SOLIDWORKS Reverse Engineering – Surface Modeling and the Legacy Part Problem – Part 2

Article by Mike Walloch, CSWE updated January 4, 2023

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In the previous blog, SOLIDWORKS Reverse Engineering – Surface Modeling and the Legacy Part Problem – Part 1 we explored a method of re-creating a legacy part with nothing but an incomplete manual drawing, an old part, and a pair of calipers to guide us. The method used was heavy on surface modeling, creating a nearly complete hollow exterior of the finished part before using the Thicken feature to convert it into a solid body. This worked but resulted in an unacceptable total rebuild time of 31.45 seconds. Now we’ll look at an alternate hybrid approach where we switch from surface to solid modeling earlier in the game.

Surface Modeling in SOLIDWORKS

Ridged Knob – Finished Part

Thanks to Brian Mitchell and Austin White at Barrett Plastics Inc. of Harrison, Arkansas for providing us with this modeling problem.

 

Same but Different

Some former colleagues and I had a running joke whenever we started working on a new project. “It’s the same as the last one, except everything is different.” In this particular case, the new part’s feature tree is going to be the same as the old part up to a point. After that, it will be different. Our initial setup is the same, with the same sketches and planes. Our initial surface modeling is also the same, up until we have our first 4° slice showing the peaks of two ridges and one groove.

reverse engineering in solidworks

Initial Setup – Planes and Sketches

Surface Body

Path to a Solid Model – Hybrid Surface Modeling

In the first attempt, a Circular Pattern was used on the above surface body to create 90 copies. This resulted in a lot of curved surfaces, causing subsequent Trim and Knit Surface features to be expensive in terms of processing power.

Performance Evaluation – Part 1

For our hybrid modeling approach, we’re going to continue with surface modeling to create a solid body representing a single 4° slice of the part. Standard solid modeling tools can take it from there to the finish line.

Extruded and Planar Surfaces

The image above shows two new surface bodies. The sketches which created them are shown in red. One is a cylindrical Extruded Surface, and the other is a Planar Surface covering one side of the original Swept Surface.

Mirrored Planar Surface

Trim Surface

The Planar Surface is mirrored across the Right Plane. Trim Surface gives us an almost complete internal volume of one slice.

Planar Surface and Knit Surface

One more Planar Surface caps off the bottom giving us an air-tight enclosed volume. Knit Surface joins the 5 surface bodies together and converts them into a single solid body. From here on out we only need a few solid modeling tools.

Circular Pattern

Extruded Boss

Finishing Touches – Extruded Cut and Edge Fillets

A Circular Pattern results in 90 solid bodies. A cylindrical Extruded Boss merges all the intersecting bodies into a single solid body. An Extruded Cut and Edge Fillets add the finishing touches.

 

Which Part is Better?

The part is now geometrically identical to the first attempt covered in Part 1 of this blog. But the FeatureManager Design Tree tells two very different stories after the Valley Fillet feature.

Feature Trees – Part 1 vs Part 2

Part 1 used surface modeling to create the exterior of the part, converting it to a solid long after the Circular Pattern. Part 2 used surface modeling to create a small solid body, which was then patterned. Part 1’s Total Rebuild Time was 31.45 seconds. Part 2’s Total Rebuild Time is only 2.27 seconds. Part 2 is almost 14 times faster than Part 1!

Performance Evaluation – Part 2

Conclusion

Surface Modeling is an amazing toolset. The SOLIDWORKS Surface Modeling class opened my eyes to many new and creative approaches to modeling challenges. However it’s important to know the strengths and weaknesses of each tool in your toolbox. SOLIDWORKS provides many ways to solve the same problems. Here we’ve looked at just two approaches to modeling this part. While both methods worked, in this case, the second is clearly the superior choice.

To learn more about surface modeling, find more blog articles here. 

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Mike Walloch, CSWE

Mike Walloch is a Certified SOLIDWORKS Expert (CSWE) and works as a Process & Training Consultant at TriMech