NX标准件库建模规范-英文版

Table of Contents
Table of Contents (1)
Revision History (2)
Introduction (3)
Model Data Collection: (3)
NX Version: (3)
NX User Defaults (3)
Enforce as Piece Part (4)
Units (4)
Template Part (4)
Part Names (4)
Layers (4)
Reference Sets (5)
Model Base Features-Datum CSYS (5)
Model Feature Attachment (5)
Part Origin and Orientation (5)
Construction Geometry (6)
Feature Names (7)
Sketches (7)
Expressions (7)
Key Parameters (7)
Feature Order (8)
Thread Feature (8)
Materials (10)
Part Attributes (11)
Saved View (13)
Visualization/Background (13)
Preview Image (13)
Weight (14)
Materials Textures (14)
Remembered Mating (14)
Part Families Modeling Procedure (15)
Dialog Image (16)
Quality (18)
Validation Check List (18)
Appendix: Referenced files (19)
Revision History
Introduction
This document explains how the Part Families for the Reuse project are to be modeled. This plan is based on a current NX version 5.0.0.25
Model Data Collection:
Find the part family that you will be modeling from the work list.
Examine the model that exists in the source data to understand the features, parameters and their values.
You will need to have the following information to complete a part:
o Part Family Mast er Name. See document “Naming schema for Reuse content.doc”
o A list of part family members, See template part reuse_teplate_mm.prt
o A part file naming scheme to define part names for all of the Part Family members. See document “Naming schema for Reuse content.doc”
o Design Data for the form of the part, see example part reuse_example_mm.prt o Dimension values for each part family member configuration, see example part reuse_example_mm.prt
o Knowledge of how the part is positioned in practice, see example part reuse_example_mm.prt
NX Version:
Standard parts will be modeled in NX5.0.0.25
The reasons for this are as follows:
The Datum CSYS which became available from NX4 will be used as the base feature of all standard parts.
NX User Defaults
The following user defaults settings must be made before modeling any parts. [Please copy nx5_user.dpv to folder C:\Documents and Settings\your_user_name\Local Settings\Application Data\Unigraphics Solutions\NX5, this file include the default setting for reuse content]
Assemblies -> Site Standards -> True Shape
Cell Size:
Inch: 0.2
Millimeter: 5.0
(Check) Generate Component Shape Representation on Save
Assemblies -> Site Standards -> Reference Sets
Model Reference Set, Name [MODEL]
Lightweight Reference Set, Name [FACET]
Enforce as Piece Part
[It is set in template part reuse_teplate_mm.prt]
File –> Utilities -> Enforced Piece Part
Units
参考标准中的单位
Template Part
All parts will originate from a template part. This is done so that any work that should exist in all part does not need to be repeated. A template part is provided.
Part Names
Part names will be provided in a work list spreadsheet.
To create a new part, save the template as the part to the name of the component you will model. See Naming schema document
Layers
[It is set in template part]
Reference Sets
In NX5 there is a new set of functionality to automatically include the solid body in the MODEL reference set and create a new FACET reference set. When the parts are saved in NX5, two reference sets will be created according to the definition in Customer Defaults. Reference Sets page: MODEL and FACET.
Model Base Features-Datum CSYS
Two Datum CSYS are built into the template model.
The first f eature in the template part is a Datum CSYS named “ORIGIN_CSYS” it is colored Blue. ORIGIN_CSYS is a fixed CSYS that is always located at the absolute WCS. Do not reposition or rotate this CSYS, it must always be in the original position.
The second featu re in the template part is a Datum CSYS named “OFFSET_CSYS” it is colored Green. OFFSET_CSYS is an offset CSYS that is positioned by the expressions by the expressions listed below.
ORIGIN_OFFSET_X
ORIGIN_OFFSET_Y
ORIGIN_OFFSET_Z
ORIGIN_ROTATE_X
ORIGIN_ROTATE_Y
ORIGIN_ROTATE_Z
See example file
Model Feature Attachment
All model features will originate from sketches that are attached to the OFFSET_CSYS. The purpose of this requirement is to enable the position of the part body to be moved parametrically within the part.
Note: The modeling features; Block, Cone, Cylinder, and Sphere may not be used because these features do not attach to datum CSYS.
See example file
Part Origin and Orientation
The origin of the part will be modeled coincident to the origin point of the
OFFSET_CSYS.
