Uncoiling Inventor’s Coil Command28 Feb, 2014 By: Chris Griffith
IMAGINiT Tricks Tutorial: Don’t get twisted up over this easy-to-use tool.
Editor's note: This tutorial courtesy of IMAGINiT Technologies.
In Autodesk Inventor, the coil command is used to create springs, threads, or flights along a cylindrical object, or as a multibody part by creating a helix-based feature. Students often express that they do not understand the Coil command. Once explained, however, it becomes a relatively easy and useful tool that can increase productivity. So let’s start learning about this tool.
Location and Functions
Let’s begin with where to find the command and an outline of the coil command options to get a better understanding of how they work. The coil command is located in the ribbon; navigate to the 3D Model Tab > Create Panel > Coil.
Once active, the Coil dialog box will open, and you’ll see three tabs with multiple options to create the coil:
- Coil Shape
- Coil Size
- Coil Ends
Let’s explore those options and see what each tab has to offer.
Let’s begin with the Coil Shape tab. While in this tab, we will be selecting our profile and axis, and selecting a rotational direction. Note that unless the axis is a work or origin axis, the sketch and axis must be created in the same sketch.
Coil shape options:
- Profile: Used to select the sketch profile needed to create the coil. Inventor selects the profile for you automatically.
- Axis: The axis can be a sketch line or a work axis. This is what the profile sketch is revolved around. Note: The axis cannot intersect the Sketch profile.
- Solid: If the model contains one or more solids, this button can be used to create a new solid out of this coil feature.
- Rotation: Used to select a clockwise or counterclockwise coil rotation.
Output: The output functions are used to define what type of feature you are creating.
- Solid: By choosing this option, a solid will be created from your sketch profile.
- Surface: This option allows you to create a surface feature from an open or closed sketch profile.
Operation: The operation dictates if material is added or subtracted, and in what way.
- Join: Join adds the created feature to another solid.
- Cut: Subtracts material from another solid.
- Intersect: Creates the feature by intersecting the coil with another solid and deleting the unused mass out of the other solid.
- New Solid: This option is the default if there isn’t another solid in the model; it creates a new solid from selected sketch geometry.
This part of the dialog box allows us to determine the coil’s pitch, revolution, and height. The nice thing about this command is that we only need to specify two of the parameters; the third is calculated for us.
Coil size options:
Type: Gives us the option to choose the parameters we want.
- Pitch and revolution
- Revolution and height
- Pitch and height
- Pitch: Pitch determines the amount of elevation for each revolution.
- Height: Determines the height of the coil from the center of the beginning profile to the center of the end profile.
- Revolution: Determines the number of revolutions. It must be greater than zero, but can be a fraction.
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