Offset

The command Parallel allows a contour to be created parallel to another sketch element.

Creation Stages / Use:

Select the 2D sketch > Operations > Offset... command from the drop-down menu.

Select a profile to parallelize.
By checking the Construction option, the selected profile will become a construction profile and will be internal. The offset will not be a construction profile.
Select the parallelization mode:

Local mode:

The default offset distance is 0. It is necessary to provide a list of segments to offset with an offset value for each of them thanks to the Special Segments option.

Global mode:

An offset distance has to be entered. Select the side of the offset or if it is centered.

	One side: The parallel is on the side indicated by the arrow.
	Both sides: The parallel is on both side of the selected element. 2 different offset can be entered.
	Centered: The parallel is on both side of the selected element and centered. The entered value corresponds to the distance between the selected element and one of the two parallels.

Revolution mode:

A distance for segments parallel to the revolution axis and a distance for other segments have to be entered.

Lettering:

Allow to quickly create parallels of several closed profiles.

	Explicit list of closed profiles: Allow to manually select the profiles to be parallelized.
	Provided list of closed profiles: Allow to parallelize all profiles in a sketch.

TopSolid displays an arrow with a label allowing the distance and the direction of the parallel to be modified dynamically:

Dynamic modification of the distance	Click the end of the arrow and move your mouse while holding down the button.
Reversal of direction	Double-click the end of the arrow.
Modification of distance	Double-click the label displaying the distance and enter the distance value.

It is not possible to create the parallel from a construction element or from an element inside the sketch.
This command is a sketch operation.

This command creates a new sketch profile.
With Local mode, if the selected profile in the one of the edited sketch, the result will be superimposed sketches.
Fillets near special segments are not built again. Blends are added in some cases.

Available Options:

Reverse:

The Reverse option allows the dimension of the parallel to be changed, this action can also be carried out by double-clicking on the end of the arrow.

Special Segments (not available with lettering mode):

This dialog allows to give a special offset value on some segments of the selected profile.

You can apply the special value between the selected segment and an end segment thanks to the Until... option available in the contextual menu of the special value label.Then the Reverse option allows you to change the way to browse the profile.

Special Fillets (not available with lettering mode):

This dialog allows to select an explicit list of segments for which fillets will be treated differently.

Extract: The selected fillets will be removed from the parallelization result.
Keep: The selected fillets will be kept with the same radius value in the parallelization result.
Replace: The radius value is specified for the selected fillets.

The selected mode will be applied to all selected fillets (Inherit icon). However, by right-clicking on the dialog icon or double-clicking on the icon in the graphics area allow to impose another mode.

Number (only available in global mode):

You can indicate an instance number, each instance will be offset from the distance indicated.

Rounded joins (only available in global mode and lettering mode):

This option allows a fillet equal to the offset distance to be created on all the convex vertices of the parallel profile. This fillet will be reported on all the instances of the parallel profile.

Strict (only available in lettering mode):

This option ensures that all profiles will have their parallel. With this mode active, if a profile cannot be parallelized, it will not be possible to validate the dialog. Or if the reference profile is modified after parallelization, the operation may become invalid if parallelization is no longer possible.

Without this option active, the parallelization operation is still possible and profiles that cannot be parallelized are ignored.

Profiles to reverse (only available in lettering mode):

This option allows to select an explicit list of profiles for which the the parallelization direction will be reversed.