Intro to Conversational Programming - 2OP

CNC Mill 1 training that has been adapted for use with the 2OP machines.

Table of Contents

Overview

These lab instructions are for the CNC Mill 1 upgrade. If at any point during the training you have any questions please contact staff.

Machine Guides

Part Files

Material Requirements

Parts A & B will be made on the same piece of HDPE stock (one on top face, one on bottom face). The material will be given to you when you arrive for your Mill reservation. You will also be given a sharpie marker in a holder that is used for the trial run to verify your part. 

Tools

See Jay or a staff member on where to locate your tools.
NOTE: Tool numbers start at 9 to allow you to manually load and unload tools while running your program. This behavior will make more sense after completing the CNC Mill 3 upgrade.

Part A

  • Tool 9 - 1/4" Spot drill
  • Tool 10 - 1/4" drill
  • Tool 11 - 1/4" center-cutting end mill
  • Use 11/2" Parallels located in the appropriate tool box

Part B

  • Tool 11 - 1/4" center-cutting end mill
  • Use the same 11/2" Parallels that you used for part A

Terminology

Jump to Table of Contents

Absolute (ABS) and Incremental (INC)

Absolute positions are plotted on a three dimensional coordinate plane. All absolute dimensions are relative to the origin set on the DRO as (0,0,0).

Incremental positions are plotted relative to the last absolute position. If the DRO reads (1,0,0) ABS and the machine is told to move (1,1,1) INC, the machine would move to (2,1,1) ABS.

Some Rules for Incremental Reference Positions

When you want to continue a movement from the previous events ending point, utilize incremental references for the X, Y, or Z begin positions. Setting the begin position to (0,0,0) INC is a useful way to just continue from the ending position of the previous event. Below are various events and how the next event will create an incremental reference to them.

If the event is a:

  • DRILL, then an incremental move is from the X, Y programmed in that previous event.
  • BOLT HOLE, then an incremental move is from the X CENTER, Y CENTER programmed in that event.
  • MILL, then an incremental move is from the X END, Y END programmed in that event.
  • ARC, then an incremental move is from the X END, Y END programmed in that event.
  • CIRCLE POCKET or FRAME, then an incremental move is from the first or X1, Y1 corner programmed in that event.
  • REPEAT, then an incremental move is the same as for the event types shown above, but shifted by the programmed OFFSET.

Tool Compensation

One of the things that makes the ProtoTRAK TMX so easy to use is that you get to program the dimensions of the finished work piece that are right on the print, instead of the center line of the tool. Let's say you programmed the square shape below shown as the solid line.

tool compensation example

The ProtoTRAK has no way of knowing whether you want to cut a pocket out of the material, so you want your tool to follow Path A, or if you are squaring up a block so you want your tool to follow Path B. This is what tool cutter compensation (or cutter comp) is about.

Tool cutter compensation is always specified as the tool either right or left of the work piece while looking in the direction of the tool motion.

Examples of tool right are:
tool right compensation

Examples of tool left are:
tool left compensation

Tool center means no compensation either right or left. That is, the centerline of the tool will be moved to the programmed points.

Conrad (Connecting or Corner Radius)

Conrad is another really nice feature of the ProtoTRAK EMX. In the example below you could machine a straight line from Point A to B, then an ARC with radius R from B to D, then another straight line from D to E.

Connecting radius example

The problem is that the arc is not easy to program because you often don't know where point D or B, or the center of R is located. However, you may know where Point C is, or you may be able to figure it out easily. In that case you can program the above part by programming a straight line from A to C, tell the control when it asks that you have a CONRAD equal to R, and then program another straight line from C to E. The ProtoTRAK will automatically blend the connecting radius (CONRAD R) between the two straight lines with no additional input.

For Rectangular Pockets or Frames, CONRAD stands for corner radius. You may input any value that makes sense considering the size of the pocket and the diameter of the tool.

Operations

First, startup the machine. Reference the machine guide on how to do so, here.

