In this Skill Builder, you use the Sculpt tool on a supplied sample file to create complex part shapes. So you can refer to the finished product, the sample file is delivered in a finished state. To complete the Skill Builder, you roll back the End of Part marker, delete the existing sculpt features, and then re-create the sculpt features using the remaining surface geometry.
Sculpt uses surfaces, faces, or work planes in selection sets to define 3D regions where material is either removed or added. Surfaces and faces created using complex lofts or sweeps can produce quite sophisticated shapes. A sculpt can take that sophistication to the next level. Sculpt gives you the ability to create complex and refined solid shapes that would otherwise be very difficult if not impossible to construct.
Download the associated zip file, extract, and then open the part. The solid portions of this part were created using three sculpts: two to define the pitcher body and one to define the handle.
Fillets and rounds were then added to finish the part.
The time-consuming portion of the Sculpt workflow consists in creating the defining geometry, such as lofted surfaces, in the needed positions and desired shapes. Like anything else, you get what you pay for: to get the desired sculpt shape, you will probably need to spend a fair amount of time creating and adjusting the defining surface geometry. By comparison, the sculpt operation itself is very quick. Keep in mind that sculpt is like other workflows within Inventor: it pays to plan before you begin your modeling work so that your design will be as simple, economical, and robust as possible.
Note: For expediency, the skill builder reviews various details of how the defining geometry was created but you will not need to create that geometry.
To begin, drag the End of Part marker just below the Sculpt – interior node.
Select both sculpt nodes, right-click, and then select Delete.
If the Delete Features dialog box appears, remove the check mark next to consumed sketches and features. Click OK.
The three lofted surfaces used to define the pitcher body should remain.
First, let’s examine the lofted surface that defines the pitcher exterior face. Drag the End of Part marker just below the LoftSrf – exterior node. Expand the node.
Pause the cursor over each sketch node to highlight the sketch in the browser. Sketch1 defines the base of the pitcher.
This sketch was created on a work plane offset from the origin XY Plane.
Sketch3 and Sketch4 were created on the origin XZ Plane and were used as guide rails to define the side profiles.
When creating part models it’s almost always wise to define feature geometry with respect to the origin geometry, whenever possible. Since the origin geometry is unchanging and therefore stable, this helps ensure that your models are stable, as well as economical. For example, because Sketch1 and Sketch2 are centered on the origin Center Point, the guide rail sketches can be created on the origin XZ Plane. The design intent is that the guide rails are located on the central cross section of the part – intelligent use of the origin geometry naturally ensures that the rails are centered, without any further use of added construction geometry.
Drag the EoP marker just below LoftSrf – top.
Expand the node and pause the cursor over Sketch5. This sketch defines the central profile of the loft, which, in turn, will help define the central profile of the pitcher spout.
Sketch6 and Sketch8 define the beginning and ending loft extents.
Sketch9 is a guide rail and works in close conjunction with Sketch5 to define the spout region of the loft.
Sketch11 defines the guide rail opposite Sketch9.
Without this guiderail, the shape defined by Sketch5 and Sketch9 would propagate all the way across the loft profile – undesirable for this design intent. The following image shows the surface without Sketch11.
Sketches 6, 8, 9, and 11 were created on work planes offset from the origin planes.
Finally, drag the EoP marker just below LoftSrf – interior. This loft helps determine the interior shape of the pitcher.
Sketch12 defines the bottom of the loft.
Sketch13 defines the top of the loft. This sketch was created by projecting Sketch2 (contained in LoftSrf - exterior) and then offsetting.
Sketch14 and Sketch15 are guiderails and closely follow their companion guide rails Sketch3 and Sketch4 (contained in LoftSrf – exterior).
When setting up bounding geometry for the sculpt, you need to be able to roughly visualize how the surfaces and faces in conjunction will define the sculpt shape. But don’t be overly concerned if you can’t picture the final shape exactly – you can edit and fine tune the various surfaces after creating the sculpt.
We are now ready to create the first sculpt – the exterior portion of the pitcher. Click the Sculpt tool.
Ensure that Feature Preview is selected.
Select LoftSrf – top. You can select in the browser.
Select LoftSrf – exterior.
The solid does not yet preview because the sculpt still contains an open region – a successful sculpt requires that the sculpt region is completely enclosed. In this example the bottom of the sculpt is not yet defined.
