Reference Tool

Jump to Table of Contents

The reference tool (similar to or the same as what is shown above), used with a tool setter, is used to set the tool setting reference position.

Tool Setter

Jump to Table of Contents

The tool setter is used to set the reference tool, all tool offsets, and the Z-zero reference off the top of the part.

Tool Holders and Tool Holder Setup

Jump to Table of Contents

The Trak DPM SX2 uses the R8 collet system. This is the same system used on the Eisen manual mills. Tool holders are pictured below:

Drill Bits

Jump to Table of Contents

For drill bits, they can be secured in a non-keyed drill chuck, but they must be bottomed out in the chuck (as far as they can go in the chuck).

If it is not possible to bottom out the drill bit in the chuck without clamping on the cutting surface, use a smaller drill chuck, a collapsible collet (same size as shaft diameter), or a keyed drill chuck to ensure that it is secure in the holder.

For a keyed drill chuck (used for tool #4: ¼” drill bit in this training), hand tighten the chuck on the tool. Then, use the key to tighten your tool in the chuck with all three key holes (across from each jaw) on the chuck (shown below).

 

End Mills

Jump to Table of Contents

End mills must be securely fastened in a collet or solid style holder that is the same size as the shaft of the end mill.

Use the tool holder block and collet wrench below to tighten collapsible collets.

Before tightening the collapsible collet (used for tool #3: ⅜” spot drill in this training), make sure that the collet is seated all the way into the holder and not at an angle (see a properly seated collet below). This could damage the collet or it could cause the tool to not be tightened properly in the holder if it is not seated properly.

Solid style holders will be used for tool #1: ½” end mill, tool #2: ⅜” end mill, and tool #5: ¼” end mill in this training. Solid style holders use a set screw that needs to be located on the flat of the end mill’s shaft.

It is easiest to remove the set screw, locate the flat, line up the flat with the tapped hole for the set screw, and then screw the set screw back in. (Note: The set screw should not be flush with the holder or raised out of the holder. It should be set in some if secured properly.)

Other Tools (Without a Flat)

Jump to Table of Contents

Other tools like spot drills and countersinks without flats or long shafts will need to be secured in a collapsible collet or a keyed drill chuck to secure them from moving in the Z-axis or loosening in the tool holder.

Tool Holder Block

Jump to Table of Contents

All tools should be tightened in the tool holder using the tool holder block shown below.

This block should be secured tightly in the vise so that it is tightened as much as you possibly can. Otherwise, you risk it being too loose and the wrench or other tools for tightening tool holders slipping while trying to tighten tools.

Make sure to face the slot on the tool holder block forward when securing it in the vise.

Line up the slot on the tool holder with the slot on the tool holder block so the holder locates inside the holder block.

Overview of Order of Operations

Jump to Table of Contents

The following procedure is for general machine operating use.

For the purposes of this training, you will be using the same general procedure with some repeated steps since you are going to run both a 3-axis and 2-axis program.

When running multiple different programs as in this training, you may need to repeat 2 vs 3-axis selection, conversational vs DXF file program, Z-zero location, and/or the procedure for running your program.

1. Start Up

2. Select 2 or 3-Axis machining option

3. Select whether you will be Conversational Programming or DXF File Conversion

4. Set Tool Change Reference Position (for 3-axis)

5. Set up TOOL TABLE

   1. Set Tool Setting Reference Position and tool offsets (for 3-axis program with multiple tools)

   2. Set tool diameters and description (for any 2- or 3-axis program)

   3. Note: This can be set up ahead of time for ALL programs that you intend to run, regardless of whether you will run both 2-axis and/or 3-axis programs. This is what is done in this training.

6. Set program origin on stock

7. Set Z-zero location on stock

8. Run your Program

9. Shutdown

Start Up Procedure

Jump to Table of Contents

1. Rotate the ON/OFF switch (shown below) located on the back of the machine to the ON position.

2. Flip the toggle switch for computer ON/OFF located on the right side of the control panel to the UP (ON) position.

3. Press the CHECK SYSTEM button when the screen turns on. Please note that this is not a touch screen. Use the soft buttons located below the display.

The Trak DPM2 is now ready to run!

3-Axis Selection

Jump to Table of Contents

1. To switch between 2 & 3 axis modes, press the soft key labeled SYS located on the far left side of the pendant. It doesn't look like a button, just the letters SYS.

2. For the purpose of the first part of the program, you will be in 3 axis mode of operation.

   1. If it says GO TO 3 AXIS on the bottom of this screen (as shown below), press the soft key and it should change to GO TO 2 AXIS. You should now be in 3 axis mode of operation.

2. If it says GO TO 2 AXIS on the bottom of this screen (as shown below), it should already be in 3 axis mode of operation.

3. To escape this screen, press MODE and DRO.

4. If you look at the top of the screen while in DRO, you will be able to see if you are in 3 axis mode of operation (as shown below).

Basic Machine Operation

Jump to Table of Contents

The following operations can be accessed by going to MODE and then DRO. The DRO screen is pictured below:

JOG

Jump to Table of Contents

Follow along with the instructions below:

1. You can move the X, Y, and Z manually, if desired. Press the JOG soft key to activate jogging the axes at a specific feed rate.

   1. Note: The JOG feature appears in several other modes that require Z-axis movement such as in SETUP > TOOL TABLE > JOG and has the same operation as in DRO > JOG.

2. A flashing message will appear in red saying CAUTION: JOG KEYS ARE ACTIVE (shown below).

3. To jog, press the X, Y or Z hard keys (shown above). To stop jogging, release the key. Note that the X and Y handles do not fold in, but they will not spin as you press the keys to JOG.

