Autodesk Inventor: 3D Sketches for Assembly Routing

Autodesk Inventor: 3D Sketches for Assembly Routing

This month's tutorial presents some tips and techniques for creating 3D sketches. A 3D sketch is the basis for a 3D swept feature in a part. You can use a 3D sketch to define a path for a lip or other feature that crosses multiple non-coplanar faces. Alternately, you can use a 3D sketch to define the routing path for an assembly component such as a pipe or duct. We'll use the assembly-routing example in this tutorial, but many of the techniques are applicable to other 3D sketches.

Download (zip - 1449 Kb)
You can download the files used in this tutorial from here.

The zipped download file contains the following:

              Rack.iam

              Rack.idv

              Base.ipt

              Brack02.ipt

              Valve.iam

              Valve.idv

              Valve_Sol1.ipt

              Valve_Sol2.ipt

              Layout.ipt

Unzip 3Dsketch.zip and place all files in the same folder.

3D Sketch Overview
The 3D sketch environment in Autodesk Inventor is not as user friendly as the 2D sketch environment. Even so, you can include (project) existing geometry in a 3D sketch, and you can manually add line segments between work points or model vertices. You can also specify a default radius between line segments. An example of using part edges to define a 3D path for a swept feature is shown in Figure 1.

3D Routing Paths

Many mechanical assemblies include routed systems such as piping, wiring, or ducting. Nonlinear paths such as wiring are difficult to capture accurately in Autodesk Inventor because splines are not yet supported in the 3D sketch environment. However, a route for rigid components such as piping is a good candidate fo 545f520f r a 3D sketch.

You can make extensive user of the Autodesk Inventor adaptive technology during 3D sketch creation to provide a path that intelligently updates to match changes to referenced assembly components. In a complex 3D sketch, keeping track of work features that are automatically added as you reference other component in the assembly can be a challenge. We'll work through the creation of a 3D sketch from scratch to get a taste for this, and we'll look at another approach that can reduce the complexity of routed parts while retaining the advantage of adaptive relationships.

Simplifying 3D Routing

In fact, let's look at a simplified method first. As mentioned, you can include existing geometry in a 3D sketch. You can project part edges and vertices and geometry from visible sketches. In a significant number of cases, a 3D route can be described as a combination of lines that lie on just a few planes.

If there are a number of similar routes that follow the same general path, creating a few 2D sketches on adaptive work planes can greatly reduce the effort and complexity of 3D sketch creation. Figure 2 shows two 2D layout sketches that define most of the routing for five separate tubes in an assembly. To create separate parts for each tube, you can derive the same sketches into each new part and create a single tube from the sketch geometry.

Let's start by opening an assembly that contains a layout part with sketches defining the routes for a number of hydraulic tubes. 1. Open the Rack.iam file. The assembly should match the one shown in Figure 3.

2. Open or in-place edit Layout.ipt. It contains four sketches that map the centerlines of five separate hydraulic lines from a valve stack. Note that Work Plane1 and the first four sketches in Layout.ipt are adaptive and related to geometry on the base part. Any changes to the position of the obround openings in the base part will update the 2D sketch geometry in the layout. Any 3D path generated from geometry projected from the 2D sketches will also update to match.

Deriving from a Master Model

Depending on the requirements for detailing the routed components, you might choose to create all five 3D paths in the layout part. In this example, we'll assume that we need each hydraulic line in a separate part file in order to pass production information to a CNC bending machine. Creating the sketches that define all the paths in a single part file makes sense because you can relate all the paths with a minimum number of sketch constraints. Open Layout.ipt and examine the relationships between the paths.

Let's start a new part and derive the layout into the part as the basis for our 3D sketch.

1. From the Assembly panel bar, click the Create Component tool .

2. Enter Tube01 as the file name.

3. Base the part on the Standard (in).ipt template.

4. Clear the check box labeled Constrain sketch plane to selected face or plane.

5. Click OK.

6. Expand the Origin folder under Rack.iam, and select XY Plane as the sketch plane for the new part.

The layout part was also created in-place in this assembly, and the start plane for that part was the assembly XY plane. By selecting this plane as the start plane for the tube, the derived layout in Tube01 will be oriented exactly the same as the layout part. You can then simply ground Tube01 knowing that it is aligned with the part it is derived from. Here's a detailed description of the steps required.

1. Exit Sketch1 without creating any sketch geometry.

2. Delete Sketch1.

3. From the Features toolbar, click the Derived Component tool .

4. Browse to the folder containing the tutorial files and select Layout.ipt. Click Open. The Derived Part dialog box shown in Figure 4 is displayed. Because the layout part has no solid geometry, the Derived Part dialog box defaults to importing sketches and work geometry from the layout part (see Figure 4).

5. Click OK.

The derived layout is aligned with the original layout.

6. Return to the assembly environment. Turn off the visibility of Layout.ipt.

7. Ground Tube01.ipt

8. Activate Tube01.ipt in-place in the assembly (see Figure 5).

Creating a 3D Sketch From Existing Geometry

Now we'll create the 3D path from the connected 2D sketch geometry derived into the part.

