Pro/MFG R18 Tutorial 1

Pro/MFG R18 Tutorial
For Use With HAAS and Cincinatti Milacron
Vertical Milling Centers
NCSU MAE Dept.
This tutorial is designed to run using Revision 18. It is assumed that the user has a good understanding of Part and Assembly modes before starting this tutorial. This tutorial will take you through an entire machining process for a simple part.
This tutorial only shows some of the simple things that Pro/MFG can do.

Note: Any questions may be answered by referring to the Pro/MFG and Pro/NC- CHECK User's Manual found in proguide.

It may be advantagous to set up a manufacturing sub-directory in your home directory. The process will generate serveral files throughout.

In order to be able to copy the design model and other files that are used in this tutorial and can be used in future applications, you need to issue the following commands:

eos% attach mae_design
eos% cd /ncsu/mae_design


A design model represents the final product. The color is shown as white.

A workpiece represents the size of the piece of stock to be machined. The color is shown as green in the Manufacturing window.

After the design model has been successfully created in Part mode, the manufacturing process may begin.

Note: On command sequences, the > sign indicates the command is on a different menu and the | sign means the command is on the same menu.

1. CREATING A MFG FILE
From the MODE menu, select Manufacture.
Select Create to make a new manufacturing file or retrieve an existing file.

From the MFG TYPE menu, select Part.

It will prompt you for the design part name. Retrieve the desired design model. (the design model used throughout this tutorial is /afs/eos.ncsu.edu/service/mae/project/design/simple.prt, shown in Figure 1. The part can be copied into your home directory so that you can work along with this tutorial)

*
Figure 1 Simple Part

The design model will be opened up into your current Manufacturing window.

Next, a manufacturing model must be defined. A manufacturing model consists of a design model and workpiece. At the end of the manufacturing process, the workpiece and design model geometry should be coincident. If you are not concerned with material removal, you don't have to define the workpiece geometry. For our purposes, we will define it.

From the MANUFACTURE menu, select MFG Model.

2. WORKPIECE CREATION
We want to create the workpiece, so select Create from the MFG MDL menu.
Select Workpiece.

Enter a part name for the workpiece. (Since the workpiece is stock, I have used stock as the name for my workpiece.)

Now create the workpiece. The process is the same as in Part Mode. The workpiece should be made to be the same size as the outside of the design model or larger if sacrificial material will be removed or any facing needs to be done. We can assume that 1inx 6inx 6in Aluminum stock is easily attainable. The design model may be referenced when creating the workpiece. The Use Edge option to select outside surfaces and Up to Surface option for extruding up to surfaces are valuable when creating the workpiece. Simplified versions of the design model may help in cutting down regeneration time and calculation of machine tool paths.

When you are satisfied with the workpiece, choose Done/Return from the MFG MDL menu.

From the MANUFACTURE menu, select MFG Setup.

A workcell is a workpiece (or assembly) feature that specifies a machine tool using different specifications, such as name, type of machine, a set of parameters that describe the physical system, and associated tools. Workcells can be created from either the MFG SETUP menu or when operations are defined. We will define them when setting up operations.

3. OPERATIONS
An operation is a series of NC sequences performed at a particular workcell with a particular setup and using a particular coordinate system for CL data output.
Since no operations have been defined, the DEFINE OPER menu will appear. The items with checks in front on them must be defined. Figure 2 shows the default checks. The other items are optional and definitions are available in the Pro/MFG User's Manual.


*Figure 2 Default Check marks.

Once the appropriate items are checked, choose Done Oper. As items are successfully defined, the next item will open up for definition and so forth until all of the items with check marks have been defined.

3.a. WORKCELL
For the purposes of this tutorial, we will always have a 4 Axis milling workcell. The next part of the tutorial deals with setting up a workcell. If you are working on HAAS Milling Machine in Broughton Hall, the workcell file, /afs/eos.ncsu.edu/service/mae/project/design/Haas/haasmill.gph, should be copied into your home directory and used. If you are using the Cincinnati Milacron Milling Machine in Park Shops, then you will want to copy its workcell file, /afs/eos.ncsu.edu/service/mae/project/design/Cincinnati/cincinattimill.gph , in to your home directory. You can Retrieve the Workcell and use it as your workcell. The CM workcell already has certain tools associated with it. More about tooling later.
If you do not use either of these predefined workcells, you will need to set up a new workcell. To do this, choose Mill |4Axis |Done. After the type and number of axis has been selected, the workcell particulars need to be defined. The CELL SETUP menu appears and different items may be defined, such as the name of the workcell, the machine parameters, the associated tools, and the corresponding tool table.