   1. Note: If you hold down one of these hard keys and press the button on the handheld pendant, you can release the key and hold the button on the handheld pendant to continue jogging in that axis. Release the button on the handheld pendant to stop jogging.

4. The feed rate, or speed, of JOG is displayed in the box next to the words Feed Rate (shown below) on the lower left side of the screen.

   1. Press the +/- hard key to reverse direction. When the number in the Feed Rate box is negative, this indicates the negative direction.

5. Setting the feed rate

   1. Using Override: You may override the feed rate with the OVERRIDE display hard key.

      1. Press the F / S key until the LED above the F (for Feed rate) is lit, if it is not already.

      2. Use the up/down arrows to increase/decrease the JOG speed in 10 percent increments.

         1. The changes in feed rate may be seen in the Feed Rate box.

         2. The amount of override is displayed in the Override box.

   2. JOG at a certain rate:

      1. Enter the number for the desired feed rate as inches or mm per minute, and then press the X, Y or Z key.

      2. Note: You can use the override operation described above to adjust this number.

To exit JOG, press the RETURN key at the bottom right.

DO ONE

Jump to Table of Contents

DO ONE in the DRO mode allows you to do one CNC operation while machining manually without having to write a program. Make sure to set up the TOOL TABLE and REF POSN before using DO ONE.

The programming and tool path of the events in DO ONE are nearly identical to those in the Program Mode.

To exit DO ONE, select MODE and then DRO to return to the DRO screen.

GO TO

Jump to Table of Contents

The GO TO function in the DRO mode allows you to set a dimension in X or Y at which you want the machine to stop moving when you are manually moving the machine.

• For example, if you wanted to machine manually from your current position to exactly 2" from the X-zero, you would input: GO TO, X, 2, ABS SET. While the GO TO window is displayed, the ProtoTRAK SMX will not let you pass that 2" dimension you set.

1. Press the GO TO key.

2. Enter the axis (X, Y, or any combination). Input the dimension(s).

3. Press INC SET or ABS SET.

4. Crank the handwheel. Motion will stop at the entered dimension even if you continue to crank the handwheel.

To exit GO TO, press the RETURN key at the bottom right.

Spindle Operation

Jump to Table of Contents

Spindle speeds are set and adjusted through the controller. They are set either directly in the program for any speed used during program RUN or using this SPIN SPEED feature for any speeds used in DRO mode.

Follow along with the instructions below:

1. To set spindle speed, press the SPIN SPEED softkey.

2. The Data Input Line will prompt “Spindle RPM”.

3. Enter an RPM value between 300 and 5000 (for high gear) and press ABS SET.

   1. If you enter a value outside of the range, there will be a yellow error message. Enter a speed in the range for the error message to disappear, or check that you are in the correct gear for your RPM range.

   2. Note: If the spindle was already on when you began to enter the new speed, it will stay at the current speed until you press the ABS SET key.

   3. If you need to use the low gear range of 40 to 600 RPM, see pro-staff about setup and operation.

4. You can also override the spindle speeds with the OVERRIDE display hard key.

   1. Press the F / S key until the LED on the S (for Spindle) side is lit.

   2. Use the up/down arrow keys to increase/decrease the spindle speed in 5% increments per button press.

To exit SPIN SPEED, press the RETURN key at the bottom right.

Tool #

Jump to Table of Contents

To change tools, press the TOOL # soft key and enter the tool number when prompted by the Data Input Line.

To exit TOOL#, press the RETURN key at the bottom right.

Power Feed

Jump to Table of Contents

The servo motors can be used as a power feed for X, Y, and Z-axes.

1. Prior to using POWER FEED, set your RPM with SPIN SPEED.

2. Press the POWER FEED soft key.

3. Bring the spindle down about an inch with the quill handle and lock it.

4. A green message box will appear that shows the power feed dimensions. All power feed moves are entered as incremental moves from the current position to the next position.

   1. If you try to enter a power feed dimension with ABS SET instead of INC SET, the value will not appear in the green message box until you select INC SET.

5. Enter a position by pressing the axis key, the distance to go and the +/- key (if needed to travel in the negative direction). Input the entry by pressing INC SET.

   1. For example, if you wanted to make a power feed move of 2.00" in the negative Z-direction (i.e. move down in the Z-axis), you would enter: Z, 2, +/-, INC SET.

6. Turn the spindle on.

7. The feed rate is automatically set to 10 ipm (or 254 mm per min). Use Feed rate Override up/down arrows to adjust the feed rate to any value from 1 ipm to 100 ipm (25 to 2540 mmpm).

8. Initiate the power feed move by pressing GO on the handheld pendant.

   1. Note: Any power feed move beyond the first programmed movement will not be initiated by the first button press, you will need to press GO on the handheld pendant again.

9. Once the power feed move is initiated, you will see the dimension you entered disappear from the message box and the DRO values on the screen will start changing to your programmed incremental dimension.

10. You can adjust your spindle speed or feed rate using the OVERRIDE keys as needed.

11. Press STOP to halt power feed. Press GO to resume.

12. Press RETURN soft key to return to DRO.

To exit POWERFEED, press the RETURN key at the bottom right.

Return to Absolute Zero

Jump to Table of Contents

This section is meant to inform you about this feature and that it is available to you. No need to follow along with these directions.

At any time during manual DRO operation, you may automatically move to your absolute zero location in X and Y and your Z RETRACT location by pressing the RETURN ABS 0 soft key.

When you do, the message window will read "Ready to Begin. Press Go when Ready.” Make sure your tool is clear, press GO on the handheld pendant, and hold on to the pendant to press STOP quickly if things go wrong.

