LAB 2: Optimization and HSM

ET 449 LABORATORY 2

Mini Punch and Die Set: Optimizing Tool Paths and High Speed Machining Methods

PURPOSE:

The purpose of this laboratory exercise is to increase machining efficiency by implementing tool path optimization and High Speed Machining (HSM) principles. Tool paths developed in LAB 1 for the punch and die set will be recreated in OneCNC. However, LAB 2 will focus on reducing machine
cycle times. Inefficient motion including, "air cutting", low rapid rates, slow feed rates, and unnecessary tool changes will be evaluated. The same 3D parametric files and corresponding 2D dxf files will be used in this laboratory exercise. The primary goal is improving production efficiency through reduced cycle time.

As was the case in LAB 1, OneCNC will be used to make editorial changes, create the appropriate tool paths for contouring and pocketing, create a CNC program, simulate the program execution, develop a set-up and operation sheet, and produce a final part on the HAAS vertical milling machine.
One of the components (either the male punch or the female die) will be simulated and evaluated for cycle time. Your lab partner will produce the corresponding mating component.
Each team member must use their lab partner's program and set-up procedures to determine the total cycle time for the final punch and die. Teams will be evaluated on documentation, operations, precision, methods. A written lab report is required. Illustration 1 shows a view of the project to be completed.

Illustration 1: MINI DIE SET (PUNCH AND DIE)

OBJECTIVES:

After completing this laboratory exercise you should be able to do the following:

Manipulate a 3D model and generate a 2D dxf file.
Import the dxf file into OneCNC
Translate the axis for part zero
Select required geometry for drill cycles
Select required geometry for pocketing operations
Select required geometry for contouring
Select the appropriate tooling for machining operations
Implement methods for HSM machining operations
Determine more efficient feeds and speeds
Generate required tool paths
Run a simulation to verify part cut
Determine the machining time required to produce the part
Evaluate both mating parts (work with your lab partner to determine the total cycle times (both parts)
Record machining cycle times
Compare cycle times to Lab 1
Evaluate improvements in production rates

TERMS:

Die set
Punch
Die
OneCNC
dxf
XFA file
NC file
Part Zero (origin)
Tooling Set up
Transform
Pocking Operation
Contour Operation
Verify Operation
Tool Offsets
High Speed Machining
Multiple "H" offsets

Laboratory Preparation and Procedure

1.   Study the drawing shown in Illustration 1, select the component, and identify the geometry to be machined. The first step for this lab will include evaluating inefficient
      motion implemented in LAB 1. Identify specific areas where improved efficiency may be recognized. An example will be provided in step 2. After you have
      identified areas for improved production rates, import the required dxf file into OneCNC and window around the part geometry. Select COPY/MOVE/. When prompted for MOVE FROM, select the left endpoint of the top object line.   When prompted to enter MOVE
     TO, select KEYBOARD, and make sure the coordinates are set to zero. Press enter and the origin should then be located
     at the top left corner of the part. Continue operations as required to produce the selected part.

ILLUSTRATION 2: MINI DIE SET ENGINEERING DRAWING

2.    Determine the operations and steps in creating the required geometry. You should develop a set-up sheet as you produce the required CNC
       operations in OneCNC. Note specifically the required tools, tool number, feeds, and speeds. This information must be provided for the operator
       on the set-up and operation sheet. NOTE: While the ET 349 class focused on the basic steps for creating CNC programs, this class will focus
       on the precision and efficiency of producing parts. Pay particular attention to correct feeds, speeds, material, and tooling information. Efforts should
       be made to reduce the cycle time of producing the part. In OneCNC complete the required CNC operations to produce your part.
        NOTE: FOCUS ON CYCLE TIME REDUCTION! As an example, consider the female die component. Assuming a .250 two fluted end mill is the cutting tool
       selected, the normal procedure during set up would be to touch the tool off of the top surface of the part. A pocketing operation to remove material from around the
       guide pins to a depth of .350 inches may seem to be a logical first operation. However, in doing so, when the one inch center pocket is produced, the first .350 Z
       depth will result in the tool only cutting air. Since no material is removed, the result is wasted motion and increased cycle times. An improvement can be made by
       creating multiple "H" offsets. Let's assume that Tool number 1 is to be used for the machining operation. Typically all "T" values and "H" values must agree for a
       given operation. However, we will create an "H01" value corresponding to the top surface of the stock, and a second "H02" value corresponding to the elevation where
       the center one inch diameter pocket will be machined (.350 " below the top surface). By using the H)2 as the tool offset, wasted "air cutting" can be eliminated. The
       following steps will be described in regard to how this procedure can be carried out. Note that your lab instructor must change a machine parameter to allow multiple
       "H" offsets. This will be done prior to running your part on the HAAS mini-mill. Assuming this procedure has been completed, the following steps must be taken:

