This chapter will cover the tools of the routed systems environments found in the Inventor Professional suite and the Inventor routed systems suite. Two primary tool sets comprise Inventor routed systems: tube and pipe and cable and harness. The tube and pipe tools are used in routing pipe and hosing through mechanical assembly designs. The cable and harness tools are used for electrical design where routing wires and cables around obstacles and checking for fit are important.
In this chapter, you'll learn to:
Create routes and runs
Author a tube and pipe component
Author an electrical component
Create and document cable and harness assemblies
The tube and pipe tools are based on Inventor fundamental concepts such as sweeps, 3D sketch paths, adaptive parts, subassembly structure, and more. The tube and pipe tools automate many of these fundamentals, making the design of tube and pipe routes faster, more intuitive, and less tedious. However, it is best to have an understanding of these fundamental concepts before jumping into the tube and pipe tools so you can understand how Inventor does things and therefore how to proceed when required to manually adjust or repair your designs. A lack of understanding of these fundamentals can often bring inexperienced Inventor users to a screeching halt in their tube and pipe endeavors and may leave them with a perception that the tools just don't work. Therefore, in the following sections, you will explore how to create routes, runs, and general tube and pipe assembly structure, as well as tube and pipe styles.
Understanding the way that tube and pipe assembly structure is created is an important part of successfully creating and managing your tube and pipe designs. There are three primary levels to any tube and pipe assembly:
A top-level assembly
A tube and pipe runs assembly
A run assembly
All tube and pipe designs are comprised of runs. A run is a subassembly that contains one or more route paths, pipe or hose segments, and fittings. For instance, a standard hot-water supply line is a run.
When you begin a tube and pipe design, you start with a new assembly template and click the Tube And Pipe button on the Assemble tab. Doing so opens the Create Tube & Pipe Run dialog box, prompting you to set a name and location for the tube and pipe runs assembly file and the first run assembly file. Figure 18.1 shows the Create Tube & Pipe Run dialog box for a top-level assembly named mi_18a_051 being created.
Notice that the default paths are created based on where the top-level assembly is stored. In this case, mi_18a_051.iam is stored in a directory called Workspace. The tube and pipe runs assembly is simply a container assembly created to contain the multiple runs you might create in the design. It is prefixed with the top-level assembly name and defaulted to a folder under it named the same as the top-level assembly and then AIPTube and Pipe.
The run assembly is prefixed with the top-level assembly name, given an incremental suffix (in this case 01), and defaulted to the same directory structure plus a subfolder named Run plus the increment number. Although you can change this file structure per tube and pipe assembly, accepting the default does maintain a certain standardization of structure. Figure 18.2 shows the assembly browser structure and file structure of a tube and pipe design set to the default paths.
Once a run is created, you can create a route within it. Routes are 3D sketch paths created to define the path for pipes, tubes, or hoses to follow. In Figure 18.2 there are two elbow fittings (DIN 2605 90 Deg Elbow) that were placed outside of the run and in the tube and pipe runs assembly. Route01 was then created as a component of Run01, starting from one of the DIN elbows and running to the other. Run01 consists of Route01, three Pipe Segments, and two 90 Deg Elbows.
Although the pipe segments and the route path files were saved under the Run01 folder, you'll notice that the elbow files were saved to the Content Center Files path. Because fittings such as elbows, tees, and couplings are generated from Content Center, these part files are automatically saved to the Content Center Files path defined in either your project file or your Application Options settings.
Here are a few things to note when working with tube and pipe runs:
A unique part file is created for each pipe, tube, and hose segment in the run, even if more than one segment is the same length. Although this may seem a departure from what you'd expect, this is key to allowing runs to be edited downstream.
Enter meaningful names for the runs and routes as you create them. As you create more complex designs, the abundance or multiple Route01s scattered throughout the assembly may create confusion during edits.
Runs and routes are determined by tube and pipe styles. Properties such as material, diameter, and fitting types are set in the tube and pipe style. Rules such as minimum and maximum segment length can also be set in the style. The Inventor tube and pipe tools load with several default styles based upon the ANSI, DIN, ISO, and JIS tube and pipe standards and the Parker hose and fittings. Styles fall into three primary categories:
- Flexible hoses
These are single hose segments connected by a start point and endpoint selection. The hose style can include, but is not required, to have fittings for the start and stop points.
- Rigid tubing
This does not contain elbows and follows a default bend radius. The radius can be set per bend as needed. Minimum and maximum segment lengths are set in the style, and couplings are placed where segments connect.
- Rigid piping
These styles are required to include 90-degree elbow fittings and can include 45-degree elbows, flanges, and couplings. There are three subcategories for rigid piping styles:
- Self-draining
These styles require a pipe, a coupling, a 45-degree elbow, a 90-degree elbow, and a custom elbow or tee to match the desired slope angle.
- Welded
These styles require a pipe and a 90-degree elbow. Butt welded styles require a weld gap size.
- Flanged
These styles require a pipe, an elbow, a flange, and optionally a gasket.
