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Designing with Style—Turning Sketches into Successes
By Michael A. Brattoli, Moen Incorporated
Turning conceptual designs into finished products is at the core of product design. For many years, however, the ability to capture the design intent of industrial design models, sketches, and renderings within the CAD model has been limited at best. Translating the aesthetic sense of a design into the mechanical reality of the product is often more art than science.
Industrial designers use a variety of tools to produce their conceptual designs, but many still present their concepts as sketches and renderings. Interpreting these hand-generated ideas and capturing them accurately is the challenge of the mechanical designer and engineer. The Interactive Surfacing Design Extension (ISDX) within Pro/ENGINEER, also known as the “Style module,” provides the tools that make this process as painless as possible.
The Style module includes functionality known as “trace sketches,” allowing the designer or engineer to import images into the model and ensure the end-product conforms to the aesthetics of the initial concept. The trace sketch images can be placed on any planar object within the Pro/ENGINEER model (Wildfire 2.0 lets you use datum planes and/or flat surfaces) and then can be manipulated for position, scale, and orientation.
Trace Sketch Manipulation—Step by Step
The key to capturing aesthetic design involves the information contained within the image. Knowing the interface dimensions of key features within the design simplifies the manipulation of the trace sketch.
Reference features, or sketched sections, represent the interface dimensions of the part being modeled. These features can consist of datum planes, points, and/or sketched curves (Fig. 1). In this example, the interface measures horizontally 4.00 inches by vertically 7.00 inches.
Figure 1.
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1. Importing the Trace Sketch
Select the Style Icon in the Base Features toolbar (Fig. 2), or choose Insert, Style from the top pulldown Insert menu. NOTE: THE ISDX MODULE IS OPTIONAL IN PRO/ENGINEER.
Select Style, Trace Sketch from the top pulldown Style menu.
The Trace Sketch dialog box will open. Selections matching the three default datum planes in the model will be listed, although images will not be allocated by default.
Select the Front sketch orientation. A dialog box will open. Browse to the location of the desired file, select it, and pick Open. The image will appear on the front datum plane (Fig. 3).
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Figure 2.
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Figure 3.
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2. Manipulating the Image
Expand the Properties portion of the Trace Sketch dialog box. The following tools will appear (Fig. 4):
- Fit locates the image by fitting it horizontally and vertically using dimensional input. The values are applied based on the position of the Image Fit Lines.
- Transparency controls the visibility of the imported image.
- Rotate rotates the image up to 360 degrees about an axis normal to the screen.
- Move provides horizontal and vertical movements of the image.
- Scale scales the image. By default, the horizontal and vertical scale controls are locked together, applying the same changes to both.
- Image Fit Lines assist in locating and sizing the imported image. These lines work in conjunction with the Fit tools.
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Figure 4.
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In this example, the image must be positioned to match the 4.00 x 7.00-inch dimensional reference. The baseline position is located at the bottom center of the spout, indicated by the dimensional references and heavier lines shown in the image.
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Select the bottom left intersection or the vertical left image fit line, and drag it using the left mouse button to the desired intersection on the image.
Pick the bottom right intersection, or the vertical right image fit line, and drag it using the left mouse button until it lines up with the desired intersection on the image—in this case, the discharge end of the spout indicated by the dimensional references and the intersection lines (Fig. 5).
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Figure 5.
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In the upper half of the Trace Sketch dialog box, enter a horizontal fit value of 4.00 inches and pick the Fit button. The image will be resized to match the position of the image fit lines to the 4-inch horizontal input. The bottom left intersection of the image fit lines will be moved to the intersection of the default datum planes.
Now repeat this process to control the vertical sizing of the image. In the upper half of the Trace Sketch dialog box, select the vertical fit option. The image fit lines will change, allowing you to control the sizing of the image vertically.
Select the top and bottom image fit lines, and drag them as needed to match the dimensional reference sketch (top and bottom curve lines).
Input a value of 7.00 in the Vertical fit field and select the Fit button. The image will be resized to match the position of the vertical image fit lines to the 7-inch input.
If additional manipulations are necessary, use the Move, Scale, and Rotate options in the dialog box. Pick OK to close the dialog box and complete the manipulation of the image.
3. Inserting Datum Curve Features into the Style Feature
The image has been successfully imported into the Style feature. Note that you can import additional images in the same manner and place them on other planes or planar surfaces as needed (side or top images, for example).
The ISDX module lets you interact with the curves and surfaces created within a single Style feature, dynamically manipulating and updating the model without the need to modify a single feature, then regenerate the model. It is common practice to include all Style curves and surfaces within a SINGLE Style feature! This provides maximum flexibility as you work with an industrial designer to refine your design.
In this example, the base of the spout is 3.00 inches in diameter and the discharge end of the spout is 1.5 inches in diameter, inclined on a 15-degree angle as indicated in the imported sketch. It is important that core datum feature references (sketches, points, axis, etc.) be in place prior to the Style feature, so that you can select them when creating the required free-form aesthetic curves. This can be easily accomplished using the previously sketched curve.
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Complete the Style feature by selecting the Blue Checkmark icon in the Style toolbar. You will be inserting the datum features prior to the Style feature.
Select the Insert Here arrow in the model tree and drag it above the Style feature. It will be suppressed, and any new features will be placed prior to it in the model.
Construct the required datum features.
Once these features are complete, Resume the previously suppressed Style feature by dragging the Insert Here arrow below the Style feature in the model tree, or by picking the Style feature, holding down the right mouse button, and choosing Resume from the popup menu (Fig 6).
Redefine the Style feature by picking it and selecting Edit, Edit Definition.
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Figure 6.