Part A

Program Strategy

If you wish to place the part in the vise before programming consult section Set up the Part Reference. Before programming a part, it's important to figure out what you want to do and what order you want to do it. Part A's programming strategy is as follows:

  1. Decide that the lower left corner of the part will be our absolute zero or absolute reference and enter the absolute zero location.
  2. Spot drill the left most hole in the row using a Position Drill Event.
  3. Spot drill the next 3 holes using a Repeat Event.
  4. Spot drill the 8-hole bolt circle pattern using a Bolt Hole Event.
  5. Repeat steps 2 - 4 with the drill instead of the spot drill.
  6. Mill the diagonal in the upper left corner using a Mill Event.
  7. Mill the arc in the lower left corner using an Arc Event.
  8. Mill the circular pocket with a Pocket Frame Event.
  9. Mill the rectangle profile with a Pocket Frame Event.

Making and Inputting the Program

Reference the 2OP mill guide while programming events. Information is provided on each programs input parameters.

The Program Part Number

  1. Press MODE and then press PROG EDIT soft key to enter the Program Mode.
  2. The conversation display says, "Program Name". Input 123, SET (INC SET or ABS SET). If there is a program already in the current memory, you can erase it by pressing Erase in the Prog In/Out Mode before entering the program number. Select GO TO BEGIN to start programming your first event.

Event 1 — Spot Drill the First Hole

  1. The conversation says, "Select an Event". You press POSN/DRILL soft key. Now, press DRILL for our first drilling event.
  2. The right side of the information area shows that Event 1 is a Position/Drill and it lists what data is required. The blue box indicates where the cursor is and you can scroll around using the electric hand wheel (EHW). 
  3. Conversation says, "DRILL,BORE,TAP". You press 1 for DRILL, ABS SET.
  4. "X". You press 2.75, ABS SET. Remember the lower left corner is our Absolute zero.
  5. "Y". You press .75, ABS SET.
  6. "Z RAPID" will almost always be set to 0.1 ABS. This is the point at which the tool will slow down from rapid speed before cutting.
  7. "Z END" Enter -0.050 ABS. This is the final depth of our cut. Note: We are using the spot drill and will not be going to full depth in this cut. Also, write down this number as it will be important during the repeat events.
  8. "# Pecks". Enter 0.
  9. "RPM". Enter 2000.
  10. "Z FEEDRATE". Enter 10.
  11. "TOOL #". You press 9, ABS SET.
  12. Tool number 9 is the spot drill, so diameter is not important, press ABS SET.

Event 2 — The Next 3 Holes

  1. "Select an Event". You press the SUB soft key, and then the REPEAT soft key for Event 2 to make the next 3 holes in the row.
  2. Event 2 is a Repeat Event and the data needed is shown on the right of the information area. Notice Event 1 has shifted to the left.
  3. "First Event #". You press 1, ABS SET because we want to repeat Event 1.
  4. "Last Event #". You press 1, ABS SET because the only event we want to repeat is Event 1.
  5. "X Offset". You press .75, INC SET because that's the distance between the holes in the X direction.
  6. "Y Offset". You press 0, INC SET because the other holes are not shifted in the Y direction.
  7. "Z RAPID OFFSET". You press 0, INC SET because we want this value to remain 0.1 ABS.
  8. "Z Offset". You press 0 INC SET because we are still using the spot drill to the same final depth. 
  9. "# Repeats". You press 3, ABS SET because we want 3 more holes each offset .75 inch.
  10. "% RPM", "% FEED". You press 100 ABS because we will keep the same speed and feed.
  11. "Tool #". You press 9, ABS SET because we're using the same tool.
  12. "Tool Dia." You press ABS SET because we don't want to change the diameter for this tool.