Figure 18.3 shows a flexible hose run, a rigid tubing run, and a rigid piping run, from top to bottom.
You can access the Tube & Pipe Styles dialog box from the master tube and pipe runs assembly, the run assembly, or the route by clicking the Tube And Pipe Styles button on the Ribbon or by using the default right-click context menu. The dialog box is divided into a pane on the left listing the styles and two tabs on the right controlling the general settings and the styles rules. Figure 18.4 shows the Tube & Pipe Styles dialog box with a Hydraulic Hose style set active, denoted in bold. A second style is selected and has been right-clicked, showing the options that correspond with the buttons along the top of the dialog box.
When editing, copying, or creating a new style, some components may be either required or optional, depending upon the style type. If the component is not specified and it is required, it will be marked with a red arrow next to it in the General tab. If it is empty and shows a gray arrow, it is optional. When the component is selected, the arrow will be green. Figure 18.5 shows two style types being created from scratch.
On the left side, a Butt Welded style required a pipe and a 90-degree elbow. The pipe has been selected, but the elbow is still required, as indicated by the red (dark) arrow. The 45-degree elbow is not required, and its optional status is indicated by the gray (light) arrow. On the right side of Figure 18.5, a Flanged pipe style is being created; note that more components are listed. Pipe, Elbow 90, and Flange are the component categories required for this style, with Pipe having already been selected. In both images, the user has right-clicked in the Elbow 90 row and selected Browse in order to specify the required elbow type. You can also double-click a row to open the style library browser.
In the style library browser, you can select from the list of available styles based upon the size, schedule, and material settings made in the General tab and the availability from the Content Center library. You can set additional filtering in the style library browser. When you set the filter to a particular standard, the materials available for that particular standard are listed. If an asterisk is displayed, all the content for that setting is displayed.
Back in the Tube & Pipe Styles dialog box, you can specify a minimum and maximum size range for creating route segments on the Rules tab. It is recommended that you set the minimum segment length to at least 1.5 times the nominal diameter value to avoid minimum segment length violations that occur when pipe segments are too small in relation to the nominal diameter.
Each style type has different rule criteria:
For Rigid Tubes, you can set the default bend radius for the bends.
For Flexible Hoses, you can set a minimum bend radius and hose length round-up value.
For Butt Welded pipe styles, you can set the gap size for the groove welds and control the display of the gaps in the graphics display and in drawings.
For a Butt Welded Flanged pipes, you can specify the coupling style.
Fitting connections are determined by the end treatment set for the particular fitting.
All other end treatments use a gap at segments and fitting joints.
Generally, it is best practice to set the style before creating routes and placing fittings. However, you can create and apply styles at any time. Setting styles can be done in a number of ways. You can change the active style for the tube and pipe assembly so that all new runs follow the style; you do this by selecting a style from the Style drop-down. Or you can change the style for the active route by setting that route active and using the Style drop-down to select a different style. You cannot change a rigid pipe route to a flexible hose style, or vice versa. To make such a change, you must delete the route and re-create it.
Tube and pipe components, like components for other applications, require authoring before they can be published into Content Center. The tube and pipe authoring process is more complex because the router uses the component geometry. For example, the router needs to know the difference between a tee and an elbow, and it needs to know how much the connector overlaps the pipe.
In this example, we will show how to author a PVC pipe to an NPT adaptor:
On the Get Started tab, click Open, and browse to the Chapter 18 directory in the Mastering Inventor 2010 folder.
Open file
mi_18a_010.ipt.Switch to the Manage tab, and select Tube And Pipe from the Authoring drop-down list. The Tube & Pipe Authoring dialog box displays, and the part changes to shaded wireframe display.
Select Adapters from the Type drop-down, as shown in Figure 18.6.
Change the number of connections, and observe that the connection buttons update to match. Confirm that Connections is set to 2.
Confirm that the End Treatment is set to Threaded, and enter 1/2 in for the Nominal Size setting.
By default, the button for connection 1 is active. Select one of the circular edges to define the connection point. Click the Axis button, and select the z-axis from the Origin folder in the browser. An arrow displays, showing the connection direction, as shown in Figure 18.7. The default connection type is Female, but you can set it to Male or Neutral (for flanged or butt welded fittings).
The Engagement defines the maximum and minimum overlap between the connector and pipe. The router needs a range because the pipe usually has a minimum length increment. The engagement range allows the router to adjust the position of the pipe in the fittings.
To determine the Engagement, go to the Design Data folder (the default location is
C:Program FilesAutodeskInventor 2010Design Data), and openThreads.xls. Select the NPT For PVC Pipe And Fitting tab. For tapered threads, the engagement value depends on how tightly the fitting is screwed onto the pipe. You need the maximum engagement value, so add the Handtight Engagement value, which is 0.32, and the Wrench Makeup, Internal value, which is 0.1429. Set Max to Distance, and enter 0.4629 for the total value. For Min, divide the hand tight engagement, 0.32, by the total engagement, 0.4629, which comes to 69%.Click the 2 button to define the other connection.