The Name of the workcell and the Mach Params are optional. Mach Params define the physical system of the workcell, such as maximum and minimum X, Y and Z travel, maximum cell feed, etc. These are already defined in the haasmill.gph and cincinnatimill.gph workcells.

After all items have been defined, choose Done from the CELL SETUP menu.

Next, you will be asked to create/select a coordinate system.

From the MACH CSYS menu, choose Create or Select a coordinate system. Defining a coordinate system in Part mode may make things simpler here. The coordinate system needs to be oriented as shown in Figure 3a or Figure 3b, depending on the machine you plan to use. placed in the corner closest to the coordinate system shown on the haasfixture.prt(Figure 4) or cmfixture.prt. Select the the coordinate system of simple.prt (shown in Figure 1).

* Figure 3a CSYS setup of HAAS Machine.



* Figure 3b CSYS setup of Cincinnati Milacron Machine.


Choose Done Oper to commit the new operation.

Now, you will be in the MFG SETUP menu. If you know which tools you will be using, you may be added at this point. However, we will define them when defining NC sequences.

4. FIXTURES
Next, the fixture that the workpiece sits in must be defined.
Choose Fixture from the MFG SETUP.

Choose Create from the FIXTURE SETUP menu.

At this point, you may define the fixture. You may also create the fixture in Part or Assembly modes. You may use fixture components from Pro/Library. Pro/Library has many standard components that may be used to secure the workpiece to the machine. It may be wise to use these components along with other created components to fully secure the workpiece to the machine. This maybe helpful when running the tool paths to make sure that the tool paths do not interfere with the fixture or hold down components.

Choose Component. The fixture may be assembled or created at this point. It may be advantageous to create the fixture in assembly mode because the workpiece may be directly referenced using the Use Edge command. A standard fixture (Figure 4a) is available either for the Haas ( /afs/eos.ncsu.edu/service /mae/project/design/Haas/haasfixture.prt.1), Figure 4a, or for the Cincinnati Milacron ( /afs/eos.ncsu.edu/service /mae/project/design/Cincinnati/cmfixture.prt.1) . The only difference between the HAAS and CM Fixtures is the placement of the coordinate systems. It may be copied into your home directory and modified to fit your workpiece. Only the parallels (d8, d9, d10) and the clamping length (d16) need to be modified. The fixture sits in the HAAS machine as shown in Figure 5a and in the Cincinnati Milacron machine as shown in Figure 5b.


* Figure 4a Haas Fixture


Assemble the workpeice to the fixture as shown in Figure 4b.


Figure 4b Assembled Workpiece/Haas Fixture


Figure 5a Picture of HAAS machine with Workpeice/Fixture in it.



Figure 5b Picture of Cincinnati Milacron machine with Workpiece/Fixture in it.


After the fixture component has successfully been created and/or assembled, choose Done/Return from the FIXT SETUP menu.

Fixture setup time may be added at this point, but is optional. This would be necessary if the entire manufacturing process was to be defined.

After the fixture has successfully been defined, choose Done from the DEFINE FIXT menu. This will bring you back to the FIXTURE SETUP menu. Fixtures may be created, modified, deleted or activated from this menu. Choose Done/Return.

This will bring you back to the MFG SETUP menu. Choose Done/Return.

The assembling of fixtures to the workpiece is an optional step. It is not needed to reach the final product, the cutter location data. It is however, very helpful in visualizing the tool path with respect to the fixture and workpiece to make sure that the machine will not run into the fixture or workpiece and potentially damaging the the workpiece, fixture and most importantly, the machine.

5. MACHINING AND NC SEQUENCES
There is not a set procedure for deciding which NC sequences to use. Machining experience is the only helpful tool in deciding how to machine the workpiece.
An overview of the machining processes for the simple part:
Make a rough volume cut with a voluming sequence.
Clean up the volume cut with a profiling sequence.
Drill the holes with a holemaking sequence.
From the MANUFACTURE menu, select Machining.
The MANUFACTURING INFO window will appear. This contains information regarding such things as operation name, workcell, type, etc.

Operations may also be set up from the MACHINING menu. Since our operation is already specified, we can now generate NC Sequences.

Note: You have to set up an operation before you can start creating NC Sequences.

Some of the milling options available are listed below with a short description. For further detail, refer to the Pro/MFG User's Guide.