1. From the Command bar, click the arrow next to the Sketch tool and select the 3D Sketch tool (see Figure 6).

The 3D Sketch panel bar has a limited number of tools (see Figure 7). We need to use the Include Geometry tool to project existing geometry into the 3D sketch, and then use the Bend tool to create radii between the projected line segments.

2. From the 3D Sketch panel bar, click the Include Geometry tool.

3. Zoom in on the layout geometry and select the sketch lines highlighted in Figure 8.

4. From the 3D Sketch panel bar, click the Bend tool.

5. Change the bend radius to 1 inch in the 3D Sketch Bend dialog box.

6. Add a bend at each intersection of the projected lines (six bends in total).

7. Close the 3D Sketch Bend dialog box, right-click, and select Finish 3D Sketch from the shortcut menu.

8. From the Features panel bar, click the Sweep tool .

9. Zoom in on the valves as shown in Figure 9. Click between the two circles to select the profile for the sweep.

10. In the Sweep dialog box, click the Path tool.

11. Click the 3D path in the graphics window.

12. Click OK. The Sweep feature shown in Figure 10 is created.

You can repeat this procedure to create four additional tubes, all derived from the same layout. Deriving multiple parts from a common parent is an excellent modeling tool in many situations other than 3D sketches.

3D Sketch Between Work Points

In addition to using existing geometry, you can use the Line tool in the 3D Sketch environment to build a series of line segments connected with automatically generated bends. In most instances, you will use the work feature tools to create a series of work points, which you will then select as the endpoints of the line segments.

You can also select a model vertex as the endpoint of a line, but this has limited practicality as you can only select an endpoint of a model edge or a part-level work point. An adaptive work point is attached to the selected vertex, and the work point is used to define the 3D sketch line.

We'll create one additional 3D sketch in a new part in the assembly that uses a series of work points to serve as the endpoints of our line segments. You can create work features prior to defining the work points, or you can create in-line work features during the work point definition. Although a combination of the two techniques is almost always used, we'll create all the work points using in-line work features to demonstrate the full use of adaptive relationships in 3D sketches.

1. Return to the assembly environment. Turn off the visibility of Tube01.ipt. Turn off the visibility of Layout.ipt if it is still visible.

2. Create a new in-place part named Tube06, using the Standard(in).ipt template. Select any plane as the start plane for the part.

3. Exit the initial Sketch environment and then delete Sketch1 from the part.

You must follow the following sections carefully to create the work points for the 3D sketch. The position of the work points is defined by work features that are created by referencing geometry on other components in the assembly. As mentioned, you can create some or all of these work features outside the 3D sketch, or you can use the work feature tools in the 3D sketch environment.

Let's create the first work point. The tube will pass through the rightmost lower obround shape in the vertical face of the base part. A number of work points will lie on a plane defined by the two axes through the obround. We'll create this in-line work plane for the first 3D sketch work point, and then refer to it again as we create additional work points.

1. Start a new 3D sketch.

2. Zoom in on the valves.

3. From the 3D Sketch panel bar, click the Work Points tool .

4. Right-click and select Create Plane from the shortcut menu. Right-click again and select Create Axis. Select the cylindrical face shown in the left-hand image in Figure 11.

5. Right-click again and select Create Axis from the shortcut menu. Select the cylindrical face shown in the right-hand image in Figure 11. A small work plane is previewed near the first axis.

6. Right-click and select Create Axis from the shortcut menu. Highlight the rightmost hole in the valve as shown in Figure 12. Click to create the in-line work axis and the work point at the intersection of the in-line work plane.

7. Expand 3D Sketch1 in the browser.

8. Expand Work Point1 in the browser. The in-line work plane and work axis are listed as children of the work point. The lowest level in-line features are adaptive and tied to the referenced geometry by assembly constraints.

Next, let's add the work point directly below the first point, just above the valve face.

1. From the 3D Sketch panel bar, select the Work Points tool .

2. Right-click and select Create Plane from the shortcut menu. Click and drag off the valve face shown in Figure 13. Enter 0.500 in in the Offset edit box and click the green check mark to create an adaptive offset work plane.

3. Expand Work Point1 in the browser and click Work Axis3 (this is the in-line axis created from the hole in the valve). A work point is created at the intersection of the new in-line work plane and the in-line axis created for Work Point1.

The next work point is created at the intersection of three planes, two that are created during this work point creation, and the in-line work plane created for Work Point1.

1. From the 3D Sketch panel bar, select the Work Points tool .

2. Right-click and select Create Plane from the shortcut menu. Click and drag off the face on Base.ipt as shown in Figure 14. Enter 1.500 in in the Offset edit box, and press the Enter key to create the in-line work plane.

3. Right-click and select Create Plane from the shortcut menu. Click the thin face on Base.ipt as shown in the left-hand image in Figure 15. Click one of the 3D sketch work points in the graphics window (see the right-hand image in Figure 15). An in-line work plane is created, parallel to the selected face and through the work point.

