Solidworks - Comments Off - Posted on January, 21 at 9:52 pm
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.
Posted in Solidworks | Comments Off