Parts, Solid Edge, Synchronous Technology, Tips

Back in the late 90’s Rick Mason was the guru when it came to Solid Edge and I was recently asked for Rick’s guidelines for robust modelling practice and thought it still useful and relevant to those users using feature based modelling (included below). This does also highlight to me the advances that Siemens have brought to Solid Edge with the introduction of Synchronous Technology. How much time is wasted in doing all this pre-planning when modelling in ordered mode and ensuring that the model is robust? This is a quote from a recently released ebook by Siemens which sums it up nicely:

You may have become numb to the pain of history – The shortcomings of history-based methods are often overlooked because history-based modeling has been considered the only seriously viable method for decades. But synchronous technology has strengths where history-based modeling has weaknesses, so these methods can and should be used together to make the most robust models possible. We are not proposing that you should entirely abandon history-based modeling and only model synchronously. We generally like the idea of using synchronous and history for their respective strengths, using them together as appropriate. This allows you to avoid the weaknesses of both History and synchronous. Combining modes greatly simplifies the parent/child tangle that can result from inter-associativity between straight history-based parts, especially when designing in-context parts in assemblies. Using these technologies together is really where the biggest value lies. Anyone who has used 3D CAD in the last couple of decades has dealt with the workarounds and frustrations of history-based modeling. For example, editing features that you made early on in the process causes features that you made at the end to disappear as they are rolled back and then recompute when the edit is complete. This is made necessary by the linear nature of the history tree, but from a design point of view makes no sense, and simply wastes time. We have all used history-based CAD for so long we just accept its shortcomings without question. 


It is also interesting to see that Rick talks about “Design Intent” in his rules which has now become the cornerstone of Synchronous Technology!

Rick’s Rules for Robustness in Solid Edge

November 1998

RULE #1: PLAN your work! Remember we are modeling, not “drawing”. Spend a few minutes with a sketch-pad and pencil to:

a) Identify important datums which should be tied to Reference Planes
(these include locating / mating faces, common centrelines, extents of non-
orthogonal features etc.) Placing the major axes of the Part and/or its primary
locating feature onto the base Reference Planes makes for not only a well-
constructed Part, but more robust Assemblies downstream.

b) Imagine the basic set of features which define the part-structure. Is the
part best represented initially by a rotated, linear, lofted or swept protrusion?
Should it be modeled as a piece of bar-stock then material removed as it will be
in the toolroom? If the part is a moulding, casting or forging, does it require a 2-
step process to allow for trimming/cleanup/machining to be defined? Is it one of
a Family of Parts, or of a Handed Pair? This analysis is difficult for a beginning
user of Solid Edge, but it is an essential part of robust technique.

c) Identify common or linked features (eg aligned cutouts) which can be
linked to initial sketch geometry to control their placement without risk of a failed
feature compromising the model. Sketch geometry is a valuable tool in building
robust models and is also a useful way of incorporating 2D reference geometry.

Try to visualise the approximate order in which the model will be built – this will
become easier with experience and experimentation. It is desirable to keep
features as independent of each other as possible, whilst keeping the required
relationships between features – this may seem antithetical at first, but read on!

RULE #2: Build on good foundations. Global (Primary) Reference planes are your most trusted ally – they are:

a) Indestructible and immovable (but can be conveniently re-sized
before commencing your model).

b) The most reliable foundation on which to build your model.

c) The most reliable features when placing part-models into assemblies.

RULE #3: Anticipate! Designers change their minds, stock shapes get discontinued, mating components alter, stresses change etc. Make allowance for:

a) Dimensional changes in your parts. Use driving dimensions to ‘test’
that profiles behave predictably when re-sized. Develop techniques which give
maximum flexibility, controlability and reliability in your models.

b) Changes in configuration – If the locating-face changes from front to
back of the part, does it mean 2 minutes or 2 hours to incorporate the change?
With planning and a little experience, you’ll be able to say “Yeah, no problem”
instead of “You wanna do WHAT????”

c) The ‘Back Burner’ syndrome – don’t use such confusing techniques that
when the job’s back on the boil after 6 months delay, you can’t understand what
the heck you had done so far.