The servos will turn on, move the Z-axis to Z retract (this is set in REF POSN - see Tool Change Reference Position), and then move at rapid speed to your X and Y absolute zero position, and then turn off. You will be at ABS 0 while in manual DRO operation.

When you are in 2-axis CNC operation, only the X and Y-axes will move and the Z-axis will not.

To exit RETURN ABS 0, press the RETURN key at the bottom right.

Programming the Part

Jump to Table of Contents

Material

4” x 6” HDPE stock

Tools

• 3-Axis Program

  • Tool # 1: ½” Diameter 2-Flute Center Cutting End Mill

    • Holder 1: ½” Solid-Style Holder with Set Screw

  • Tool # 2: ⅜” Diameter 2-Flute Center Cutting End Mill

    • Holder 2: ⅜” Solid-Style Holder with Set Screw

• 2-Axis Program

  • Tool # 3: ⅜” Spot Drill

    • Holder 3: ⅜” Collapsible Collet 

  • Tool # 4: ¼” Drill Bit

    • Holder 4: Keyed Drill Chuck

• DXF Program

  • Tool # 5: ¼” Diameter 2-Flute Center Cutting End Mill

    • Holder 5: ⅜” Solid-Style Holder with Set Screw

• 1-½” Parallels

• Edge Finder

• Deburring Tool — Swivel Type

• 6" Rule
• Caliper

Setting Up Tools in the Tool Holders

Jump to Table of Contents

Place the tools in the holders noted in the section above (shown above). See the description of tools above to use the proper tools to tighten them and to set the tools in the holders properly.

See proper use for the tool holder block (tightened in the vise as much as you can) below:

Program Part Number

Jump to Table of Contents

1. Go to MODE, and then PROG to start programming.

2. Select HELP to select the blue question mark to bring up the keyboard on the screen to name your program.

   1. Letters and Characters

      1. Use the up, down, right, and left arrow soft keys to navigate to a letter or character.

      2. Select the ENTER soft key to select the letter or character.

   2. Numbers are still on the number pad on the controller.

3. Select the END soft key to enter the program name.

4. Select GO TO BEGIN to start the program.

3-Axis Milling Program

Jump to Table of Contents

Below is the part drawing of what you are programming the machine to make. This will be done in two programs: a 3-axis program for all milling events and a 2-axis program for all drilling events.

Conversational Program Part Drawing

Event 1 - The Upper Left Diagonal

1. Select PAGE FWD to get to the end of the program and add a new event. Select the MILL soft key.

2. X BEGIN: 0, ABS SET

3. Y BEGIN: 3.25, ABS SET

4. Z RAPID: 0.5, ABS SET

   1. This is the Z-value where your tool will slow down from rapid and begin moving towards the part at the programmed feed rate and where your tool will go prior to all other events as it rapids across the part. This value is set to make sure your tool does not crash into any part features during these rapid movements.

5. Z BEGIN: -0.125 ABS SET (Z depth at the programmed beginning position)

6. X END: 0.5, ABS SET

7. Y END: 0.75, INC SET

8. Z END: 0, INC SET (Z depth should not change from beginning to end)

9. CONRAD: 0, ABS SET (no conrad)

10. TOOL OFFSET: 2, ABS SET (offset to the left)

11. RPM: 1100, ABS SET

12. Z FEED RATE: 5, ABS SET

    1. This is the plunge feed rate of the Z-axis.

13. XYZ FEED RATE: 5, ABS SET

    1. This is the feed rate that the X and Y-axes will move.

14. TOOL #: 1, ABS SET

Check your first 3-axis event with the image below:

