Groundhog Day All Over Again.2 (Part 1)

The Pros and Cons of different approaches to duplicate NX11 model shapes.

 

Overview

Having witnessed the culmination of today’s CAD modeling philosophies and trends as they came to be over the last 20 or so years, there’s a primitive theme: reduce duplicative effort and take advantage of the reuse of data whenever possible. In an effort to increase productivity by eliminating the non-productive and making efficient the inefficient, CAD users now have the ability literally drag and drop into today’s task what was created just hours before or years before. This extension of the concept of duplication carries over what was first started in the earliest of CAD systems and across the board, from AutoCAD patterns to the Move/Copy and Copy/Paste commands from the wireframe modeling days of the last millennium.

screen-shot-2016-10-27-at-3-23-24-pm

An HO train layout plan “modeled” in Unigraphics V9 wireframe, opened directly into NX11

 

Wow, when you say it like that, it sounds so archaic! But the best concepts are eternal truths.

When parametric feature based modeling in NX started in the 80’s (Unigraphics) the goal was to capture and preserve design intent through expressions and associativity, which presented the user tremendous improvements in reducing the effort to make design changes. In addition, it also took advantage of a computer’s innate nature to calculate and reference errorlessly, virtually eliminating mistakes.

One of the things that has not changed, however, is still the greatest challenge in CAD modeling – how to plan the construction of the model to comply with design intent in a productive, efficient approach that follows some fundamental rules:

  • Keep it simple whenever possible
  • Use a faster approach but not necessarily the fastest.
  • Capture the Design Intent that best returns the investment of time.
  • Plan for possible/inevitable changes – fast, easy, and accurate.
  • Adhere to mono-detail part philosophy!

One of the more common comments about the available functionality in NX is always: “There are six different ways to do anything!”  So it is with duplicating shapes. This “PART 1” installment addresses those modeling tasks that involve multiple instances of shape, in other words, duplication of features and objects.

When duplication is required, which approaches impact performance the least?

  • Copy/Paste options? Pattern options? Are there other options?
  • Duplicate features &/or Sketches vs geometry: curves, faces, & bodies?
  • One large pattern or multiple small patterns?
  • Can repetitive tool geometry be used efficiently?

 

With those questions in mind, lets explore the many methods of duplicating shapes in NX11

  • Pattern Feature
  • Pattern Face
  • Pattern Geometry – bodies, faces
  • Pattern Curve (Sketch command)
  • Copy/Paste Face
  • Copy/Paste Feature
  • Move/Copy Object
  • UDF

NX11 Modeling Methods that Duplicate Shapes

 

Pattern Feature

  • Perhaps the most popular of all methods.
  • Creates multiple instances of one or more features.
  • A variety of layout patterns many of which appear in other duplicating commands including Sketch and Assembly functionality.
  • Can repetitive tool geometry be used efficiently?

screen-shot-2016-10-27-at-3-59-38-pm

 

 

 

 

screen-shot-2016-10-27-at-4-01-50-pm

Controls orientation of the features.
                                                                                                                 Methods:screen-shot-2016-10-27-at-4-17-42-pm
Simple:
    • Simple design features, such as holes and extruded features are supported
    • One input feature pre output pattern.
  • When to Use:
    • When you need to accomplish unique patterns (along path, staggered, fill, circular, suppressed instances, etc. but nor Linear or Circular).
    • Limited number of instances required
screen-shot-2016-10-27-at-4-02-29-pm

Controls 1 or 2 linear pattern directions (#2 can be any vector) and symmetry, including staggering rows/columns.

 

screen-shot-2016-10-27-at-4-26-46-pm

Variational:
    • All features which support Copy/Past feature are supported.
    • Detail features such as Blend and Draft are supported
    • Works with multiple input features
    • Advanced Hole functions are supported.
    • Sketches are supported.
  • TIP:
    • If Possible, Keep it Simple.

 

Pattern Face

  • Copies a set of selected faces in linear (1 or 2 directions), Circular, or Mirrored modes.
  • Result is a single feature.
  • Select:
    • Insert-> Associative Copy-> Pattern Face… or
    • Insert-> Synchronous Modeling-> Reuse-> Pattern Face
When to Use:
  • When considering a rectangular or circular pattern that is comprised of several features that do not require variation of individual instances.
screen-shot-2016-10-28-at-9-38-53-am

TIP:
  • Rectangular direction vectors do not need to be perpendicular from each other.

 

Pattern Geometry

  • Allows you to create multiple instances of geometry and Datums.
  • Can create instances of
    • Bodies
    • Faces
    • Edges
    • Curves
    • Points
    • Datums
  • Result is a single feature comprised of 1 or more objects.
  • Face/Body geometry is independent of original, thus you may need to sew, trim, of Boolean resulting faces or bodies.
  • A variety of Instance Types:
    • From/To – Creates instances from one point/CSYS to another.
    • Mirror – Mirrors geometry about a plane.
    • Translate – Creates instances at a specified direction and distance.
    • Rotate – Creates instances around a specified axis (allows for an offset distance to achieve helical placement).
    • Along Path – Creates instances along a curve/edge (allows rotational offset angle to each instance).
When to Use:
  • When you require instances of geometry other than features and faces.
screen-shot-2016-10-28-at-9-56-13-am

 

 

 

 

 

 

 

 

TIP:
  • Good for extending other patterns of model geometry.

