To Create a Solid Protrusion
1. Click > 
Extrude. The Extrude tab opens.
Extrude. The Extrude tab opens.2. To define the body to which the feature is added, click the Body Options tab and select an option:
◦ To add geometry to an existing body, click the body collector, and then select the body to which geometry is added.
◦ To create the feature in a new body, select the Create new body check box. The name of the new body appears in the body collector.
3. Select a sketch to extrude, or to create a sketch, click the Placement tab, click Define, sketch a section, and click 
OK.
OK. | You could also select a sketch first, or select a datum plane or planar surface first, and then click > Extrude. |
4. Select a depth option from the menu:
◦ 
Variable. Type a value.
Variable. Type a value.◦ 
Symmetric. Type a value.
Symmetric. Type a value.◦ 
To Next. The extrude stops at the first surface of a solid that it reaches (not available in Assembly mode).
To Next. The extrude stops at the first surface of a solid that it reaches (not available in Assembly mode).◦ 
Through All. The extrude stops at the last surface it reaches.
Through All. The extrude stops at the last surface it reaches.◦ 
Through Until. Select a reference surface (not available in Assembly mode).
Through Until. Select a reference surface (not available in Assembly mode).◦ 
To Reference, and then select one of the following options:
To Reference, and then select one of the following options:▪ 
—Extrude to a selected point, curve, plane, surface, quilt, or body.
—Extrude to a selected point, curve, plane, surface, quilt, or body.▪ 
—Extrude to an offset of a selected point, curve, plane, surface, quilt, or body, and then set a value for the offset distance. To flip the offset direction, click 
.
—Extrude to an offset of a selected point, curve, plane, surface, quilt, or body, 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, surface, quilt, or body, and then set a value for the translation distance. To flip the translation direction, click .
—Extrude to a translation of a selected point, curve, plane, surface, quilt, or body, and then set a value for the translation distance. To flip the translation direction, click .5. To flip the direction of feature creation in relation to the sketching plane, click .
.6. (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.
7. 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.
8. If required, to add a taper to the extrude, click the Options tab, select the Add taper check box, and then type a value from -89.9° through 89.9° for the taper angle.
| | You can add a taper to an extrude if the section of the feature is a closed loop. You cannot taper an extrude if  Thicken Sketch is selected. |
9. Click 
OK.
OK.