Event 3 — The Bolt Hole Pattern

  1. "Select an Event." You press POSN DRILL, then the BOLT HOLE soft key for Event 3.
  2. "DRILL,BORE,TAP". You press 1 ABS SET for a drilling event.
  3. "# Holes". You press 8, ABS SET because there are 8 holes.
  4. "X CENTER". You press 1.5, ABS SET.
  5. "Y CENTER". You press 2.5, ABS SET.
  6. "Z RAPID". You press 0.1 ABS SET.
  7. "Z END". You press -0.05 ABS SET.
  8. "Radius". You press 1, ABS SET because the radius of the bolt hole pattern is 1.000 inch.
  9. "Angle". You press 90, ABS SET. This is the angle measured in the counterclockwise direction from 3:00 o'clock and sets the first hole position you want to drill. We could have input 0 and then we would drill the right most hole first. Instead we are going to drill the top/highest hole first.
  10. "# PECKS". You press 0, ABS SET.
  11. "RPM". You press 2000 ABS SET.
  12. "Z FEEDRATE". You press 10 ABS SET.
  13. "Tool #". You press ABS SET. We're still using tool number 9, but notice we didn't press the 9. If you don't input a number, the ProtoTRAK assumes the last tool is used again.
  14. "Tool Dia." You press ABS SET.

Event 4- Sub Repeat to drill holes after spot drilling

  1. "Select an Event". You press the SUB soft key, and then the REPEAT soft key for Event 4 to drill all the holes you have just spot drilled.
  2. "First Event #". You press 1, ABS SET because we want to repeat Event 1.
  3. "Last Event #". You press 3, ABS SET because the events we want to drill, are all the holes we have spot drilled.
  4. "X Offset". You press 0, INC SET because the holes to be drilled are in the same position.
  5. "Y Offset". You press 0, INC SET because the other holes are not shifted in the Y direction.
  6. "Z RAPID OFFSET". You press 0 INC SET because our Z offset should never change.
  7. "Z OFFSET". You press -0.075 INC SET because we want to go a depth of -.125 and our offset will reference the -0.05 depth of the spot drill.
  8. "# Repeats". You press 1, ABS SET. If you wanted to countersink the holes you are drilling press 2, ABS SET. This would enable all the holes drilled to be immediately countersunk as well.
  9. "% RPM" and "% FEED". You press 100 ABS SET because we already set a SPEED and FEED that is applicable for the drill.
  10. "Tool #". You press 10, ABS SET because we're using a different tool.
  11. "Tool Dia." You press .25 ABS SET since the diameter of the drill bit is 1/4".

Event 5 — The Upper Left Diagonal

  1. "Select Event". You press MILL soft key for Event 5.
  2. "X Begin". You press 0, ABS SET to define the beginning of the milling cut at its lower left point on the diagonal.
  3. "Y Begin". You press 3.25, ABS SET to define the beginning of the milling cut.
  4. "Z RAPID". You press 0.1 ABS SET.
  5. "Z DEPTH". You press -0.125 ABS SET because this is the depth our drawing calls for.
  6. "X End". You press .5, ABS SET to define the end of the milling cut.
  7. "Y End". You press .75, INC SET to define the end of the milling cut. Notice we defined this as an incremental change of .75 inch from the beginning. We could have also input 4.0, ABS SET to also define the end point. Think about this and make sure you understand.
  8. "CONRAD". You press ABS SET because we don't want to blend this mill cut into another cut.
  9. "Tool Offset". You press 2, ABS SET because you're selecting that the tool is to the left of the work piece as it moves from beginning to end.
  10. "RPM". You press 4000 ABS SET.
  11. "Z FEEDRATE". You press 20 ABS SET. With the increased spindle speed and carbide cutter, we are able to use a moderately high number here.
  12. "XYZ FEEDRATE". You press 20 ABS SET. 
  13. "Tool #". You input 11, ABS SET because we're calling the 1/4" end mill tool number 11.
  14. "Tool Dia." You press .25 ABS SET.
  15. "Continue". You input 2, ABS SET because this is not continuous path milling.