All parts will be oriented so that the top of the part is oriented in the +Z direction. For example the top of the head of a screw will face the +Z direction.
The origin of the component is the intersection between the primary revolve axis and the mating face of the part.
As a reference; the proper origin for some common parts is indicated in the image shown below. Notice that the Z Axis is collinear with the Z axis of the OFFSET_CSYS and the origin of the part along the part axis is the contact face of the part.
AXIS_ORIGIN_X
AXIS_ORIGIN_Y
AXIS_ORIGIN_Z
DATUM_ORIGIN_X_Y
DATUM_ORIGIN_X_Z
DATUM_ORIGIN_Y_Z
AXIS_OFFSET_X
AXIS_OFFSET_Y
AXIS_OFFSET_Z
DATUM_OFFSET_X_Y
DATUM_OFFSET_X_Z
DATUM_OFFSET_Y_Z
Construction Geometry
Construction geometry such as datum, sketches, and trim-sheets may be used in creating the model however there may be only one solid body in the part file.
Feature Names
Features will be named; for example, the sketch that is used to extrude the head of a screw would be named HEAD_SKETCH, the extrusion would be named
HEAD_EXTRUDE.
Sketches
Each Sketch will be designed with one profile to make one extrusion or revolve using the “Feature Curves” selection option. Do not use the “Single” or other options to select curves from the sketch. If you must use construction curves in the Sketch, use the “Convert to Reference” operation on those curves in the Sketcher so that those curves will not be included in the “Feature Curves” selection.
Expressions
All expressions will have meaningful names that match the features they define.
There should be no expressions with the original system names such as p1, p2 etc. so that it will be easy to understand and edit a part in the future.
Do not abbreviate words in the expression names.
Expression are written in upper case, with no spaces
Expression names are written with the name of the object being dimensioned first followed by an underscore followed by the name of the dimension. For example the expression that defines the diameter of the head of a screw would be named
HEAD_DIAMETER.
If a part contains expressions that are used to calculate values for other expressions they will begin named with the word “CALC” as in the following example.
Key Parameters
[]
Key parameters will be directly used in NX dialog and bitmap, in a part family user will index or select members by key parameter. With the width limitation of NX dialog, so those key parameter name should keep short and have consistent naming for the different part file, following is recommendation:
For Bearing:
Inside_Diameter
Outside_Diameter
Width
For Nuts:
DIAMETER
Thread, Width_Flat, [ This is optional. Only for GOST]
For Pins:
DIAMETER
LENGTH
For Screw:
DIAMETER
LENGTH
For washer:
DIAMETER
For Profile with L shape:
Width_1
Width_2
Thinckness
For Profile with I shape
Nominal _Depth
[]
Generally Expression is used to present key expression, but for some case, the key parameter value include string, such as Norminal_Size=M5x1.5; before NX5, the string expression is not supported, in this case, part attribute will be used to present key expression.
Feature Order
When the Part Navigator is viewed in the “Timestamp Order” the features should be ordered in the following sequence:
1.Datum
2.Sketch
3.Extrude, Revolve
4.Boolean
5.Blend, Chamfer
Thread Feature
In the new version, for the part that contains thread, we need to provide not only symbolic thread but also detail thread, which can be switched by a key parameter on UI. For this function we can depend on two suppress expressions to control the thread display. For example:
We define a suppress expression SYMBOLIC_THREAD_SUP_STATUS for the feature Symbolic thread (15) and another suppress expression: DETAIL_THEAD_SUP_ STATUS for the feather Threads (19) in the next part. AS the capture showing below: When SYMBOLIC_THREAD_SUP_STATUS = 1 and DETAIL_THEAD_SUP_ STATUS = 0, the symbolic thread is active, but when DETAIL_THEAD_SUP_ STATUS = 1, and SYMBOLIC_THREAD_SUP_STATUS = 0, the detail feather is active.
Materials
The Part material will be specified in NX through the Materials database.
Modeling -> Tools -> Materials->Library
If the material is not known or is not supported in the NX library, please keep a record of these cases and u se “Steel” for the material type unless another material seems more appropriate. In either case keep a record of this so that we may update the library and parts.
Part Attributes
The table below lists the Part Attributes that are included in the template part and explains their purpose. Edit the values of these Part Attributes as needed for each part.