 

Pattern Curve

  • Allows you t0 create a pattern of Sketch Curves with in the sketch.
  • There are three layout patterns:

screen-shot-2016-10-28-at-10-01-12-am

  • No “pattern” feature is created but there is an option to create pitch expressions.

screen-shot-2016-10-28-at-10-02-32-am

  • When there are “many” curves and a Sketch becomes a “Large Sketch”, NX11 prompts the user for options to increase performance:

screen-shot-2016-10-28-at-10-04-35-am

When to Use:
  • When building a 2D profile of a design feature that requires unique patterned shapes/sections.
  • When you require point patterns for Holes (much harder using just the Hole feature).
  • When a unique pattern needs to be projected/wrapped onto face.

 

 

Copy/Paste Face

  • Copies 1 or more faces.
  • Can both copy and paste in one action.
  • Common Motion options including None, which copies to a feature for future usage.

screen-shot-2016-10-28-at-10-09-26-am

  • Once copied, Paste [Face] can be used to add sheet bodies onto solids similar to Patch/Patch Body.
When to Use:
  • When duplicate features are needed at non-repetitive locations and/or orientations.
  • When building sheet body models or a sold body comprised of individual sheet bodies – faces ca easily be duplicated, then trimmed, sewn, patched, etc.
  • Possibly used in combination with Pattern Feature after a Copy Face feature is created.

 

 

Copy/Paste Feature

  • Copies features and/or objects to Windows/OS clipboard.
  • Can paste into same or different part file.
  • Paste create new features. If originals contained expressions, options are:
    • Create New
    • Link to Original
    • Reuse Original

screen-shot-2016-10-28-at-10-09-26-am

  • Paste Special creates new objects with options for:
    • WCS or specified CSYS
    • Work, Original, or as Specified Layer
  • Paste only one at a time but can use Apply to repeat Paste quickly
  • When pasting features with expressions, Expressions Mapping is only available with “Select Parents” Datum References option.
  • Reference resolution has 4 options:
    • Unresolved – The reference is currently not resolved
    • Resolved by user – The reference is resolved by a user selection.
    • Resolved by inference – The reference resolved by the software inferring the required geometry.
    • Resolved by copying geometry – The reference is resolved by the software copying the original parent geometry.
  • You do not always have to resolve every reference to paste copied feature.
When to Use:
  • When duplicate features are needed at non-repetitive locations/orientations.
  • When only a few features are being copied or when only a few copies are needed.
  • When all parent/child feature need to be selected – automatically selection is available.

screen-shot-2016-10-28-at-10-37-02-am

 

 

Move/Copy Object

  • You can use the Copy option in the Move Object dialog to duplicate objects.
  • Because object are copied, not features, standalone features (bodies) need to be copied before Boolean operations.
  • Motion types include standard options:

screen-shot-2016-10-28-at-10-39-36-am

  • NO associativity option – results in “dumb” features.
  • Does not accommodate Boolean options – must be added as additional features afterwards.
When to Use:
  • When associativity (automatic update of changes to a model) is not a requirement.
  • Before Boolean operation is executed:
    • Create base solid
    • Create solid feature to be copied
    • Copy the solid(s)
    • Create Boolean with base solid as Target and select all copied solids as Tools, by using rectangle selection.

 

 

User Defined Feature (UDF)

  • Legacy function, now enriched as part of Reuse Library resources, drag and drop option.

screen-shot-2016-10-28-at-10-45-08-am

  • Can be created from any model and can contain more than one feature (solid, sheet, sketch [associative] explicit curve, Datums, etc.)
  • Creates hidden “.udf” file that contains reuse data.
  • Must be created/saved into a library which must be configured correctly.
  • Part file containing a UDF is independent (not linked) from source .prt/.udf files but can be used by any user in any NX part file.
When to Use:
  • When desired shape needs to be added to many more individual parts ion the future.
  • When a sold/sheet with multiple features need to be added as one “feature”
  • When unique iterations of the shape are needed for each application.
  • Different sizes, diameters, angles, lengths, thickness, etc.
  • Different locations/orientations/normal direction.
  • Options to include/exclude sub-features of the shape such as Chamfers, Blends, Holes, Boolean targets, etc.
  • Should be managed/organized with standard procedures to avoid duplication and abuse.

 

Summary

So those are the more rational options to duplicate existing geometry in NX11. There are still other possibilities but none that we would suggest using without some additional enhancement such as contained within a script, NX Open routine, or other programming option and certainly not without specific standard procedures in place.

Recommended for duplicating model shapes in NX11:

  • Pattern Feature
  • Pattern Face
  • Pattern Geometry – bodies, faces
  • Pattern Curve (Sketch command)
  • Copy/Paste Face
  • Copy/Paste Feature
  • Move/Copy Object
  • UDF

So which is best for you?

Obviously not a question that we can answer. However, if you catch the next installment of this blog, PART 2, we will provide specific, statistical analysis of each of these approaches, including time of update, total memory comparison, and more! That should give you some obvious and consoling direction to increase that productivity and regain the efficiency in your NX modeling efforts!

Hey, haven’t we been here before?

 

 


garrett_150Garrett Koch | PLM Application Engineer, Swoosh Technologies

Well-accomplished in drafting, design, and engineering in many industries since 1973, Garrett has been developing patentable designs and has taken on large-scale engineering projects. In 1994, he embarked on a different career in CAD training, courseware development, and technical support – where he focused on teaching a variety of students (including PhD’s from MIT, project engineers at Los Alamos National Labs, officers at NASA, and users across the continent at major manufacturers of aerospace, automotive, and power generation). Garrett excels at the knowledge transfer of NX mechanical CAD and Teamcenter and is considered an expert in NX installation, configuration, and technical support.

Want to learn more about NX? Contact us at 314-549-8110 or use the contact form to get in touch!

Leave a Reply