Volume - Used to remove a specific volume, such as a pocket.
Local Mill - Used to remove material left after a rough NC sequence. Can be used to finish corners.
Conventl Srf (Conventional Surface) - Used to mill horizontal or slanted surfaces.
Contour Srf (Contour Surface) - Used to mill horizontal or slanted surfaces by following either a user-defined pattern or the natural curves of the surface
Face - Used to face off a workpiece.
Profile - Used to finish vertical or slanted surfaces.
Pocketing - Used to mill horizontal, vertical, or slanted surfaces. A combination of Volume and Profiling sequences.
Holemaking - Drilling, boring, tapping of holes.
Thread - Used to make threads.
A. VOLUME MILLING
Choose NC Sequence>Volume |Done
In the SEQ SETUP menu, default check marks will be placed beside the different parameters that must be defined. Figure 6 shows the SEQ SETUP menu with the default check marks.


* Figure 6 SEQ SETUP Menu showing default checks.

Choose Done.

This will bring up the TOOL PARAMS menu. Tooling may created or prior tooling may be retrieved from a tooling file or from the Pro/E tooling library. For our process, choose Set. This will invoke Pro/Table. Edit the necessary parameters. We are using a 1/2 in square end mill that is 2 in long. If desired, you may save this tool as a specific file name. Exit Pro/Table and choose Done from the TOOL PARAMS menu.

The HAAS machine has 18 tool capacity and the Cincinnati Milacron machine has a 21 tool capacity. As many as 18 (or 21) tools may be placed in a workcell. Standard milling, turning, and drilling tools may be found in Pro/LIBRARY.

As mentioned earlier, the CM already has 11 tools associated with the workcell. There are several end mills, reamers and a center drill that you may use as your tool when defining NC sequences. Other tools may be added and should be placed in empty pockets. Pocket number 10 has a Jacobs Chuck in it which will accomidate most tools and pocket number 7 has a 3/8" tool holder in it. You may view the tooling table by going to the MFG SETUP menu, select Workcell > Modify > CINCINATTIMILL > Tool Table . This will envoke Pro/Table and you can see what the tools are and where they are located.

Pro/LIBRARY has a standard set of tools that can be used in your manufacturing process. The process is similar to adding any other tool and will be shown below in the holemaking sequence.

If you select an existing tool, it will be displayed in a subwindow.

*
Figure 7 MILL Tool

Next, the MFG PARAMS menu will appear. At this point, parameters such as feed rate, spindle speed, tolerance, and tool overlap must be specified. The manufacturing parameters will need to be specified for each NC sequence. However, if you are preforming more than one NC sequence, you may use a previous sequence's parameters.

Select Set.

NOTE: Any parameter with a default of -1 must be changed.

A Param Tree window will appear. By clicking of the manufacturting parameter, its definition will appear in the bottom of the window. Edit the necessary parameters and Exit. The units are the same as used in the design model and therefore need not be specified here. In this table, set CUT_FEED to 25, STEP_DEPTH to .25, STEP_OVER to 0.1, SCAN_TYPE to TYPE_1, ROUGH_OPTION to ROUGH_ONLY, SPINDLE_SPEED to 3600, and CLEAR_DIST to 1.

The HAAS and Cincinnati Milacron machines have full circular interpolation capabilites and therefore the CIRC_INTERPOLATION option should be set to ARC_ONLY. The NUMBER_OF_ARC_PTS option must also be set. The defualt is 3. If you want to modify a parameter that is not shown on the simplified parameter list, click the Advanced button and all of the parameters will be presented. In order to change the CIRC_INTERPOLATION parameter, you will have to do this.

The MACH_ID is important when post processing and needs to be set at this point. It is also under the Advanced Parameters. The HAAS machine uses a FANUC controller and the Cincinnati Milacron uses a Cincinnati Acramatic controller. For operating on the HAAS machine, a MILL302 post-processor will be used when post-processing is enacted. The Cincinnai Milacron machine will use a MILL303 post-processor. More about post-processing later. For the example, MACH_ID needs to be set to 302(or 303 for the Cincinnati Milacron). **After these have been set up for the first NC sequence, they do not need to be set up again. Save and Exit.



Figure 8 Parameter Tree (Simplified)

At this point, all of the manufacturing parameters have been defined. They may be saved now and retrieved later for machining processes that have similar parameters. If you select Save, the program will ask you for a filename. This will create another file. If you do not to save at this time, the manufacturing parameters will be saved with the *.mfg file that you are creating. Exit.

Select Done from the MFG PARAMS menu.

This will bring up the RETRACT menu. The retract plane is the plane to which the tool will retract to once finished. It is defined by a modifiable value representing the distance in the positive Z-dir from the coordinate origin.

Select Specify >Make Datum and create a plane offset from the top of the workpiece a distance of 1.5 in. This will vary for different machining processes.

After the retract plane has successfully been defined, the DEFINE VOL menu will appear. Choose Create Vol.

