CNC Router

Laguna CNC Router

Make: Laguna

Model: SmartShop II

Serial Number: 16124390

Ace: Luke Roderick (lroderick20@georgefox.edu).

Location: Wood Shop

Description

The Laguna SmartShop II is a CNC wood router capable of cutting out complex shapes that would otherwise be difficult to create by hand. Like all CNC machines, the SmartShop II is most useful when a design calls for a high level of precision, or is being mass produced.

Here is an example of this piece of equipment being used.

Documentation

Terminology

• ZPO (Zero Point Offset) - The selected X and Y position on the material that coordinates with the program zero point.
• Collet- A piece of machined steel that clamps down and locates the cutter in the tool holder.
• Dust Shroud- A combination of sheet metal and flexible brush material that performs a seal around the area of material during the cutting process.
• Spoil Board- A porous sacrificial board used on top of the router bed but under the work piece.
• Regenerative Blower- This device produces the vacuum needed to pull material down onto the spoil board.
• Tool Holder- Cutters are placed in the tool holder and each holder gets pulled into the spindle during a tool change.
• Up Shear Router Bits- Normally used for deeper pockets as they evacuative chips better.
• Down Shear Router Bits- Normally used for shallow pockets and leaves a very clean edge. Tend to pile up the chips as they don't evacuate the chips very well.
• Combination (Compression) Router Bits- Helps keep a good finish on the material when using a laminate on both sides.
• Tool Touch-Off- A process of setting the Z axis height of a tool using the sensor built into the machine.

User Manual

Training

Operation

To get started you will need to get a .DXF file from Solidworks or another program. The .DXF file will need to be imported into VCarve Pro software. VCarve is used to create the G-code used by the router. You will select the type of cuts and tooling inside the software. Most cutting jobs can be done using a 1/4" cutter. A good rule of thumb is to not exceed the diameter of the tool in depth per pass. In foam or soft materials you can cut deeper per pass. The large switch near the middle of cabinet is the main power. There is a key located on the control panel that also needs to be turned to the on position for the PC inside the machine to boot. After power up, make sure the table is clear before pressing the home button. The machine will move to the corner closest the control panel after moving the Z, X, and y axis to home position. Always keep your body outside the safety line while the machine is moving.

Demonstration

For the demonstration you will need to import a DXF file into VCarve Pro and convert it to G-code. You will also need to demonstrate safe startup and use of the router using the G-code file you produced.

Open VCarvePro software.

1. To start a new project, you must first select “Create a new file.”
2. Next, you will be prompted to input the width, height, and thickness of the material you are using.
3. Ensure that the Z Zero Position is set to "Machine Bed." Our Smart Shop II machine is calibrated for this setting. If you use the material surface option, the end-mill will carve into the machine bed causing damage and potential injury.
4. Select the XY Datum Position. Typically, it is easiest to not use an offset and origin your part off the bottom left corner of the material. If you are cutting a part that needs to be rotated and cut in 2 or more orientations an offset may be useful to line up your jig.
5. If you wish, you may adjust the modeling resolution and color. Otherwise select OK.
6. Now select "import vector".
7. Make sure all the imported pieces are close together, but make sure they don't overlap.
8. Starting with the inside features, you will hold the shift key and select all of the holes. Once they are all selected, go to Tool Path and select the appropriate Profile or pocketing Tool Path. Choose your cut depth, tool, parameters, and then select OK. Double-check that Inside Cut is also selected, and check the box for Ramp.
9. To save the inside cutout tool path, select Calculate and OK.
10. Select "preview selected tool path" to ensure the path is correct.
11. Switch back to the 2D view and begin the process for cutting out your design. This starts by holding down the shift key and selecting the items.
12. Select VCarve, and make sure the settings are correct. If you are satisfied, select Calculate and OK again. You can preview this part of the process as well.
13. Go back to the 2D view to begin the outside cutout process.
14. Holding the shift key down, you can now select the outer pieces that need to be cut out. Then select Close on the right side of the screen.
15. Next, choose Tool Path, select Outside Cut, and change your tool and parameters as needed. Check the box for adding a Ramp, and hit Calculate.
16. Preview the entire process before saving the file.
17. Once you are happy with the design, select "Laguna SmartShop BR ATC(inch)(*prg)" post processor and "save toolpath(s)". You can copy the files onto a flash drive to import into the machine.