In this example, Socket Welded was chosen as the End Treatment setting, since that seemed to be the best description. You should choose an end treatment that is consistent with your other parts.
Select a circle at the opposite end of the part for the connection point, and select the z-axis again. You will see that the arrow points into the adapter, and the orange line representing the engagement is outside of the part. Using the flip/arrow button next to the Axis button, change the direction so that the arrow is to the outside, and then engagement is to the inside, as shown in Figure 18.8.
The depth of the socket is 0.84 inch. You don't want to design to full depth engagement because of tolerances, so set Max to Distance and specify 0.75 as the depth. For Min, accept the default value of 50%.
The ISOGEN data is optional. For this exercise, this information will be left blank. Click OK to complete authoring the adapter.
Now that the part has been authored as a tube and pipe adaptor, it is ready to be published to a read/write Content Center library. You can find more information on publishing parts to Content Center in Chapter 7.
Fittings can be placed from Content Center or from a user-created directory of authored fittings. As a rule, you should use the place tools found on the tube and pipe tabs rather than placing fittings as you would normal assembly parts. The place options on the tube and pipe tabs ensure that the authored connections are used as intended. Figure 18.9 shows the place options available on the Pipe Run tab.
When fittings are placed, either from Content Center or from a user-defined library of authored fittings, you can drag the fitting over the route segments or nodes, and you will see the placement point appear. Use the spacebar to toggle through available orientations if more than one exists. When you click to place the fitting, the Select Orientation tools appears, allowing you to rotate the orientation to the desired position.
You can edit connections by right-clicking them while the route is active for edits and choosing Edit Fitting Connections. In the Edit Connections dialog box, you can select a segment and then use the X button to remove the connection. You can also select Change Fitting Diameter and Edit Fitting Orientation, as shown in Figure 18.10.
Routes define the path for pipe and hose segments and the corresponding fittings. Route paths can be comprised of only a start point and endpoint or can include as many intermediate points as are required. Several tools and options are used to start and create route paths:
- Authored connection points
You can use any the predefined connection points for any library fitting or custom-authored part. When you move your mouse pointer over the library fitting, the connection point(s) will highlight.
- Circular edges
You can use any circular edge in the assembly to set the route point at the center of it, with the exception of authored parts such as fittings. For those parts, only the authored connection points can be used.
- Precise and offset start points
You can hover your mouse pointer over an edge to display a direction arrow. Running your mouse pointer along that arrow allows you to select the arrow to set the offset at that distance, or you can right-click and choose Enter Distance. If the arrow points the wrong direction, you can use the spacebar to toggle it or right-click and choose Select Other Direction. Figure 18.11 shows the offset start point options.
- 3D Orthogonal Route tool
Once a start point is selected, run your mouse pointer along the projected axis and click or use the right-click menu's Enter Distance option to set a value for the second point. You will then be presented with the 3D Orthogonal Route tool. You can use the control handles to change the angle or rotate the control. The cross arrow toggles between 90-degree and 45-degree solutions, and the arc arrows allow you to rotate the route tool. You can also right-click and choose Custom Bend to enter an angle other than 90 or 45. When the 3D Orthogonal Route tool is displayed, you can use the + and - keys to change the size of it onscreen. Figure 18.12 shows the 3D Orthogonal Route tool used to rotate the route at 60 degrees.
- Route nodes
When placing a point along a route or setting an offset start point, you will see a colored dot tracking along the route tool. If it is a yellow X, the offset is not enough to create a minimum segment as set in the style rules, and the point cannot be selected. If it is a blue dot, the segment might be too short to accommodate an elbow, but you are allowed to select it. If it is a green dot, the location is satisfactory to all of the style rules. In Figure 18.13 the node showing 5.537 appears in is green and indicates the location will produce no issues.
- Autoroute options
You can select the start point and endpoint of a route and use the Autoroute tool to flip through the available Autoroute solutions. You can also use this to close two parts of an already created route. Use the Select Other tool to toggle through all the Autoroute variations. Once an Autoroute is created, use the Move Segment button to adjust the segments and create new solutions. Figure 18.14 shows a variation with five segments at 29.268 inches on the left and an adjustment being made later using the Move Segment tool on the right.
- Sketched routes
You can use the Include Geometry tool to include any existing part edges in the route. You can also switch to the 3D Sketch tab while creating a route and use the standard 3D sketch tools to create route geometry as required.
Rigid pipe routes consist of a series of line segments connected by arcs. They are essentially just specialized 3D sketch paths created with the purpose-built tube and pipe tools. To create rigid pipe runs, use these general steps:
From an assembly containing objects you want to create a route between or around, click the Tube And Pipe button found either on the Assemble tab or on the Environments tab.
Enter the name of the master tube and pipe run assembly name and the name of the first run. Set the save location as well if they differ from the default file paths.
Click the Tube And Pipe Style button, or use the Style drop-down to set the active style.
With the run active, click the New Route button, and enter a new route name (and location if not using the default).
Place fittings or other component as required.
Click the Route button, and then select the start point of the route.
