Solidworks 2008 – 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

Solidworks 2008 screenshot

Developing software must be like tightrope walking for established vendors. On the one hand a loyal, partisan ‘power’ user base has invested in developing skills and a customised interface to maximise their productivity. They seek little change, whereas occasional, new and future users stand to benefit from evolution, even revolution, as the technology and skill of the developer advances. And so some applications have withered behind dated interfaces while SolidWorks maintains its resolve to take the short term pain for the long term gain.

The SolidWorks 2008 release has a lighter, more graphical interface that will undoubtedly need some, albeit quick, relearning and customising for power users, but achieves its aim of maximising the graphics area and providing rapid access to essential commands and options.

Selection of an entity, including feature manager tree entries, pops up a semi transparent context specific toolbar of options that can be ignored and fades as the mouse moves away or solidifies when approached to select an option. Pressing the S key also pops up a customisable shortcut tool palette of the most commonly used commands at the cursor location. The application border that in most applications is blank between the document and application name on the left and the window control buttons on the right now contains key system commands and pops out the menu bar to save the screen space required for one customary tool ribbon. Unless ‘pinned’ to appear permanently, the absence of the customary ‘window’ menu item prompts more use of the File Explorer tab that itself pops out a more comprehensive listing of files currently open in the SolidWorks session or, for simplicity, the R key pops up a graphical menu of Recent documents.

SolidWorks Explorer also now has an iTunes-style ‘cover flow view’ to rapidly scroll through previews.

The next standard horizontal tool bar down the screen is the Command Manager. This initially has part, drawing and assembly environment tabs below on the left hand side for the major command groupings. In line with these tabs, in the centre of the graphics area, is a customisable toolbar of view related commands. Although the command icons appear superimposed on the model, the toolbar itself is transparent so it acts as a visually unobtrusive heads-up display. When the graphics area is split into multiple view panes, it appears in each to provide pane specific control.

Real time modelling in an almost photorealistic environment

The overall visual richness is further enhanced by RealView functionality which allows real time modelling in an almost photorealistic environment. This incredible performance utilises graphics card processing capabilities and is therefore not achievable on older systems so the SolidWorks web site helpfully includes a comprehensive listing of compatible hardware. The standard graphics display is by no means bad but dynamic use of materials, textures, shadows and realistic environment reflections brings a model to life and can communicate a design far better.

The Appearances Property Manager allows mapping style, orientation and size to be optimised. Basic scenes provide simple backgrounds and lighting, presentation scenes use a background image that become a part of the scene and studio scenes enable the combination of floor/wall backgrounds with the added impact of real world reflections.

RealView and PhotoWorks use the same material database, so with RealView enabled the PhotoWorks materials override the SolidWorks colours and textures. This makes RealView a great way to quickly preview PhotoWorks set-ups. Despite the quality of RealView in realtime, PhotoWorks can deliver even higher quality images using more accurate, fully ray-traced scenes with high dynamic range indirect illumination.

In fact a huge number of changes have been made in PhotoWorks to improve both usability and image realism. More tools are available to adjust the orientation and offset of environment elements which include cubic environment mapping. Background scenes use 360 degree high dynamic range images enabling representation of contrast ratios where an object and therefore image pixel can be a million times brighter than another rather than the 255 times available in standard images. Several HDR images are supplied but commercial collections are also available for download. Of key interest to product designers is the availability of emissive light emitting objects such as LEDs, neon tubes, back lights etc. and realistic falloff to better simulate how light intensity diminishes as a function of distance. A post rendering editor is also available to adjust brightness, contrast and colour saturation.

Instant 3D functionality for streamlined workflow

The workflow for many features has been streamlined with Instant 3D functionality. Rather than selecting a sketch plane, then sketch tool, then feature as previously, with any sketch tool selected entities can be created onto any existing planar face. Sketch entities can be edited without specifically entering the sketch environment and simply by selecting an entity a drag arrow allows a 3D extrusion or cut to be created. A dynamic scale enables an approximate size to be set very rapidly and the Alt key enables the modified feature to be snapped to an existing face of vertex. Many features can be modified directly; for instance, by dragging the size of a fillet the model updates dynamically and if, for example, a resized feature will make a shell fail the shell disappears from view at the point the dimension causes the failure.