                       1.   Touch off the tool to be used for pocketing around the guide pins on the top surface of the work part
                       2.   Physically change T01 to tool position T02
                       3.   Next, touch off the tool in position two to the correct height for the center one inch pocket (.350 below the previous surface).
                             (Note: an alternative method would be to simply change the tool offset value for T02 to reflect the .350 change in elevation.
                                      This can be done by editing and entering the desired value in the offset menu for T02 on the HAAS controller).
                            4.    With these changes made, continue to create the appropriate pocketing operations in OneCNC; one for pocketing around the guide pins, and one for
                              the one inch center hole pocket.
                       5.    Once the operations have been completed and verified, post process for the HAAS 2 axis mill setting.
                       6.    Edit your program, and change H01 to H02 for the second operation. Note: If this is the only change made, then the tool will return home before
                              rapiding back down to the surface of the center hole pocket. This problem can be avoided by deleting the M05 and G28 CNC words.
                              NOTE: THIS CAN BE EXTREMELY DANGEROUS!
                              By deleting only partial codes, the machine tool may, in fact, lose the current reference location and cause a machine crash.
                              NEVER ATTEMPT THIS PROCEDURE UNLESS YOU ARE ABSOLUTELY SURE THAT ONLY NON CRITICAL CODES
                              HAVE BEEN DELETED.
                       7.    A safer method is to use one of the two methods shown below:
                                                 Method 1: Create two separate CNC programs (one for each operation) by posting each operation separately.
                                                                   Edit the first CNC program and insert a subroutine call at the end of the code for operation 1 just prior to the M05.
                                                                      The second operation can be used as a subroutine, executed, then a return will enable operation 1 again to complete the
                                                                      M05, G28, and M30.

Method 2: Merge the two programs as one single program, and delete the M30 from operation 1.

8. After all edits have been made open the file using the APT file generated by OneCNC
9. Run a back plot and analysis to determine the estimated machine cycle time for the part and record the value(s).

3. After completing the previous CNC operations, the next step will be evaluating improvements by implementing these procedures.

4.    Continue to evaluate all operations required to produce the part and look for any methods for reducing cycle time. One procedure may involve changing
       the rapid plane value. NOTE: THIS CAN BE DANGEROUS! YOU MAY RUN THE RISK OF PLUNGING THE TOOL INTO THE WORK PIECE
       AT A HIGH RATE. DO NOT MAKE CHANGES UNLESS YOU ARE ABSOLUTELY CERTAIN THAT THERE IS NO CHANCE OF CRASHING.

5. After you have evaluated all the CNC operations and are satisfied that you have an optimum solution to minimized cycle time, save your file, and run
another verification.

Next, click on the OPERATIONS MANAGER icon.
SAVE YOUR WORK
At this point, you can run a graphical simulation; however you must set up the stock.

6. After you have post processed the file, edit the program and provide the following comments.
NOTE: ALL CNC PROGRAMS SHOULD HAVE THIS INFORMATION IN THE FUTURE!

        %
     O1234
        (PROGRAM/PART NAME:                                                  )
        (PROGRAMMER:                                                                )
        (DATE DEVELOPED:                                                          )
        (DATE RAN:                                                                        )
        (CNC MACHINE PART RAN ON:                                        )
        (OPERATOR:                                                                       )
        (REFERENCE FILE NAME:                                                  )
        (REFERENCED SET UP SHEET NAME:                              )
        (REFERENCED OPERATIONS SHEET NAME:                    )
        (G54 OR EQUIVALENT LOCATION                                   )
        (TOOL TYPE, NUMBER, TOOL CHANGER I.D. #             )
        (MAT'L TYPE:                                                                    )
        (SPECIAL SET-UP OR OTHER INSTRUCTIONS:               )

7. You can now save the file as LAB2.txt on a floppy disk and transfer to the HAAS CNC mill.
Check with your instructor for assistance, follow set-up and operation sheets, RUN THE PART.

NOTE: MAKE A DRY RUN FIRST.
AFTER THE PROGRAM HAS BEEN CHECKED, RUN THE PART AND
RECORD THE TIME TO COMPLETE: ____________ MINUTES.

8. SUBMIT A LAB REPORT USING THE FORMAT SHOWN BELOW:

LABORATORY REPORT FORMAT

Title:
Your Name:
Lab Partner:
Lab Section:
Date:
ABSTRACT: (One paragraph stating, what, when, where, how, and OUTCOMES).
Statement of Problem: (One paragraph concisely describing the problem under study).
Objectives: (One introductory complete sentence following by a listing of specific objectives.
                   Note: There should be one tangible outcome for each objective stated).
Terms and definitions: (List and define any terms that are unique to the laboratory or terms that could
                                   be used in another context that need clarification as to the use in this lab).
Procedure: (One introductory complete sentence describing the overall procedure followed by
                   a description of steps taken).
Results: (One paragraph describing the outcomes followed by appropriate tables, graphs, charts, etc.
              Reference should be made to tangible deliverables that must include a minimum of the following:

1. Part drawing (dwg) showing G54 or equivalent location
2. Program Listing
3. Printed tool path simulation
4. Program Listing
5. Set-up Sheet
6. Operations Sheet
4. Actual Machined Part

Conclusion/Discussion: (One to two paragraphs. Restate the problem, discuss the outcomes and descriptions of any difficulties encountered.
Make recommendations any changes for improvements). NOTE: FOCUS YOUR CONCLUSION ON HOW CYCLE TIME IMPROVEMENTS
IMPLEMENTED RESULTED IN CHANGES IN CYCLE TIME. After all, this was the main purpose in carrying out LAB 2.
References: Cite any references using APA format.

NOTE: YOU WILL BE GRADED ON CONTENT, FORMAT, GRAMMAR, AND SPELLING! MAKE SURE YOUR WRITE IN
COMPLETE SENTENCES AND CHECK SPELLING. WRITE IN THIRD PERSON, PAST TENSE, AND TREAT THE LAB REPORT
AS THOUGH IT WERE AN ON-THE-JOB TASK AND RESPONSIBILITY. LAB WRITE UP AND DELIVERABLES ARE DUE AT THE
BEGINNING OF THE NEXT SCHEDULED LABORATORY SESSION.