Introduction

On an imported part, it is now possible to modify operation because there are none. (However, it is possible to create new operations to modify the shape's geometry.)

This is why, when working with a rather simple imported shape, we can imagine wanting to manipulate it as with sketches, moving the faces (instead of sketch segments) with the mouse, or having dimensions or relationships that would impose constraints on the imported geometry.

This is possible with FreeShape.

Creating a FreeShape

When a file is imported that contains geometric solids with conversion, the shapes of the produced parts are FreeShape by default.

It is also possible to create a FreeShape by converting a shape produced using operations in TopSolid, using the FreeShapes > FreeShape... command. .

This command removes all operations from the existing shape and creates a new Resolution operation that handles the form as FreeShape (like for sketches whose constraints are resolved by such an operation).

Using commands to work on the FreeShape is done in edit mode. Commands in the FreeShape menu are therefore accessible only if the user is currently editing the FreeShape.

Editing a FreeShape

A FreeShape is modified just like a sketch. You must first edit it, then you can add dimensional or relationship constraints or any other modification using functions in the Shape > FreeShape menu.

It is also possible to make some modifications directly with the mouse by selecting a face and moving the mouse without releasing the button.

To edit a FreeShape, use the Edit command in the shape's popup menu to move to edit mode for the resolution.

To finish the FreeShape edition, click the  button upper the graphic area..

Automated dimensioning

To avoid having too many degrees of freedom, which would lead to uncontrollable behavior, it is useful to impose some natural constraints, such as the fact that a planer face retains its orientation.

Other common constraints include maintaining the coaxiality of two aligned holes or even multiple faces making up the same hole (smooth hole with spot facing).

These constraints can be created at the time of conversion by using the command in TopSolid or by using the FreeShape > Automatically Constrain... command later. (This command must be used for imported FreeShapes, which are not constrained.)

As fro a sketch, it exists a color code to indicate the level of constraint of an element. Under-constrained is magenta, totally constrained is blue, fixed is gray.

This color code can be modified in the Tool > Options > Design Colors command.

Operation Extraction

The main interest of FreeShape is being able to easily and quickly work with a shape that is essentially made up of faces with a simple geometry: plane, cylinder, sphere, etc.

It is therefore often useful to get rid of all the small complex faces that can cause problems during resolution.

In particular, if the shape has fillets or chamfers, they should be extracted, or removed from the "resolution" portion, to make traditional operations from them, to recreate the resolved shape, with the resulting shape being the same.

To do this, edit the FreeShape and use the FreeShape > Extract Operation... command. .

Operation Deletion

On the same principle, it is possible to simply delete an operation/geometry. Unlike extract, deletion does not recreate an equivalent operation outside of FreeShape. The operation must therefore be manually created once the valid FreeShape is edited.

To delete a face, use the FreeShape > Delete Faces... command.

Insertion

Conversely, we may want to add faces to a FreeShape to be managed with constraints.

The shape should then be modified using traditional operations (pocket, boss, etc.), and the result should be converted into a FreeShape with the FreeShapes > FreeShape... command.

Dimensions

Once the FreeShape geometry is finalized, it will be possible to constrain it by adding dimensions with the FreeShape > Dimension... command, in the same way as for a sketch.

Relations

Similarly to dimensions, it will also be possible to impose relationships between faces through the FreeShape > Relations menu commands.

Geometry:

Associated geometries (points, axes, planes, etc.) can be created on the shape's entities using commands in the FreeShape menu.