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How to make a Sheet Metal Transition


A sheet metal transition is generally a piece of duct work that changes in cross section from one shape to another, typically from a rectangle to a circle. You can model a part like this in Solid Edge sheet metal and flatten it.



Sheet metal parts have a special file type in Solid Edge, so you have to create a file that is dedicated as a sheet metal part from the start. You should have at least a default sheet metal template in your list of templates. Also, this part has to be done in Ordered mode, so transition to Ordered before you start sketching and save yourself some time.


Start with a rectangle with fillets in the corners, and a gap in one side. The gap is for the sides of the flat sheet. This can be smaller than shown in the image. The rounded corners are to help accommodate the transition to the circle.


Make an offset plane to represent the length of the transition. Open a sketch on the offset plane. The second shape doesn't have to be lined up with the first shape - there can be some lateral offset between the centers or the shapes.



On the offset plane, again sketch a rectangle with rounded corners, but this time, make the fillets very large so that the flat sections are very small. The 1.000 dimension above refers to the flat section. Notice at the top there is still a gap, with a .250 flat on either side of the gap. These sketches look like they are on top of one another, but they are offset by some distance in the Y direction (out of the screen).


SNAG-0003.pngClose the sketch, and initiate the Lofted Flange command. You will find it on the drop down list from the Contour Flange.


SNAG-0004.pngAs usual with Solid Edge, follow the PromptBar for the steps of working through this feature. Select the first sketch, right click, select the second sketch, right click. Set the side of the material (inside or outside the first sketch). Set a thickness for the material.


You may also need to edit the Options for the sheet metal part to satisfy your needs. In the image below you can see the bend lines through the solid. SNAG-0005.png


To flatten the part, go to the Tools tab, and at the left hand side of the ribbon is the set of toggles for Synchronous, Ordered, Simplify, and Flatten. This step is omitted from all of the Help documentation I've read, so make sure you remember to do this.


Next you need to specify a face to keep flat and an edge to lie on the X axis.


You can turn off the display of the original sketches and planes in the Pathfinder.

Retired Community Manager for Solid Edge. This account is no longer active.
Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

In addition to Matt's info above.....with displaying the triangulated [which can sometimes take a little time to calculate before being displayed] bend lines, in lower powered PC's the graphics performance can take a bit of a hit, and while it looks visually quite technical, it is also very untidy with them being visibe through the part. I do wish these were calculated behind the scene, more like at the time of flat patterning only...however, currently you need to have them activated on the model, in order to show them on the flat pattern, both in Draft and when exporting via the Save As Flat command. [as always, it’s worth checking through the "Options" available for any import/export]


Lofted Flange Options_Triangulated Bending [Check Box]



Save As Flat_Options



Save As Flat as opened in AutoCAD, a few tweaks and its ready for laser etching & cutting.