Establishment of Best Practices for Large NX Models and Drawings TU-EPM-12-017 Instructor: Kevin Thompson
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Purpose and Overview 1. The purpose of this presentation is to formally establish the “Best Practices for Large NX Models and Drawings” 2. Creation and update of large assembly drawings is computationally expensive a)
Particularly, hidden line renderings of views 1) Requires all relevant components to be loaded into the session 2) Also demands significant memory and processor resources for hidden line calculation
3. UG/ NX provides many options for making the process more efficient a)
Reduce the amount of data that typically needs to be loaded to create or annotate a drawing and its views 2
Master Model Strategy B/E Required 1. Drawings are separate files from models and assemblies a) Instead of creating the drawing in the assembly itself, create a non-master in Teamcenter that references the UG-Master
2. Promotes concurrent engineering by enabling a user to modify the drawing without locking the UG-Master a) Drafting and modeling changes can happen in parallel
3. Separates annotation data from the UG-Master a) A user can load the master assembly without needing to load the drawing data into the session, improving load times and reducing memory usage 3
Reference Sets B/E Recommended
1. A named collection of objects that you can reference from another part or sub-assembly. a)
Can drastically reduce, or even eliminate, the graphical representation of portions of the assembly without modifying the actual assembly structure or underlying geometric models
2. There are two primary reasons to use Reference Sets: a) b)
Filter unwanted objects in a component part so that they do not appear in the assembly. Represent a component part in the assembly with alternative or simpler geometry than the complete solid body (NOT B/E Recommended)
3. There are two types of Reference Sets: a) b)
Automatic Reference Sets that are managed by NX User-defined Reference Sets 4
Reference Sets (cont.) 1. A well-managed Reference Set strategy can lead to: a) Faster load times b) Reduced memory usage c) Less cluttered graphics displays
2. This command is located at Format→Reference Sets within UG a) Use Reference Set commands and options to control the display of a component or subassembly part in higher level assemblies b) Reference Sets are a named collection of objects in a piece part or subassembly 5
Lightweight Loading B/E Recommended 1. Can load an assembly with Lightweight or Exact representations a) Using lightweight representations saves on memory usage, and improves load and display performance b) Switch between Show Exact and Show Lightweight commands on selected components manually by using MB3 on component in Assembly Navigator
2. Use the Use Lightweight Representations load option to specify which representation appears when components are loaded a) Select the Use Partial Loading assembly load option to fully realize the performance and memory benefits 6
Lightweight Loading (cont.) 1. Can load any reference set lightweight, as long as lightweight representations exist for the contents of the reference set a) Use the Automatic Lightweight Generation customer default to control whether UG maintains lightweight representations for all bodies or just those belonging to certain reference sets
2. Can select lightweight geometry such as faces, edges, and vertices for NX commands when Load Smart Lightweight Data customer default is active a)
This is known as seamless lightweight loading; allows interaction with lightweight representations as if they were solid bodies
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Representations B/E Tucson Recommended 1. Describes how to create alternate representations: Faceted bodies associated with the solid face or body from which they are derived. a) Can set customer defaults to automatically create lightweight representations as specified through control tolerance parameters such as the number of facet edges, distance tolerance, angle tolerance, convex facets, and the number of facets. b) Can also create manual representations with the Assemblies →Advanced→Representations command 8
Representations (cont.) 2. Use the Representations command to manually create a lightweight representation a) Faceted bodies are often used as a lightweight alternative, and can significantly improve performance
3. Faceted bodies are stored in the current work part when you create them a) Can create representations of bodies directly in the part that owns the body, or in an assembly that contains components with solid or sheet bodies
4. Particularly useful for visualization or use with Clearance Analysis a) Faceted representations can be used for shading or designate for partial shading or translucency as well 9
Linked Exterior B/E Recommended 1. Extracts the exterior faces of an assembly into a LINKED_EXTERIOR feature a) b)
c)
Can extract all faces or a selection of them Edit your selection of faces before extracting them. This command is on the Assemblies →Advanced menu Gives an appearance virtually indistinguishable from the original
2. Adjacent faces from the same body are joined into a single body that is similar to a linked region a) b) c)
Adjacent faces from different bodies are not joined NX does not attempt to sew separate regions into a single body, because the faces may be disjoint or may meet at a "T", making sewing impossible. A face that is partially interior and partially exterior is not split. 10
Component Groups B/E Recommended 1. Lets you conditionally apply actions to all or part of the assembly structure from the Assembly Navigator through selection of logical subsets of assemblies a) b) c)
2.
