid.sldasm (in the same folder as Piping-Tubing.sldasm)

· Assembly already contains a filter, a regulator, and three flanges that need to be connected by pipe or tube routes

· If shadows are on, turn them off by clicking Shadows In Shaded Mode (View toolbar)

· Start first route by dragging a flange into assembly

· Use tools on View toolbar to zoom, rotate, and pan model view to facilitate working with model

· In Piping toolbar

· Click Start by Drag/Drop

· Design Library opens to piping section of Routing Library

· In lower panel double-click flanges folder

· Drag Slip on weld flange.sldprt from library to the flange face on the regulator

· Drop flange when it snaps into place

· In the dialog box

· Select Slip On Flange 150-NPS4

· Click OK

· Route Properties PropertyManager appears

· For this tutorial use default settings

· Click OK (green check)

· Click Yes to message

· Want to turn off the option Update component names when documents are replaced

· The following happens

· A 3D sketch opens in a new route sub-assembly

· Pipe1-MySkid appears in FeatureManager design tree

· A stub of pipe appears, extending from flange we just placed

· Creating the Route

· Start creating segments of route

· Drag endpoint of stub to increase pipe length

· We do not need to be exact

· Message appears about not adding automatic relations

· Click OK

· Add the horizontal flange to the route, so you can connect the pipe to it

· Zoom to the horizontal flange

· On View menu make sure Routing Points is selected and Hide All Types is cleared

· Move pointer over connection point (CPoint1) in center of flange

· When connection point is highlighted

· Right-click CPoint1 and select Start Route (Add to Route!)

· A stub of pipe extends from flange

· Add a line to connect the two pipe segments

· Click Line (Sketch toolbar)

· Sketch a line between the endpoints of the stub and the longer pipe segment

· A new segment of pipe is added

· Elbows are automatically added

· In Line Properties PropertyManager, under Add Relations, click AlongZ

· The line aligns along the Z axis

· The lengths of the other pipes adjust

· Click in the Confirmation Corner to exit the sketch

· A part file is created for the pipe segments you defined. A message informs you that you need to name the part file

· Click OK

· Click Save

· The part file is saved using the default name 4inSchedule40-Pipe1-MySkid.sldprt

· In the FeatureManager design tree, expand routeAssembly1-MySkid

· The components of route sub-assembly are listed

· Flange

· Two elbows

· Three pipe segments

· Adding a Tee Fitting

· First add a point where you want to place the fitting

· Click Edit Pipe Route (Piping toolbar)

· The 3D route sketch opens

· Click Split Entities (Sketch toolbar)

· Click the centerline of the pipe approximately where shown to add a split point

· End Split Entities command before next step

· Use Esc key or click selection arrow

· Drag a tee fitting to the split point

· In Design Library, click tees folder in the upper panel to display its contents in lower panel

· Drag (but do not drop) reducing outlet tee inch from the Design Library to the split point

· Press Tab to rotate the tee fitting

· Drop fitting when it is oriented up

· Adding a Flange

· Now route the pipe from the tee fitting to the upper flange

· First you need to add the flange to route

· Zoom to the upper flange

· Move the pointer over connection point (CPoint1) in center of flange

· Pointer changes and connection point is highlighted

· Right-click CPoint1 and select Add to Route

· Stub of pipe extends from flange

· Creating an Orthogonal Route

· Use Auto Route to automatically create an orthogonal route from the tee fitting to flange

· Click Auto Route (Routing Tools toolbar)

· Select the endpoints of two stubs (one at tee fitting, the other at the flange)

· Points are listed under Current Selection in PropertyManager

· Because this is a rigid pipe route, Orthogonal route is automatically selected under Auto Route

· An orthogonal route between the two points appears in the graphics area

· In PropertyManager, under Auto Route, for Alternate paths, click the up and down arrows until path appears as shown

· Click OK (green check mark)

· Click icon to exit 3D sketch in Confirmation Corner to exit the sketch

· Click OK

· Save new pipe part

· Adding a Ball Valve Assembly

· Create another split point

· Click Edit Pipe Route (Piping toolbar)

· The 3D route sketch opens

· Click Split Entities (Sketch toolbar)

· Click centerline of pipe approximately where shown to add a split point

· Press Esc to turn off Split Entities tool

· Manually Sketching a Route

· Create a route from lower flange to pipe that runs between ball valve assembly and tee fitting

