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SolidWorks Tips & Tricks
Sponsored by
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Getting a Clean Tapered Edge in the Flat Pattern
Many times when you design a part with a
tapered edge, you really want the flat pattern to have a clean, single line
edge without the bumps along the bend area. This tip will show you how to
accomplish this, looking at several techniques in SolidWorks to see which
one really gets the job done.
Click to enlarge
Take, for example, the tapered
Z-bracket above. Your first instinct might be to create a
base flange with tapered sides and then add two edge flanges to complete the
part. This allows you to hold your key dimensions, but notice the end of
each bend
area in the flat pattern. The edge of the bend area does not line up with
the edges of the flanges. This creates a stepped or irregular edge. Whether
you are punching or cutting on the laser, you really want this to be a
single, continuous line.
So, how can you avoid the jagged edge
and create an 80 degree angle down the whole side? One method that comes to
mind is the Sketched Bend command. I was able to use Sketched Bend to create
the shape and hold the tapered edge, but the problem that exists is that you
have to manually calculate the overall flat pattern length in order to get
the correct size part.
The Jog command gives you control over
the length, but the Fix projected length check box stretches the
original shape you created as shown below, not producing the desired result.
I found that the easiest way to avoid
all of this is to create your base flange as the cross section of the part. Then,
unfold the part and use an Extruded cut to create the taper.
To
show you what I mean, create a new Part
document. Then from the Sheet Metal CommandManager, create a base flange
using the Base-Flange/Tab command. Create the sketch on the Right Plane
and dimension it as shown below. You'll have to come back and add the last
dimension with an equation after the sheet metal part has been created.
Then, in the Base-Flange
PropertyManager, I set the Depth to '200.00mm', the Thickness
to
'2.00mm'
and the Bend Radius to '5.00mm'.
In the FeatureManager design tree, right
click on Base-Flange1 and pick Edit Sketch. Add a dimension to
the bottom left horizontal line. Modify the dimension. In the Modify
dialog box, pull down the menu and pick Add Equation. In the Add
Equation dialog box, type "D3@Sketch1" = 50-"Thickness" and click
OK.
Exit the sketch. The Z-bracket is almost complete. The
key dimensions from the drawing are held correctly. All that's left is to
add the taper. To do this, click Unfold in the Sheet Metal CommandManager,
or pull down the "Insert" menu and pick Sheet Metal - Unfold.
Pick the bottom flange as the Fixed face and then in the Unfold
PropertyManager, click the
Collect All Bends button and click OK.
Next, click Extruded Cut in the Sheet Metal CommandManager,
or pull down the "Insert" menu and pick Cut - Extrude. Pick the top
of the part and sketch the two triangles as shown. I linked the two angled
dimensions using Link Value.
In the Extrude PropertyManager, check Link to
thickness and click OK. Finally, click Fold in the Sheet Metal CommandManager,
or pull down the "Insert" menu and pick Sheet Metal - Fold. Click the
Collect All Bends button and click OK.
That's it! The flat pattern has a nice, clean, single line tapered edge and all
the dimensions hold their desired values.
To learn more about sheet metal part
creation, click here.
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