Event 2 - The Lower Left Radius

1. Select the ARC soft key.

2. X BEGIN: 0, ABS SET

3. Y BEGIN: 0.5, ABS SET

4. Z RAPID: 0.5, ABS SET

5. Z BEGIN: -0.125 ABS SET (Z depth at the programmed beginning position)

6. X END: 0.5, ABS SET

7. Y END: 0, ABS SET

8. Z END: 0, INC SET (Z depth should not change from beginning to end)

9. X CENTER: 0.5, ABS SET

10. Y CENTER: 0.5, ABS SET

11. Z CENTER: 0, INC SET (Z depth should not change from beginning to end)

12. CONRAD: 0, ABS SET

13. DIRECTION: 2, ABS SET (CCW)

14. TOOL OFFSET: 1, ABS SET (offset to the right)

15. RPM: INC SET (same tool so same RPM)

16. Z FEED RATE: 5, ABS SET

17. XYZ FEED RATE: 5, ABS SET

18. TOOL #: INC SET (still using tool 1)

Event 3 - The Circular Pocket

1. Select POCKET soft key, then select CIRCLE PCKT.

2. X CENTER: 1.5, ABS SET

3. Y CENTER: 2.5, ABS SET

4. Z RAPID: 0.5, ABS SET

5. Z END: -0.125, ABS SET

6. RADIUS: 0.75, ABS SET

7. DIRECTION: 2, ABS SET (CCW)

8. # PASSES: 1, ABS SET

9. ENTRY MODE: 2, ABS SET (to set PLUNGE)

10. FIN CUT: 0.02, ABS SET

11. RPM: 1500, ABS SET

12. FIN RPM: 1500, ABS SET (keep the same RPM for finish pass)

13. Z FEED RATE: 5, ABS SET

14. XYZ FEED RATE: 8, ABS SET

15. FIN FEED RATE: 8, ABS SET

16. TOOL #: 2, INC SET

Event 4 - The Rectangle Profile

1. Select the PROFILE soft key, then select RECT PROFILE.

2. X1: 3.75, ABS SET

3. Y1: 1.75, ABS SET

4. X3: 1.5, INC SET

5. Y3: 1.25, INC SET

6. Z RAPID: 0.5, ABS SET

7. Z END: -0.125, ABS SET

8. CONRAD: 0.3, ABS SET

9. DIRECTION: 2, ABS SET (CCW)

10. TOOL OFFSET: 2, ABS SET (offset to the left)

11. # PASSES: 1

12. FIN CUT: 0.03, ABS SET

13. RPM: INC SET (same tool so same RPM)

14. FIN RPM: INC SET (keep the same RPM)

15. Z FEED RATE: 5, ABS SET

16. XYZ FEED RATE: 5, ABS SET

17. FIN FEED RATE: 5, ABS SET

18. TOOL #: INC SET (still using tool 2)

LOOK for 3-Axis

Jump to Table of Contents

Press LOOK to see the graphical representation of your cutter paths. It gives you the ability to see your cutter paths in the XY, YZ, and XZ planes, as well as 3D.

Once the program is complete, make sure that your part looks like the image below when in the LOOK page:

Tool Change Reference Position

Jump to Table of Contents

1. Press the MODE, SET UP, and REF POSN to set the tool change reference location.

2. Bring the spindle down about an inch with the quill handle and lock it. This is meant to prevent issues with accidental crashes as mentioned in the note above in the section on JOG.

3. Hit the JOG soft key (located directly in REF POSN - this feature operates the same as described above) and manually move the Z-axis to a safe location for changing tools in and out of the spindle.

   1. Note: The Z-axis position should allow enough room for your longest tool to easily clear the top of the part when it is being inserted into the spindle.

4. Press RETURN once you have moved the Z-axis in the position you want. The reference position page should appear back on the screen.

5. Use the DATA FWD/DATA BACK soft keys to highlight the words NOT SET if not already highlighted, and press ABS SET. Notice it changes to SET and the cursor automatically moves to X HOME.

6. The X HOME and Y HOME can be left as 0” ABS since the Z RETRACT has been set to allow enough room for tool changes.

The REF POSN page should look like the below image after completing the previous steps:

The DPM2 will now move to this programmed X, Y, and Z location each time a tool change is called for in a program.

Press MODE to exit the Tool Change Reference Position page.

When in 2-axis mode, you will NOT see Z Retract, X HOME, or Y HOME as described above.

Tool Setting

Before setting any tool length offsets, you must set a Tool Setting Reference Position. This reference position sets a zero reference for all tool offsets. These tool offsets and the Z-zero for the first tool in your program are then used to calculate Z-zero for every tool. You will need the reference tool and the tool setter to set this.

Setting the Tool Setting Reference Position

Jump to Table of Contents

1. Press MODE, SETUP, and then TOOL TABLE.

2. Load the reference tool into the spindle.

3. Bring the spindle down about an inch with the quill handle and lock it.

4. Make sure the tool setter block and vise are clean.

5. Set the tool setter on the solid jaw (back jaw) of the vise so that it is sitting flush on the solid jaw and the digital readout is visible (proper placement shown below).

6. Align the reference tool directly over the tool setter using the X and Y-axis handwheels with FINE feed.

7. Use JOG (located directly in the TOOL TABLE page) to move the Z-axis down until the reference tool is within 3” to 4" of the top of the tool setter.

8. Hit RETURN to take the machine out of JOG mode.

9. Use the manually operated quill feed lever to carefully lower the reference tool until the digital readout reads 0 (shown below).

10. Lock the quill in place when the reference tool is properly set on the tool setter.

11. Make sure the cursor is highlighting the words NOT SET under the Z offset column and press ABS SET.

12. It should now read SET under the Z offset column.

13. Manually raise the quill handle so the tool is above the tool setter by about 3” to 4”.

Setting Multiple Tools for 3-Axis

Jump to Table of Contents

1. The cursor should be at the REF 1 position, all the way to the left under the DIAMETER column.

   1. If it is not, use the DATA LEFT/RIGHT and DATA UP/DOWN keys to move the cursor to this position.

2. Enter the diameter of the tool and press ABS SET. You should now see the diameter you entered displayed in the REF 1, DIAMETER column.

3. The cursor should automatically move to the right, highlighting the Ref 1, Z OFFSET column.

4. Press JOG. Use JOG to move the Z-axis up until you can safely remove the reference tool and load tool #1.

5. Bring the spindle down about an inch with the quill handle and lock it.

6. Use JOG to move the Z-axis down until the tool is within 3” to 4" of the top of the tool setter.

7. Hit RETURN to take the machine out of JOG mode.

8. Use the manually operated quill feed lever to carefully lower the tool until the digital readout reads 0.

9. Lock the quill in place when the tool is properly set on the tool setter.

10. Make sure the cursor is still in the REF 1, Z OFFSET column.

11. Press ABS SET, and the Z-offset value will automatically be loaded into the REF 1, Z OFFSET column.

12. The cursor will again move to the right, highlighting the Z MODIFIER column. Pressing the ABS SET key will load this column with zeros and move the cursor to the right.

13. You will now see a small green pop-up window containing a table of 14 different tool types. Enter the number which best describes the tool you currently have in the spindle, followed by ABS SET. A description of the tool will appear on the screen under the REF 1, TOOL TYPE column.

    1. For example: You have an end mill in the spindle, enter the number 3 for a roughing end mill, followed by ABS SET. Rough end mill should now appear in the REF 1, TOOL TYPE column.

