By Chris Smith
When creating our designs in Inventor, we may need to sweep a profile along a helical path (as above). When the profile is normal to the sweep path, we can use the twist option in the Sweep tool to rotate the profile around the sweep path.
If the profile is tangent to the sweep path however, we would fail to create the sweep as the solid body would have no volume. To work around this issue, we can use surface tools to build a sweep path.
- Starting with a profile and sweep path (See Figure 1), we need to add a sketch line between the sweep path start point and the profile we would like to sweep (See Figure 2).
- Start the Sweep tool, but select surface mode, Top right of the tool window as per Figure 3 below.
- Select the line you have just drawn for the sweep profile….
- Then select the sweep path.
- We can now add a “Twist” to the sweep to suit our design specification.
- Select Ok to create the sweep surface. This surface can then be used to create our helical sweep path. Although the sweep tool will allow an edge as input for a sweep path, I am going to use the 3D sketch tool to create a sweep path for each section of the curve. Create a 3D sketch and the use the Include geometry to select the helical edge.
- Repeat the previous task for each section of the sweep path.
- When helical paths have been created for each section, we can use the helical paths to create our sweep. Start with the first section….
- Create a sketch on the end surface of the new swept model and project the profile to continue the sweep.
- Repeat steps 8 & 9 until your model is complete
Depending on the complexity of your sweep curve you may be able to sweep the model in one sweep command. In my case, with such a close profile, it would cause intersecting surfaces causing the sweep command to fail. Building the sweep in sections allows me to circumvent this issue.
Thank you for taking the time to read my tutorial.