Primarily used for loading and unloading operations, but many hundreds of other operations are conceivable. Examples of component groups: Components larger than a certain size, those in a certain region, those that share a certain property (e.g. matching a certain attribute), or simply those named X, Y, and Z. Dynamically evaluated, and can also be combined for powerful logical results. Large assemblies depend on component groups to efficiently navigate through large amounts of data
To see the component group section of the Assembly Navigator, it must be turned on in the Assembly Navigator toolbar by selecting the Show Component Groups button:
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Component Groups (cont.) 1.
Can save component groups in the part or for just the current session.
2.
Advantages of session component groups are write access to assembly not needed, creation of as many temp component groups as you want without fear of cluttering the main assembly a)
3.
Can save these session component groups in bookmarks.
Owner of large assemblies should create a set of generally useful component groups to be saved with file, such as: a) b) c) d)
Major and minor functional areas; for example, all electrical components Zones or plane-based component groups; for example, through a particular section of an aircraft Size based component groups; for example, smaller than ¼ inch Attribute or name-based component groups; for example, all those matching TYPE = FASTENER 12
Component Groups – Favorite Methods By Name – Due to common naming conventions, it is relatively easy to pick certain types of files and put them in a component group
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Component Groups – Favorite Methods By Attribute – Since B/E has standards for file and part attributes, they are also easy to use
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Component Groups – Favorite Methods By State – While this can be a bit of work, it allows maximum flexibility in only loading the components of interest; two common preferences: 1. Loaded Components – allows you to take advantage of the filtering you have already done to load you what you want into memory 2. Visible Components – allows you to create a group out of the Components currently shown
1 2
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Component Groups – Basic use File Options Load Options Change to “Specify Component Group”
Select the “Component Group” of interest from the List and click OK
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Reducing Complex Assembly Displays B/E Recommended 1. Wireframe vs. Shaded a)
2.
Simplified Solids a)
3.
When adding a component or sub-assembly to a model, you must pick a pre-existing Reference Set to specify amount of data you wish to see. If you pick EMPTY, you will add a link to the component or sub-assembly without any graphical information. NOTE: If the creator of the component or sub-assembly created a “lighter weight” Reference Set, you can use it if appropriate
Hide a)
5.
Level of detail is always going to affect complexity of the display. Important for memory usage and display purposes to keep things as simple as possible
Reference Sets a)
4.
Wireframe is lighter weight even if it is more difficult to see what you want. Not really an issue when opening a file, but becomes a problem when you zoom or rotate a part / assembly
Although this works for temporarily reducing the complexity of the display, it is against BE standards to save a file with things hidden / blanked
Suppressing Features and Components a)
Although this works for temporarily reducing the complexity of the display, it is against BE standards to save a file with things suppressed 17
Open By Proximity B/E Recommended 1. Lets you open a small set of components in the vicinity of the selected component(s) a)
Can identify the components to be opened by several factors, such as distance from the selected components and size.
2. Especially good for the following: a) b) c)
Loading components in a region of interest to limit graphic and memory overloading Limiting solids to a region of interest when doing a clearance analysis Limiting display clutter to enable easier creation of mating conditions and WAVE interpart links
3. Where do I find it? a) b)
Click Open by Proximity on the Assemblies toolbar Select Assemblies → Context Control → Open by Proximity
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The next section of slides contain recommendations, not B/E requirements
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Recommendations – Load Scope All Recommendations are preferred but not mandatory
1.
Fully Loaded a) b)
2.
All of the data in the file is loaded into memory Use with small assemblies or with a subset of large assembly component to edit or create links to parametric data.
Partially Loaded a) b) c)
3.
Enough data is brought into memory to display the part; Parametric data is not loaded into memory Use to open large assemblies faster than when you use Fully Loaded and to conserve computer memory for those components that you are going to modify Can fully open partially loaded components at any time if you want to edit their data
Structure Only a)
b)
Assembly components are not loaded into memory at all. The assembly has information about the position and the bounding box size of the unloaded part(s) Use to manage very large assemblies, for which you can manipulate only a relatively small amount of data at any one time. Fully or partially load only those components of immediate interest, and leave the rest unloaded
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Recommendations – Saving 1. When doing a “Save As” on a large assembly, open it in NX with Load Options set to “Structure Only”. a) This will keep local memory use at a minimum and focus on the assembly structure first
2. File Size a) The following operations add additional weight and overhead to a file and should be avoided: 1) Changing component color, translucency or partial shading of components 2) Editing a portion of a drawing view with “View Dependant Edit” 3) Creating drawings inside of part or assembly files. (The use of “Master Model” has been mandated by BE for this reason.)
