DRAWING SHEET CREATION IN CREO PARAMETRIC
DWG Sheet Size Layout, ANSI Y14.1, Inch
DWG Sheet Size Layout, ISO, Millimeter
Recommended Lettering Heights for Mechanical Drawings: Lowercase letters is seldom found on engineering drawing except for the drawing notes since long columns of uppercase characters are not as pleasing to the eye and are harder to read. Uppercase letters are used unless lowercase letters are required to conform with other established standards, equipment nomenclature, or marking. According to ANSI/ASME standard, the default font type is ASME Y14.5MIn general, standard font type Gothic letter is required on mechanical and electronic drawings
When you start a new drawing, you are prompted for a format file (.frm) to associate with the drawing. This file carries all the format graphical information, and it can also carry some optional default attributes like text size and draft scale. For a multisheet drawing, you can have two default formats—one for the first sheet and another for the remaining sheets.
CREATING DRAWING SHEET FORMATS IN CREO
Creo Parametric Drawing Mode: Create Drawings | Export Drawings | Import Drawings | Use Layers to Manage the Display of Different Items | Work with Various view Types | Works with Multiple Sheets | Add & Modify Textual & Symbolic Information | Define Mapkeys for Drawing Operations | Create Custome Drawing format | Create 3D Parametric, Feature-based Models From 2D Drawings Data Using Autobuild.
Create a Format with Empty Template: File —» New —» Format —» Name: type a name (B-Format_mm) —» OK —» New Format —» Empty —» Landscape —» Standard Size: B —» OK
Drawing Formats: The size and style of lettering on drawing formats is to be in accordance with ANSI Y14.2M. To provide contrasting divisions between major elements of the format, the following guide should be used on all projects taken from the text:
Drawing Format Parameter: Tools —» Parameter —» Look in (Drawing) (B-Format_Inch —» Filter By: select Default —» + (to add) —» type a name (example: FILE_NAME) —» Type: Integer (số nguyên/whole number), Real Number (adds a double parameter / Value can accommodate decimal places, String (chuỗi, chùm / Adds a parameter in the form of a text string as a value), Yes/No (Adds a parameter with a value of yes or no) —» Designate (to make the parameter visible to database management) —» Value —» Access (Full) —» Source (User-Defined) —» Restricted —» OK
A typical drawing format can contain both plain text and parametric information such as company details, drawing name, sheet number, and tolerance information.
System parameters – With system parameters, the parameter value is automatically evaluated when the format is added to the drawing. System parameters, including
Working with Drawing Parameters: Using the Tools —» Parameters menu you can access drawing parameter functionality for drawings and drawing formats. Drawing parameters work in the same way as do model parameters. A drawing parameter is nongraphical information you can add to a drawing. It is useful for keeping some additional information with a drawing that you may not want to include in a note. You can show the parameter value in a note by including [¶meter] in the note string. —» ...
User-defined parameters – Prompt you to type values when the format is added to a drawing. If you do not include these parameters in a table, then you are not prompted for a value when adding the format to a drawing. These parameters can be store on the format as drawing parameters if you
To Use Parameters in Labels in a Format Table: Double click the table cell —» enter the appropriate label (such as &dwg_name) —» OK. The label appears in the table exactly as you typed it until you add the format to a drawing.
Adding drawing notes – Drawing notes can be include in formats containing standard company information. The notes can include plain text and parametric information. System parameters evaluate when the format is added to a drawing. However, you are not prompted for user-defined parameters and they should only be included in drawing tables.
Create a drawing format by importing IGES data and retrieving tables —» continues here
DRAWING TITLE BLOCK LAYOUTS IN CREO
The title block is one of the most important parts of the drawing. The title block is located in the lower right corner of the format. Normally, the title block includes spaces for the following information, in column from right to left, top to bottom. Below format is for B size drawing:
TITLE BLOCK & AUTOMATICALLY POPULATED FIELDS
Create Title Block Using Table:
Attach The Formatted Title Block to Drawing Border: Select the table from the Drawing Tree —» Table tab —» Select Table —» Move Special —» pick the bottom right corner —» select Move object to location defined as X and Y coordinates —» X: 16.38 —» Y: .38 —» (alternative) select the table bottom left corner —» X:. 62 —» Y:. 38 —» OK—» (to attach).
Create A New Drawing and Apply Different Formats To It.
TITLE BLOCK & ANGLE PROJECTION SYMBOLS
Creating Symbols. Drawing symbols consist of draft geometry and text. It is important to understand the options available when creating symbol geometry and text. A symbol, when created, is added to its parent drawing's symbol gallery as a symbol definition. When you add the symbol to the drawing, it is added as a copy of the definition called a symbol instance. To use the symbol in a different drawing you must save it as a .sym file. You can set up a default symbols directory using the configuration option pro_symbol_dir.
Symbol geometry can be a simple draft using various drafting tools – Copy from a drawing (copy draft entities) to create symbol geometry – Copy an existing symbol and modify it to create a new symbol – Import 2D data in the form of IGES, DXF, SET, TIFF, or CGM files then modify the imported data to configure the symbol geometry.
Symbol text can be created using free note. By default, the text is placed as invariable. The text cannot be edit and remains the same as symbol. To create variable text, add variable text to the symbol. To create variable text, you need to enclose the text within two back slashes, for example, \note\. This enables you to change the value of the text when you place the symbol on a drawing. You can specify the type of text to show in the note. This can be text, integers, or floating points. You can also use parameters in variable text, enabling the text to update when the parameter value changes.
Create a Simple Symbol with Invariable Text: New —» Drawing —» Name: type a name for the symbol (example: third-angle-proj) —» OK —» Default Model = none —» Empty —» Orientation = Landscape —» Size = A —» OK —» Sketch —» (draw the symbol) —» Save (third-angle-proj.dwg) —» OK —» Keep the active drawing open —»
Place Symbol Instances On A Drawing: Open a drawing —» Anotate tab —» Symbol —» select Custom Symbol —» Browse —» Working Directory —» select the symbol —» Open —» place it on the drawing —»
Create Symbol Types. There are two types of symbols that can be configured. Simple and Generic.
Insert a Custom Symbol / Logo: Annotate tab —» Symbol —» Custom Symbol —» Symbol Name: Browse to locate it / New: enter a new symbol name —» Create a new symbol —»
DEFINE THE LOCATION CALLOUT GRID IN DRAWING
Define a location grid on the format file (.frm) B size drawing referencing. In a Format file —» Layout tab —» Sheet Setup —» Location Grid —» select Define —» Rows —» Letters —» By Number —» type 4 + Enter —» Done/Return —» Column —» Numbers —» By Number —» type 8 + Enter —» Done/Return —» Done/Return.
To Show the Location Callout in a New Drawing: In Drawing —» Annotate tab —» Note —» type a note, and then type —»