UG建模应用--3

nullModeling Applications of Unigraphics 建模应用 （Ⅲ）Modeling Applications of Unigraphics 建模应用 （Ⅲ）Trim Body / Split Body 修剪 / 分割物体 Trim Body / Split Body 修剪 / 分割物体 学习目的：掌握 Trim Body 和 Split Body 的不同。 Trim Body 修剪物体 Insert  Feature Operation  TrimTrim Body是一种常用的操作特征。用a face, datum plane, or other geometry 修剪一个或多个target bodies（Solid or sheet)。你可以决定哪一部分保留，修剪后的实体获得了修剪几何体的形状。 注意：修剪后的几何体仍具有参数。Trim Body Feature 可以进行编辑。练习：CAST :fmf_trimbody_1.prtTarget Bodynull1. 选择被修剪的目标体2. 定义修剪面3.确定修剪方向（移去材料侧）Procedure： 选择 Trim Body 图标。 选择一个或多个，then choose OK. 选择a face or datum plane, or define other geometry, to trim the target bodies. 矢量箭头为要去掉的部分。 选择accept the direction of the vector or reverse.nullSplit Body 分割物体 Insert  Feature Operation  Split这个操作将移去目标体上的所有参数。分割后的几何体为Unparameterzed feature. 分割后两部分几何体均保留。操作步骤与Trim Body 类似。Target Body练习：CAST :fmf_splitbody_1.prtnullExtract 抽取Insert  Form Feature  Extract 从一个几何体上抽取 curves, faces, a region of a body, or an entire body.At Timestamp —— ON，要时间标记, extracted feature 按时间的先后顺序排放。 At Timestamp —— OFF，不要时间标记，extracted feature 特征排在所有特征之后。 Extract Curve： 抽取曲线， 从几何体上抽取边缘、曲线等。创建的特征为：EXTRACTED_CURVE，可以用特征的编辑方法进行编辑。 注意: 不要把这个选项与 Insert Curve Extract（不是特征，要用 Edit Curve 进行修改〕混淆。 抽取曲线抽取体抽取区域抽取面nullExtract Face：抽取面，把 body上的一个或多个Face转化为Sheet Body. 当你想把sheet body 的类型转化为B-surface，以便与向其他的系统传输数据时，这个选项很有用。 Same Type Surface 把Faces转为Sheet Body,且与原曲面类型相同， Polynomial Cubic 把Faces转为polynomial cubic B-surface类型的Sheet Body，是近似的方法。 General B-Surface Extract Region This function lets you create a sheet body that is a collection of faces that are related to a "seed face" and limited by boundary faces. Seed Face - This step identifies the seed face. All other faces in the feature are related to the seed face. Boundary Faces - This step identifies the boundaries of the Extract Region feature. 练习：Cast :fmf_extract_3.prt Cast :fmf_extract_2.prtnullExtract Body This option creates an associative copy of an entire body. Features can then be added to the Extract Body feature without appearing on the original body. One use for an Extract Body feature is when you want to have an original solid and a simplification available at the same time.nullThread 螺纹 Insert  Feature Operation  Thread Other Feature Operations 其它特征操作 nullTo create symbolic threads: Choose Symbolic for the Thread Type in the Create Threads. Choose the thread manufacturing Method. Examples are Rolled, Cut, Ground, and Milled. Choose the Form for the thread. Select one or more cylindrical placement faces Modify the parameters as desired. (Some parameters, such as Callout, cannot be modified directly.) Callout references the thread table entry that provides the default values. Choose from Table lets you choose a different entry (and, therefore, a different set of default values). Choose Tapered if you want the thread to be tapered. If you want the thread to update when the cylinder changes, choose Full Thread. (Length grays out.) If a selected face belongs to an instance array, you can apply the thread to the other instances by choosing Include Instance. Decide whether you want a Right Hand or Left Hand thread. You can specify a new starting location for the thread by selecting the Select Start option. Select a planar face on a solid body, or a datum plane, as the starting location. Choose OK or Apply. Detailed To create detailed threads: Choose Detailed for the Thread Type in the Create Threads dialog.ProceduresSymbolicnull Select a cylindrical placement face. Default parameter values appear, based on the diameter of the face. Modify the parameters if required. The parameters that appear on the Create Threads dialog for detailed threads are Major Diameter, Minor Diameter, Length, Pitch, Angle, Direction (Right Hand or Left Hand), and Select Start. Choose OK (or Apply if you want to create more threads), and the system creates the thread.Scale Body 缩放体This option lets you scale solid and sheet bodies. You can use uniform, axisymmetric or general scaling methods. This operation is fully associative.Lets you choose the type or method of scaling: Uniform - scale uniformly in all directions. Axisymmetric - scale with a specified scale factor (or