Detailed Procedure

Software

VCarve Pro is the software used in conjunction with the CNC router and may be found on the eight rolling computers in the The Hub.

Job Setup

1. Select the appropriate job type: single or double sided.
2. Enter the size of your work-piece.
3. Set the Z Zero Position to "Machine Bed." The Smart Shop II machine is calibrated for this setting. If you use the material surface option, the end-mill will carve into the machine bed causing damage and potential injury.
4. Select the XY Datum Position. Typically, it is easiest to not use an offset and origin your part off the bottom left corner of the material. If you are cutting a part that needs to be rotated and cut in 2 or more orientations an offset may be useful to line up your jig.
5. If you wish, you may adjust the modeling resolution and color. Otherwise select OK.

Vectors

1. To Import the design you wish to cut go to File>Import>Import [your file type] and find your design. If you import a non-vector based design you will need to trace bitmap once imported.
2. Select your design and use the arrow keys to position it to the desired location.
3. Sometimes paths will not be joined properly (i.e. selecting one side of a rectangle does not select the entire rectangle). Vectors that aren't joined are treated as separate paths. Separate paths that should be joined may cause the bit to cut on the wrong side of the path. To join vectors simply press j to open the Join Vectors menu, select the vectors you wish to join and click Join.

Toolpaths

Creating tool-paths is a complex process that involves critical thinking and foresight into the cutting process. Please recognize that these instructions are by no means comprehensive and only address the simplest of the 2D tool paths features. If you wish to engrave, inlay, or do 3D carving do some research to determine the appropriate procedure. Finally, recognize that YOU ARE THE SAFETY MECHANISM on the CNC router. It will do what it is told even if that means crashing into the table or a tool holder because you accidentally told it to. All this to say that when you make a tool-path, be aware that the computer is dumb and will do what you tell it, not what you meant to tell it.

1. To open the Toolpaths menu click the Toolpaths tab on the top right of your screen. Once the menu appears, turn off auto hide by clicking on the push pin icon.
2. Before defining any Toolpaths it is a good idea to open the material setup menu and double check that everything is set up correctly.
   1. Thickness: It is obviously important that the thickness of your material is accurate to avoid cutting deep into the spoil-board or not all the way through your part.
   2. XY Datum: Ensure that you understand where the datum is so you can accurately position your part inside your lumber.
   3. Z -Zero MUST be set to Machine Bed. (This has been mentioned many times because it is very important).
   4. Model Position in Material: This is for 3D carving and is used to tell the computer where you want to *gasp* position the model in the material.
   5. Rapid Z Gaps above Material: This is very important if you are using any clamps, jigs or anything that sticks above the surface of your material to secure it to the spoil-board. The rapid z clearance tells the computer how far above your material surface it is safe to do rapid movements during the cutting process. 0.2 inches is a good height if you don't need a fixture. Otherwise, make sure that it is set high enough so that you will not crash into your fixture. Plunge tells the computer the height it is OK to do a rapid plunge at. This value will typically be equal to the rapid z clearance.
   6. Home: Defines where the start position is. Do not change this setting.
3. Always perform inside cuts and pockets prior to cutting the outline of your part. Failure to do so may result in incorrect geometry due to the part shifting during the cutting process. The goal here is to leave the part as stable as possible for as long as possible.

General 2D Toolpath instructions:

1. Cutting Depths: Start Depth tells the computer at what depth you wish to begin a cut. Unless you have already removed material over the entire path of the cut, the start depth should be zero. Cut depth is how deep you wish to cut. For a through cut set the cut depth equal to the thickness of the material. Do not set the cut depth deeper than the thickness of the material because it will cause unnecessary wear on the spoil board.
2. Tool: Selecting your tool is important. For most operations a 1/4" end-mill will be sufficient. The biggest things to be aware of are the tool number and spindle speed. The tool number tells the computer which tool it is to pick up. The CNC is dumb and will not know what tool it is holding at any given time. All it knows is the tool number. it is ABSOLUTELY CRITICAL that you enter the correct tool number for all of your tools. Breaking off an end-mill spinning at 18000 rpm causing it to shoot across the room and impale you or your beloved engineering classmates will not win you favor. Also check that the rpm are appropriate, typically the default is fine. For a 1/4" end-mill set the speed to 18000 rpm.
3. Passes: Adjust the number of passes such that the pass depth is less than the diameter of the end mill you are using.
4. Ramp Plunge: This option plunges the end-mill on a ramp instead of going straight into the material. Generally it is wise to use this feature because it reduces the forces on the end-mill.

