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A considerable advance in the interface
Solidworks 2001 from SolidWorks Corporation
Of the enormous range of new features and functionality in the 2001 release of SolidWorks, the most obvious is the considerable advance in the interface.
It is not that earlier versions were particularly lacking, but given the increasing complexity of the product SolidWorks have held true to their development strategy of avoiding the historic trap of getting locked into legacy technologies to appease current users that inevitably causes compromises in the longer term.
The goal has been heads-up user interaction.
Many commands have dynamic shaded previews, with handles for dynamic drag and driving dimension callouts displayed on the model.
Entities selected within a command such as guide curves and profiles in a loft are colour coded to indicate their selection set and labelled by callouts to uniquely identify them and aid correct ordering.
Most command dialog boxes have been replaced by the PropertyManager that appears in place of the FeatureManager down the side of the screen without obscuring the model.
The FeatureManager can fly-out temporarily from behind the PropertyManager in particular circumstances where a feature needs to be selected directly from the history tree.
The PropertyManager also dynamically displays properties while sketching so that accurate angles and lengths can be sketched and once committed automatically displays captured constraints.
When selected each constraint appears as a callout, highlighting any referenced entities.
Basic profile sketching is enhanced with the ability to sketch a sequence of lines and tangent or normal arcs without changing command simply by the travel of the cursor.
Sketches on two intersecting planes can be projected together to create a 3D curve representing the intersection of surfaces extruded from them.
3D UV curves can also be extracted from a face or surface.
Combined with a useful ignore holes option, this can be used to create editable surface definitions even from imported data.
There is a new Improve Geometry function added to the Import Diagnosis tool.
Imperfect geometry is simplified but there is always the risk that it may prevent full rebuild of the imported body.
Incomplete imported surfaces can be improved using the delete hole command that allows the selection of any closed profile hole.
For more control the fill surface command allows the creation of a surface patch with any number of sides, within a boundary defined by existing model edges or sketches.
This includes options to maintain tangency with patch edges and use of a constraint curve for greater control.
A single sweep feature can contain multiple contours for multiple lumen or hollow forms.
Alternatively sweeps and lofts can be used to create thin features of a specified wall thickness.
Tangency magnitude and direction can be specified in a loft including editing by dragging handles with a dynamic preview.
A keep feature option on constant large radius fillets avoids the elimination of other features that are entirely overlapped while the graphical callouts make the labelling of values for variable fillets far easier.
The hole wizard for creating complete hole and counter bore specifications in a single feature can be applied on a reference plane so that holes can appear on non planar surfaces.
Sheet metal modelling has had a major overhaul with new features offering an alternative way of working to create parts directly rather than as a conversion from a shelled solid.
The base flange can be a single open or closed profile or incorporate multiple enclosed profiles to create initial cut-outs.
A sheet metal feature contains all the default bend parameters such as bend radius, allowance or deduction and default relief type.
Bend tables are now embedded Excel spreadsheets.
All features created in the folded position are added to the Flat-Pattern1 feature which by default is suppressed but allows the part to be toggled flat by unsuppressing or using the Flattened button.
This avoids the need to roll back the history to add features to the folded part.
One or more folds can be manually unfolded if required for visualisation or the addition of features that cross the fold.
Cuts added to the folded part can be specified to be normal to the sheet as would be the case if cut when flat in production.
A line sketch can be used to create a simple bend while a Mitre-Flange feature can contain flanges on one or more edges with mitres automatically created at tangent corners.
A major enhancement to assembly modelling is control over mirrored parts.
Even within a single assembly some components may be additional identical component instances whereas others may be handed.
The Insert Mirrored Components command allows the appropriate status to be assigned to each component with the option to save mirrored parts out as new files.
For large assemblies parts can be loaded lightweight where only a subset of the model data is loaded in memory and the remaining data is loaded on an as-needed basis.
Control has been extended so that resolved parts can be returned to lightweight status and lightweight parts can be suppressed without being fully resolved first.
Visibility of components can also be controlled by configurations rather than requiring them to be suppressed.
A symmetry mate has been introduced to force two similar entities to be symmetric about a plane.
Existing mates can also be switched to a different type rather than having to delete and recreate as has been the case.
Individual components can be moved within sub-assemblies whilst still within a parent assembly.
The dynamic clearance function has been extended from only reporting the minimum distance between components to prevent components from moving or rotating within a specified distance of each other.
Visio has established a strong reputation as the tool of choice for drag-and-drop electrical circuit, piping and pneumatic diagrams and schematics.
SolidWorks have struck a deal with Microsoft to provide a complimentary license of Visio Technical 2000 to all subscription customers for the shipping cost only.
SolidWorks enables OLE embedding of Visio objects into drawings and changes can be made using the PropertyManager.
Associative drawing view layout has many new capabilities.
Even after placement the orientation of a named view can be revised.
Section views can now be generated from existing section views including hidden edges if required.
Since feature manager data exists for all views it is possible to select individual features to be shown as hidden detail.
Detail, auxiliary and projected views can be created from an exploded view and the extents of assembly motion depicted in an alternate position view.
Again the usability of the dimensioning interface has been addressed with the ability to move, modify and delete dimensions without leaving the dimension command.
Dimension leader lines can be dragged and reattached to entities as required.
Both drawings and sketches can use ordinate dimensions with dynamic updating of values if the zero position is dragged.
Geometric tolerances can incorporate more than two feature frames.
The 2001 release introduces a wide range of new and improved functionality.
SolidWorks determination to rework elements such as the interface that to many was already acceptable points to a long-term strategy of delivering the best possible modeller.
Already the tools for creating complex forms are the best among the design centric modellers and improvements to drawings and sheet metal modelling keep SolidWorks at the front of the pack.
With innovations such as eDrawings to distribute software independent fully shadeable and animated drawings and provision of 3D instant website publishing tools and server space, a credible framework is being created around the modeller for sharing 3D data to enable rich 3D commerce.