multiplier), symmetrically about a specified axis. This involves assigning one scaling factor along an axis you specify, and another, single scaling factor to be applied to the other two axis directions. General - scale with different factors in all three X, Y, Z directions.nullSew 缝合This option lets you join together two or more sheet bodies, thus creating a single sheet. If the collection of sheets to be sewn encloses a volume, a solid body is created. Procedure To sew sheets together: Ÿ Choose Sheet. The Target sheet icon is selected. Ÿ Select the target sheet. Ÿ Choose the Tool sheets icon, and select the tool sheet(s) to be sewn to the target. Ÿ If you want to create more than one sewn sheet, choose Output Multiple Sheets. Ÿ Define the Sew Tolerance. Ÿ Choose Apply or OK.This option also lets you sew two solid bodies together if they share one or more common (coincident) faces.Insert  Feature Operation  Sew 练习：Cast :fmf_sew_1.prtnullTo sew solids together: Ÿ Choose Solid. The Target faces icon is selected. Ÿ Select the target face(s). Ÿ Choose the Tool faces icon, and select the face(s) on the tool solid that are coincident with the target solid's selected face(s). Ÿ If a selected body is part of an instance array, and you want all the instances to be sewn, choose Sew All Instances. Ÿ Define the Sew Tolerance. Ÿ Choose Search common faces if you want to see where the sewing will occur. Ÿ Choose Apply or OK.Choose Edit®Blank® Unblank All of Part 练习：Cast :fmf_sew_2.prt练习：Cast :fmf_patch_1.prt fmf_patch_1.prtModeling Application of Unigraphics References CardModeling Application of Unigraphics References CardASSOCIATIVE, PARAMETRIC PARTS ( Process Outline of building Solid Bodies, incorporating Design Intent, and anticipating changes.) 1) Create new part ( inches or millimeters ) or open seed part, then Save Part As necessary. 2) Set attributes and Preferences as necessary. 3) Decide on part origin/orientation. 4) Strategy: take time to “break part down” into individual features. a) Consider use of Hollow to create cavities and achieve constant wall thickness. b) Consider Multiple Sweeps-look for distinct profiles. 5) Decide on 1st feature based on fundamental shape of part=Primitive or Sweep. (See Other side) 6) Generally speaking, create features that add material first. 7) After 6 above, generally speaking, create features that remove material. 8) Generally speaking, create Blends, Chamfers,and Tapers last. Remember that a Taper after a Blend is different than the other way around. 9) Create relative datum planes ( for placement faces and Positioning Target Edges) instead of Fixed Datum Planes. Likewise, Relative Datum Axis instead of Fixed. 10) Avoid using Multiple Primitives _ lack of associativity to other features UG 建模应用参考卡片nullASSEMBLIES - Bottom Up Method ( For creating either multi-piece part assemblies or Master Model Drawing files. Assumes a piece part has been created.) 1) Create new part or open seed part, then Save Part As necessary. a) Add assembly designation in the file name. b) Consider future Load Options and directory pathnames as file are named $ saved. 2) Add the component. 3) Consider the Layer of all the objects in the piece part for control of the display of objects in the assembly. DRAWINGES ( Assumes a Solid Model has been created. Process below is identical whether or not the Master Model Concept is being used.) 1) Modify the Drawing made when entering the Drafting Application or create a New Drawing. a) Consider the size of the model and define the appropriate Drawing Scale, Drawing Units, Projection Method, and standard Drawing name. b) Consider if the model is too complex for one sheet or Drafting standards will require multiple sheets. ( BOMs, Specification sheets , etc.) 2) Set Attributes and Preferences as necessary ( Colors, Display, View Display, Layer, etc.)null3) Add any Drawing borders, title blocks, geometry for tables, Revision Blocks, or other necessary Drawing criteria in order to see available space in the field of the drawing for views. 