Set route points using the 3D Orthogonal Route tool, or select the endpoint of the route and use the Autoroute option to generate the route.
When the route is complete, right-click and choose Continue, and then right-click and choose Done to exit the route tool.
Select the Finish Route button.
On the Pipe Run tab, click the Populate Route button. If you are creating many routes, you might want to leave them unpopulated until the end, because populated routes require more system resources.
Flexible hose routes are similar to rigid pipe routes with a few exceptions. The primary difference is that flexible hose paths consist of a single spline segment, whereas rigid pipe paths are a series of line segments connected with arcs. Flexible routes offer a couple of tools and options specific to this type of route, such as the ability to right-click a surface, select Enter Offset, and then adjust the hose length. You can use these options in the general steps to create flexible hose routes listed here:
From an assembly in which you want to create a route, click the Tube And Pipe button either on the Assemble tab or on the Environments tab.
Enter the name of the master tube and pipe run assembly name and the name of the first run. Set the save location as well if it differs from the default file paths.
Click the Tube And Pipe Style button, use the Style drop-down to set the active style, and choose a flexible hose style.
With the run active still, click the New Route button, and enter a new route name (and location if not using the default).
Place fittings or other component as required.
Select a start point for the route to place the first fitting (assuming a hose style that includes fittings).
Select an endpoint for the route to place the second fitting (assuming a hose style that includes fittings).
Select additional geometry to use for the route. For instance, you can right-click and select Enter Offset to specify an offset distance from the location you select on the reference face.
Right-click and select Done. Use the Insert Node tool to add adjustment nodes if required.
Select the Hose Length tool on the Manage panel of the Route tab, and adjust the hose length to add or remove slack.
Finish the edit, and populate the route.
Often isometric centerline drawings are required for straight pipe fittings documentation of tube and pipe designs. The ISOGEN Output tool is available on both the Tube And Pipe tab and the Pipe Run tab. You can save all your tube and pipe runs as an ISOGEN (*.pcf) file directly from the master run assembly; just click the ISOGEN Output button on the Tube And Pipe tab. Or you can use the ISOGEN Output button while at the individual run level to save just that run. When flanged routes are created, gaskets are required for flanged connections if ISOGEN files are to be created from them.
The cable and harness tools in Inventor are based on the fundamental tools of part and assembly creation; however, the parts and assemblies created with the cable and harness tools are structured differently than standard part and assembly models. Understanding these differences requires a solid understanding of the way that standard part and assemblies are created and structured. In the following sections, you will explore the creation and placement of electrical parts, harnesses, wires, cables, and segments, as well as how to copy and document cable and harness designs.
You can use any Inventor model as an electrical connector by adding cable and harness–specific pin features to them. Parts can be created from scratch using standard modeling techniques or downloaded from supplier websites, as well as a number of 3D content websites such as http://mfgcommunity.autodesk.com/content/. When downloading content from the Internet, you will often find models in other formats such as STEP, IGES, Solidworks, and so on. These files can be translated into Inventor files using the methods described in Chapter 14.
The basic steps to turn a standard Inventor part into an electrical component are as follows:
Open the part file in Inventor.
Click the Place Pin tool in the Harness panel of the Model tab.
Select one of the following to place the pin:
Center point of any circular edge, face, or hole
Visible sketch points
Work points
Model vertex points
Any model face
Enter a unique pin name/number.
Click the Harness Properties button in the pin naming input box to enter additional pin properties if required.
Repeat steps 3 through 4 for each pin.
Click the Harness Properties tool in the Harness panel of the Model tab.
Enter a reference designator (RefDes) placeholder. The RefDes property is intended to be used at the assembly level where each instance of the connector will have a unique RefDes.
Select a Gender option (Male, Female, or None).
Set a wire offset point if required.
In the following steps, you will open an existing Inventor part file and create pins as just described. Figure 18.15 shows the Harness tools available in the parts environment.
On the Get Started tab, click Open.
Browse for the file named
mi_18a_007.iptin the Chapter 18 directory of the Mastering Inventor 2010 folder, and open it.Click the Place Pin button in the Harness panel of the Model tab.
Enter A1 in the Place Pin input box, and click the Harness Properties button.
Select the Custom tab, click the Name drop-down, and select Embedded Length.
Enter 5mm in the Value input box, and then click OK. Then click the green check mark, or press Enter on the keyboard to set the pin.
To place the next pin, click the rounded edge on one of the top cutouts, enter A2 for the pin name, and then set the pin without entering any harness properties.
Click roughly in the center of the blue square face to set the third pin, and enter B1 for the name.
Right-click and click Done to exit the Place Pin tool.
In the Work Features panel of the Model tab, click the Point button to create a work point.
Right-click and select Loop Select, and then click the square profile edge for the remaining cutout. Be certain you are selecting the outer edge loop and not the inner loop. Right-click and click Done.
Select the Place Pin tool again, and select the work point you just created. Set the name to B2, right-click, and choose Done.
Next edit Extrusion1, and change the Distance from 10mm to 15mm.
