Manuals - PARTsolutions

Chapter 7. PARTdesigner

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.^[77]

Create a new project in PARTproject create a new project. You can find a small example of this at 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 opens.
Confirm with OK.
-> It opens PARTdesigner opens with the docking windows 3D History, 3D View [3D view], Variable Manager and Table.

Note
You can position the docking windows as you wish. See Section 2.1.5.4, “Placing method for dockings ” in PARTsolutions - User.

The 3D history [3D History] docking window contains the three basic levels for the construction sketches.

Click with the secondary mouse button on one of these layers (here XY) and select the menu item New sketch.... [New sketch...] in the context menu.

New sketch...

-> This command calls up the Sketcher.

	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.

Variables are to be used in this example.

Create the variables L (Length), W (Width) and H (Height) for a cuboid in the variable manager [Variable Manager]. Details on the variable manager [Variable Manager] can be found at Section 7.8, “ Docking window " Variable manager" ”.
1. First select the Only in geometry option under Storage location [Save location].
  -> Now only the input fields for Name, Description and Formula [Equation] are active.
2. Confirm by clicking " Apply Changes [Accept changes]."
3. For each variable, create a new line by clicking .
The variables H, L, and W have been created.

-> Now these variables can be referenced in the drawing.
First, draw a rectangle which will be extruded later. Details on the sketcher can be found under Section 7.9, “ Docking window "Sketcher " ”.
Click the Insert Rectangle [Insert rectangle] button.
When you move the mouse pointer away from the base point, you can resize the rectangle. You can also lock the size of the rectangle by simply clicking the mouse.

Draw rectangle
In the "Edit Element [Edit element]" docking window, adjust the [Base point] X and Y base points [Base point].
Under " Width " and " Height," replace the fixed values with the variables you defined earlier.
In the Sketcher, click the Apply changes [Accept changes] to confirm your enrollments.

-> The Sketcher is closed.
-> The design step Sketch 1 appears in the 3D history [3D History] docking window.
-> In the 3D view docking window, the rectangle lies on the XY plane.
Click on Sketch 1 with the secondary mouse button and select the command Solids [Base] -> Extrude.... [Extrude...]

Solids [Base] -> Extrusion [Extrude...]..

-> The Extrusion [Extrusion solid] body window opens.
Determine the length [Length] by entering the variable W and confirm with OK.

-> In the 3D History menu area, the design step " Base extrude 1" now appears in connection with Sketch 1.
-> In the 3D view, the rectangle with the value W is extruded into a cuboid.

Cube created
Execute the Check part [Test part] function function.
-> The part's integrity is checked. This is of importance, because only then a faultless export to the different CAD systems is ensured. For details see Section 7.24.2, “ Test part ”.

Set " Storage Location [Save location] " to " In Geometry and Table [In geometry and table]."

Note

If a table is to be created, it is necessary to change the storage location [Save location] of the individual variables in the variable manager [Variable Manager] from Only in geometry to In geometry and table.

You can recognize the storage location [Save location] by the corresponding color.

Only in table
In geometry and table
Only in geometry

Details can be found at Section 7.8.11, “ Storage location: Only in geometry | Only in table | In geometry and table ”.

Simply select the desired variable, change the selection in the list field and confirm with Apply [Commit].

Finally, click on the Save button.
-> The Identification details [Identification data] window is opened with the Geometry tab page.
1. Fill in the mandatory fields Component name [Part name], Author and Catalog key.
  If a valid catalog key [Catalog key] is not specified, OK remains greyed out and cannot be saved.
  The scheme for a valid catalog key [Catalog key] is as follows:^[78]
```
CNS2009*CATALOGS*KATALOGNAME
```
  Here in the training example, the catalog key [Catalog key] is
```
CNS2009*CATALOGS*TRAINING
```
2. Switch to the Table tab page.
  Fill in the mandatory fields Standard designation [Standard name], Parts list designation [Description for BOM] and Standard number. Details can be found at Section 7.18.9, “ Identification data ”.
Confirm with OK.

The creation of the component is now complete.

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

	Note
	Detailed information on the docking window table [Table] can be found at Section 7.12, “ Docking window " Table " ”.

^[77]You can find a suitable example in the training catalog in the directory \v11_news\starting_point_table_or_sketch\cuboid2.prj.

^[78]Since V9 the license key starts with CNS2009*CATALOGS*

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