Fundamental primitives – extrude, revolve, sweep, loft (blend)
Modifying volumes – fillet, chamfer, hole, shell
Replicating geometry – mirror, pattern
Top Down
Don’t get taken in by the hype, be critical
The Creo vs. SW debate has been raging for years with no definite winner, that’s because there is no winner, each package has strengths and weaknesses and it’s unlikely (unless your purchasing for personal use) that any decision will be based solely on the core modelling functionality.
If you understand the fundamentals of CAD it is an easy transition between the two and having skills in multiple packages is always great for your CV. Use these pages to redo your assignments in SW, tell me how you get on.
Here I shall give a brief transition introduction from Creo to SW. Education edition of SW 2013 is installed in LDS003 and LDS011
SW is not my main modelling package so if you see any issues in the text, have a suggestion for a better method or more efficient technique then please tell me.
Reading: Solidworks Surfacing and Complex Shape Modeling, Matt Lombard, Wiley, 2008, ISBN978047025823 – also available as an ebook.
This book may be a bit out of date and may discuss a few modelling issues which have been addressed in the current release but it is still a good text.
Function mapping – SW to Creo
RMB > Setup in the Creo search window to activate SW to Creo function mapping
Fundamentals
Solidworks is a parametric, feature based modeller and is probably the closest in appearance and functionality to Creo amongst the current popular CAD packages.
It has broadly the same construction methodology and toolset in part modelling. The basic work flow is fundamentally the same; choose a plane or planar surface, create a sketch, develop sketch or sketches into 3D volume though the extrude, revolve, sweep or loft (blend) functions.
Protrude, cut or surface
Unlike Creo each of the fundamental tools is split into 3 separate tools, you have to choose the protrude, cut or surface option and you can’t generally (drag a sketch with Instant 3D will change the operation) switch once the feature is created.
Bodies
A body is a single volume in the part model but may be the product of multiple features.
Solidworks blurs the distinction between parts and assemblies by recognising multiple bodies in the part environment and allowing different mass properties to be assigned to each body. It allows a ‘quick and dirty’ assembly to be constructed. Always use a formal assembly structure once past the concept stage.
By default all intersecting volumes are merged to form a single volume or body, if you untick the Merge Result option in the property manager then the volume will be listed as a separate body in the feature manager.
Separate bodies can cause conflicts with some features only recognising the initially selected bodies ie. holes and fillets/chamfers
I get the impression from old posts that the multi-body approach was originally design as SWs approach to a top down design methodology, top down and ‘in context’ modelling seems pretty sorted now so my advice – keep your modelling generic, use assemblies not multi-bodies.
Productivity
Learn your shortcuts and customise the interface, check out the S key and Keyboard shortcuts. Also checkout Mouse Gestures – RMB and drag to select tool.
All these elements can be customised – RMB > Customise on an icon. Always reduce your mouse miles. There is no equivalent to the MMB for OK in SW but if you keep your mouse in place when finishing an operation you can sometimes use the RMB to OK.
Rollback and Flat Tree View
You can drag the Rollback bar at the bottom of the FeatureManager design tree to any point in the build to insert new features. Because this is something we do a lot of in surface modelling this can become messy when dealing with absorbed features ie. a sketch is effectively listed after the extrusion it is used in when it becomes absorbed.
RMB > Tree Display > Flat Tree View to show parent features unabsorbed to allow simpler rollback.
CADCAM Resources 