Notice which work points hold their positions relative to the geometry and which ones remain at the position they were created in. You can right-click the pins that didn't update as expected and choose Redefine Feature. Note that when redefining a pin you can right-click and choose Loop Select; this option is available when redefining a pin but not when placing the pin originally. Understanding how pin locations will update is important when defining a connector part intended for use in iPart creation where you will want the pin location to update as different pin sizes are created. For static pins not likely to change, nonassociative pins work just fine.
In addition to redefining the pin location, you can right-click any pin in the browser and choose Harness Properties to change the name or add/edit properties. Keep in mind that pin names must be unique.
Although the Place Pin tool works well for defining pins not arranged in a pattern or for small numbers of pattered pins, you can use the Place Pin Group tool to place larger numbers of patterned pins. The following steps explore the Pin Group tool:
On the Get Started tab, click Open.
Browse for the file named
mi_18a_009.iptin the Chapter 18 directory of the Mastering Inventor 2010 folder, and open it.Click the Place Pin Group button in the Harness panel of the Model tab.
For Start Location, select WorkPoint1.
Enter 8 for the number of pins per row.
Enter 4.5mm for the pin pitch (spacing), and then select an edge to establish the pin direction. Use the flip arrow if required.
Enter 2 for the number of rows.
Enter 4.5mm for the row pitch, and then select an edge to establish the pin direction. Use the flip arrow if required.
Enter A for the prefix letter and 101 for the start number.
Switch the radio button for the numbering scheme options to Sequential Column, Circumventing and then back to Sequential Row to see differences in each.
Click OK to set the pins. Figure 18.16 shows the Place Pin Group dialog box settings and pin group.
Notice the 16 pins created and listed in the Model browser. You can right-click any of the pins and choose Edit Pin Group to change the start point, spacing, and direction if required. You can also right-click and select Delete Pin Group to start over, or you can select Delete to remove an individual pin. Note too that you can right-click any of the pins and choose Redefine Feature to set an individual pin to a nonpatterned location.
As a final step, you will create four work points in front of the connector for use later as a stop point for the wire or cable segment.
Click the Point button on the Work Features panel of the Model tab.
Right-click and ensure that Loop Select is not selected.
Click the edge of the visible work plane and then one of the work axes. You'll see a work point created at the intersection. Do the same for the remaining three axes, and then right-click each axis and the plane and turn off their visibility.
The work points allow you to place the end of wire segments appropriately off the connector. Figure 18.17 shows a connector utilizing a segment-end work point.
Electrical components including connectors, wires, and cables are assembled and constructed within a harness subassembly. Although you can place connectors at any structure level within the assembly and route wires to them, as a rule you typically place connectors within the harness assembly when the harness and connectors are purchased together so that your BOM will reflect the harness as an item. The general steps for creating and routing a wire harness are as follows:
In an assembly file, place and constrain connector parts that will not be part of the harness assembly into the assembly either at the top level or within a subassembly.
Click the Cable And Harness button in the Begin panel of the Assemble tab.
Enter a name and location for the harness subassembly file to be created.
Place and constrain connectors to be part of the harness.
Use the Create Wire, Create Cable, or Create Ribbon Cable tools to connect the pins of the connectors.
Use the Create Segment tool to create wire bundles, routing them around geometry obstacles of other parts in the assembly.
Use the Route or Automatic Route tool to route the wires or cables through the segments (wire bundles).
Use the Create Splice tool to create wire or segment splices as required.
When a harness is created, it is composed of a harness assembly file and a harness part file of the same name. The part file is the container in which the wires, cables, and segments will be built as they are added. Both files comprise the overall harness and are required for the harness to work. Inventor will warn you if you try to edit these files directly rather than through a top-level assembly using the wire harness tools.
In the following steps, you will open an existing Inventor assembly file, create a simple harness assembly, and then place connectors.
On the Get Started tab, click Open.
Browse for the file named
mi_18a_018.iamin the Chapter 18 directory of the Mastering Inventor 2010 folder, and open it.On the Assemble tab, click the Cable And Harness button in the Begin panel.
Accept the default name and location for new harness assembly, and click OK. Note the harness subassembly and part nodes listed in the browser.
Click the Assemble tab, and then click the Place Component button.
Browse for and locate the connector file named
mi_18a_004.ipt, and click Open.Click twice in the graphics area to place two instances of the connector; then right-click and click select Done.
To assemble the connectors (residing in the subassembly) to the base part (residing in the top-level assembly), you'll need to return to the top-level assembly and place the constraints. Parts within the harness can constrain to the parts in the top-level assembly because the harness subassembly is adaptive.
Click the Finish Cable And Harness button to return to the top-level assembly.
Place an Insert constraint on the connectors and the holes on the outside flanges. Ensure that the connector pins face the inside of the base part.
Click the Finish Cable And Harness button to return to the top-level assembly. You can close this file when done.
This simple exercise illustrates the steps required to create a harness subassembly and place connectors within it. You can also place connectors in the top-level assembly before creating the harness assembly and then demote components from the top-level assembly into the harness subassembly. To do so, follow these steps:
Place the connectors in the top-level assembly.
