Print Queue

Navigation Tips

• Use Next or Previous at the bottom-left to advance to the next page or return to the previous one.

Next

1. To create a backup copy of the sample tutorial files, open the Tutorial Files Tube and Pipe folder. Then copy the files into your backup folder.
   TipAfter you finish the exercises, you can replace the changed sample files with the original files.
2. To set the project, click ManageProjects.
3. In the Projects dialog box, double-click the tutorial_files project to make it the active project.
4. Review the setting of Use Style Library property. If appropriate, change the setting.
   NoteTo ensure that conduit parts are created with the correct material definition, Use Style Library must be set as Yes or Read Only.
5.  Click the Configure Content Center Libraries button and confirm that Content Center libraries are available and selected. Then close the Configure Libraries dialog box.

   Tube and Pipe assemblies use Content Center parts. If Content Center libraries are not available, you cannot populate Tube and Pipe routes. If needed, see the Content Center or Tube and Pipe chapter in the Help for more information.

6. Click Save and Done to close the Projects dialog box.

Previous | Next

1. Click Open.
2. Open the AirSystemAssy.iam assembly in the Tutorial Files Tube & PipeAir System folder.
   
3. On the ribbon, click Environments tab Begin panel Tube and Pipe.
4. On the Create Tube & Pipe Run dialog box, enter AirSystem1 as the Run File Name. Accept the other defaults and click OK.

   The individual run is activated in the browser. The Pipe Run tab displays on the ribbon.

5. On the Manage panel of the Pipe Run tab, select the ASTM A53/A53M-ASME B16.11 - Welded Steel Pipe from the list to set it the active style.

   A tube and pipe style is a named group of settings that describe tube and pipe characteristics for automatic populating routes and runs. The selected style will be used after you finish creating the route.

Previous | Next

1. On the ribbon, click Pipe Run tab Route panel New Route.
2. On the Create New Route dialog box, accept the default route file name and location, and click OK.

   A pipe route is added to the active run and activated. The Route tab displays on the ribbon.

3. On the ribbon, click Route tab Create panel Route.
4. In the graphics window, zoom in the model. Then pause the cursor over the circular geometry of the first Air Cylinder as shown in the following image. If appropriate right-click and click Select Other Direction.
   
5. Click the circular geometry to select it as the start point.

   This point is associated with the component that contains the selected circular edge. A work point is added to the piping route.

6. For the second route point, select a point on the line extender or existing geometry. To route through the IBeam, pause the cursor over the left arc of the IBeam opening.
   

   Rotate and zoom in to view the arc. Make sure that the line is pointing to the approach direction of the route.

   NoteTo flip the direction of a displayed axis, press the spacebar or use the Select Other tool.
7. Click the geometry to select it as the second point.

   As soon as you make your selection, the route generates to that point and the Select Other tool appears indicating that multiple solutions exist. Click the arrows to cycle through the solutions.

   
8. Click the green area in the Select Other tool to select the solution from the previous image.
   
9. In the Model browser, verify that the Autoroute browser node is added and contains five route points.
   

Previous | Next

1. Right-click in the graphics window and verify that Auto-Dimension is enabled.
2. Pause the cursor over the red line extender, right-click, and select Enter Distance.
   
3. Enter 3.4 inch in the Enter Distance box, and then click the green check mark.

   The point is created on the screen, and the 3D Orthogonal Route tool is displayed at the new point. This time, since the new point is an arbitrary point in space, all directions are enabled and selectable, except backwards.

   

Previous | Next

1. Rotate your view to look at the front of the assembly.
   TipClick Right on the view cube to rotate the view to the desired position.
   
2. Pause the cursor over the red direction axis of the 3D Orthogonal Route tool, right-click, and select Parallel With Edge.

   The system prompts you to select a linear edge.

3. Select the linear edge on the path part as shown in the following image, and click to set the selection.
   

   The red direction axis is reoriented to the direction of the selected edge. The included reference geometry is added to the Included Geometry folder in the Model browser.

   
4. Pause the cursor over the red axis, right-click, and select Enter Distance. Then enter 4.3 inch in the Enter Distance box, and then click the green check mark.
   
5. Verify that a bend is automatically added between the new segment and the preceding segment.
6. For the next point, right-click the red direction axis again and select Parallel With Edge.
7. Select the other linear edge on the path part as shown in the following image.
   
8. Before creating the next route point, right-click in the graphics window and clear the Auto-Dimension check mark.
9. Click anywhere in the forward direction on the red direction axis. The segment length is not important.
10. Right-click in the graphics window and select Done.
11. Verify that the new segment is not dimensioned.
    

