Solidworks 2007 – the CAD-Reviews independent review

Please Note: You may be looking for our review of the most recent version of SolidWorks, which can be found here

Best Solidworks ever at same cost

Solidworks 2007 review screenshot

Solidworks 2007 from SolidWorks Corporation

SolidWorks continues to develop apace with the usual extensive mix of new features ranging from me-too catch-ups to improved surfacing tools and innovative usability aids.

One of the key introductions in 2007 is the award winning SolidWorks Intelligent Feature Technology, a range of tools collectively known as Swift.

They aim to enable users to focus more on the design task in hand rather than grappling with a modeller and learning or applying CAD workarounds.

The FeatureXpert supports constant radius fillets, neutral plane drafts and reference planes.

Multiple fillets, for instance, can be applied in one command, creating the minimum necessary number of features to achieve the required result.

If any of the new features need to be earlier in the history they will be automatically inserted at the optimum position.

Subsequent editing allows individual edge fillet values to be modified with separate features being automatically created if required.

Of course this level of automation always raises the question as to whether ease of use that enables new users to be rapidly productive creates a plateau of learning; in this case it may be that learners do not progress to fully understand the nuances of fillet control and existing expert users will wish to retain control over where features come in the design tree.

This is not to say that for the majority of users facing a deadline the ability to solve a tricky failing fillet operation won’t be greatly appreciated! Other Swift tools include MateXpert which replaces mate diagnostics to view errors and force mates to resolve using graphical call-outs, SketchXpert to help understand how dimensions are conflicting in over defined geometry by toggling through possible solutions to maintain the design intent and DimXpert which recognises manufacturing features such as patterns and pockets and applies a user definable scheme so they are fully defined in the drawing.

The 2007 release offers a range of usability enhancements, including the valuable ability to undo edits after leaving a sketch.

The behaviour when a rebuild error occurs can be set to stop, continue or prompt to aid problem solving.

A new transparent dialog can be set to appear after a specified time or number of changes to prompt to save the current or all open documents before fading gradually away.

Models can be saved and therefore reopened with the rollback bar in any position, also allowing rapid access to assemblies that have parts in roll back mode.

To overcome the complexities when transferring large data sets of associative files, a new pack and go utility is available either from inside SolidWorks or on a right click menu when SolidWorks files are selected in Windows explorer.

This combines all SolidWorks file types including parts, drawings, assemblies, Cosmos results etc.

and enables them to be copied to a specified folder or to create a Zip file.

Other methods of sharing data include an updated eDrawings that supports DXF and DWG layers and AutoCAD solids and includes a stamp tool to apply bitmap labels for approved, draft etc.

New methods include a dedicated screen grab to clipboard tool for pasting into documents and Save As 3D PDF that should be viewable by any recipients with the latest Acrobat viewer.

This provides controls to rotate, zoom, colour, illuminate and select individual faces to be hidden.

In the interest of better defined sketches and therefore controlled models, a single command can be used to fully define all or selected entities in a sketch.

Options in the Property Manager include specifying which types of relations should be applied, whether a chain, baseline or ordinate dimension scheme is appropriate and datums for horizontal and vertical dimensions using existing entity points or lines but not planes as would be familiar to users of Pro/Engineer.

This can of course lead to a sketch which is not fully defined as although all entities can be defined to each other, the whole sketch is not defined in space and still needs to be referenced to a coordinate system origin or existing model geometry.

The usability of blocks and sketches has been enhanced in the sketch environment with the ability to change their origin and orientation to be aligned to existing entities.

All entities within a block can also be toggled between normal and construction geometry.

A significant addition is the traction relation that creates rotation constraints between blocks that contain circles and lines allowing simulation of gears and rack and pinion motion.

The Belt / Chain command creates tangent lines and arcs into a continuous belt around circular sketch blocks with the option to toggle the belt route around the correct side of each circle.

Belt length can be determined by pulley location or known belt dimensions in which case idler positions are automatically defined provided at least one pulley has an adequate degree of freedom.

A similar Belt / Chain assembly feature is available to create 3D belts which can be dragged to rotate each pulley at the correct ratio and the Rack and Pinion mate translates a linear motion to the correct rotation of another part.

Gear ratios can also be specified by applying a gear mate between cylindrical faces or circular edges.

Cam motions are created in sketches using blocks of sketch entities and the Make Path tool which can again be manipulated dynamically to analyse the resultant travel.

Where similar mates are required, for instance numerous components needing to be aligned onto a shaft, the Multiple Mate mode can create a Multi Mate folder so that the common reference, mate type or distance parameters can be updated in one edit.

Use of the alt key as a behaviour modifier when dragging components in an assembly enables mates to be created rapidly and intuitively with a pop up toolbar for any modifiers such as distance.

To aid editing of large assemblies, the Isolate pop up toolbar enables the visibility of all but the selected components to be set to hidden, transparent or wireframe.

This view can also be saved as a display state for instant recall.

Of particular interest to industrial designers are the significantly improved controls for fully defining and dimensioning splines.