14. Manually raise the quill handle so the tool is above the tool setter by about 3” to 4”.

15. Press JOG and move the spindle up high enough to remove tool #1 and load tool #2.

16. Manually raise the quill handle all the way up to complete the tool change and lock the quill.

17. Repeat the process for the other end mill under REF 2 (skipping step 2)

Setting Tools for 2-Axis and DXF

Jump to Table of Contents

For the 2-axis portion of this training, you will be drilling the holes. Drilling holes is faster in 2-axis than it is in 3-axis (unless you have a lot of holes to drill).

You will also be using the DXF File Converter in this training in 3-axis. Since this is a one tool program, you don’t need the Z OFFSET for this tool. You will set Z-zero later.

You will set up these tool diameters and descriptions in the tool table now so that you can call those tool numbers when programming the 2-axis portion of this training.

1. Remain in 3-axis mode of operation while setting up this portion of the tool table. All values will remain in the TOOL TABLE after switching from 3 to 2-axis (or vice versa), starting a new program, or loading a new DXF file.

2. Make sure you are in the TOOL TABLE page.

3. Move the cursor to the REF 3 position, all the way to the left under the DIAMETER column.

4. Enter the diameter of the tool and press ABS SET. You should now see the diameter you entered displayed in the REF 3, DIAMETER column.

5. The cursor should automatically move to the right, highlighting the REF 3, Z OFFSET column. Press the DATA RIGHT key to advance to the Z MODIFIER.

   1. Note: The Z MODIFIER column does not appear in 2-axis mode of operation, only 3-axis.

6. Pressing the ABS SET key will load this column with zeros and move the cursor to the right.

7. You will now see a small green pop-up window containing a table of 14 different tool types. Enter the number which best describes the tool you currently have in the spindle, followed by ABS SET. A description of the tool will appear on the screen under the REF 3, TOOL TYPE column.

8. Repeat the process to enter the information for the drill under REF 4 and the ¼” end mill (used for the DXF program) under REF 5.

Check your final tool table setup against the image below. Note that your offset values will be different.

Part and Tool Path Verification

Below are two additional methods of verifying your part and the tool path that it is going to take prior to running your program. They can only be used for verification after setting up the tool table.

TOOL PATH

Jump to Table of Contents

Select the SET UP soft key and then select TOOL PATH.

TOOL PATH is similar to LOOK except it allows you to see the path that the tools will take during your program rather than just the outline of what your program looks like.

You can change the view of this from XY, YZ, XZ, or 3D to see the tool path from different perspectives. Selecting the STEP soft key allows you to step through the path that the tools will take.

VERIFY PART

Jump to Table of Contents

Another way of viewing the tool path and part is VERIFY PART (only available on Trak DPM2 - 2). This feature is located in SET UP. See the procedure below for verifying the part:

1. Select SET UP, and then VERIFY PART.

2. Select DEFINE STOCK.

   1. Define your stock to have the same zero reference in all axes as the program you intend to run. Adjust the size to be that of your actual stock.

   2. X MIN: 0 ABS, Y MIN: 0 ABS

      1. Lower left of stock

   3. Z MIN: -0.5 ABS (bottom of stock)

   4. X MAX: 6 ABS, Y MAX: 4 ABS

      1. Upper right of stock

   5. Z MAX: 0 ABS (top of stock)

3. Select RETURN to escape this screen

4. Select MAKE PART to go into the simulation.

   1. You have the option to view this in 3D, XY, XZ, or YZ. 3D will work best for this part.

 

5. Select VERIFY PART to see the simulation of the program running with the tool.

   1. SHOW PART will not go through the simulation. It will just show the end result.

 

6. Select EXIT to escape this screen and return to SET UP.

Setting up the Stock

Jump to Table of Contents

Place the stock on 1-½” parallels with about 1-½” of the stock out of the left of the vise for milling the upper corner and the arc at the bottom left.

Zero Location

Jump to Table of Contents

Setting X & Y Axis Zero

1. Use an edge finder loaded into a drill chuck to find the lower left corner of the stock and set this as your X and Y zero locations.

2. Bring the spindle down about an inch with the quill handle and lock it.

3. Press DRO, then SPIN SPEED.

4. Enter an RPM between 600 and 800 and press ABS SET.

Use JOG (make sure that you exit JOG before setting any axis to zero) and the X and Y-axis handwheels in COARSE mode (LED above the C on the F/C button is lit) to get within a few inches of the part.

Use the X and Y-axis handwheels in FINE mode (LED above the F on the F/C button is lit) and manual quill feed lever for fine adjustments. You risk crashing into the part or vise if you don't, which could damage the tool and/or spindle.

Setting Z-Axis Zero for 3-Axis Program

Jump to Table of Contents

1. Load Tool # 1 into the spindle.

2. Press MODE, DRO and TOOL #. Enter 1 followed by ABS SET. You should see TOOL #1 in one of the boxes near the top right side of the screen.

   1. DO NOT continue if you don't see TOOL #1 appear! Ask pro-staff for assistance.

3. Bring the spindle down about an inch with the quill handle and lock it.

4. Use JOG to move the tool down to within 3" to 4" of the top of the workpiece.

5. Press RETURN to stop jogging at this point.

6. Place the tool setter on the top of the part.

7. Bring the tool down with the quill handle so that the setter reads 0 on the digital readout and lock the quill.

8. (Make sure that you are indeed out of JOG at this point since pressing the Z-axis button in JOG could ruin the setter or tool.) Press the Z-axis button, enter 2” for the thickness of the setter, and then ABS SET while in the DRO page to set your Z-axis zero point. This will already account for the height of the setter so the tool will actually be set to Z-axis zero on the top of the part (as shown below).

9. At this point, you can set a stop (shown below) about an inch from the top for the tools in your 3-axis program. This is the stop where all tools will be lowered to after the tool change. This helps prevent an excessive quill travel error and keeps the tool rigid while machining.

