Trim Entities
Select the trim type
based on the entities you want to trim or extend. All trim types are available
with 2D sketches and 2D sketches on 3D planes.
To trim a 3D sketch:
Start the 3D sketch on a 2D plane.
Then do either of the following:
You can use any of the following trim options:
Power
Trim
Use Power
trim to:
Trim multiple,
adjacent sketch entities by dragging the pointer across each sketch entity.
Extend
sketch entities along their natural paths.
Arcs have a maximum extension length on either side of the
arc. Once you reach the maximum extension length, the extension shifts
to the opposite side.
To trim with the Power trim
option:
Right-click the sketch and select Edit
Sketch.
Click Trim Entities
Sketch toolbar) or Tools,
Sketch Tools, Trim.
In the PropertyManager, under Options,
select Power trim 
.
Click in
the graphics area next to the first entity, and drag across the sketch
entity to trim.
Continue
to hold down the pointer and drag across each sketch entity you want to
trim.
Release
the pointer when finished trimming the sketch, then click OK
.
Power trim - trim
To extend with the Power trim
option:
Follow
steps 1 - 3 from the preceding procedure.
Select
anywhere along the sketch entity to extend.
Click
and drag the pointer as far as you want to extend the sketch entity.
Release
the pointer when finished extending the sketch entity, then click OK .
Power trim - extend
Return
to trim options
Corner
Extends or trims two sketch entities until they intersect at a virtual
corner.
To trim with the Corner option:
Right-click the sketch and select Edit
Sketch.
Click Trim Entities
on the Sketch toolbar, or click Tools,
Sketch Tools, Trim.
In the PropertyManager, under Options,
select Corner 
.
Select
the two sketch entities you want to joined.
Depending on the sketch entities and their relative position
to each other, the software extends or trims each entity to join them.
A message appears when the operation cannot be completed.
Click OK .
Corner
Return
to trim options
Trim
Away Inside
Trims open sketch entities that
lie inside two bounding entities.
To trim with the Trim away inside
option:
Right-click the sketch and select Edit
Sketch.
Click Trim Entities
on the Sketch toolbar, or click Tools,
Sketch Tools, Trim.
In the PropertyManager, under Options,
select Trim away inside 
.
Select
two bounding sketch entities.
Select
the sketch entities to trim.
The sketch entities you select to trim must either intersect
each bounding entity once, or not intersect the two bounding entities
at all.
Click OK .
Trim away inside
Return
to trim options
Trim
Away Outside
Trims open sketch entities outside
of two bounding entities.
The same rules
that govern the Trim away inside
option govern the Trim away outside
option.
Right-click the sketch and select Edit
Sketch.
Click Trim Entities
on the Sketch toolbar, or click Tools,
Sketch Tools, Trim.
In the PropertyManager, under Options,
select Trim away outside 
.
Select
two bounding sketch entities.
Select
the sketch entities to trim.
Click OK .
Trim away outside
Return
to trim options
Trim to Closest
Right-click the sketch and select Edit
Sketch.
Click Trim Entities
on the Sketch toolbar, or click Tools,
Sketch Tools, Trim.
In the
PropertyManager, under Options,
click Trim to closest 
.
The pointer
changes to 
.
Select
each sketch entity you want trimmed or extended to the closest intersection:
To
extend, select the entity and drag to the intersection.
To
trim, select the sketch entity.
Click OK .
Trim to closest
Return
to trim options