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Recommendations – Interface Options 1. Fixed Frame Rate a)
You can greatly improve the effectiveness of zoom, pan, and rotate by selecting the Preferences Visualization Performance Large Model tab Fixed Frame Rate check box. Objects can be automatically hidden, or shown as simple boxes, during view manipulations to provide fast and maintain smooth view transitions
2. Preselect a)
Set this to a high time interval or even turn it off so that you don’t inadvertently pick a large subassembly and have to wait a long time to move on.
3. Work Part Emphasis a)
When working in context of large assemblies (making a component the work part), the display overhead increases when NX “grays-out” the non-work parts. You can avoid this by clearing the Preferences Assemblies Emphasize check box. 22
Recommendations – Drafting 1.
Faceted Representation Views a) b) c)
d)
Provide a high performance, memory efficient way of generating hidden line views on a drawing Hidden line rendering is stored in the drawing part and can be viewed without needing to load the assembly components Functional limitations and procedures required for dimensioning mean that faceted representations are not appropriate for many drawings. However, when functional limitations are not a problem, faceted representations provide the fastest and most memory efficient way of adding a view to a drawing Not essential that all components be loaded using a faceted representation. Unigraphics NX can create faceted data on the fly for the hidden line calculation. However it is more efficient if the components are loaded as faceted representations. 23
Recommendations – Drafting (cont.) 1. Setting up faceted representation views – The following procedure is the most efficient way to create a faceted representation view on an assembly drawing: a) b)
c) d) e)
Open drawing part with no components loaded Toggle on “Use Lightweight Representations” and “partial loading” in the Assembly Load Options and set the default reference set to “Model” to minimize what is displayed in the drawing view Use the Assembly Navigator or component filters to open only the components needed for the view Start Drafting and create your drawing Add your view. When adding your view, click on the Right Mouse Button and select Style. On the Base tab, toggle on Faceted Representation
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Recommendations – Drafting (cont.) 1.
Perform your normal View Cosmatizing: a) b)
2.
Having done this, follow this process to re-open and annotate the drawing if you are required to close the file. i.e. For the end of day. a) b)
3.
Use Hide Components to hide all unloaded components in every view so that they are not included in future drawing updates or use layer masks Save and Close the part
Open the drawing with no components loaded using File Options Load Options Structure Only Under Preferences Drafting View, toggle on “On Faceted View Selection” and “On Faceted View Update” in the Load Component section.
Limitations – Faceted representation views are only suitable for certain types of drawings due to some functional limitations. a)
For Example: 1) 2)
A section view cannot be a faced representation view, although its parent view can be. View display settings do not apply (e.g. the ability to generate virtual intersections or show hidden lines is dashed font.) 25
Recommendations – Preferences Preferences Drafting General Drawing Workflows should all be toggled OFF Preferences Drafting Preview Style should be set to Border
Preferences Selection Rollover Delay should be 3 or more
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Recommendations – Preferences (cont.) 1. Toolbar Options – When placing a view, turn OFF the snap point toolbar. That way only cursor position will be available. 2. Changing the View Display Tolerance – You can change the accuracy to which hidden line renderings are displayed on a per view basis. Loosening the tolerance typically improves performance but can lead to curved edges being less smooth. 27
Recommendations – Preferences (cont.) 1. Removing unneeded component from a view – If some components need to be excluded from specific views in a drawing there are 2 options: a) Assemblies Context Control Hide Component in View 1) Use this method to hide components from a specific view without affecting other views. 2) Especially good for hiding specific parts if you know the part number(s). 3) Also reduces the amount of geometry that needs to be processed in a view update, making drawing performance and later updates faster and more efficient.
b) Format Layer Visible in View 1) Most commonly used when parts are of a “mixed” nature showing various systems on the drawing face. 28
Recommendations – Preferences (cont.) Comparison of View Types in Drawings Standard views
Associative extracted edge views Not BE Recommended
Can be created & rendered without loading solids
No. Solids must be loaded.
No. Solids must be loaded.
Yes. Hidden line can be created from faceted representations.
Existing views be displayed without loading components
No. Must have solids loaded to display hidden line.
Yes.
Yes.
Existing views can be annotated without loading components
No. Solids must be loaded.
Yes.
Yes. System will load some components automatically.
Views can be updated without loading solids
No. Solids must be loaded.
No. Solids must be loaded.
Yes. Views can be updated using faceted representations.
Standard.
Standard.
High.