10. Move the tool so it is off the part, and make sure the quill is locked tight against the stop.

Running 3-Axis Programs

Jump to Table of Contents

1. To run your program, press MODE, RUN, START and then TRAKing.

2. Use TRAKing until you verify the Z Offset for the first tool as described below.

   1. When running your program, you must use TRAKing after every tool change.

      1. TRAKing allows the operator to control the feed using the X and Y-axis handwheels.

         1. The X-axis handwheel is the coarse feed.

         2. The Y-axis handwheel is the fine feed.

2. To verify Z offset for the tool, check to see that the tool tip reaches the top of the part when the readout reads about 0.

• If there is an existing hole or feature that prevents you from seeing when chips are first cut, try to visually look at it from eye-level to make sure it is lined up close to the top of the part at where the DRO reads about 0.

3. If the value is far off from 0, reset it in the TOOL TABLE.

2. Note what the machine will do while running TRAKing:

   1. The machine will go to your programmed tool change position from REF POSN, and then prompt you to change the tool and start the spindle.

   2. The spindle will initially not be at your programmed RPM until you start TRAKing with the handwheels or you start CNC Run.

   3. The X and Y will move to your programmed start point.

3. Once verified, run the program in CNC RUN until the next tool change. Go to CNC RUN via one of these options:

   1. Press STOP on the handheld pendant, press CNC RUN, and then press GO on the handheld pendant.

   2. Double click the button on the top of the handheld pendant.

4. When the first two events are complete you will be prompted for a tool change. Complete the tool change.

5. After the tool change, cycle the spindle switch OFF (0) then ON (2 - FWD) again.

6. Select TRAKing, not CNC RUN. Verify the Z Offset for this tool with TRAKing.

7. Once the Z Offset is verified, run the remainder of the program in CNC RUN until it says RUN OVER.

Hold on to the handheld pendant while running your program in CNC RUN mode to press STOP quickly if things go wrong.

See the key features in RUN below:

• START EVENT # allows the operator to start at a known event number.

• TRIAL RUN allows you to quickly check out your program with no Z movement before you actually start to make parts.

• The table will move at rapid speed regardless of what feed rates are programmed (the rapid speed may be overridden with the up/down arrows).

• The table will stop at each "stop" location (for example, at each drill location) but immediately continue on without your input.

• Warning: Ensure that the z-axis is high enough above the stock to avoid hitting it and run a trial run of your program.

2-Axis Drilling Program

DO NOT remove your part after running the 3-axis program. Otherwise, you will have to reset your X and Y-axis zero references with the edge finder.

2-Axis Selection

Jump to Table of Contents

1. For the second part of the program, you will be in 2-axis mode of operation. Press the SYS key to get to the screen to change to 2-axis.

2. It should say GO TO 2 AXIS on the bottom of this screen so press this soft key to switch to 2-axis (as shown below).

3. You will be prompted to confirm the change since it will erase the current program in memory. Select YES since you will now be programming the 2-axis drilling program.

4. It should change to GO TO 3 AXIS. You should now be in 2 axis mode of operation (as shown below).

5. To escape this screen, press MODE and DRO.

6. If you look at the top of the screen while in DRO, you will be able to see if you are in 2 axis mode of operation (as shown below).

Program Part Number

Jump to Table of Contents

1. Go to MODE, and then PROG to start programming.

2. Select HELP to select the blue question mark to bring up the keyboard on the screen to name your program.

   1. Letters and Characters

      1. Use the up, down, right, and left arrow soft keys to navigate to a letter or character.

      2. Select the ENTER soft key to select the letter or character.

   2. Numbers are still on the number pad on the controller.

3. Select the END soft key to enter the program name.

4. Select GO TO BEGIN to start the program.

Event 1 - Spot Drill the First Hole

1. Select the POSN DRILL soft key.

2. X: 2.75, ABS SET

3. Y: 0.75, ABS SET

4. RPM: 1500

5. TOOL #: 3

Check your first 2-axis event with the image below:

Event 2 - The Next 3 Holes

1. Select the MORE soft key, then SUB. Select the REPEAT soft key. You will be repeating this first hole with an X offset to program the remaining holes in the bottom right. This will be a subroutine event since you do not need to edit these events later.

2. FIRST EVENT #: 1, ABS SET

3. LAST EVENT #: 1, ABS SET

4. X OFFSET: 0.75, INC SET

5. Y OFFSET: 0, INC SET

6. # REPEATS: 3

7. % RPM: ABS SET for 100% (still using the same RPM)

8. % FEED: ABS SET for 100% (still using the same feed rate)

9. TOOL #: INC SET (still using tool 3)

Event 3 - The Bolt Hole Pattern

1. Select the BOLT HOLE soft key.

2. # HOLES: 8, ABS SET

3. X CENTER: 1.5, ABS SET

4. Y CENTER: 2.5, ABS SET

5. RADIUS: 1, ABS SET

6. ANGLE: 90, ABS SET

7. RPM: INC SET (same tool)

8. TOOL #: INC SET (still using tool 3)

Event 4 - Repeat to Drill Holes after Spot Drilling

1. Select the MORE soft key, then select SUB. Select the REPEAT soft key.

2. FIRST EVENT #: 1, ABS SET

3. LAST EVENT #: 3, ABS SET

4. X OFFSET: 0, INC SET

5. Y OFFSET: 0, INC SET

6. # REPEATS: 1, ABS SET

7. % RPM: ABS SET for 100%

8. % FEED: ABS SET for 100%

9. TOOL #: 4, ABS SET

LOOK for 2-Axis

Jump to Table of Contents

Once the program is complete, make sure that your part looks like the image below when in the LOOK page:

Setting Z-Axis Zero for 2-Axis Program

Jump to Table of Contents

1. Load Tool # 3 into the spindle.

2. Press MODE, DRO and TOOL #. Enter 3 followed by ABS SET. You should see TOOL #3 appear in one of the boxes near the top right side of the screen.