RULE #4: Keep features independent of each other as far as possible. Solid Edge has a host of tools which allow us to build complex models in various different ways – some are inherently robust, some not. Try to follow these guidelines:

a) Use primary reference-planes for feature profiles and to attach driving
dimensions at every opportunity. You’ll be surprised how often this is, in fact,
possible once you start to practice. AVOID using ‘consumable’ faces, edges etc.
for profile-planes or dimension attachment. Once you start to re-order features,
the only guaranteed datums are the three primary reference-planes.

b) Practice re-ordering features and using the ‘go to’ function in Pathfinder.
(you ARE using Pathfinder, aren’t you?) See what breaks and what hangs
together when you alter the sequence of your model. Avoid deeply-nested
groups of features which ‘lock’ you into a set, inflexible path. If a feature cannot
be re-ordered (UPWARD is the only option, by the way) then it has down-line
dependencies which prevent this, or there are no ‘break-points’ in the model
above that feature, into which it can be re-located. To bring a feature DOWN
the tree, it may be necessary to cut-and-paste its Profile (using a Draft file as
a buffer) and delete & re-create the feature. Be careful that the robustness of
the Part is not compromised by these changes.

c) Use open profiles to avoid unnecessary interdependence of features.
For example, a boss modeled as a rotated protrusion does not need the open
ends of the profile to be related to the parent model – the boss will always meet
the parent body, so why introduce unnecessary complications? If the boss’s
Profile is sketched on a base Reference Plane and dimensioned to the other
2 plane-edges, it becomes completely independent of the parent and therefore
extremely ‘robust’.

d) Create a secondary reference plane – either global or feature-specific
(local) – from which to project back onto the parent solid rather than picking a
face on the parent body from which to create a feature profile. This technique
gives the maximum flexibility and independence of features, and eliminates the
possibility of features or relationships failing because the ‘supporting’ face has
been either altered or removed.

e) Avoid reliance on included edges where there is a likelihood that the
parent feature will be significantly altered, re-ordered etc. Sketches offer a
MUCH more robust method of controlling linked features or shared geometry.

RULE #5: Learn which are the most robust relationship types. Sadly, not all relationships are created equal (pun intended!). Symmetric relationships are probably the most ‘fragile’ and easily broken, whereas ‘connect’ and ‘align’ relationships are nearly bullet-proof. Where symmetry is required, it may be preferable to use equality / alignment relationships or else Construction elements in lieu of the actual symmetry function. In case you haven’t yet discovered Construction Elements, they are ordinary profile entities which are ‘toggled’ as Construction elements which withdraws them from the Profile but leaves them as ‘scaffolding’. Take the case of a rectangular pattern of holes placed as a User Defined Pattern, where the centre-point of the pattern must be controlled by a driving dimension. A line can be drawn between diagonally- opposite hole centres, then the Driving Dimension applied to the mid-point of this Construction line (lines & arcs drawn whilst in the Hole Step are automatically identified as Construction Elements although they initially display as solid not chained).

For any given profile, there may be many different ways of applying relationships (and in different order) which achieve the same end result, but some will be more robust than others. Most of us have had the experience of a Profile turning itself ‘inside out’ or going feral – often it is simply the ORDER of construction or of applying relationships which determines how robust the construction will be. It is good practice to try several different configurations for a profile (by varying the value of Driving Dimensions etc.) to verify that the geometry behaves as you expect. There’s always the ‘Undo’ icon ……

RULE #6: Utilise the power of Open Profiles. Solid Edge has an extraordinary ability to interpret Open Profiles. As long as the ‘projected’ envelope properly intersects the parent solid, open profiles can be used for Ribs, Bosses, Webs, Gussets, Fins, Cutouts, Section cuts, Grooves, Notches …… and in many cases, smart selection of both the Profile Plane and orientation will result in the Open Profiled feature being completely independent of the topography of the parent solid. This means that the feature will regenerate successfully even if significant changes are made to the parent – a great ‘robustness’ attribute.