Create the harness assembly.
Next while the harness subassembly is active, expand it in the browser.
Click the connector components in the browser, and drag them down into the harness assembly.
Once the harness assembly is created and the electrical connector parts are added and constrained, you can add wires and/or cables. When wires are created, you enter a unique wire ID name, select a wire category, and set the wire name (type). Then you select the two pins you want to run a wire from and to. To see how the Create Wire tool works, open the file named mi_18a_020.iam in the Chapter 18 directory, and follow these steps:
Double-click the Harness subassembly to set it active for edits (or right-click it and choose Edit).
Set Wire ID to Wire101.
Select Generic from the Category drop-down.
Set the Name drop-down to 14AWG-BLK.
Select the Pin 1 (work point) on one of the red connectors for the Pin 1 selection. You'll see the pin number when you pause your mouse pointer over the pin. Figure 18.18 shows the pin selection and wire settings.
Select the Pin 1 (work point) on the other red connector for the Pin 2 selection.
Click Apply to set the wire. It should run in a straight line between the two connectors.
Set the remaining three pins for the red connectors as listed here:
Pin 2 = Wire102, Generic 14AWG-RED
Pin 3 = Wire103, Generic 14AWG-WHT
Pin 4 = Wire104, Generic 14AWG-GRN
Once you set all four wires, click Cancel to exit the Create Wire dialog box.
In this assembly, a segment (blue wire bundle) has already been created. Click the Route button to route a wire through the segment.
Click just one of the wires for the Wires selection, and then click the segment for the First Segment selection.
Select the Single Segment check box, and then click Apply. Note that the segment will shrink to size based on the wire.
Click Cancel to exit the Route dialog box, and then click the Automatic Route button.
In the Auto Route dialog box, select the All Unrouted Wires check box, and click OK.
Expand the Harness1 part node in the browser, and you'll notice a Wires folder containing all of the wires you created. Right-click Wire101, and choose Harness Properties. Browse the tab to examine the read/write and read-only properties available for this wire. When finished, return to the Occurrence tab, set the Bend Radius to 2× diameter, and then click OK.
Right-click the Wires folder in the browser, and select Bend Radius
Note that you will receive a warning stating that one or more objects contain an empty bend radius. Click OK, and note that wires 102 through 104 are marked with a warning icon in the browser. In this case, the warning indicates the bend radius has not been set. You can edit the wire property, set the bend radius, and then repeat the bend radii check. If the bend radius for each wire in the model is in compliance with the setting for that wire, then the check will clear. Editing segments will be covered more in the "Placing and Editing Segments" section. Now that the problem area is identified, you could make decision to either change the general layout of the assembly or edit the segment route to change the fit so that the bend isn't so sharp.
Click the Finish Cable And Harness button to return to the top-level assembly. You can close this file when done.
This simple exercise demonstrated how to create wires in a harness and the routing of these wires in an existing segment. The wire categories and names listed in the Create Wires dialog box are drawn from the Cable And Harness library.
The Cable And Harness library is located in the Design Data folder but can be set per harness. In most cases, you will want to configure it per the Inventor Design Data folder. You can set this option by right-clicking a harness assembly while it is active for edits, selecting Harness Settings, and then going to the File Locations tab.
The library file name that installs by default is Cable&HarnessDefaultLibrary.iwl. You can locate this file by checking the Design Data path in your Inventor project file (*.ipj) or by going to the File tab of the Application Options dialog box. Recall that the project Design Data path trumps the application's Options path if set.
To add objects to the Cable And Harness Library, click the Library button on the Manage panel of the Cable And Harness tab. You can add new wire, cable, and segment objects, just to name a few, and you can create your own custom object type. Figure 18.19 shows the library being edited.
Adding cables is much like adding wires. To explore the cable tools, open the file called mi_18a_022.iam in the Chapter 18 directory of the Mastering Inventor 2010 folder.
Double-click the Harness subassembly to set it active for edits, or right-click it and select Edit.
Click the Create Cable button on the Cable And Harness tab.
Set Cable ID to C201, and set Category to Alpha.
Select 2254/4 from the Name drop-down.
Note that Conductor ID 1 is set active. Select the Pin 1 (work point) on one of the gray connectors for the Pin 1 selection. You'll see the pin number when you pause your mouse pointer over the pin.
Select the Pin 1 (work point) on the other gray connector for the Pin 2 selection. Note that the conductor ID advances automatically to the next line.
Set the remaining three pins for the gray connectors as listed here:
Pin 2 = C201:2, Red
Pin 3 = C201:3, White
Pin 4 = C201:4, Green
Click OK to set the cable.
Click the Automatic Route button, select the All Unrouted Wires check box, and click OK.
Expand the Cables folder in the browser and then right-click the listed cable and choose Harness Properties. Note the Bend radius is set to 10 × diameter. If you click in the input box, you will see that the value is being pulled from the Cable And Harness Library. Click OK to exit the dialog box.