Event 6 — The Lower Left Radius

  1. "Select Event". You input soft key ARC for Event 6.
  2. "X Begin". You press 0, ABS SET because we're going to start at the top and mill down and to the right.
  3. "Y Begin". You press .5, ABS SET.
  4. "Z RAPID". You press 0.1 ABS SET.
  5. "Z DEPTH". You press -0.125 ABS SET.
  6. "X End". You press .5, ABS SET.
  7. "Y End". You press 0, ABS SET.
  8. "X Center". You press .5, ABS SET, or we could have input 0, INC SET since the X Center is the same as the X End.
  9. "Y Center". You press .5, ABS SET.
  10. "CONRAD". You press 0, ABS SET.
  11. "Direction". You press 2, ABS SET because we are milling in a counterclockwise direction.
  12. "Tool Offset". You press 1, ABS SET because looking from beginning towards end (the direction of the tool cut) the tool is to the right of the work piece. Think about this to be sure you understand.
  13. "RPM". You press 4000, ABS SET.
  14. "Z FEEDRATE". You press 20, ABS SET.
  15. "XYZ FEEDRATE". You press 20, ABS SET.
  16. "Tool #". You press 11, ABS SET because that's still our tool.
  17. "Tool Dia." You press .25 ABS SET (or just ABS SET).
  18. "Continue". You press 2, ABS SET because this is not a continuous milling path.

Event 7 — The Circular Pocket

  1. "Select Event". You press POCKET PROFILE soft key for Event 7.
  2. "Select". You press CIRCLE PCKT soft key because our pocket is circular.
  3. "X Center". You press 1.5, ABS SET.
  4. "Y Center". You press 2.5, ABS SET.
  5. "Z RAPID". You press 0.1, ABS SET.
  6. "Z END". You press -0.125, ABS SET.
  7. "Radius". You press .75, ABS SET defining the radius of the pocket.
  8. "Direction". You press 2, ABS SET to select counter clockwise tool motion.  (Climb milling is preferred.)
  9. "# PASSES". You press 1, ABS SET. Please reference the 2OP mill guide to understand what this value changes.
  10. "ENTRY MODE". You press 1, ABS SET. The Zigzag Ramp to decreases stress on the tool by ramping down to the Z-depth.
  11. "Fin Cut". You press .02, ABS SET to select a finish cut of .020 inches. When machining, the program will hog out the pocket .020 undersized then make a finish cut pass to the proper size.
  12. "RPM". You press 4000, ABS SET.
  13. "FIN RPM". You press 5000, ABS SET. This is the speed during the finishing pass.
  14. "Z FEEDRATE". You press 10, ABS SET.
  15. "XYZ FEEDRATE". You press 20, ABS SET.
  16. "FIN FEEDRATE". You press 10, ABS SET (the finishing feed rate doesn't have to be the same as the roughing feed rate).
  17. "Tool #". You press ABS SET.
  18. "Tool Dia." You press ABS SET.

Event 8 — The Rectangle Profile

  1. "Select Event". You press POCKET PROFILE soft key for Event 8.
  2. "Select". You press RECT PROFILE soft key for the rectangular frame.
  3. "X1". You press 3.75, ABS SET which is the distance to corner number 1, which we will say is the lower left corner of the frame.
  4. "Y1". You press 1.75, ABS SET.
  5. "X3". You press 1.5, INC SET because corner number 3 is the diagonal corner and it is 1.5 inches in the plus X direction from X1.
  6. "Y3". You press 1.25, INC SET.
  7. "Z RAPID". You press 0.1, ABS SET.
  8. "Z END". You press -0.125, ABS SET.
  9. "CONRAD". You press .3, ABS SET because the corner radius of the frame is .300 inch.
  10. "Direction". You press 2, ABS SET to choose counterclockwise.  (Climb milling is preferred.)
  11. "Tool Offset." You press 2, ABS SET because when the tool moves counterclockwise around the inside of the rectangle frame, it is to the left of the work piece.
  12. "# PASSES". You press 1, ABS SET.
  13. "Fin Cut". You press .02, ABS SET to select a .020 inch finish cut.
  14. "RPM". You press 4000, ABS SET.
  15. "FIN RPM". You press 5000, ABS SET.
  16. "Z FEEDRATE". You press 10, ABS SET.
  17. "XYZ FEEDRATE". You press 20, ABS SET.
  18. "FIN FEEDRATE". You press 10, ABS SET.
  19. "Tool #". You press ABS SET because we're still using tool number 11.
  20. "Tool Dia." You press ABS SET.