It will prompt you for a milling volume name. Enter a name. (mill1)

Choose Sketch. The sketching menu is the same as the Cut/Protrusion menu in Part mode. For our example, sketch the center volume of the simple part offset from the edge of the pocket by 0.05 to the inside of the pocket. We will mill out the rest of it in the next NC sequence. Use of the Offset Edge>Sel Loop option under the Geom Tools menu is helpful. Extrude the volume up to the bottom surface of the cavity.

Volumes may also be "gathered" by selecting Gather instead of Sketch. More about that may be found in the Pro/MFG User's Guide
Choose Done/Return from the CREATE VOL menu.
The first NC sequence is now complete. By choosing Done Seq from the NC SEQUENCE menu, the sequence will be saved to the *.mfg file when it is saved. For any completed NC sequence, you can simulate the tool path and material removal by using the Play Path command. The options available for Play Path are:

NC Check - It produces a simulation of the material removal process by shading the different pieces. Figure 9a
Screen Play - Shows the path of the tool as a red line. Figure 9b
Show File - Shows the contents of the cutter location (CL) data file in an Information Window.

Choose NC Check >Run. The program will calculate the tool path and run through other necessary operations and finally give you an simulated NC sequence.


*Figure 9 a.C Check After Simulation Completion



*Figure 9 b. Screen Play After Simulation Completion

B. Profiling
Choose NC Sequence > New Sequence >Profile |Done.
The program will assume that you are using the same tool for this NC sequence as the one before. Therefore, only place a check mark in front of Tool if you are using a different tool.

Check off parameters that need to be defined. Usually, it check only those parameters that need to be defined. Select Done from the SEQ SETUP menu.

If the MILL is not already choosen, choose it.

Choose Done Sel.

Next, the MFG PARAMS menu will appear. Choose Use Prev and select 1:Volume Milling . From the MFG PARAMS menu, select Done.

From the SURF PICK menu, choose Model |Done.

From the SELECT SRFS menu, choose Add .

Now select the walls of the pocket in the design model, simple.prt. They can be selected one at a time or the loop can be picked by picking the bottom loop of the pocket. When the walls have all been selected, choose Done.

The profiling NC sequence is now complete. Select Done Seq to commit the NC sequence.

The Play Path option may be performed the same as in the previous NC sequence.

C. Holemaking
Choose NC Sequence > New Sequence > Holemaking |Done >Drill |Deep |Constant Peck | Done
We will be using a twist drill instead of the end mill for the holemaking sequence. Check off tool and other options that need to be defined. Select Done.

At the TOOL menu, check Specify Tool.

We will retrieve a standard tool from the Pro/E Tooling Library. Choose Retrieve from the TOOL PARAMS menu. From the RETRIEVE TOOL menu, select Tool Library and then By Copy |Done from the USE TOOL menu. Enter a question mark, ?, when the program asks for a model name. If you know the Instance Name, you may enter this instead of the question mark. Select Pro/Library from the SELECT FILE menu.

Now, it's just a matter of working through the menus till you come to the file that you want. The drill we will be using is found at /mfglib/tools_lib/standard_t/drills_s/ssjl.prt. It is helpful to have the Pro/E Tooling Library Catalog to look up the specific tool that you want. We want a 1/2 in twist drill which has an instance name of SSJL461. Move up and down the INSTANCES menu until SSJL461 appears and then select it. Because there is such a large number of standard tools, these menus tend to be quiet long. After you have selected the tool, it will be added to the workcell.

Another way to find the tool that you want is to select it by the tool parameters that define that tool, such as drill diameter and length. From the RETR INST menu, select SelByParame and check off which parameters you wish to define. Check DRILL_DIA_FRACTION and Done Sel and then choose the 1/2 drill. It will be added to the workcell.

If you are using the Cincinatti Milacron machine, you should specify the pocket number to be one that is empty or Pocket #10, which has the Jacobs Chuck. To do this choose Pocket Num from the TOOL PARAMS menu and then Enter from the SEL POCKET NUM menu. Enter in the appropriate pocket number.

Next, the Mfg parameters need to be set. Choose Set and edit the parameters the same as before.

The HAAS and Cincinnati Milacron machines have built in pecking capabilities. The tool cuts to the peck depth and retracts. It proceeds cutting at peck increments and retracting until it reaches the bottom of the hole or goes through. In order for the machine to use this capability, the PECK_DEPTH parameter needs to be changed to something other than 0. (PECK_DEPTH=0.2in).

Note: If you do not want to use the pecking capabilities, then choose Standard | Done from the HOLE MAKING menu.

The HOLES menu will appear with Hole Set already highlighted. It will then go to the next menu after this, DRILL DEPTH. Choose Thru All |Axes | Done.

