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Chapter 7.  PARTdesigner parametric tool
7.4. Create 3D model: Small example from A to Z
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7.4. Create 3D model: Small example from A to Z

A 3D solid must always be created on a 2D sketch. This 2D sketch is created in its own docking window, the Sketcher.

In the following, with the help of a simple cuboid, the procedure is explained step by step.[75]

  1. In PARTproject, create a new project. A small example can be found under Section 5.5, “Create project - Small example from A to Z ”.

    In the project to be edited select the *.3db file.

    Click on Edit.

    -> The Edit file dialog box is opened.

  2. Confirm with OK.

    -> PARTdesigner is opened with the docking windows 3D History, 3D view, Variable Manager and Table.

    [Note] Note

    You can place the docking windows as you wish. On this see Section 3.1.5.4, “Placing method for dockings ” in PARTsolutions / PARTcommunity4Enterprise - User manual.

  3. In the 3D History docking window, you can find three basic planes for the design sketches.

    With the secondary mouse button, click on one of these planes (in this case XY) and select the menu item New sketch... in the context menu.

    New sketch...

    New sketch...

    -> This command opens the Sketcher.

    [Note] Note

    Now you have two general possibilities:

    • Drawing a sketch with fixed values

      The option is suited for demo purposes if you just want the 3D model in a quick way.

    • Drawing the sketch with variables

      When using variables, you can fill them with table values later.

    In the example in hand variables shall be used.

  4. In the Variable Manager, create the variables L (Length), W (Width) and H (Height) for a cuboid. Details on the Variable Manager can be found under Section 7.8, “ Variable Manager docking window ”.

    1. First under Save location, select the option Only in geometry.

      -> Now only the input fields for Name, Description and Equation are active.

      In this example, H (Height) with value 10 has been entered.

      In this example, H (Height) with value 10 has been entered.

    2. Confirm by clicking Commit.

    3. For each variable, create a new line by clicking .

    -> Now these variables can be referenced in the drawing.

  5. First, draw a rectangle which will be extruded later. Details on the sketcher can be found under Section 7.9, “ Sketcher docking window ”.

    Click on the button Insert rectangle .

    Draw rectangle

    Draw rectangle

  6. Set a center point by moving the cursor to the KO origin and simply fix it with a mouse-click.

  7. When moving the mouse cursor, you can draw the rectangle. Fix the size of the rectangle by a simple mouse click.

  8. The following happens simultaneously:

    1. -> In the docking window Sketch history the design step is recorded.

    2. -> In the drawing, the Change parameter window is opened. There, you can exactly determine size and position of the drawing element.

      Here, use the respective variables for Length and Height.

  9. Click on the Accept changes button, in order to confirm your entries.

    -> The Sketcher is closed.

    -> In the docking window 3D History the design step Sketch 1 shows up.

    -> In the docking window 3D view the rectangle is located on the Plane XY.

  10. With the secondary mouse button, click on Sketch 1 and choose the command Base, Extrude....

    Base -> Extrude...

    Base -> Extrude...

    -> The Extrusion solid dialog is opened.

  11. Specify the Length by entering the variable W and confirm by clicking on OK.

    -> Now in the docking window 3D History, in relation with Sketch 1 the design step Base extrude 1 is displayed.

    -> In the 3D view the rectangle with the value W is extruded to a cuboid.

    Cuboid

    Cuboid

  12. Finally click on the button Save .

    -> The Identification data dialog box is opened with tabbed page Geometry.

    1. Fill out the mandatory fields Part name, Author and Catalog key.

      Without entering a valid Catalog key OK remains disabled (grayed out) and you cannot save.

      The schema for a valid Catalog key is:[76] 

      CNS2009*CATALOGS*KATALOGNAME

      Here, in the training example in hand, the Catalog key is:

      CNS2009*CATALOGS*TRAINING

    2. Switch to the tabbed page Table.

      Fill out the mandatory fields Standard name, Description for BOM and Standard number. Details on this can be found under Section 7.12.7, “ Identification data ”.

      [Note] Note

      Standard title is not a mandatory field anymore as of V11 SP4.

    Confirm with OK.

    -> The drawing is finished.

[Note] Note

If a table shall be build, it is necessary to change the parameter Save location in the Variable Manager for all variables from Only in geometry to In geometry and table.

You can recognize the Save location by the respective color:

  • Only in table

  • In geometry and table

  • Only in geometry

Details on this can be found under Section 7.8.10, “ Save location: Only in geometry | Only in table | In geometry and table ”.

Simply select the desired variable, change the list field option and confirm with Commit.

Immediately after the change to Save location "In geometry and table" a table with default values is created. This table can be extended anytime.

[Note] Note

Also see the related example under Section 7.5, “Create table: Small example from A to Z ”.

[Note] Note

Detailed information on the docking window Table can be found under Section 7.11, “ Table docking window ”.


[75] The corresponding example can be found in the Training catalog, under \v11_news\starting_point_table_or_sketch\cuboid2.prj.

[76] As of V9 license keys start with CNS2009*CATALOGS*

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7.3. User interface   Home  7.5. Create table: Small example from A to Z