Pro/ENGINEER NC and Tooling Solutions is one of the most powerful and capable CAM systems available. Unfortunately, many of us fail to set it up properly, and therefore waste a lot of time creating programs because we are forever starting from scratch. This article will review several important Pro/ENGINEER setup tips that will help get you making chips in no time at all.

Tip #1: Important config.pro options

Set up your NC environment with these config.pro options:

pro_mf_workcell_dir (path to where workcells are stored)

pro_mf_tprm_dir (path to where tool parameters are stored)

pro_mf_param_dir (path to machining parameters and site files)

postpp_dir (path to post processor library)

pro_library_dir (path to standard libraries, including Tooling library)

start_model_dir (path to the location of start models and drawings)

search_path (path to any folders that contain required models such as fixtures and solid tools)

cl_arrow_scale (0 means no arrows show up on the tool path – helps when spinning the model with a tool path displayed)

rename_drawings_with_object (a value of “both” will automatically create drawings when creating a new mfg  model; think automatic setup sheets)

Tip #2: Use site files for default parameter settings

Are you tired of turning the coolant on for every NC sequence because the default is “off”? Use a site file to specify your own default parameter settings.

To create a site file:

Pick Mfg Setup > Param Setup > Site > Create > enter a name > select a type. Then set the parameters as desired, and save it (it is saved as a .sit file in pro_mf_param_dir).

To use a site file:

Method 1: Mfg Setup > Param Setup > Site > Create (Retrieve) > Activate > choose site.

Method 2: In the Machine Tool Setup (workcell) dialog box, pick the Defaults button and choose a site file to activate for that workcell.

Method 3: During NC sequence creation, select Site from the Mfg Params menu, and select which site file to use.

Tip #3: Save and reuse your workcells

Don’t create that same three-axis mill workcell named “MACH01” and populate it with cutting tools every time you start a new program, retrieve it instead!

1. To save the workcell after you’ve created it, pick File > Save in the Machine Tool Setup dialog box. The workcell is saved as a *.gph file in the pro_mf_workcell_dir folder.

2. When you create the workcell, selecting “Defaults” allows you to select a default site file to use with this workcell. The active associated site file will be saved in the workcell.

It is also a good idea to create or retrieve any standard cutting tools that are always loaded in the machine (more on cutting tools in tip #4). Any cutting tools defined with the workcell remain with it when it is saved.

3. Add PRINT settings as desired; these too are saved in the workcell.

Tip #4: Tools

You don’t have to create a new half-inch end mill for every new program. Spend a few minutes or an hour to create a cutting tool library, and then use it.

To add a tool to your library:

1. Open the Tools Setup window by picking Mfg Setup > Tooling > select a workcell. (Tip: you must first create a workcell—even a “dummy” one—before creating cutting tools.)

2. Name each tool, and set parameters, comments, etc. as needed. (Tip: you may also use File > Open Tool Library to retrieve solid tool parts or assemblies.)

3. To associate material cutting data with the tool, see Tip #5.

4. Save the tool (parameter tools are saved into pro_mf_tprm_dir). Saved tools may be retrieved at any time into other workcells.

5. To retrieve a saved tool, open the Tools Setup window and select File > Open Parameter File.

Tip #5: Associating machining parameters with cutting tools and workpiece materials

Capture and reuse your machining knowledge by storing material cutting data with your cutting tools.

Define your materials by creating a folder structure as follows:

1. Start Windows Explorer and navigate to your pro_mf_tprm_dir.

2. In that folder, create a folder called “materials.”

3. In the materials folder, create a folder for each material type.

 Add the cutting data to each tool for each material and cutting condition.

4. Open the Tool Manager.
5. Create or retrieve the tool and open the Speeds & Feeds tab.

6. Select a stock material (your materials will be in the pulldown list).

7. Select an Application (Roughing or Finishing).

8. Supply speed, feed, axial depth, radial depth data.

9. Save the tool.

10. Repeat steps 1-5 for each material, as desired.

11. Perform all of the above steps for each tool as needed.

To use these parameters in an NC sequence, use either of the following methods:

(Tip: it helps to first specify the Stock Material in the Operation Setup dialog box.)

1. In the Parameter Tree in an NC sequence, select Edit, Copy From Tool, All/Spindle/Feed/Depth, Roughing/Finishing - the speed/feed/cut depth parameters for the current stock material will be read from the tool file.

2. Or use relations in the parameters to call out the cutting data. The parameter names for use in relations are shown in the table that follows.

The use of relations applies to individual parameter files, and also to site files, which makes this a very powerful technique. For example, if in your active site file, STEP_DEPTH is set to TOOL_ROUGH_AXIAL_DEPTH, then the STEP_DEPTH will always be set for you to the proper value (assuming that the tool contains that information for the material).

Tip #6: Tie it all together into a manufacturing template

The fastest way to begin a new job is to use a manufacturing template (available in Pro/ENGINEER Wildfire 2.0 and up). You can create and use any number of template models, also known as start models. You may, for example, have a different template for each machine, or even for each material or product.

Here’s how to create a template. Only the first and last steps are required. However, the more items you include in your template, the greater the benefit:

Create a new manufacturing model, and give it a name such as “inlbs_nc_3x_haasvf8”). (Tip: use the default mfg start model to save yourself step 3 below.)

1. Set the units (Setup > Units).

2. Create a default coordinate system and datum planes, if necessary.

3. Create layers to hide items such as datum planes (don’t forget to “save status”).

4. Set up named views as desired (for example, an XZ view for a lathe; or top, front, and side views for a mill; or a view for each operation).

5. Create one or more operations, setting the default stock material if desired (see tip #5).

6. Retrieve/create a workcell for each operation. Retrieve/define cutting tools for the workcells if needed.

7. Create/retrieve and activate site files as desired.

8. Make any other settings as needed. Basically, anything that will never (or rarely) change, and that you don’t want to set up every time. An example here might be a fixture setup such as the table, tombstone, clamps, etc.

9. Create a drawing (e.g., setup sheet or process drawing) of the start model, using the same name as the start model, using the manufacturing .asm as the “default model”. Set it up as desired, then save it.

10. Save the manufacturing model; the filename.mfg, and filename.asm will be saved (along with any fixture components that you created). Put these files (and the setup drawing if you made one) into your start_model_dir. It is recommended that these files be made Read Only.

11. To use the template, select it from the list when creating a new mfg model (you must first uncheck the “use default template” box). If you have followed tips 1-5 above, then all you need to do is assemble your reference model, create or assemble a stock model if needed, and begin creating NC sequences.

(Tip: if a drawing file (e.g., a setup sheet) with the same name as the mfg template exists, a drawing of your new mfg model will be created at the same time. Set the config option rename_drawings_with_object to “both” in order to do this automatically.)

Bonus Tip: Helpful web pages:

PTC web pages—available to customers on active maintenance—contain useful information. Check out the following:

• Pro/NC Central
  
• GPOST Central - includes links to post processor downloads.
  
• Vericut Central
  
• Educational Resource Library (tutorials, demos, tips & techniques)
  
• Software Update Downloads (can download Tooling library, for example)
  

 Was this tip helpful? Let us know.