· Zoom to the lower flange

· Move pointer over connection point (CPoint1) in the center of flange

· Right-click CPoint1 and select Add to Route

· Click Line (Sketch toolbar) and sketch lines approximately

· Sketch the straight lines only - sketch fillets are added automatically

· Make endpoint of new route coincident with centerline of larger pipe

· Press Esc to turn off Line tool

· Select end point of the newest route

· Hold down Ctrl and select centerline of larger pipe

· In PropertyManager under Add Relations select Coincident

· Last route segment and all segments in same plane move to a plane coincident with the centerline of the larger pipe

· Align pipe with weldment section in bottom frame of main assembly

· Click Top (Standard Views toolbar)

· Drag the route so that pipe is over weldment section

· Click Isometric (Standard Views toolbar)

· Close sketch, and save new pipe part when prompted

· Creating A Flexible Tube Route

· All route segments you have created so far are part of same route sub-assembly

· Now create a new route sub-assembly containing a flexible tube route between tube fittings on the tops of regulator and filter

· First Change editing focus from route sub-assembly back to the top-level assembly

· Click Edit Component (Assembly toolbar)

· The editing focus changes back to the top-level assembly

· Save assembly

· Click View Routing Points (View toolbar)

· Right-click CPoint2 on fitting on top of regulator and select Start Route

· In PropertyManager under Tube

· Open tube-rubber.sldprt in ...\tutorial

· Or use default stainless steel part tube-ss.sldprt

· Click OK

· A stub of tubing extends from fitting

· Drag endpoint of stub to make stub longer

· Add other fitting to route

· Right-click CPoint2 on other fitting (on top of the filter) and select Add to Route

· Drag endpoint of stub to make stub longer

· Create the route

· Click Auto Route (Routing Tools toolbar)

· For Current Selection in PropertyManager

· Select the endpoints of two stubs

· A spline is added to complete route between two points

· Click OK

· Close sketch, and save new tube part when prompted

· New route sub-assembly appears in FeatureManager design tree

· Click Isometric (Standard Views toolbar)

· Click Edit Component (Assembly toolbar) to change the editing focus back to top-level assembly

· Click View Routing Points (View toolbar) to turn off display of routing points

· Save assembly

· Congratulations! We completed Pipe and Tube Routes lesson.

· Route Drawings

· Open FinalSkid.sldasm in ...\samples\tutorial\routing-ipes\FinalSkid.sldasm

· Click New

· In New SolidWorks Document dialog box

· Click Advanced

· On the Templates tab, click Drawing

· Click OK

· In the Sheet Format/Size dialog box

· Select Standard sheet size

· Select D - Landscape

· Click OK

· A new drawing opens and Model View PropertyManager appears

· Inserting a View

· Place a view of assembly on drawing sheet

· In the PropertyManager

· Under Part/Assembly to Insert

· Select assembly

· Click Next - right facing arrow at top of Properties (PropertyManager)

· Under Orientation, for Standard views, select *Isometric

· Under Display Style, select Shaded With Edges

· Under Dimension Type, select True

· In graphics area, click to place view

· Click OK (green check mark)

· Add a BOM

· Click Bill of Materials (Assembly toolbar)

· In PropertyManager

· BOM Type

· Select Parts only

· Click OK

· In graphics area, click to place BOM

· Click OK

· Zoom to BOM table

· Notice there is no information about pipe lengths

· Change DESCRIPTION column to display information about pipe lengths

· Move the pointer over column header (C) for DESCRIPTION column

· Pointer changes to down arrow

· Click to select column

· The column pop-up toolbar appears

· Click Column Property (column pop-up toolbar)

· In dialog box

· For Column type

· CUSTOM PROPERTY

· Property name

· Select SWPipeLength (only LENGTH available)

· Column heading changes to LENGTH and lengths appear for all pipe and tube parts (No lengths?)

· Double-click column heading and change it to Pipe Length

· To change units of measure for Pipe LengthClick Options > Document Properties tab

· Select Units

· Select desired units

· Changing the View

· Change scale of the view by changing scale of drawing

· Click Zoom to Fit (View toolbar)

· In the FeatureManager design tree, right-click Sheet1 and select Properties

· Change Scale to 1 : 8 (was 1 : 20)

· Click OK

· Select view in graphics area

· Drag to position it on sheet

· Adding Balloons

· Select the drawing view

· Click AutoBalloon (Annotation toolbar)

· In PropertyManager

· Balloon Layout

· Select

· Square

· Ignore multiple instances

· Balloon Edges

· Click OK (green check arrow)

· Save drawing

· Congratulations! Tutorial completed.