4) Identify part origin/ orientation relative to the canned views (ABS CSYS ). Identify parent view for Orthographic projections, if any. 5) Consider view(s) necessary to fully dimension and clarify part design. Plan ahead for projected views and necessary space for dimensions. 6) Remember Hidden Line removal and Smooth Edges in Preferences. Add views. Remember layer settings before placing views or changes later with Visible in View. 7) Add Utility symbols onto a separate layer. a) Again， consider Preferences. b) Be conscious of the point Method when selecting. 8) Add Dimensions onto a separate layer. a) Dimensions to Utility Symbols instead of model geometry whenever possible. b) Remember the point method when selecting and be careful not to select Midpoints accidentally with the control point or Infer option. Gaps between the object and the extension lines are very important. c) If plotting with a pen plotter, eliminate any coincident drafting objects such as extension lines or utility symbol components on top of one another. 9) Check all the above for accuracy and conformance to any applicable standards.nullPRIMITIVES ( as a first feature in a part ) 1) Decide on the part origin or orientation. 2) Set Attributes and Preferences as necessary（ Color， Solid Density， Layer， etc.） 3) Select the type of Primitive. 4) Based on the type created, enter or define the following ( not necessarily in the same order for each method) : a) Select the method of creation. b) Enter the feature sizes or select curves （ if necessary to define parameters.） c) Define Vector for Axis（ for Cylinder or Cone ）or consider WCS orientation （ for Block) . d) Define Origin (for all the Tube/Cable). e) If creating a Tube/Cable, Select Guide String. 5) Do not create any more primitives in this part.EXTRUSIONS ( Assumes 1 or more Curves, Edges or Faces exist in the part file ) 1) Select the Section String. 2) If using Direction and Distance : null a) Define the Extrusion Vector. ( When using either a Fixed or Relative Datum Axis as the vector, selection will incorporate associativity to the Datum Axis). b) Select Trim face(s) and Trim Face Extension option as necessary. c) Enter the Extrusion parameter values as necessary. 4) Through Multiple Bodies option is not recommended. ( Monodetail Part File concept.) 5) If any Bodies exist, select a Boolean Operation or create as a separate Body and create a Boolean Feature afterwards.FORM FEATURES ( Assumes a Solid Body exists in the Part File ) 1) Consider selectable objects to position to ( Body edges, Reference Features, etc.) Create them first if necessary. 2) Select type of Form Feature. 3) Select Placement Face ( planar) . 4) Select Through Faces for Holes or Slots, if necessary, Datum Planes can be used. 5) Select Horizontal or Vertical reference direction ( for Slots, Pockets, Pads). 6) Enter sizes and / or angles (real numbers, algebraic phrases, expression names). 7) (Optional ) Locate the feature relative to its parent body using Positioning.nullREFERENCE FEATURES ( Make them Relative when Possible. ) 1) Identify object(s) to be selected for creation based on desired Associativity. 2) Change Work Layer from that of the solid. 3) Select a point, Curve, Edge, Face, Datum Plane, Datum Axis, or combinations and enter parameters as necessary. 4) Choose OK or APPLY after selection of objects. Choosing OK or APPLY before selecting objects will create non-associative, Fixed Reference Features. 5) Datum Planes: a) If an edge is desired, be careful not to select one of its Control points. b) When selecting faces: planar faces establish angular or offset relationships; cylindrical faces establish axial relationships or 1 of 4 tangential positions. 6) Datum Axes: offer more editability than explicit point and vector definitions, i.e., a circular array is associative to a datum Axis but not to a point, curve, or edge. Prevent redundancy of creating through linear edges of a solid if not advantageous. 7) Other Considerations: a) Consider changes that may cause unwanted changes in Reference Features. b) Consider creating Reference Features needed for placement of Form Features, Sketches, etc., on a separate layer and create a Category or Description for that layer identifying the feature for which they are necessary.