Creating Machining Processes with Knowledge

You can create a Machining Process containing a sequence of Machining Operations.

1. From any Product:

   1. Select Start > Machining > Machine Programming.

      A PPR context with an empty Machining Cell is created. An empty Activities Process Tree opens automatically.

   2. Create a generic machine or assign a machine from the database.

      As soon as a machine is assigned to the Machining Cell, a Part Operation and a Manufacturing Program are created in the Activities Process Tree.

   3. Alternatively, open an existing Machining Process or PPR context .

      By default, the Activities Process Tree opens automatically.

2. Select Machining Process View in the top left toolbar.

   The Machining Process View is displayed:
   
   
   

   • : creates a new Machining Processes_Product containing one Machining Process,
   • : searches an existing Machining Processes_Product, and opens it.
   • : creates a new Machining Process in the current Machining Processes_Product.

3. Click New Machining Process Product.

   A Machining Processes_Product is created. It contains an empty Machining Process
   
   

4. Optional: Double-click the Machining Process you have created to rename it in the dialog box that appears.

5. Optional: Click Machining Process .

   A new Machining Process is added to the Machining Processes_Product.

   
   
   

6. Click Axial Machining Operations.

   1. Select Spot Drilling in the Drilling Operations sub-toolbar, and a Machining Process

      The Spot Drilling dialog box appears.

      At this stage you can set certain parameters such as feeds and speeds and machining strategy. However, there is only limited access to geometry parameters and it is not possible to specify a tool.

   2. Click OK to add a reference Spot Drilling operation to the Machining Process.

      The reference Machining Operation has an associated Tool Query, named Tool Query.
      
      

7. Still in the Drilling sub-toolbar, click Drilling and click OK in the dialog box that appears to create a Drilling operation.

   The Drilling operation is created after the previous one.

   1. Repeat the same with Tapping in the Threading Operations sub-toolbar.

   The Machining Process View is updated as shown.

   
   
   

You can associate Checks to the Machining Operations.

1. Right-click the Spot Drilling operation in the Machining Process View and select Edit Checks.
   
   

   The Checks Editor dialog box appears. See About Knowledge in Machining Processes.

2. Define a Check as shown below.

   It corresponds to the criteria: the Spot Drilling operation is only available for design holes with a diameter greater than 2mm.

   1. Select the Knowledge Package (Part Design Features)
   2. Select the Type (Hole).
   3. Select the Attribute (Diameter (Length))

      Hole.Diameter is displayed.

   4. Select the Operator (>) and enter the value.

      Hole.Diameter>2 is displayed.

   5. Select the Unit, (mm)

      Hole.Diameter>2mm is displayed.

   6. Click the Up arrow, the expression is added to the list.

   Important: Operator, Function, Unit, Type and Attribute must be inserted from the lists, not entered by hand. Only values can be entered by hand. Do not enter a check by Copy/Paste.

   
   
   

3. Click OK to associate the Check to the Spot Drilling operation.

You can associate Knowledge expressions such as Formula, Checks, and Tool Queries to each Machining Operation of the Machining Process.

1. Right-click a Machining Operation in the Machining Process View and select Edit Formula.

   The Formula Editor dialog box appears.

2. Define a Formula as shown below.

   
   

   • The operating mode is the same as for the Check.
   • The Formula corresponds to the following criteria: the tool tip approach clearance is half the depth of the Spot Drill machining feature.

   
   
   

3. Click OK to assign the Formula to the Spot Drilling operation.

   You can assign Formula to the Drilling and Tapping operations in the same way.

You can define the Tool Queries attached to the Machining Operations.

1. Double-click the Tooling Query associated to the Spot Drilling operation.

   The Tool Query Definition dialog box appears.

2. Define a simple Tool Query as shown below.

   
   

   • The operating mode is the same as for the Check.
   • The query corresponds to the criteria: find a Spot Drill in the ToolsSampleMP tool repository whose name is Spot Drill D10.

   
   
   

3. Click OK to assign the Tool Query to the Spot Drilling operation.

4. Define the Tool Queries of the Drilling and Tapping operations in the same way (to find tools Drill D10.5 and Tap D12, for example).

   You can assign more than one Tool Query to a Machining Operation using Copy/Paste. When you apply the Machining Process, the first query is executed. If there is no tool found, the next query is executed and so on until a result is obtained or the last query is reached. This enables you to query several tool catalogs, different tool types, and have less constrained queries.

You can apply the Machining Process to features, at the required level of the Manufacturing Program.

1. Right-click the Machining Process and select Machining Processes Application .

   The Machining Processes Application Manager dialog box appears.

   
   
   

2. From the Manufacturing View or the authoring window, select the features to which you want to apply the Machining Process.

   The Features Selection is updated.

3. In the Activities Process Tree, select the activity after which you want to apply the Machining Process.

   The Insertion Level in Program text is updated.

4. Click OK or Apply to apply the selected Machining Process (and all the Machining Operations it contains).

   Note: Tool Queries that are attached to instantiated Machining Operations are performed either in the current Machining Cell, or in 'tools catalog' excel files.