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4. Creating the Profile Curves
Select the ActivePlane icon in the Style toolbar (second icon from the top) and choose the Front datum plane (plane of symmetry) in the model.
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Figure 7.
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Pick the Style Curve icon (Fig. 7). In the curve dashboard, make sure the Planar radio button is selected. This will place the curve on the active plane previously selected.
Use the Shift key and select the datum point for the inner profile of the spout with the left mouse button. Pick the actual point, not the text. (Alternatively, use the Shift key and pick on the base curve with the left mouse button, near the desired location. The curve point will snap to the point on the curve that intersects the Front datum plane.)
Three curve points are needed for this curve. The second curve point will be placed on the active plane, approximately halfway between the initial point and the desired end point of the inner profile of the spout. For the final point, again use the Shift key and left mouse button to select the end point where the curve intersects the active plane.
Pick the Green Checkmark icon in the curve dashboard to complete the Style curve feature.
To make the Style curve match the imported image, select the Edit Curve icon in the Style toolbar (looks like the Style Curve icon with a pencil on it). Pick the curve you just created, and choose the middle point on the curve.
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Using the left mouse button, drag this point until it lies on the upper half of the inner profile curve (Fig. 8). |
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Figure 8.
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Figure 9.
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When you pick the end point of the curve, a tangency manipulation line will appear (Fig. 9). Place the cursor over the tangency line and hold down the right mouse button.
Select Normal from the tangency popup menu and pick the angled datum plane. The tangency control line will become perpendicular to the angled plane.
Using the left mouse button, drag the length of the line until the upper end of the curve matches the image of the inner profile curve.
Repeat this operation at the bottom end of the curve, this time leaving the tangency control line Free. Using the left mouse button, drag the control line as needed (angle and length) until the Style curve matches the inner profile curve on the image.
Select the Green Checkmark in the Edit Curve dashboard to complete the modifications.
Repeat this process to create the outer profile curve, again creating a three-point Style curve, making it Normal to the angled datum plane.
5. Creating the Style Surfaces
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Figure 10.
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Creating surfaces within the Style module environment is similar to creating surfaces with the Boundary Blend command in core Pro/ENGINEER. Style surfaces require a minimum of three boundary edges, with a maximum of four that can be selected during initial surface creation. Other “internal” curves can be added after the surface has been created.
Choose the Style Surface icon (Fig. 10) in the toolbar.
Using the Ctrl Key, select the four boundary curves on one side of the symmetry plane. (Surfacing within the Style module always involves half of the model.) The surface connection icon lines will appear. You can adjust the length of these lines by changing the value in the Icon Length field of the dashboard.
Complete the surface by selecting the Green Checkmark in the dashboard (Fig. 11).
Once you have created a Style surface, you can add other internal curves to further define the desired shape. Temporarily hiding the Style surface greatly simplifies this process. Pick the surface, hold down the right mouse button, and select Hide from the popup menu.
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Figure 12.
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Select the Style Curve icon. Place the view in a side orientation.
In the dashboard, pick the Free radio button, which lets you modify the curve after creation (Fig. 12).
Pick the top outer profile curve using the Shift Key. The end of the new curve will snap to the curve, displaying as a circle.
Use the Shift Key to repeat this operation, selecting the lower profile curve. The circular ends of the curve represent “soft points,” meaning they can slide along the profile curves, following their form and curvature.
Pick the Green Checkmark in the dashboard to create the curve.
Modify the newly created curve by making the ends normal to the Front datum plane and controlling the length of their tangency lines to ensure the form of the curve is identical at both ends. Pick the Edit Curve icon and select the newly created curve.
Pick one end of the curve to expose the tangency control line. Place the cursor over the line, hold down the right mouse button, and select Normal from the popup menu.
Choose the plane called Front and drag the line with the left mouse button to the desired length. Repeat this process with the other end of the curve.
In the dashboard, pick the Tangent option. In the pulldown menu, check the box marked Length, and enter a value of 1.000.
Figure 13.
Pick the other end of the curve and repeat this process. This will cause both ends of the curve to have identical tangency influence, regardless of where the curve may be positioned in the model (Fig. 13).
Choose the Green Checkmark in the dashboard to complete the curve edit process.
Unhide the surface, holding down the right mouse button, and selecting Unhide All Entities. Pick the surface and choose Edit Definition from the popup menu.
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Figure 14.
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In the dashboard, choose the Internal Curve arrow button (Fig. 14). Pick the curve you just created. It will be added to the surface curve set.
Select OK in the Menu Manager. The surface will update to reflect the inclusion of the internal curve (Fig. 15).
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Pick the Blue Checkmark in the Style toolbar to complete the Style features.
Using layers, hide the datum curves and Style curves within the model, saving the layer status when complete. Select the Style feature and mirror it about the Front plane.
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Figure 15.
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You can now merge the Style surfaces together and use standard surfacing practices to create a closed quilt, constructing flat surfaces to close the ends of the spout. Once the quilt has been closed, it can be converted into a solid protrusion and additional internal
features can be added to the model. The completed model can then be prototyped, machined, and/or rendered in the same manner as any other Pro/ENGINEER part (Fig. 16).
Figure 16.
Summary
With the capabilities of Pro/ENGINEER’s ISDX module, you can address any surfacing challenge while also improving the turnaround time from design concept to finished product. Proper implementation of Style, combined with core modeling techniques, makes it much easier for designers or engineers to capture a part’s aesthetic appearance as well as its functional requirements. From a simple sketch to a part with Style — that means success by any definition of the word! 
Mike Brattoli is the engineering systems administrator at Moen Incorporated in North Olmsted, Ohio, USA. This article is based on his presentation at the PTC/USER World Event 2005. Mike can be reached by email at Mike.Brattoli@moen.com.
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