4. Finally, in the browser, expand Work Point1 and click Work Plane1. A work point is created at the intersection of the three planes.

We can create the next work point from work features created for earlier work points.

1. From the 3D Sketch panel bar, select the Work Points tool .

2. In the browser, expand Work Plane1 under Work Point1. Click Work Axis2.

3. Expand Work Point3 in the browser and click Work Plane3. A work point is created at the intersection of the axis and plane. Figure 16 shows the work plane and work axis selections and the resulting work point.

OK, we're almost done with the in-line work features. Let's create a point along the same axis (Work Axis2) and on a plane through the obround cuts on the top face of Base.ipt.

1. From the 3D Sketch panel bar, select the Work Points tool .

2. In the browser, click Work Axis2 (see Figure 16).

3. Right-click and select Create Plane from the shortcut menu.

4. In the browser, click Work Plane3 (see Figure 16).

5. Click the vertex of the obround cut shown in Figure 17. A work plane is created through this point and parallel to Work Plane3. A work point is then created at the intersection of the selected axis and the new work plane.

Two more work points to go.

1. From the 3D Sketch panel bar, select the Work Points tool.

2. Right-click and select Create Axis from the shortcut menu. Click the cylindrical face shown in Figure 18.

3. In the browser, click Work Plane1 (under Work Point1). A work point is created at the intersection of the axis and plane.

The final point is along the work axis created for the previous work point and is offset from the top surface of Base.ipt.

1. From the 3D Sketch panel bar, select the Work Points tool.

2. Right-click and select Create Plane from the shortcut menu. Click and drag off the face on Base.ipt as shown in Figure 19. Enter 1.250 in in the Offset edit box, and press the Enter key to create the in-line work plane.

3. In the browser, expand Work Point7 (the last work point you created) and click Work Axis4. A work point is created at the intersection of the axis and plane. Figure 20 highlights the position of all work points created in the preceding steps.

Now let's create the line segments for our 3D sketch.

1. From the 3D Sketch panel bar, select the Line tool .

2. In the graphics window, select the work points in order, starting at the work point near the valves. Your 3D Sketch should match the one shown in Figure 21. The visibility of all in-line work features has been turned off in Figure 21.

3. The bend radius between the line segments is the default, 0.250 inch. Double-click the radius value at the intersection between the first two line segments. Enter 1 in the edit box, and press the Enter key to change the radius of all bends (see Figure 22).

Finally, let's sketch the tube profile and sweep it along our 3D sketch to create the model.

1. Exit the 3D sketch environment.

2. In the browser, right-click Work Plane2 (under Work Point2), and select New Sketch from the shortcut menu.

3. From the Sketch panel bar, click the Project Geometry tool.

4. Click the 3D line segment perpendicular to the sketch plane as shown in Figure 23.

5. From the Sketch panel bar, click the Center Point Circle tool .

6. Sketch two concentric circles centered on the projected point as shown in Figure 24. Dimension the two circles as shown in Figure 24.

7. Finish the sketch.

8. From the Features panel bar, click the Sweep tool.

9. Click between the two circles to select the tube profile.

10. In the Sweep dialog box, click the Path tool. Select the 3D sketch as the path.

11. Click OK. The tube should match the one shown in Figure 25.

With a little practice, creating work points with in-line work features becomes easier. Although you can use in-line work features exclusively, creating a few key work features (usually work planes) prior to creating 3D sketch work points can simplify the creation process and reduce the complexity of the 3D sketch in the browser.

Checking Adaptive Behavior

Both Tube01 and Tube06 are related to geometry from Base.ipt, which contains patterned features evenly spaced along the part. Let's change the overall length of Base.ipt to see the effect on the 3D tubes.

1. Ensure that Layout.ipt and Tube06.ipt are marked as Adaptive in the assembly.

2. In-place edit Base.ipt.

3. Edit the Contour Flange1 feature. Change the length of the feature from 90 inches to 112 inches.

4. Return to the assembly environment. Click Accept if you are given a warning about losing cross-part associativity.

5. The tubes will not update on returning to the assembly. Do a Full Update on the assembly. If Tube01 is still misaligned with the openings in Base.ipt, do a second Full Update on the assembly. The tubes adapt to the changes in Base.ipt (see Figure 26).

Summary

You can create highly adaptive 3D sketch based parts in an Autodesk Inventor assembly. Look for opportunities to create 2D sketches to hold coplanar geometry for the 3D path. You can use existing geometry, as well as create work points from adaptive work features to define end points of 3D line segments. A 3D sketch based on work points can be somewhat awkward to create, and tracking the resulting work features can be difficult for complex designs. However, by planning ahead and using proper techniques, you can create 3D sketches that reliably capture design intent.

This article was in response to a request (see, it does work). As always, topics for future tutorials are always welcome. Contact me at [email protected] with your suggestions.