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SolidWorks Tips and Tricks
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Helical Threads
How to create a helical thread.
A lot of us have seen a plastic bottle created in
SolidWorks. It's a common demo that resellers use. One feature on a plastic bottle is the helical thread on the
neck of the bottle. To some, it looks like a very complicated feature. There are
various opinions on the best way to create a helical thread. I will show you
how to use the Variable Pitch option of the Helix command and the
Face Delete command to create the neck of the bottle.
To start us out,
open up a new part document. I just used the default mm part template. I
will just show you the technique. Then, you can apply it to your part. Create an Extruded Boss/Base on the Top plane. Create
two circles centered on the origin and dimension them as shown.
Exit the sketch.
In the Extrude PropertyManager, set the Depth to '50.00mm'
and click OK. Now, I want the helix to start a little below the top
of the extrude. To do this, create an offset reference plane by pulling down
the "Insert" menu and picking Reference Geometry - Plane. Select the
top face of the part. In the Plane PropertyManager, set the
Distance to '5.00mm'. Make sure that the plane is below the
top face. I had to check the Reverse direction check box to get my
plane below the top surface. Click the OK button.
With the new
plane selected, start a sketch. Press Ctrl+8 to switch Normal to the
sketch. Pick the outside circle and pick the Offset Entities button
from the Sketch tab on the CommandManager, or pull down the "Tools"
menu and pick Sketch Tools - Offset Entities. In the Offset
Entities PropertyManager, set the Offset Distance to '5.00mm'.
Check the Reverse check box and click the OK button. This will
ensure that the helix will begin inside the part, allowing a nice lead in
and lead out for the thread.
With the sketch
still active, pull down the "Insert" menu and pick Curve - Helix/Spiral.
Press Ctrl+7 to switch to the Isometric view. In the the
Helix/Spiral PropertyManager, check the Reverse direction check
box so that the helix will go down. Set the Pitch to '15.00mm'.
To vary the diameter of the helix, pick the Variable Pitch radio
button. A small chart will appear allowing you to enter the revolutions, the diameter,
and the pitch.
During the first quarter revolution, we want the diameter to expand from
90mm to 100mm. So, modify line 2 in the chart to show the values '0.25'
for the Rev, '100mm' for the Dia, and '15mm' for
the P. We then want two full revolutions, maintaining the 100mm
diameter at the same pitch. So, add the 3rd line in the chart as shown
below. Then, for the last quarter revolution, we want it to return to the 90mm
diameter. To do this, add the 4th line as shown below.
Make sure that
the Start angle is set to '0.00deg' and click the OK
button. In the FeatureManager design tree, right click on Plane1 and
click Hide.
Next, start a
sketch on the Right plane and draw a profile of the thread off to the
side of the part, as shown. I just kept it a simple shape. Once you learn
how to do this, you can create a better thread profile.
Ctrl
select the right end point of the horizontal centerline and the helical
curve. In the Properties PropertyManager, click the Pierce
relation to connect the profile to the path. Click the OK button and
exit the sketch.
Now sweep the
profile along the path. In the FeatureManager design tree, select the last
sketch that you just created. Then, pick the Swept Boss/Base button
from the Features tab on the CommandManager or pull down the "Insert"
and pick Boss/Base - Sweep. In the Sweep PropertyManager,
click in the Path box, and then, pick the helix in the graphics area.
Once you see the preview, click the OK button. You should see a nice
thread with a lead in. But you also can see that the thread sticks through
the inside of the part as well.
To fix this, you
can use the Face Delete command. Pull down the "Insert" menu and pick
Face - Delete. Pick all 8 faces that came through into the middle of the
part. I right clicked and used the Select Other command to get the
bottom faces.
Once all 8 faces
are highlighted, make sure that Delete and Patch is selected in the
Delete Face PropertyManager.
Click the OK
button. The middle of the part is back to how it should be. If you want you can
add fillets to the threads.
That's it! That should get you going to add your own helical threads on your
parts.
To see a video of the entire bottle by
SolidWorker.com,
click here.
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