Right-click the cable, and choose Bend Radius
Note that the cable browser node has turned red to indicate a problem. Right-click it in the browser, and select Bend Radius
Click the Finish Cable And Harness button to return to the top-level assembly. You can close this file when done.
The check bend radius function allows you to locate problem areas with the design. You could remedy the violation either by adjusting the segment points in an attempt to modify the fit of the cable route or by moving components and/or features in the assembly. Often a design might require adjusting both the assembly arrangement and the cable routing. But it's important to be able to check for bend radius violations so that you can determine what needs adjustment. In the next section, you will explore segment creation and editing.
Segments are used to define the route path in which wires and cables will be run though a design so as to avoid interference and identify possible problem areas where bend radii may be too tight. A segment is created by selecting geometry on-screen, either outright or as an offset base. For each selection or offset point, a work point is created.
Once segments are created, you can refine them by adding points or redefining existing points. To explore the cable tools, open the file called mi_18a_024.iam in the Chapter 18 directory of the Mastering Inventor 2010 folder.
Double-click the Harness subassembly to set it active for edits, or right-click it and select Edit.
Click the Create Segment button on the Cable And Harness tab.
You will first run a route segment from the red to green connectors. Select the work point in front of the red connector for the start point of the segment.
Next click any circular edge on the black grommet hole; this will select the center. Repeat this for the green grommet hole.
For the third point, you will specify an offset value and then select the flange with the two square shaped notches along the top.
First right-click and choose Edit Offset.
Enter 10mm in the Edit Offset box, and then click OK.
Rub your mouse pointer around on different faces to observe the way the offset behaves. Then select roughly in the center of the face of the notched flange in front of the green connector.
Next select the work point in front of the green connector.
Right-click and choose Continue.
Next you'll create another short segment from the orange connector and tie it into the first segment. Select the work point in front of the orange connector.
Then click the work point at the center of the green grommet hole, and click Finish. Figure 18.20 shows the segments.
Use the Automatic Route tool and select the All Unrouted Wires option to route the wires through the segments. Upon doing so, you'll notice two things:
The segments adjust to compensate for the wire diameters.
The cable coming off the blue connector has routed in an undesirable way.
Use the Unroute tool, and select any of the wires at the blue connector. Because they all belong to a cable, you need to select only one, and then they all highlight. Once they are unrouted, you can use the Create Segment tool to create a new segment from the blue connector to the black grommet hole and then use Route or Automatic Route to reroute the cable.
You'll notice that the middle section of the segment needs to be adjusted. To do so, follow these steps:
Run your mouse pointer over the centerline of the segment, right-click, and choose Add Points.
Select roughly in the middle of the segment, and then click Finish.
Right-click, select Edit Offset, enter 10mm for the offset value, and click OK.
Click roughly in the center of the square emboss on the base part.
Next you'll make an adjustment using the 3D triad. Right-click the same work point, and select 3D Move/Rotate.
Click the blue cone (z-axis) of the triad, enter 4mm, and then click Apply.
Select the small plane between the blue arrow and the green arrow (YZ plane), enter −6mm in both the Y and Z inputs, and then click OK.
Next you'll edit the segment type. Select Assign Virtual Parts on the Cable And Harness tab, and select the centerline of all the segments. From the Type drop-down, select Loom, set the Category drop-down to Sample, set the Name drop-down to Wire Sleeve, click the Add button, and then click OK. Note that the selections in this dialog box are interdependent. For instance, you might need to set the category first in order to get the option selections for the name.
Because the middle segment routes all the wires and the cable, it is larger in diameter. This is based on a setting in the harness properties. To determine its evaluated size, right-click the segment center line, and choose Harness Properties. You can determine the diameter at the bottom of the Occurrence tab. Because the grommet holes have an inside diameter of 10mm, you can make a judgment as to whether a larger hole size is required.
On the Wire/Cables tab of the Segment Properties dialog box, you can review the wire and cable information. Double-clicking a line item will open the properties of that wire or cable. Figure 18.21 shows the wire properties of a wire contained in a segment.
Because of the adaptive relationships between assemblies and the harness assemblies and their containing harness part file, copying existing harness and assembly designs must be done in a particular way so as not to break the adaptive relationship between the original files when working on the new files. Before looking at the steps to copy a harness, take a look at Figure 18.22 to understand the files involved. Each harness is comprised of an assembly file, where you can place connectors and other components, and a part file, where the wires, cables, segments and other harness components are created.
To copy a harness design, open the file called mi_18a_028.iam in the Chapter 18 directory of the Mastering Inventor 2010 folder. Then follow these steps:
Expand the assembly browser so that you can identify the harness assembly and part nodes.
Notice the harness used in the assembly is called
mi_18a_26.Harness2and the part within is named the same. This is because this top-level assembly file was created by using the Save Copy As tool and therefore still references the original harness. Although it may seem logical to use the assembly Replace tool or some other method to swap out the harness, such methods can't be used because the adaptive relationships must be updated throughout the file references.Right-click the
mi_18a_26.Harness2file in the browser, and choose Delete.Click No in the prompt box so that adaptively is not cleared in the original assembly.