Hidden line performance & memory efficiency Main advantages
Main disadvantages
Faceted representation views
No functional limitations. No special Ability to view and annotate drawing Fastest and most memory efficient set-up or maintenance required. without needing to load way to add a view to a drawing. components. Ability to view and annotate drawing without loading components. Performance and memory usage. Makes drawing part file larger. Functional limitations make it only Small additional overhead on view applicable to some drawings. update. Requires good reference set management. 29
Recommendations – Preferences (cont.) 1. 2.
Extracted Edges – Do not use per BE standards Simplifying small features– To improve the updating of hidden line renderings in views of large assemblies, you can simplify or omit small unessential features a)
Simplifies or removes the display of small features in a view 1)
A small feature is a set of connected faces which are smaller than a specified size expressed as a percentage of the model 1)
2) 3)
b)
Use the Small Features tolerance slider to set the size percentage between 0,10 and 5 percent of the total model size
Most useful in large scale assembly drawings where it can improve print quality and speed up performance time to update views When a small feature is simplified, its set of faces is replaced by a loop of edges which represents the boundary between the small feature and the model.
Options: 1) 2) 3)
Show All — Displays all hidden lines according to hidden line preference settings Simplify — Displays features that are smaller than the specified tolerance value as a set of simplified boundary edges Hide — Hides features smaller than the specified tolerance value. 30
Recommendations – Preferences (cont.) 1. Delay View Update – a) Major contributor to performance and memory usage issues with large assembly drawings is the amount of resources required to update views, particularly hidden edge renderings b) To suppress view updates: 1) Choose PreferencesDrafting 2) On the View tab, select the Delay View Update check box
c) In most circumstances, this will prevent hidden line recalculations when the assembly changes d) Updates can be initiated explicitly at a convenient time or can be delayed on a per-view basis by leaving the Automatic Update checkbox checked: Preference View General.
2. Cross Hatching – Only cross hatch what is needed. Keep it to a minimum. 31
Recommendations – Special Cases 1.
General Assemblies – Contain all the parts that buildup into a “ship set”. Therefore, these files can get extremely large. a)
2.
Don’t try to open the complete assembly. You probably don’t have enough memory. Use the tools outlined above.
8 Character Assemblies (model used for “family drawing”) – Depending on what the “family” is, this assembly can also get rather large. a)
An optional method for creating 8 character drawings: 1) 2) 3) 4) 5) 6) 7) 8) 9)
Open the appropriate GA with Load Options set to “Structure Only” Completely open the components of interest. Export Parasolid of chosen parts and sub-assemblies, selecting only enough data to generate the required drawing views. Create the 8 character “family collection model”. (UG-Master) Import the Parasolid exported in step 3 above. Save the new 8 character model. Create the drawing for the 8 character (UG-Part) Add UG-Master to the drawing file (UG-Part) Add components (regular method) as necessary for other background material for views, to the drawing file. 32
Product Outline NOT B/E Recommended 1. Lets you define a set of geometry that gives a hint of the overall size and shape of an assembly without having to load components 2. The Define Product Outline command is on the Assemblies →Context Control menu
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Zones NOT B/E Recommended 1. A way of partitioning an assembly into meaningful regions. a) Can be either boxes or planes b) Command is on the Assemblies →Advanced menu c) Use the Zones command to partition an assembly into meaningful regions bounding by boxes or planes d) Zones are: 1) Created in the displayed part with reference to its absolute coordinate system. 2) Named uniquely with upper case letters. 3) Available for use in component groups. 34
Wrap Assembly NOT B/E Recommended 1. Creates a simplified feature from the exterior of an assembly a) Can be useful when you do not need to work with the details of an assembly, but only need an object that is its size and general shape b) Simplifies a complex assembly by computing a solid envelope of planar faces that encloses the assembly c) Command is on the Assemblies →Advanced menu. d) Gives a “shrink-wrapped” appearance
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Scripts NOT B/E Recommended 1. Maps one or more user defined filters to actions a) Options on the Scripts dialog box let you define, rename, or delete scripts b) Command is on the Assemblies →Advanced menu
2. Can be used to build up a simple program to manipulate the assembly 3. Option to create and immediately execute the script, or name and save it for later use a) Script names can be up to 29 upper case characters 36
Scripts (cont.) NOT B/E Recommended
1. Example: Assuming you have a component group called “work_part_proximity” which matches all components within a specified distance of the work part, a script can contain the following commands: a) b) c)
Open (work_part_proximity); Close (work_part_proximity); SetRefSet(“SOLID”) (work_part_proximity);
2. This example loads components near the work part, unloads components that are not near the work part, and sets the reference set to solid, for components near the work part 37
Questions?
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