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‘Impossible’ Modeling Challenges Part 3: (Un) Bend a Square Profile in Multiple Directions

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‘Impossible’ Modeling Challenges Part 3: (Un) Bend a Square Profile in Multiple Directions

This is the third installment of the SOLIDWORKS Power User Challenges (SWPUC). The first and second articles in this series are still available to read.

The Challenges

SOLIDWORKS does not have built-in functionality for flattening—unbending, straightening—bent structural members. This has been pointed out to us multiple times by our customers.

It has been submitted as an Enhancement Request under SPR 542568:  It should be possible to unfold a bent tube like a SHM part. If you need this functionality, please vote on this SPR and ask all your colleagues and friends to do so.

Figure 1 – Example of a square profile bent in multiple directions.

When faced with this problem, experienced SOLIDWORKS users think first about the Sheet Metal functionality. After all, sheet metal parts with complex shapes can be bent and flatten at will.

When attempting to create the part shown in Figure 1, the limitation in the current version of the software becomes visible: a bend can be applied only normal to the sheet thickness.

Applying the first bend is no problem, as shown in Figure 2. A base flange or an edge flange could be used, as expected.

Figure 2 – First bend—no problem.

Attempting to apply a second edge bend, normal to the plan created by the first bend—along, what is in effect, the thickness direction—will trigger the warning shown in Figure 3.

Figure 3 – Warning when attempting to add a bend along the thickness.

What better place to ask these questions and turn them into challenges than the SOLIDWORKS Forum? There were 109 replies to this Weekly Power-User Challenge on the forum, with multiple solutions for all above challenges. We were able to prove again that the talent on the SOLIDWORKS Forum transcends the limitations in the software. One solution, in particular, was to “trick” SOLIDWORKS into changing the direction of the thickness inside the same part.

Solution #1 – Using Combine-Add

The first solution was submitted by Bjorn Hulman. He was able to create the model with only four features and found a subtle way to flatten it.

First, he created the base flange shown in Figure 4.

Figure 4.

Next, Hulman used the Copy Body feature to get the model shown in Figure 5. Notice that at this point, there are two solid bodies in this model. Each body can be independently flattened.

Figure 5 – A solid body for each bend.

The bodies need to be fused together, so Hulman used the Combine-Add feature.

Figure 6 – Notice that the edges around the origin disappeared. There is only one body.

There is still a problem when attempting to flatten this part. One of the bends cannot be flattened.

Figure 7.

In order to generate a Flat Pattern Configuration, Hulman added an Unfold feature, right after the Base Flange, and completely ignored the Flat Pattern feature. When the Unfold feature is suppressed, the model is bent. When the same feature is unsuppressed, the copy of the first body is also flattened. Therefore, the Combine feature will create a flat solid body.

Unfortunately, one of the bend lines will be missing and no bend notes will be added on the drawing.

Figure 8 – Bjorn’s Solution – using an Unfold feature to replace the Flat-Pattern feature.

Solution #2 – Using the Move Face (Rotate) Feature

The second solution was submitted by Ryan Dark. It was one of the most original methods used to solve this challenge.

Dark started by building both bends in the same plane.

Figure 9 – So far, standard Sheet Metal functionality.

The second step was an excellent example of a power-user thinking “outside the box.” Employ the Move Face feature to artificially set the second bend along the thickness.

Figure 10 – Rotate the blue faces by 90˚.

The result is shown in Figure 11.

Figure 11.

With this solution, Dark can continue to use the Flat-Pattern feature for the flat configuration by suppressing the Move Face feature in the flat.

The only drawback to this method is that the bend lines are not shown in the correct orientation.

Solution #3 – Using the Sweep and Extrude Features in Separate Configurations

Deepak Gupta proposed one of the simplest solutions: “A simple sweep and extrude can also be used (since using sheet metal was not mandatory). The extrude length should be driven from the sweep path.”

Figure 12 – Simple, but effective.

Of course, the bend lines are not calculated in this case, so they will be missing from the drawing.

Solution #4 – Using Cut and Move Body while Accounting for Bend Allowance with Move Face

Lee Wondra submitted one of the most thoughtful solutions, taking into account the bend allowance.

He started by performing a simple Sweep-Boss to generate the formed shape.

Figure 13 – Simple and effective technique for generating the formed shape.

To emulate the Flat-Pattern feature, Wondra used six more features, which are unsuppressed in the Straight configuration.

Figure 14 – The bends are eliminated.

Next, the bending allowance is accommodated by a smart use of the Move Face with Offset feature:

Figure 15 – The Bend Allowance is accounted for

Two simple Move Body features will reposition the ends.

Figure 16 – Repositioning the left end.

Figure 17 – Repositioning the right end.

The last feature joins all three bodies together.

Figure 18 – The Flat-Pattern has been emulated.

The drawbacks are the same as in the previous solutions: no bend lines or bend notes on the drawing.

Solution #5 – Using Equations to determine the unbent length

Bernie Daraz simply used equations to determine the unbent length.

Solution #6 – Tricking SOLIDWORKS in changing the Thickness Direction

Denis Bacon demonstrated his genius by submitting an “out-of-this-world” solution. He wondered how SOLIDWORKS maintains the thickness direction across bends and found a sneaky way to confuse the software.

Because of this, he can use standard Sheet Metal features with no loss of functionality. Unbelievable!

Bacon started with a Base Flange to create the first bend.

Figure 19 – Standard start.

The second feature is critical in “confusing” the software. He found out that by adding a cylindrical bridge, the thickness direction can be different in each side of the cylinder. Note that the length of the cylinder has been exaggerated in Figure 20.

Figure 20 – Pure genius.

Bacon added the second bend, as an independent body, using a Base Flange.

Figure 21 – Both Ends are now finished.

A Combine operation brings all three bodies into one. Note that at this time, the model can be flattened and unflattened at will by suppressing and un-suppressing the Flat-Pattern feature.

Figure 22 – Formed and Flat superimposed by using the Toggle Flat Display tool.

To make the end-result as realistic as possible, the cylinder can be as short as 0.00001in.

Figure 23 – Realistic result.

Solution #7 – Using the Flex Feature

Rob Edwards used the Flex feature to get the bent shape. He was aware that Flex is mostly an “artistic” tool and should never be trusted for accurate end-results, but he pushed it to its limits by creating an elaborate series of equations that controlled coordinate systems and angles.

Figure 24.

Figure 25 – The Trim Planes can be set by Sketch Planes.

Figure 26 – Z along path; X along axis.

Figure 27 – Flex.

Solution #8 – Building a Tube from Sheet Metal

Steve Labonte impressed by building all faces of the part from sheet metal. Imagine a bend tube.

Figure 28 – Bent Sheet Metal Tube.

Winners

All solutions were original, but two of them were off the charts.

The winners of the third SWPUC are Dennis Bacon and Ryan Dark.

 

Call for action

I will leave you with one call for action. If you want to have the functionality for unbending tube native to SOLIDWORKS, please vote and ask all you colleagues to vote on:

SPR 542568:  It should be possible to unfold a bent tube like a SHM part.

 


About the Author

As an Elite AE and Process Improvement Consultant, working for Javelin Technologies, Alin Vargatu is a Problem Hunter and Solver, and an avid contributor to the SOLIDWORKS Community. He has presented 22 times at SOLIDWORKS World and tens of times at SWUG meetings organized by four different user groups in Canada and one in the United States. Alin is also very active on SOLIDWORKS forums, especially on the Surfacing, Mold Design, Sheet Metal, Assembly Modeling and Weldments sub-fora. His blog and YouTube channel are well known in the SOLIDWORKS Community.

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