Part Modeling > Base Features > Extrude > Working with the Extruded Feature > To Create a Thickened Extrusion
To Create a Thickened Extrusion
1. Click Model > Extrude. The Extrude tab opens.
2. Select a sketch to extrude, or to create a sketch, click the Placement tab, click Define, sketch a section, and click OK.
* You could also select a sketch first, or select a datum plane or planar surface first, and then click Model > Extrude.
3. Select a depth option from the menu:
Blind. Type a value.
Symmetric. Type a value.
To Next. The extrude will stop at the first surface of a solid that it reaches.
* This option is not available in Assembly mode.
Through All. The extrude will stop at the last surface it reaches.
Through Until. Select a reference surface.
* This option is not available in Assembly mode.
To Selected, and then select one of the following options:
—Extrude to a selected point, curve, plane, or surface.
—Extrude to an offset of a selected point, curve, plane, or surface, and then set a value for the offset distance. To flip the offset direction, click .
—Extrude to a translation of a selected point, curve, plane, or surface and then set a value for the translation distance. To flip the translation direction, click .
4. To flip the direction of feature creation in relation to the sketching plane, click .
5. To add thickness to the sketch, do the following:
a. Click , or right-click the feature and choose Thicken Sketch on the shortcut menu.
b. Type a value for thickness in the box to the right of .
c. To change the side of the sketch to which the thickness is added, click to the right of the thickness box. You can switch between three modes:
Add thickness to Side 1
Add thickness to Side 2
Add thickness to both sides
6. When the system detects at least one surface that can be used to cap the extrusion and attach it to the solid geometry, specify how to attach the extrusion to the model. Click the Options tab, and perform one of the following actions:
By default, the system tries to cap the thickened extrusion with model geometry. You can cycle through the available geometry by clicking Previous and Next.
When you point to the Section end point 1 or Section end point 2 label, the corresponding end point is highlighted in the graphics window.
The sketch must intersect the solid geometry. The end point of the sketch must intersect either a reference you select, or the extension of the reference.
When the end point of the sketch does not intersect the selected reference, but intersects the extension of the reference, you must add the desired capping geometry as references to the sketch:
1. To edit the sketch, on the Placement tab, click Edit. The Sketch tab opens.
2. Click References. The References dialog box opens.
3. Select the geometry to use as references to cap the feature and attach it to the solid geometry.
4. Click Close.
5. Click OK.
If you do not want to cap the extrusion with existing model geometry, clear the Cap with model geometry check box. This caps the thickened extrusion with a surface that is normal to the end of the sketch.
7. (Optional) The section used for the extrusion is associative with the sketched datum curve you selected. To break this associativity and copy the section into the extrusion, click the Placement tab, and then click Unlink.
8. To create a double-sided feature, do one of the following actions to define the depth for the second side of the sketching plane:
Click the Options tab and select a depth option for Side 2.
Right-click the drag handle, choose Other Side, and then select a depth option.
Right-click the graphics window and select Side 2.
9. Click .