From the AXES SELECT menu, choose All Holes and select the top surface of the design model. This will select all of the holes on the surface. Holes may also be selected one at a time.

When all of the holes have been picked, choose Done/Return > Done > Done/Return.

The holemaking NC sequence has now been fully defined. Select Done Seq. to commit the sequence.

At this point our design model, simple.prt, coincides with the workpiece, our stock. Our manufacturing process is now complete. Next, we must create machine code that the HAAS or Cincinnati Milacron machines will understand. In order to accomplish this, a cutter location file data file must be created and post-processed. This will be handled in the next section.

This tutorial only demonstrates three different NC sequences. The other NC sequences can be learned easily enough by reading the Pro/MFG User's Manual. They are straight forward and can be learned without to much trouble.

6. Post Processing
After completing the above portion of the tutorial, one OPERATION should have been created which encompasses all three NC SEQUENCES to machine the stock. In order to post-process the sequences, they must be used to generate CL DATA (cutter location data) file(s). A CL DATA file may be created for each sequence individually or simultaneously for all sequences defining an OPERATION. For this tutorial, we will generate the CL DATA and MCD file (machine control data) for the entire operation simultaneously.
Note: Setting up a CL DATA library is an option that may be considered. In doing so, all your CL Data files created from that point on, will be automatically stored to this library. To establish the library, the following command should be added to your config.pro file: pro_mf_cl_dir /afs/eos.ncsu.edu/users/complete the path to the subdirectory you create


First, under the CL Data menu select Output>Operation.

The SEL MENU should appear with a list of operation(s). Choose the operation to be post-processed.

Under the CUT PATH menu choose File.

Now, check the options on the OUTPUT TYPE menu as shown in Figure 10a below.


Figure 10a Output Type selections.

Choose Done.

Pro/Engineer will then prompt for a Pro/NC file name. Enter the name of your choice and hit return. The tool path will be created for each sequence after which, the PP OPTIONS menu will pop up. Check the options as shown in Figure 10b below and choose Done.


Figure 10b PP OPTIONS selections.

The PP List menu should then displayed. Select MILL 302 if using the HAAS machine or MILL 303 if using the Cincinnati Milacron machine.

The CL DATA and MCD file will now be generated with the .ncl and .tap extensions respectively. Upon completion of this, the verbose window will be displayed as shown in Figure 10c below.


Figure 10c Verbose Window

The .tap file is the MCD file. This file can be uploaded/downloaded to any DNC machine that supports the code format.

The verbose window contains some general statistics of the GENER process as well as the APT Input and the NC Control Code output.

The code generation can be stepped by clicking the right mouse button on the appropriate section of the verbose window. The code generation will be stopped and by clicking on the same area with the left mouse button it will be generated one line at a time. This will allow you time to see the process flow.

Warning
It must be noted here that the generic post-processors, MILL302 and MILL303 are just that, generic. A warning is issued at the beginning of the APT and NC Control Code. This warning will show up in the *.tap file that you generate. This does not mean that the code can't be run, just that care must be taken running any g-code generated with Pro/MFG on either the HAAS or Cinicinnati Milaron The G-code that they produce is about 90% correct for both the HAAS and Cincinnati Milacron.
The next step is to write post-processors that are specific to each of the machines. Only a few things will have to be changed in the generic post-processor provided by Pro/MFG in order for the G-code generated by Pro/MFG to be 100% compatable with either of the machines.



Examples

Figure 11 Machined Simple Part

Figure 12 Mold Half

Summary
In order to define a manufacturing process, many things must be defined.
Create or retrieve a manufacturing model.
Set up a manufacturing database:
Define the workcells that will be used for the manufacturing process.
Define the fixture setup(s). They may be created or assembled.
Perform an up-front manufacturing parameter setup, if desired.
Set up an operation:
Supply an operation name, if desired.
Specify the workcell that will be used to create the NC sequences. If workcells have already been defined, you may activate one or create another.
Select or create the coordiante system to be used as the origin for the CL data ouput.
Specify the operation parameters.
Define the FROM and HOME points, if desired.
Define the NC sequence for the operation. After specifying the type, set it up:
Select or create a tool to be used.
Set up the manufacturing parameters.
Select or create a coordinate system to define the orientation of the workpiece on the machine.
Define the retract plane.
Specify the geometric references for the NC sequence.
Define the Start and End points, if desired.
You can remove material from the workpiece to simulate the machining process.
If necessary, you can modify NC sequences by changing tool, parameters, cut motion, etc.
Generate CL Data file and post-process that file to yeild the MCD file.