Look at the Program

    1. Press the LOOK hard key to see what your program looks like. To access this function you may have to use the EHW to scroll backwards to find the LOOK button. You don't have to finish the programming to see what you've done so far.

The drawn part should look like this:

drawn part

If your part draw doesn't look like this, don't panic. The four pluses in the lower right side of the part may be squares (depending on the software version of the controller you're using), that's ok. For any other differences, see if you can figure out what piece of geometry, and therefore what event looks wrong. Go back to that part of your program and check your inputs against these instructions.

If the ProtoTRAK refused to draw your part and indicated a data error, read the explanation and solution and it will suggest the way to resolve the problem.

Program Run Preparation

Setup the Tool Table

  1. Setup your tools in their necessary tool holders. Reference the mill guide on the standard procedure for this step, here.
  2. Fill in the Z Offset values for each tool within the tool table. Reference the mill guide, here.

Setup the Work piece

Place a set of 1-1/2" parallels in the vise on edge with one parallel against the solid jaw and one parallel against to the movable jaw. (This will insure the material is above the vise.)  Place the HDPE material on top of the parallels as shown bellow and tighten the vise. Using a dead blow hammer lightly tap the material down onto the parallels. It is fine if the parallels are still slightly loose. (The material may not be uniformly flat) Make sure the material sticks out to the left of the vise by about 1-1/2".

setup

Set up the Part Reference

  1. Press MODE and select DRO soft key.
  2. Be sure the display reads the absolute position (ABS), indicated next to the position values.
  3. X and Y ABS SET should be used to zero the DRO. Use the edge finder to position the center of the spindle over the lower left corner of your part. Run the edge finder at 1000 rpm.
  4. The read out should display X 0.0000 ABS and Y 0.0000 ABS when the spindle is over the lower left corner.
  5. Retrieve Tool #9 so that it's in the spindle. Confirm on the top right of the DRO that the machine knows TOOL #9 is in the spindle, if not, see staff for assistance. Also confirm this is the spot drill.
  6. Grab a piece of paper and measure the thickness using calipers. Next, bring the spot drill down towards the top of the part. As the spot drill gets close wiggle a piece of paper between the part and spot drill until the paper just snags. You can then set your Z value to the thickness of paper about ( 0.004). This will set our Z zero to be the top of the part.

Program Run

Jump to Table of Contents

Note: You must use Traking at the beginning of every new tool. Traking allows you to safely check that all your Z offset values are correct. As the tool gets close to the top of the part, the DRO should read close to zero.

Enter the Run Mode

  1. Before beginning learn how and when the Traking feature is used, here.
  2. Press MODE and select RUN soft key.
  3. The conversation line says, "Select". You press START soft key. The START EVENT # soft key allows you to start in the middle of a program, but we don't want you to do that.
  4. Press Traking and using the EHW, you will start the program.

Part B

Jump to Table of Contents

Part B is to be completed on your own. Use what you have learned from Part A and the 2OP mill guide.

    Hint # 1: Your (0,0,0) should be the point which most/all dimensions come from.

    Hint # 2: This part should be made in one continuous cut.

    Hint # 3: You still haven't learned much about conrads.

    Hint # 4: You already have the end mill setup in the tool table.


KeywordsCNC, Mill 1, 2nd OP, 2 op, 2OP, mill, upgrade, conversational, programming, intro   Doc ID133151
OwnerSam B.GroupTEAM Lab Docs
Created2023-12-04 12:05:47Updated2024-01-19 14:13:16
SitesTEAM Lab Documentation
Feedback  2   0