   1. DO NOT continue if you don't see TOOL #3 appear! Ask pro-staff for assistance.

3. Bring the spindle down about an inch with the quill handle and lock it.

4. Use JOG to move the tool down to within 3" to 4" of the top of the workpiece.

5. Press RETURN to stop jogging at this point.

6. Place the tool setter on the top of the part.

7. Bring the tool down with the quill handle so that the setter reads 0 on the digital readout and lock the quill.

8. (Make sure that you are indeed out of JOG at this point since pressing the Z-axis button in JOG could ruin the setter or tool.) Press the Z-axis button, enter 2” for the thickness of the setter, and then ABS SET while in the DRO page to set your Z-axis zero point. This will already account for the height of the setter so the tool will actually be set to Z-axis zero on the top of the part.

9. Bring the quill back up and remove the tool setter.

10. At this point, move the tool off to the side of the part and bring the quill down until it reads approximately -0.040” in the Z.

11. Lock the quill and set the stop at this point. Bring the tool up and then back down to make sure that it is still set at approximately -0.040”.

12. Once this is confirmed, bring the quill up until it is about an inch from the top and lock it.

Running 2-Axis Programs

Jump to Table of Contents

1. To run your program, press MODE, RUN, and START.

2. Like with 3-axis, you have the option to hit either GO or TRAKing at this point. Press GO on the handheld pendant or on the controller to start CNC RUN.

   1. There is no need to run TRAKing for 2-axis, but feel free to test out the feature if you are interested. You can exit TRAKing the same way you would in 3-axis.

   2. TRAKing in 2-axis allows you to move the X and Y-axes and check that the program is running as expected.

      1. Note: The Z-axis does not move. You will see prompts for SET Z and CHECK Z similar to the Eisen manual mill controllers in the shop.

   3. TRAKing allows you to control the feed using the X and Y-axis handwheels.

      1. The X-axis handwheel is the coarse feed.

      2. The Y-axis handwheel is the fine feed.

3. Please watch for prompts to move the Z-axis manually . Follow the instructions below for SET Z Prompts:

   1. Remember that CHECK Z means that the quill should be up and out of the way since it will rapid to the next location.

   2. Spot Drill:

      1. Spot drill the holes to the stop set at approximately -0.040”.

   3. Drill:

      1. With loading the drill bit, you will likely not have enough clearance while in RUN. Since JOG is not available, you will use the feature STEP Z to bring the tool up.

         1. WARNING: STEP Z uses STEP UP and STEP DOWN to control the Z-axis movement. This feature uses a default feed rate and default of 1” increments to move the Z-axis. Be careful when using this feature as this could be prone to crashes.

         2. Best practice: Always float the quill, bring the tool 3” to 4” above the part using STEP Z (no closer), and pay attention to the direction that you are going to move the Z-axis.

      2. Use STEP UP to have enough clearance to load the drill.

      3. Load the drill into the spindle.

      4. Use STEP DOWN to bring the tool 3” to 4” above the part (if needed), and hit RETURN to go back to the RUN screen.

      5. Press GO to move to your programmed position for the first drilled hole.

      6. Use the quill to bring the drill down to the spot drill point and set zero at this point (spindle OFF).

      7. Cycle the spindle switch OFF (0) then ON (2 - FWD), and drill the hole to a depth of approximately -0.085”.

      8. Bring the tool back up and lock the quill.

      9. Turn off the spindle.

      10. Bring the tool back down to the spot you just drilled. Set the stop at this point.

      11. Drill the remaining holes to this stop until you see the RUN OVER message.

START EVENT # allows the operator to start at a known event number.

DXF File Conversion Program

In this section, you will be using the DXF File Converter to make the part below (drawing is linked). You will need to use the mouse connected to the controller in order to select the profile and program ABS zero.

DXF Part Drawing

Introduction

Jump to Table of Contents

The ProtoTRAK SMX controllers on these machines have software installed on them that has the capability of converting DXF or DWG files to program events. Below is the profile you are going to be cutting (this is not the file you will be loading):

Switching to 3-Axis

Jump to Table of Contents

For this part of the program, you are going to return to 3-axis programming. This must be done prior to uploading your DXF file. Otherwise, you will have to reload the DXF file while in 3-axis mode.

See 3-Axis Selection above for a reminder on switching between 2-axis and 3-axis mode. If prompted to delete the current program in memory, select YES.

Uploading the File

Jump to Table of Contents

To upload your DXF file, go to PROG IN/OUT. You will see the screen below:

1. Select OPEN. An example of what the screen might look like is shown below.

2. You may need to navigate using TAB, DATA FWD, DATA BACK, and OPEN FOLDER to get to the drive and folder that has your file.

   1. If you are not currently in the right USB drive, select TAB until you are at the list of drives at the top of the screen. Use DATA FWD and DATA BACK to navigate to a new drive, and select OPEN FOLDER.

      1. If you switched two USB drives in the same port, you may have to navigate to the C: drive (computer drive for the controller) and back to the D: drive or another drive (shown below).

      2. If you plugged your USB drive into an open port, then you may need to select the E: drive or another drive in the list.

2. If you are in the right USB drive and your files are located in a folder, navigate to the folder your file is in using DATA FWD and DATA BACK and select OPEN FOLDER.