Saved View
The part should be saved in the standard TFR_TRI view.
Visualization/Background
The Visualization background is set to white, the part and preview image will be saved with the white background.
[It is set in Template part]
Preferences -> Visualization -> Edit Background
Preview Image
The preview image will be saved in the standard TFR_TRI view.
The Preview Image option found at File-> Properties->Preview is set to capture the Preview Image on demand rather than on save.
Be sure to set the View to TFR_TRI before creating the preview image.
And preview should be saved with Detailed thread feature and solid body’s color should be 87 (Light Gray)
For example:
Weight
The Preview Image option found at File-> Properties->Weight is set to Update Data on Save.
Materials Textures
All parts will have rendering characteristics applied to them as found in the functions at: View -> Visualization -> Materials/Textures
The following rendering settings will be used on steel parts:
Rendering Material = “Steel"
Finish = "None"
When the parts are materials other than steel, select the closest material that is available. [See example part]
Remembered Mating（记忆装配）
New functionality for Remembered Mating will be added to NX5.
When the new mating functionality is complete in NX5, remembered mating may be added to the parts.
Part Families Modeling Procedure
Create a template part. It is usually a good idea to have the template part's name reflect the fact that it is a template
1. Modeling Procedure
1) Customer default setting, save nx5_user.dpv to folder C:\Documents and
Settings\your_user_name\Local Settings\Application Data\Unigraphics Solutions\NX4, this file include the default setting for reuse content [Just do once, if you changed NX customer
default, you need copy it again.]
2) Use template to set part attribute, layer/category, view, etc,:Open template part
save as to another name.
3) Creat geometry, expressions, and materail, see related rule in above document.
4) Create and save a family table, defining the various configurations of the family
members:
a.Open the spreadsheet from the Part Families dialog by clicking Part
Families Spreadsheet→ Create.
b.From the spreadsheet use Part Family→ Create Parts on the family table to
create a NX part file.
5) Save Part
2. Part family spreadsheet content definition
The basic columns needed in the part family spreadsheet are shown as blow:
3. Profile Standard Template（对于型材：角钢等使用外部的excel）
For the Profile Standard Template, we use external spreadsheet as driver to create instance part.
Dialog Image
Create a bitmap image in the style shown below using a bitmap editing software such as MS Paint.
All dimensions that are editable in the dialog will be shown in the image.
Note: Screen captures from the NX graphics area will not produce an acceptable image. The following parameters should be used:
Image file name: Same as Part Family Template
Image file format: [].bmp
Image Size in Pixels: Width 300, Height 200
Text Font: Arial
Text Size: 15
Object Color: Gray
Object Border: Black
Background Color: White
Quality
The following quality checks will be made to the models.
Where possible these checks will be done by automated testing done by NX Validation functionality and/or Athena Auto test.
Validation Check List
Are there any system named “p” expressions? There should not be
Are there any lower case expression names? There should not be
Are there any spaces in expression names? There should not be
Are there any Block features in the part? There should not be
Are there any Cone features in the part? There should not be
Are there any Cylinder features in the part? There should not be
Are there any Sphere features in the part? There should not be
Are there any Part Attributes with t he value “?” ? There should not be
Are there any features attached to the ORIGIN_CSYS except the OFFSET_CSYS? There should not be.
Is the ORIGIN_CSYS moved from the Absolute 0,0,0 CSYS? It should not be
Is the value of the following expressions other than 0?
ORIGIN_OFFSET_X
ORIGIN_OFFSET_Y
ORIGIN_OFFSET_Z
ORIGIN_ROTATE_X
ORIGIN_ROTATE_Y
ORIGIN_ROTATE_Z
They should not be.
Is the color of the part any color other than Yellow? It should not be
Is there any Datum or Sketches on a layer other than 255? There should not be
Is there any Solid body on a layer other than 1? There should not be
Do any features fail when updated? There should not be
Do any features fail when updated through the part family configurations? There should not be
Is there more than one solid body in the part? There should not be
Do any non-sketch curves exist in the part? There should not be
Is there any solid body that does not have Materials and Textures assigned to it? There should not be
Appendix: Referenced files
Naming Schema document------: Naming schema for Reuse content.doc Customer Default Seting--------: nx5_user.dpv
Template Part-----------------: reuse_template_mm.prt
Example part -----------------: reuse_example_mm.prt。