In the browser, expand the Origin folder and select the XY Plane. This is another example of intelligent and economical design: because this origin plane coincides with the bottom of the pitcher, the origin plane can be used to help define the sculpt – there is no need for additional work geometry or surface geometry.
Once the solver determines that the region is completely enclosed, the sculpt previews. Click OK.
To define the interior portion of the pitcher, it may seem that a shell would work. However, because the design intent is that the interior surface be tapered with respect to the exterior surface, a shell will not work. Regardless, at least two methods remain.
The first option is that you could create a lofted extrusion to remove the interior material, using the sketches currently consumed in LoftSrf – interior.
The second option is to use another sculpt. This is probably a little less efficient than using the lofted extrusion, but just for the sake of showing how a sculpt can remove material, as well as add material, we will use a sculpt.
Press the Spacebar to activate the Sculpt command again. (The Spacebar within Inventor activates the most recently-used command.)
Select the Remove option.
Select LoftSrf – interior.
Two more selections are needed. Select Work Plane6 to define the sculpt bottom.
Select Work Plane1 to define the top.
While you were selecting the sculpt bounding geometry, you probably noticed the glyphs attached to each selection. These are controls that let you specify an alternate or opposite solution.
This simplified example shows an inner surface surrounded by an outer surface, intersected by two work planes.
The preview shows the default sculpt when you select the internal surface and the two work planes.
When you select the arrow on the control attached to the surface selection, the solution flips in the direction of that arrow, in this example, to the outside of the selected surface. Notice, too, that there must be bounding geometry available to define an extent for the flipped solution.
One more sculpt and the part is nearly finished. Drag the EoP marker just below Sculpt - handle.
Delete Sculpt - handle. (The consumed surfaces should remain and be visible.)
Click the Sculpt tool.
Select each of the surfaces as shown in the image. (Mirror2 is also a selection.)
Notice that the arrow control on the inner surface – as on all the surfaces - points in both directions. This indicates that the associated region, for this particular example, will fill on both sides (if required bounding geometry is available), by default.
Click the control arrow as shown in the following image. This indicates that you want the operation – whether fill or remove – to execute on that side. In addition, the selection also indicates that the arrow on the opposite side of the control should switch to the opposite of its current state. If currently set to fill, then it switches to remove, and vice versa. In this example, this selection infers that you want fill outside the loop but not inside.
The sculpt previews. Notice that even though the glyph switches to a single arrow, the opposite arrow is still available when you pause the cursor over the glyph. (Do not select the arrow.)
In effect, the arrows act as toggles: if a fill is currently indicated, selecting the associated arrow switches to a remove, and vice versa.
Before you click OK, expand the dialog box. As an alternative to using the direction controls in the graphic window, you can instead select the direction icons to flip the sculpt solutions. (Do not select and switch the icons for this example.)
To finish a sculpted part you will almost always want to add fillets or rounds. Because the original sculpt geometry was lost in the course of this workflow, the existing fillets will fail when you move the EoP marker. The following image shows the original fillets.
You can re-create the fillets but it isn’t necessary for this skill builder. If you do re-create the fillets you may find that the creation order of the fillets and rounds on the handle is important. For example, you may need to create the fillet between the handle and pitcher body before you create the round on the outside of the handle. The fillet radius will also influence whether a fillet is successful, of course. You can also experiment with variable radius fillets to create even more refined and subtle shapes.
One more tip and you will be finished. Let’s assume that the handle shape should be tweaked slightly. Expand the Sculpt14 browser node, right-click RevolutionSrf2, and then select Edit Sketch.
The intent is to adjust the sketch spline, however, the sketch loop for the outer surface of the handle needs to be visible for reference. Right-click Sketch22, nested under RevolutionSrf1, and then select Visibility.
The outer loop is now available for visual reference as you adjust the inner loop.
Furthermore, you can also adjust Sketch22 while Sketch23 is in edit mode.
In fact, if you simply want to drag sketch geometry, a sketch only needs to be visible, not in edit mode. After you drag geometry, click the Update tool to refresh the associated geometry.
Sculpt, especially when used with other shape description tools such as Loft, Sweep, Replace Face, and Fillet, gives you the ability to create almost any complex shape. The bulk of the work lies in setting up the sculpt bounding geometry. In addition, as mentioned earlier, Sculpt is like other design workflows within Inventor: up-front planning can make the difference between a part that is intelligently structured, robust, and easy to edit…and a part that isn’t.