Previous | Next

1. On the ribbon, click Route tab Create panel Route.
2. Click the left circular opening on the valve part.
   
3. Right-click in the graphics window and select Point Snap.
4. Move the cursor over the last segment you created in the preceding exercise.

   A dashed line representing the snap point is displayed from the cursor to the preview point. A preview point is displayed at the intersection of the line and the axis.

   
5. After the dashed line and the intersection point appear, click the sloping segment to set the snapped route point.
   
6. Right-click and select Done.
   

Previous | Next

1. On the ribbon, click Route tab Constrain panel Coincident.
2. Select the two separate route points as shown in the following image.
   

   The separate sketches form a closed route.

   
3. Right-click in the graphics window and select Done.
   
4. Notice that an error icon displays beside the route.
   

   Placing the coincident constraint causes an odd (not 90-degree, 45-degree, or combined135-degree) angle between the two segments so the route is in error. In the exercise that follows, you create a bend to fix the violation.

Previous | Next

1. To verify the errors in Route01, right-click the route in the Model browser and select Show Violations.
2. To identify the route part in error, click the error on the Show Violations dialog box, and then view the error in the graphic window.

   The invalid angle is between the two segments as highlighted in the following image.

   
3. Click OK to close the Show Violations dialog box.
4. On the ribbon, click Route tab Create panel Bends.
5. Enter 0.5 inch in the Bend dialog box. Then select the two segments that form the invalid angle.

   The bend is created with a radius value of 0.5 inch. The error icon in the Model browser disappears.

   
6. Close the Bend dialog box.
7. To end the route, right-click and select Finish Edit.

Previous | Next

1. On the ribbon, click Pipe Run tab Route panel Populate Route.

   The route is populated using the selected style. When a route is populated, all segments and fittings are added to the associated run folder.

   
2. To edit the current tube and pipe style, double-click Route01 in the Model browser.
3. On the ribbon, click Route tab Manage panel Tube and Pipe Styles. The Tube & Pipe Styles dialog box displays.
4. Right-click the ASTM A53/A53M-ASME B16.11 - Welded Steel Pipe style in the style browser and click Edit.
5. Select 1/4 in from the Diameter list, and click Save.
6. Click Close to close the dialog box.
7. Right-click and select Finish Edit to populate the route using the edited style.
   

Previous | Next

1. Double-click Tube & Pipe Runs in the Model Browser.
2. On the ribbon, click Tube and Pipe tab Run panel Create Pipe Run.
3. On the Create Run dialog box, enter AirSystem2 as the Run File Name. Accept the other defaults and click OK.

   The individual run AirSystem2:1 is added and activated in the browser. The Pipe Run tab displays on the ribbon.

4. On the Pipe Run tab, Manage panel, select the Hydraulic Hose - Female Thread - Swivel style from the Active Style list.
5. On the ribbon, click Pipe Run tab Route panel New Route.
6. On the Create New Route dialog box, accept the default route file name and location, and click OK.

   A pipe route is added to the active run and activated. The Route tab displays on the ribbon.

7. On the ribbon, click Route tab Create panel Route.

   The start fitting specified by the hose style is attached to the cursor and ready for placement.

   
8. Move the cursor on the circular edge as shown in the following image. Then click to set the start fitting.
   NoteThe direction axis on the part must point in the direction of the route.
   
9. The end fitting appears and is attached to the cursor. Notice that the start fitting and end fitting reference the same part in this style.
10. Move the cursor to the circular opening on the valve part.

    If the orientation of the fitting is not correct, right-click and select Next Connection.

    
11. Click to place the end fitting. The route line displays.
    

Previous | Next

1. To add an intermediate node tangent to a circular edge on IBeam, move the cursor close to the circular edge. The circular edge is highlighted.
   

   Then click to set the hose node.

   
2. Right-click and select Finish Edit.

   The run environment is activated.

3. To populate the hose route, click Pipe Run tab Route panel Populate Route.

   After the route is populated, a Flexible Hose part, start fitting, and end fitting are added to the Model browser. Notem them at the bottom of the flexible hose assembly.

   

Previous | Next

In this tutorial, you learned how to:

• Create a tube and pipe assembly.
• Set a tube and pipe style.
• Create rigid piping and bent tubing routes.
• Populate selected routes with library components.
• Edit a Tube and Pipe style.
• Create and populate a flexible hose route.

What Next? - As a next step, you can continue with the following Tube and Pipe tutorials. For example, learn more about Tube and Pipe Styles in the Tube and Pipe Styles. Then change the styles used on the AirSystemAssy.iam to correspond to your company standards.

Previous

Click here to return to the tutorials home page