Exercise 1 - Creating the Manufacturing Model

 In this exercise you will create a manufacturing model including selection of a reference model, creation of a stock model and definition of an operation (machine tool, cutting tools and program zero).

  • The NC Model is an assembly of a part, reference model, to machining and the stock, workpiece, to machine from.
  • Creating an operation requires creating or selecting a machine and a program zero
  

Setting up the Environment

From Pro/ENGINEER, choose File and Working Directory and navigate to the directory where you have placed the models for this exercise.

There are multiple config.pro options that can be used in manufacturing mode :

  • mfg_template_dir : used to store the templates used during toolpath definition
  • pro_mf_tprm_dir : used to define the directory where the tools are stored
  • pro_mf_workcell_dir : used to define the directory where the workcell are stored

Select Tools / Options to load a pre-define config.pro file for this exercise,  Select   and then load the config.pro from the exercise directory. Select Apply and OK.

    

Creating the NC Model

From Pro/ENGINEER, select New file  to create a new manufacturing model of sub-type Expert Machinist. Set the name as XM1 and use the default template.

Select NC Setup / NC Model / Create Model  and use the default name for the NC Model  .

Select mold_plate.prt as reference model, then Open .

We are now going to create a stock model (workpiece) based on the envelope of the reference model with a .125 allowance on top of the part.

    • In NC Model menu, select Create Stock. A yellow transparent envelope is created for the reference model, it represents the stock. Select the drag handle at the top of the part and left-click to drag and add .125 allowance on top of the part. You can also use the Options menu in the dashboard to add .125 to the +Z offset.
    • Exit the dashboard creation  and then click Done in the NC Model menu.
    • We now need to assemble the NC Model to the Manufacturing assembly, right-click and set Default Constraint and then exit the dashboard  to validate the selection.
    • Select OK to accept the absolute accuracy setting.

 

It is always recommended in manufacturing mode to use absolute accuracy (config.pro enable_absolute_accuracy set to yes)  to avoid issues during feature and material removal creation.

    

Creating the Operation

We are now going to create the operation including workcell and selection of the program zero.

    • Select NC Setup / Operation. Keep the default for the operation name : OP010 .
    • Select Workcell creation  and define a 3-Axis milling workcell name MAZAK . Keep the same default settings from the previous option and select OK to create a workcell.

   

    •  Display the CSYS in the model to define the Machine zero. Select Machine Zero   in the Operation Setup and select NC_ACS0 in the assembly as zero program. 
    • Select OK to create the Operation.
    

 Adding a Fixture

A fixture is a part of an assembly that will be added to the NC model. The fixture is referred to as a hard wall in all the toolpaths.

    • Select NC Setup / Fixture. The Fixture setup panel allows you to add components. Select   to add a new component and assemble fix_dmu125.asm (see picture on the right)
      • Mate surface A on both components
      • Mate surface B on both components
      • Align with 2.5" offset for surface C on both components
      • Exit   assembly dashboard
      • Then exit   the Fixture setup window :

   

    

 Creating Some Cutting Tools

Cutting tools can be prepared up front and loaded in the workcell or can be defined when needed. Let's create some basic tools we will use during the toolpath creation.
There are multiple types of cutting tools.

  • Solid tool : Pro/ENGINEER model or assembly is used to represent the tool. Assembly parameters are used to describe the tool type and geometry that will be used to compute the toolpath. The 3D model is only used for simulation, not for degauging.
    • Select Setup / Cutting Tool Manager
    • In tool manager dialog, select File / Open Tool Library / By Reference and select fm-0400-20.asm model. The 3D model is loaded and the geometry definition (Cutter diameter and tool length)  of the tool is populated from parameters inside the assembly model.
  • Parameter tool : tool is defined in the tool setup dialog using parameters describing the tool geometry.         Let's create a flat end mill tool of 1/4" diameter.
  • In the tool setup dialog, select create an End Mill
  • Change tool name to FEM02500 and set diameter to .25", flute length to .4" and total length to 2".
  • then select Apply to create the tool
  • Select OK to exit the tools setup dialog

Save  the manufacturing model.

 

    
 

© PTC Product Management