Unfortunately, Open Profiles cannot be used for swept or lofted features as far as I am aware.

RULE #7: Use Feature Pathfinder to advantage. Solid Edge’s Feature Pathfinder has a few tricks up its sleeve which even experienced users sometimes overlook. The Playback feature functions like a VCR, allowing you to ‘replay’ the construction of the model. Features can be renamed to have more meaningful descriptions (a great habit to get into!) so that “UserDefinedPattern_23″ becomes something like “Attch_Holes_M8″ for example. This is particularly useful when interpreting someone else’s work or in the case of the dreaded ‘Back Burner Syndrome’ where a job suddenly gets resurrected after weeks or months of delay.

Individual features, planes, sketches & surfaces can be selected with the RMB (Right Mouse Button) to show/hide them, suppress/un-suppress, edit/change dimensions etc. (Try RMB with the cursor in the graphics screen, toolbars, over highlighted entities, etc. etc …….)

When selecting a feature from the graphics screen is difficult, it can be selected with precision from Pathfinder. Re-ordering of features and insertion of features in the tree can also be done from Pathfinder, both of which are vitally important tools in a robust model. Single-stepping through the construction of a part in Playback mode is a tool I use often while reviewing other peoples’ work. Often while I’m doing this I learn something new from another user’s approach to their task.

RULE #8: Apply dimensions with care. Well-applied Driving Dimensions make for a robust model. Indiscriminately applied dimensions or dimensions applied using the wrong Mode or settings can lead to disaster. When dimensioning the profile of a rotated protrusion or cutout, find and use the Diametral dimension; when dimensioning to small elements, zoom to ensure the correct attachment-point. Understand the difference between Horizontal/Vertical, 2-Points and Axis-Aligned dimensions. Remember always when placing Driving Dimensions that the base Reference Planes are the ONLY indestructible features in your part – attach dimensions to them whenever possible.

Learn ALL the functions of the Smart Dimension tool – it is surprisingly powerful, yet many users have never investigated its options on the Ribbon Bar. Don’t think that because you have used Driving Dimensions to fully control a Profile, non-driving dimensions have no place: they are often useful as reference or as checking dimensions, to save having to perform a calculation etc.

RULE #9: Capture as much DESIGN INTENT as possible in your Part. Get into some good habits when commencing a Solid Edge part. As soon as you rename the part to save it, open the File Properties notebook and fill in the relevant details. I have my Normal.par file saved with Prompts in the Properties fields, so users have a guide as to what information should be entered. Don’t overlook the Comments field as a handy note-pad for ‘To Do’ items, checking notes etc.

While applying dimensions in the Profile Step, use all the facilities at your disposal to add tolerances, prefixes / suffixes etc. to your dimensions. This is even handy for noting changes or comments (eg add dimension suffix “was 22.873mm” or “must not exceed 37.4° ” etc.) – just a little bit of extra information can avoid costly errors or time-wasting misunderstandings. The Dimension Type icon is active in the Profile Step as well as in Draft, remember – you can place Toleranced, Reference, Basic, Inspectable etc. dimensions on a Profile sketch (but NEVER out-of-scale!).

RULE #10: Be adventurous. Solid Edge has more features and options than any single User can possibly commit to memory. Investigate the function of infrequently-used Icons, Menu options etc. Leave “Tip of the Day” turned on – often it provides a little memory-jog about a forgotten function or workflow (and Dental Hygiene). Compare notes with colleagues, or (better yet) TEACH Solid Edge to a colleague, student or friend – it doesn’t matter that you are an inexperienced User, you will become a better user (and gain some valuable insights) by helping someone else discover the power of Solid Edge, and by practising Robust techniques. Use ALL the available Tools (and this includes the excellent context-sensitive Help found
in Solid Edge) to add the highest possible value to your Part Models – it’s the way ‘professionals’ work!

Prepared by: R.H. (Rick) Mason
MASCO Design Services Pty. Ltd.
Solid Edge Support (Australia)
Sydney, Australia.

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