“Impossible” Modeling Challenges Solved by SOLIDWORKS PowerUsers Part 7: Unbend a Formed I-Beam
This is the seventh in a series of articles on the SOLIDWORKS Power-User Challenges (SWPUC). You can use these links to read other articles in the SWPUC series:
- ‘Impossible’ Modeling Challenges Solved by CAD Power Users
- ’Impossible’ Modeling Challenges Part 2: Dynamic Straightening of a Bent Wire in CAD
- ‘Impossible’ Modeling Challenges Part 3: (Un) Bend a Square Profile in Multiple Directions
- ‘Impossible’ Modeling Challenges Part 4: Reverse Engineering (Surfacing and Direct Editing)
- ‘Impossible’ Modeling Challenges Part 5: Volume Limit Mate (Keep the Prisoner in Jail)
- ‘Impossible’ Modeling Challenges Part 6: Volume Control
Every professional 3D CAD software has some type of functionality for unbending models. For example, SOLIDWORKS has native capabilities for flattening bent sheet metal parts. One of the criteria defining a sheet metal part is the fact that any bend is performed in a direction perpendicular to the thickness of the part.
Typically, power users who do not need this functionality on a daily basis will not have invested in such add-ins. When facing such a challenge, however, they will need to find a solution using the built-in functionality of the software.
What about attempting to unbend a bent I-beam?
For an in-depth study of this problem, the powerusers from the SOLIDWORKS Forum competed in The 4th SOLIDWORKS Power-User Challenge (SWPUC).
This proved to be one of the most popular challenges so far, with over 3,800 views, 81 viewers and 12 participants. Some of the competitors provided several solutions.
The users were asked to:
- Download and import a Parasolid file containing the model shown in Figure 1.
- Calculate the unbend length.
- Create an unbent body.
- Link the lengths of the bent and unbent bodies, as measured on the neutral fiber.
To simplify the problem, the following assumptions were made:
- The neutral fiber goes through the center of the profile.
- An approximation of 0.001mm can be made between the lengths of the bent and unbent bodies.
- Extra consideration is given if no equations are used.
- FeatureWorks cannot be used for reverse engineering the model.
For a more in-depth explanation of the challenge, please watch this video.
Step 1: Create a sketch representing the neutral fiber of the part.
The participants proposed several solutions for this step:
1. Manually draw and constrain a 3D sketch (see Figure 3).
Note: This technique can be fast if the user knows how to apply relations in a 3D sketch. In this specific case, the workflow is significantly simplified if, after placing one point of the sketch in a correct location, the user takes advantage of the concentric relations that could be applied to the arcs.
2. Slice the model per bend (see Figure 4).
2.1. Create cutting entities (planes or sketch lines).
Note that due to the simple geometry, two 2D sketches can be created fast using SOLIDWORKSConvert Entity tool on the bend edges.
2.2. Use the Split command to create separate bodies for the straight and bend areas.
2.3. Hide the bodies containing bends.
Tip #1: Using the cursor, hover over each body you want to hide and press the Tab key.
2.4 Add Reference Points in the center of each cut face.
Tip #2: To save time, take advantage of the intelligent user interface:
- Pin the command using the handy tack.
- After selecting each face, right-click to create each point.
By doing so, all points can be created in seconds!
2.5. Create a 3D sketch using the Reference Points.
3. Use the Mid-Surface tool to create the symmetry references.
For surfacing powerusers, it was only natural for them to attempt to find a solution using surfaces.
The Mid-Surface tool is mostly used by simulation users when they want to reduce the computing time for their studies by using shell elements instead of solids.
Other users are most likely unaware that such a powerful tool exists in SOLIDWORKS.
3.1. Find the Mid-Surface icon.
The icon is not easily found in the main toolbars. A quick way to add the icon is to use the Command Search functionality. Simply search for the command and then drag the icon onto the toolbar of your choice.
3.2. Create the first Mid-Surface body.
The first mid-surface can be created automatically. Simply select the Find Face Pairs button.
The desired result appears as if by magic.
Tip #3: Isolate with Transparent option to better see the resulting surface body.
At this point, some users might simply draw the 3D sketch for the neutral fiber by using the edges of the new surface body as a reference.
Of course, the surfacing gurus would continue using surfacing tools. They would either use the FaceCurve command to quickly generate the neutral fiber at 50 percent of the surface or create a second Mid-Surface (in the perpendicular direction) to be intersected with the first.
Tip #4: If you use the Face Curves method, start a 3D sketch before starting the command. This will ensure that all resulting 3D sketch entities will be located in the same sketch.
3.3. Create the second Mid-Surface body.
If you decided to continue using the Mid-Surface feature, you are in a for a treat. First of all, since we will have to manually select all pairs of faces, let’s prepare our graphics area for quick selections.
3.3.1. For that, create a New Window and tile the window vertically.
3.3.2. Orient the part in such a way that all the required faces will be selectable in the two windows.
3.3.3. Start the Mid-Surface command and simply successively click on a face from each window. Make sure the pairs are selected in the correct order (let’s say from left to right).
The resulting mid-surface body is shown in green in Figure 19.
4. Use the Intersection Curve to create a 3D sketch representing the intersection between the two surface bodies.
Tip #5: To increase visibility, change the resulting Sketch Color.
Step 2: Use the Fit Spline to approximate the 3D sketch entities into a 3D spline.
This will allow you to use the new sketch relation Equal Length.
Tip #6: To maximize accuracy, use a small value for the tolerance.
Step 3: Sketch a line representing the neutral fiber of the unbent body.
Step 4: Add the Equal Curve Length relation between the Fit Spline and the Line.
Now, the line will always match the overall length of the neutral fiber of the bent I-beam.
Step 5: Create the Unbent Body using a Sweep feature.
Tip #7: You can select the end face as the profile. There is no need to sketch the profile!
Step 6 (Optional): Move the new body for better visibility.
Furthermore, each body can be deleted in turn in order to create two configurations, one for the bent state and one for the unbent state.
For a complete demonstration of this technique, please watch this video.
There was very nice use of the new (2017) Equal Curve Length relation and/or equations. Mati also took advantage of the new Offset on Surface tool.
Then we have Rob Edwards’ model, which uses an interesting technique to emulate the Equal Curve Length relation in 2015.
Dennis Bacon impressed us again with his three solutions. Nice to see techniques, first time introduced in the SWPUC #3, used again with great effect.
The Winner of the 10th SWPUC
The Winner of the 4th SWPUC was Erik Bilello. He received extra consideration for the originality of his solution, and especially for the fact that his model can be configured to describe the bending process bend by bend. Amazing stuff!
Even when the software does not provide a solution out of the box, powerusers can always find a way to get the job done!
Along the way, participants had the opportunity to experiment with combining advanced tools that were designed for other purposes. I hope you enjoyed discovering some of these tools.
Starring in today’s show:
- Face Curves
- Fit Spline
- Reference Point
- Intersection Curve
- Equal Curve Length relation
- Right Mouse button
- New Window
- Tab key for hiding bodies/components
- Command Search
- Isolate with Transparent option
- Sketch Color