All this direct interaction still creates and updates feature properties in the Feature Manager history tree correctly and it can be toggled off to avoid inadvertent dragging if required. It is also possible to edit dimensions for any sketch without the model rolling back to that point in the history which makes it much easier to understand the potential affect on the current model. Instant 3D also facilitates the Live Section tool allowing a section plane to be dynamically dragged and rotated through the model with any elements highlighted in magenta directly editable.

If the visual aspects of the 2008 release are dramatic, modelling capabilities also have some new twists – literally in the case of being able to sweep a revolved solid body along a tangent path – for example simulating a cutting tool passing around a cylindrical body. Although the standard Fillet PropertyManager tab remains for manual control of features, the FilletXpert dynamically manages feature order and invokes the FeatureXpert to resolve rebuild errors. When using the FilletXpert to add constant radius fillets a pop-up context toolbar provides options for additional edges to fillet such as connected loop, all or all convex on the connected body. By providing a means of selecting all fillets of a given radius it also enables the rapid updating of multiple fillets in one operation.

An additional Corner tab in the FilletXpert property manager also allows the creation and management of corner features where exactly three filleted edges meet at one vertex. Consistent with Windows standards, using ctrl + drag enables a corner arrangement to be hovered over other corners to identify incompatible or possible locations. In the sheet metal environment, weld beads can be added to improve the appearance of the 3D model but that are automatically suppressed when flattened. Flat patterns can be exported directly to the commonly used DXF format without the need to create a drawing sheet first.

Important enhancements appear in the sketcher

Some of the less glamorous, but still important enhancements appear in the sketcher. Rectangles for instance can now be specified in multiple ways including by centre point complete with diagonal construction lines that aid symmetrical location. A consolidated property manager enables rapid selection of the preferred method. Sketching now also includes a symmetry constraint and dynamic mirror so that entities are mirrored as they are created and dynamically retain the constraint as the mirror line is moved. Areas can be hatched or filled to aid legibility. Although it has previously been possible to load bitmaps onto sketch planes, tools are now available to auto trace outlines to rapidly create sketch entities as the basis for features.

To extend familiar Microsoft Office concepts, the 2008 release introduces design clipart. More than simply enabling the reuse of complete design files, the process dissects parts into extrude and cut features and features into their constituent sketches. Drawings and external DWG and DXF files are dissected into tables and blocks. All of these elements then become visible as thumbnails in SolidWorks searches for re-use in new designs. Accessible through the menu bar search tool, selected items prompt to dissect immediately or to schedule if not yet processed. When inserting bodies into a part it is now possible to create a coincident mate to locate it with the existing geometry including axis alignment to fully constrain or alternatively existing mate references can be automatically used.

Concept modelling is greatly aided by a number of assembly tools including more freedom to switch between top-down and bottom-up methods. A new Layout sketch environment is available allowing enhanced blocks and components to be constrained to each other which also facilitates quick motion simulations including out of plane movement if using a 3D sketch. Internal components, indicated with square brackets in the FeatureManager, can also be created and developed within an assembly file with the option to delete or save out as standalone parts later when the design direction is established. This not only reduces the management of multiple associative files and the sheer number of superseded part and assembly files, but also enables components to be simply renamed in the FeatureManager without resorting to the full ‘open/save as copy/replace component’ workflow.

Large assembly management is aided by the ability to select Quickview on opening. This is said to allow a thousand part assembly to open in seconds. The Quick View/Selective Open option specifies components to be rapidly opened as lightweight with other components not loaded or visible but with the effects of their mates still active. This also creates a display state that can be instantly recalled if required including in eDrawings. Visibility of specific bodies of interest can also be aided by an isolate command that enables unselected bodies to be set to hidden or transparent.