Higher quality splines can generally be achieved by minimising the number of control points and this is now possible with the ability to adjust spline handles asymmetrical about the control point, using the alt key modify when symmetrical movement is required.

New tangent or equal curvature relations can be created between faces and 2D or 3D splines to aid blending of new features with existing geometry.

A number of new and enhanced surface modelling tools also indicate SolidWorks’ ongoing commitment to achieving a comprehensive solid and surface toolset.

Perhaps of greatest benefit is the option in many instances to use a Boundary Surface instead of a loft as it can be specified to be tangent or curvature continuous to existing surfaces in both directions.

Curvature combs can be displayed in one or both directions with control over scale and density to aid visualisation.

The Fill Surface command is considerably more flexible offering curvature continuous boundary matching and a ‘Fix up boundary’ option to fill boundary gaps or trim oversize boundary faces to minimise the number of preparatory steps and separate features.

The Deform feature is superseded by Freeform to give greater flexibility using a control curve and points to directly manipulate faces using the direction triad.

Options include specifying edge continuity and symmetry as required enabling forms to be created that are not possible with loft or sweep features.

New selection options in the modelling environment include the option to select hidden edges through existing faces when creating fillets and chamfers and a selection manager available in loft, sweep and boundary surface for defining profiles, guides, paths and curve sets.

Pre-selection of closed or open loop, group or region options aids the selection of entities.

Sheet metal capabilities are extended to allow lofted forms to be flattened with the bend lines appearing in the bend regions provided each profile is defined with equivalent geometry and the form can be manufactured using the brake press process.

Flanges can also be added to curved edges provided edges are tangent and bordering a planar face.

Sketches with dimensions can be retained between folded and flattened states allowing artefacts such as surface etching to be shown without creating specific features.

When creating drawing views a task pane tab presents a View Palette that enables preview icons of the part or assembly file selected form a scroll down list to be dragged onto the drawing sheet.

Significantly, sections can now be created in the part or assembly environments and saved as ‘Drawing annotation views’ that then also appear in the View Palette.

Both horizontal and vertical breaks can now be applied in the same view and blocks can be used in drawing views as well as sketches.

A range of other enhancements include improved text alignmentand the ability for any custom properties to be displayed in balloons.

Other tools such as Find and Replace Text and a Microsoft Office style format painter only appear in the SolidWorks Utilities as part of the SolidWorks Office Professional version.

This is also true for the Design Checker which enables spell checking and correction of deviation from required standards.

Conveniently, corporate standards can be learnt from a known conforming document.

SolidWorks proudly claim that the price for SolidWorks has not risen over the years although the widespread uptake of the Office versions to access the range of add-ons has in effect raised the seat price for many, albeit satisfied, customers.

Office Professional for instance adds the fully featured version of eDrawings, PhotoWorks and Animator visualisation, Toolbox part library and FeatureWorks parametric feature recognition and, significantly, PDMWorks.

This has become essential for many users to manage the complexities of multiple referenced documents and can in itself often justify the step up to Office.

It now feels like a more fully integrated tool and the bundled version has in fact been renamed to PDMWorks Workgroup to reflect the existence of the Enterprise version for larger, more dispersed, design teams based on the Conisio acquisition during 2006.

Amongst the Workgroup enhancements are performance improvements and a useful cleanup utility to delete files from the local workspace based on user defined criteria.

It has also been integrated with SolidWorks Explorer to provide access to the vault.

SolidWorks Explorer has a redesigned user interface and rounded corners that look somewhat different from the other application windows and is available as a standalone application or from the Menu Bar in SolidWorks with results appearing in the Task Pane.

Being based on the Microsoft Windows Desktop Search engine an index of defined search paths is created providing rapid results for full text searches plus integrated understanding of SolidWorks file structures including configurations etc.

Despite being described as rendering for engineers, PhotoWorks is capable of producing stunning results with added materials including Moldtech textures and predefined scenes using high dynamic range images that generate realistic lighting environments without complex light set-up and adjustment.

Interface consistency is maintained with the ability to drag and drop materials from the task pane.

Although render time can be huge, PhotoWorks can be used to render each frame in an animation.

Lights and cameras are now supported in the timeline and the mate to curve enables parts to traverse curved paths.

The Office Premium version adds Routing for pipes and cables, more extensive FEA tools in CosmosWorks Designer, simulation in CosmosMotion and ScanTo3D reverse engineering capabilities for handling mesh or point cloud data.

Yet again SolidWorks deliver a huge range of enhancements with this release.

Many, as we have come to expect are innovative and many are user requested, although one, the addition of thumbwheels to the numeric input boxes, has also been described to me by a seasoned CAD user as having his vote for least useful enhancement.

The combination of solid, surface and 2D capabilities plus an extensive range of add-ons make it increasingly difficult to find gaps in the arsenal, but the inevitable challenges of trying to please an obviously diverse user base are shifting the emphasis from not just adding more functionality to making such a complex tool easier to use.

The development of technologies such as Swift look likely to be an interesting ride!