3. Use DATA FWD and DATA BACK to highlight the file from the USB drive that you would like to upload: DPM_DXF_File_NoConrads.DXF (shown below).

4. Select OPEN FILE.

Note the difference between this DXF file and the file shown above. The DXF file converter can have trouble reading conrads from the DXF. Instead, create your file without conrads. These conrads can be added later as you fill in missing event information.

Selecting the Profile

Jump to Table of Contents

At any point in this section, you have the ability to zoom in and out on the profile using the arrows located in the middle of the bar at the top of the screen (shown below).

To scroll up/down or left/right, use the scroll bar on the right and bottom of the screen showing the file (either full screen or on the left). Use your mouse to use these features.

1. Press the CONTINUE soft key.

2. You will be prompted to automatically close any gaps that are less than 0.005”. Select YES for this part.

3. You will select your program ABS zero. Select the C soft key for “C: Center of Arc or Circle”, and then select the arc that has a radius of 0.875” with the mouse. Once you select the arc, the center point will appear as a square with an X in it.

4. Press the CONTINUE soft key.

5. In this case, you don’t need to add a NEW POINT or NEW LINE. Press the CONTINUE soft key again.

6. Now, select the type of event. You will select PROFILE.

7. It will ask you if you want to chain. Select YES.

8. Select the entire profile starting with the 0.875” arc and then select below the lower left of the arc. This should select the entire profile.

9. Now that the entire profile (it will be blue instead of white) is selected and you are prompted to SELECT EVENT, select the EVENT button in the upper right corner of the screen (shown below).

As you will see, the software automatically enters this as an IRREGULAR PROFILE which requires all Z data, feed rates, RPM, and tool information to be entered into the first event.

Completing Events

Jump to Table of Contents

1. The 12 events will auto-populate with all the information from the DXF file.

2. For the first event that defines the irregular profile start, enter in the missing data lines with the following information:

   1. Z RAPID: 0.5, ABS SET

   2. Z END: -0.125, ABS SET

   3. TOOL OFFSET: 2, ABS SET (left)

   4. # PASSES: 1

   5. FIN CUT: 0, ABS SET

   6. RPM: 1500, ABS SET

   7. Z FEED RATE: 5, ABS SET

   8. XYZ FEED RATE: 5, ABS SET

   9. TOOL #: 5, ABS SET (This is the ¼” end mill that you entered into the tool table.)

3. Once the event has all of the missing information that it needs, it should read ALL OK (green box) instead of Not OK (red box) in the upper right corner. See the completed event below:

4. You will also add the value to the CONRAD data lines in the following events (reference the part drawing above for each CONRAD):

   1. EVENT 3: 0.125, ABS SET

   2. EVENT 4: 0.25, ABS SET

   3. EVENT 5: 0.25, ABS SET

   4. EVENT 9: 0.25, ABS SET

   5. EVENT 10: 0.38, ABS SET

   6. EVENT 11: 0.125, ABS SET

 See Event 3 completed with CONRAD information below:

Note that you will not be able to see the conrads until you end the DXF program and look at it in PROG.

5. Now select the EVENT button again to go back to the screen to select an event. Notice that the profile is now green (shown below).

6. Press the END DXF soft key in the bottom right corner, and select YES for the prompt below:

Verifying the Program

Jump to Table of Contents

Go to PROG (shown below for this program). Note that the program name appears as the name of the file.

 Then go to LOOK (shown below) to verify that your program looks correct.

You can also view TOOL PATH in SET UP to verify the path the tool will take.

Resetting Tool Change Reference Position

See Tool Change Reference Position above to reset your Z-Retract now that you have returned to 3-axis.

Setting up the Stock and Setting Zero References

Jump to Table of Contents

The stock can be flipped over and centered in the vise since you are cutting an internal profile.

Reset all of your zero locations.

For the X- and Y-zero, it is no longer at the bottom left corner. Instead, center the part in the stock with the center of the 0.875” arc as the X and Y-zero.

For the Z-zero, make sure to use TOOL #5 (¼” end mill) rather than TOOL #1 while resetting Z-zero with the tool setter in DRO since this is the tool that you will use in this program.

Don’t forget to set a stop about an inch from the top and bring the quill down tight against the stop and lock it before running the program.

Running the DXF Program

Jump to Table of Contents

Once all events are complete, you can run your program.

1. To run your program, press MODE, RUN, START and then TRAKing.

2. Use TRAKing until you verify the Z Offset for the tool. See Running 3-Axis Programs if you need a reminder of TRAKing.

3. Once verified, run the program in CNC RUN. Go to CNC RUN via one of these options:

   1. Press STOP on the handheld pendant, press CNC RUN, and then press GO on the handheld pendant.

   2. Double click the button on the top of the handheld pendant.

4. Run the remainder of the program in CNC RUN until it says RUN OVER.

5. Remember: Hold on to the handheld pendant as your program runs to press STOP quickly in case something goes wrong.

Shutdown

Jump to Table of Contents

1. Clean your machine and remove all tools before going through the shutdown procedure.

   1. Make sure to clean all tools and tool holders before putting them away.

   2. Store the key for the keyed chuck in the chuck before putting it away.

2. Re-center the vise underneath the spindle.

3. Press SYS.

4. Press SHUTDOWN (shown below).

5. Press YES to the prompt to shutdown (shown below).

 

 

6. Wait for the message below to appear on the screen. DO NOT flip the toggle switch until you see this message on the screen: “It is now safe to turn off your computer".

 

7. Flip the toggle switch located on the right side of the pendant to the DOWN (OFF) position.

8. Rotate the ON/OFF switch located on the back of the machine to the OFF position.

JUMP TO TOP