New Mate icons provide new functions

Assemblies can be checked for mis-alignment of holes, with the option to specify the maximum allowable deviation. Mirrored and derived parts can include planes, axes, sketches and custom properties with the option to break links to the original without losing the ability to edit features. Mate icons have been updated and a number of new ones added or transferred from the motion environment to assemblies. The Lock mate enables two components to be fully constrained to each other without needing to create a rigid sub-assembly. A Path mate enables any point on a component to be set to follow a defined path and the Screw mate is similar to a concentric mate with additional pitch and rotation properties. Other properties such as Load bearing Face and Friction can be applied in preparation for analysis without needing to have the CosmosMotion add-in loaded.

Dimensioning and tolerancing DimXpert and TolAnalyst tools have been significantly updated. Currently based on ANSI standards and applicable to machined components, DimXpert for parts uses model feature and topology recognition to automatically or interactively create a dimensioning scheme with the minimum number of dimensions. Under constrained features are highlighted in yellow, over in red and fully constrained in green. Significantly these schema are independent of the feature dimensions in order to avoid conflicting good modelling and manufacturing practices and facilitate geometric tolerancing.

Dimensions and tolerances created in the parts can be directly added and manipulated on drawing sheets. Having created a schema, the wizard based TolAnalyst available in SolidWorks Office Premium can be used to perform RSS worst-case tolerance stack analysis with an indication of the greatest contributors to allow rapid iteration of schema. Admittedly worst case analysis is limited but hopefully this functionality indicates a drive towards more sophisticated statistical analysis and support for a wider range of manufacturing processes in future.

Similarly the DFMXpress functionality identifies features that are likely to be difficult, expensive or even impossible to machine.

Enhancements in the drawing environment

The drawing environment has its own share of enhancements. Drawing sheets can finally be copied like tabs in Excel and pictures can be inserted into drawing sheets. Section view functionality is improved with the ability to exclude ribs and to lock break lines in place using dimensions that do not appear on the final printed drawing. Notes can include associative balloons, bent leader lines can be manually edited and, to aid formatting, text can be compressed to fit in a table cell or note. The BOM is significantly improved with the ability to edit data such as descriptions in the table to associatively update in the part properties and to be able to drag and drop rows to the required order. It can also indicate virtual parts such as grease or paint in the listing.

eDrawings continues to mature with the addition of support for Pro/E parts and assemblies, albeit with some limitations, and STL files. Pro/E data import now includes translation of constraints into assembly mates as well as features. Integration with Adobe Illustrator and Photoshop has been improved with import and export support for .ai and .psd file types. Continuing the theme of re-using design data, 3D content central the online parts catalogue is configurable within SolidWorks, has a new interface and is said to contain 50% more content.

SolidWorks’ long term drive to increase wider use of FEA is supported by further load, restraint and contact condition support in the Analysis Advisor tool including an improved workflow and database of examples. A number of new study types and the ability to mix beam, shell and solid meshes have also been added for more advanced analysis. A Design Insight plot indicates the regions of the model that best carry the loads to help rapidly optimise material reduction. Usefully, existing studies can be conveniently renamed.

Although MoldflowXpress is no longer included in the module bundles, an introductory CFD module CosmosFloXpress allows studies using single inlet and outlet to be created, reporting pressure and velocity effects in dynamic section and surface plots. All of the motion related tools have been integrated into a single timeline environment combining assembly motion, physical simulation and physics based CosmosMotion available in the Premium version. This enables the rationalised mates to be used consistently. Since the release of the 2008 product, SolidWorks has also announced the acquisition of the CircuitWorks add-in that is being made available free to all Office premium licensees. This provides a bi-directional IDF and PADS file interface allowing integration of PCB and mechanical design.

The key challenge for users? Keeping up to date

In an increasingly mature mechanical and industrial design CAD market, SolidWorks is still finding opportunities for innovation. Indeed, whilst remaining mindful of the need to avoid alienating existing users, much of the passion from executives at SolidWorks World 2008 in San Diego centred around opportunities likely to be presented by emerging technologies. In the meantime, focus on the design in hand rather than the CAD tool, re-use of data and improving designs has yielded plenty of enhancements. The key challenge for users is to keep up to date with the increasing range of functionality. If you want to know how you’re doing, try for Certified Professional accreditation which is now more cost effective and accessible via the SolidWorks web site then ever before.