Anis one or more features that you want to reuse in other designs. You can specify a feature name, set size and position parameters, attach a Placement Help document, and give the feature a unique file name.
When you place the iFeature, you select geometry on the part to position the elements listed in the Position Geometry list.
As you become proficient at creating and using iFeatures, your features can become more complex. You can decide what geometry to include in the Position Geometry list of the Extract iFeatures dialog box.
In the Position Geometry list, you can add reference edges that position the base feature sketch of the iFeature. Including reference edges captures more design intent, but it requires that the iFeature be positioned in the same way it was originally placed.
When you create an iFeature from multiple features that share geometry, by default the shared geometry appears only once in the Position Geometry list. For example, you create an iFeature from an extruded feature that terminates on an offset work plane. The work plane is offset from the same face that the extrusion is sketched on.
In the Extract iFeature dialog box, the geometry is shown in the following way:
In the Position Geometry list, you can right-click the plane and select Make Independent to list the planes separately. When the iFeature is used, you select and position each plane separately. You have greater flexibility in how the iFeature is used, but are required to select additional position geometry during placement.
In the Position Geometry list, you can rename the planes to make them easier to understand when the iFeature is placed. Rename Plane1 to Work Plane Offset Face and Profile Plane2 to Sketch Plane.
iFeatures created from multiple-sketch features (such as lofts and sweeps) can be more useful when you add geometric elements to the Position Geometry list.
Lofts Lofts contain two or more sketches on separate sketch planes. By default, the first profile selected in the loft feature is shown in the Position Geometry list. The position of remaining sketch planes is defined relative to the first profile. By including additional sketch planes in the Position Geometry list, the location of the included planes is selected when the iFeature is placed.
In the Selected Features tree, select the profile, right-click, and then select Make Independent. Individual sketch planes are listed in the Position Geometry list and can be positioned separately when the iFeature is placed.
Optionally, you can combine two or more sketch planes in the Position Geometry list so that their positions are relative to one of them. When selecting sketch planes to combine in the list, the first selected sketch plane remains in the list. The position of the other plane is relative to the first. Right-click the sketch plane, and then select Combine Geometry.
Sweeps If no dependency exists between the profile and path sketches, by default the profile sketch is shown in the Position Geometry list. In this case, the path sketch position is defined relative to the profile.
To make placement of the path sketch independent of the profile sketch, you can add it to the Position Geometry list. In the Selected Features tree, right-click the path sketch, and then select Make Independent.
For some iFeatures, such as an O-ring groove created with a sweep, you want to define the position relative to the path sketch. In the Position Geometry list, right-click the path sketch, select Combine Geometry, and then click the profile sketch. Because the path sketch was selected first, it is listed.
Use the Insert iFeature command to place an iFeature in a part file on a planar face or work plane.
The values in the Insert iFeature dialog box correspond to the Size Parameters and Position Geometry defined when the iFeature was created. You can edit the iFeature parameters and roughly position it before you insert it.
Table-driven iFeatures list available key parameters. Enable Use Key 1 as Browser Name column in the iFeature tab of the Application Options to use the Key 1 value in the browser name.
If enabled, the inserted iFeature displays the following in the browser:
Select from the defined parameters to specify the iFeature instance.
Use the following to help position an iFeature:
You can edit size and position after you place an iFeature. Only the current occurrence of the iFeature resizes or relocates to correspond with changed values.
Right-click the iFeature in the browser, and then select one of the following:
For table-driven iFeatures, you can change to a different version:
Lists names of interface geometry.
On a selected planar face or work plane, click the arrowhead on the positioning symbol, and then move the cursor to rotate. Click again to complete rotation. If you prefer, enter an angle value in the Angle field. To move, click the crosshairs on the positioning symbol, move cursor to new location, and then click again to place.
Lists named interface geometry.
Lists the default of the placement geometry on the iFeature.
Move Coordinate System
Allows horizontal and vertical axes to be precisely defined. Required when the iFeature has horizontal or vertical dimensions or constraints.
|Selects the participating solid bodies in a multi-body part file. Not available if the part contains only one body.|
When the requirements for placement are satisfied, it is noted in the corresponding row with a check mark in the left column. You can continue to click in the row to change values, or move the crosshairs or arrowheads to reposition the iFeature. Click Next or Back to continue or Finish to complete placement with current orientation.
Lists names and default values of key iFeature parameters. Click in the row to edit the value, and then click Apply to preview.
Lists parameter name.
Lists value of the parameter.
For table-driven iFeatures, click to list defined values. The current value is the default row. Select the All Values check box to list all values. Click a value or press Esc to close the list.
Upon completion of placement determines whether the iFeature can be positioned by constraints and dimensions.
Activate sketch edit immediately
Displays the sketch of the iFeature and activates commands on the Sketch tab. Use dimensions and constraints to position the iFeature on a parent feature.
Do not activate sketch edit
iFeature is positioned without constraints or dimensions. Its sketch must be activated before you can edit position.