On the Assemble tab, click the Place button.
Browse for the
Harness_Filesfolder in the Chapter 18 directory, select the file namedmi_18a_26.Harness1.iam, and click Open.Click anywhere in the graphics screen to place the harness; then right-click and select Done.
Typically you would constrain the harness using assembly constraints at this point. For the purpose of this exercise, though, you don't have to do so. Instead, right-click the harness assembly in the browser, and choose Make Adaptive. If prompted to save, click Yes.
In the Make Adaptive dialog box, you can set the new names for harness files or accept the default name.
In the Location area at the bottom of the dialog box, click the Browse button, browse for the
Harness_Filesfolder in the Chapter 18 directory, and then click OK. Note that by default a subdirectory of the same name as the top assembly is created along with subfolders for the component organization. You can accept this path and just make that part of your standard file management if you'd like.Click OK and the new files are created, are made adaptive, and are ready for your design edits.
To make copies of a harness within the same assembly, you can simply copy and paste an existing harness, or you click an existing harness node and drag and drop it into the graphics area. Then right-click and choose Make Adaptive, and follow the renaming and location options detailed in the earlier steps.
Documenting harnesses is a pretty straightforward process with purposely built tools for detailing harnesses as traditional nailboard drawings. To explore these options, open the file called mi_18a_026.iam in the Chapter 18 directory of the Mastering Inventor 2010 folder, and follow these steps:
Double-click the Harness subassembly to set it active for edits, or right-click it and select Edit.
Click the Nailboard button on Cable And Harness tab.
Select a drawing template of your choice from the Open Template dialog box, and click OK.
You will be taken into an active sketch within the drawing. Click the Nailboard tab to switch to the nailboard sketch tools.
Use the Harness Dimension tool to place dimensions from the points on the harness. These will display as driven sketch dimensions for now but will show as drawing style dimensions once out of sketch mode.
Click the Pivot button on the Nailboard tab, and then select the sketch point at one of the 90-degree intersections. Then click a sketch endpoint of the harness leg, and drag to pivot the angle. Then right-click and choose Finish.
Zoom to any end on the harness, and select all of the wires (you can use a selection window to do this quickly).
Once the wires are selected, the Fan In and Fan Out buttons are available on the Nailboard tab. Click the Fan Out button, enter 180, and then click OK. Note the change in the wire fan angle. You window the entire harness and use the Fan In/Out tools to set all the fans to the same angle as well. You can also manually click and drag each wire if needed.
Click the Finish Sketch button when you are satisfied with the dimensions, leg pivots, and fan angles.
Click the Place Connector Views button on the Nailboard tab.
Accept the defaults, and click OK.
Note that a drawing view of each connector is placed near each wire fan. Right-click one of these views, and select Edit View Orientation. Notice that you can change the styling, scale, and so on, as you would with any Inventor view, but you can also change the view orientation.
Feel free to experiment with view settings, and then click OK.
Next click the Edit button on the Nailboard tab. If the Sketch tab becomes active, switch to the Nailboard tab.
On the Nailboard tab, click the Property display button.
Set Selection Filter to All Wires.
Choose Wire ID from the Property Name list, and then click Apply.
Click onscreen to establish the position of the ID label to the wire, and you will see all the wire ID labels placed. Click OK. Click and drag labels to adjust them.
Expand the Segment browser node, select all the listed segments, and then right-click and deselect the Display As Actual Diameter option.
Expand the Wires node, right-click one of the wires, and choose View Path. Notice how the wire path is highlighted.
Click the Finish Sketch button.
Here are a few more settings and options to use when working with Nailboard drawings:
Right-click the top-level harness node in the browser, and choose Nailboard Settings to adjust the global settings of the Nailboard view.
You can open a drawing template first and use the Nailboard button on the Place Views tab to create a nailboard view and set the display settings, rotation, and other view options as you place the view.
You can use the Table tool to place wire/pin tables from existing
*.xlsfiles.You can use the Broken Sketch Entity tool in the drawing view sketch environment to break long harness runs so they will fit on the drawing sheet.
- Create routes and runs
Using routed systems tools allows you to quickly define many different routes types in order to check for clearance and fits within a design, all while creating a bill of materials that can be used downstream in the manufacturing process.
- Master It
How can you extract a bill of materials from a routed systems assembly?
- Author a tube and pipe component
To create your own fittings, coupling, and so on, to be used within tube and pipe design, you need to first author it for use with the tube and pipe tools.
- Master It
How can you set the depth at which pipe, tube, or hose segments are inserted into a fitting?
- Author an electrical component
To create your own electrical connector components be used within cable and harness designs, you need to first define pins within the parts.
- Master It
How can you create a family of electrical connectors with varying numbers of pins?
- Create and document cable and harness assemblies
Cable and harness assemblies are created using a specific subassembly and part structure. Each harness is contained in a harness subassembly, and the parts such as wires, cables and segments are created within a harness part file.
- Master It
You have a complex design that includes many harness assemblies and would like to turn some of them off while you work on others and/or create new ones. What is the best way to do this?