Pocket Toolpath

Profile Toolpath

Other Toolpath

1. Research! You are a capable engineering student. You can do 15 minutes of research on your own prior to step 2.
2. Consult the ace and technician. They might ask you questions about what you want to make. It would be great if you came in with some knowledge about the process because you spent 4 minutes reading about how to do what you want to do.

Final Steps

1. Use the Preview Toolpaths feature to double check your part. Make sure that any inner geometry is cut first. You may need to use the reset preview option.
2. Briefly look through your material set up, tool selections, and settings to be certain that you have correctly programmed the machine.
3. Check (again) that the z zero position has been set to Machine Bed.
4. Select Save Toolpath. Be sure that the "Output all visible toolpaths to one file" box is selected. Check that all of your toolpaths appear underneath "Toolpaths to be saved..." The tools should have the correct tool size and location indicated. Select the appropriate post processor: Laguna SmartShop BR ATC (inch) (*.prg).

Operation

Startup

• Connect the pneumatic air line located on the tool holder end of the machine.
• To power up the machine turn on the main power switch located on the base of the control panel.
• Turn on the key switch located near the screen located on the control panel and wait for the PC to boot.
• Make sure all of the axis are clear to move.
• Select HOME and wait for the machine to move to the 0,0 position. Make sure you are located behind the yellow tape on the floor.

Material

Only cut wood when operating this machine unless specific approval has been given by the technician. Acrylic and foam may be cut with approval.

End Mills

We have a variety of tooling but the majority of cutting should be done with a 1/4" tool. Talk with the technician while in the design phase.

Final Checks

There are some checks you should always do prior to running a program. Ask yourself the following questions before pressing the start button!

1. Is the material securely fastened to the table by vacuum or mechanical means?

2. Is the dust collector turned on?

3. Has the zero point been set in the correct location?

4. Is the pneumatic line connected to the machine?

5. Are the correct tools setup in the program and in their proper slot on the machine?

6. Is everyone clear of the machine?

7. Is the dust collection shroud going to collide with the material because I'm cutting beyond 3/4" deep?

8. Has the proper program been loaded?

9. Has the Z-zero position been set using the material bed and not the material surface?

Cutting

Always keep your finger near the stop button when starting your program. Most likely if something goes wrong it will happen early in the process so be ready to stop the machine. If you know the relationship between the brush on the dust shroud and the end of the tool you will have a good idea how deep the tool is when it cuts into the material. It is also very important to know what the program should be doing so you can verify the tool path is correct.

Reset the Space

When you have finished, park the cutting tool back into the storage rack at the end of the table. You will need to remove any material on the table and use the vacuum to clean off any leftover dust and chips. You can use the dust collector or portable vacuum. Make sure to disconnect the air hose and power down the machine with the spindle located off of the table. This will prevent any leaking oil from dripping on the table.

Safety

There are multiple hazards you need to be aware of when using the CNC router.

• The tooling is very sharp and spins at over 18,000 RPM. Keep your body parts away from the cutter and spindle. You need fingers for the ring you will get by spring.
• Stay behind the safety line when operating the router. The router is very large and will not stop if you get in its way.
• Materials need to be securely fastened to the table by vacuum or mechanical means.
  • This includes material that could be made loose during the cutting process. Use tabs to secure such material.
• Never attempt to cut a hole the same diameter as the cuter with a down cut force cutter. This will compress the chips and can create a fire due to the air draw of the vacuum table.
• Always wear ear protection when operating the CNC router.

Certification

Foxtale Course

Troubleshooting

• If none of the control functions on the control panel appear to work, make sure the machine has been homed and the E-stop is released.
• If the cutting tool height appears to be incorrect make sure the tool touch off has been performed for the tool in use.
• If your tool path appears on the inside of your part, it is likely because the paths are not joined. To join your paths, highlight the paths you wish to join and press the j key.

Maintenance

General maintenance

• The spoil board needs to be resurfaced as grooves are cut into the surface. Grooves will release a percentage of the table vacuum and increase the risk of the material moving during cutting.
• There are many bearing surfaces located on the router that need to be lubricated. The router is equipped with a central lubrication system the technician will operate on a regular basis.

Specific Maintenance Tasks

Maintenance Procedure	Frequency	Done By
Cycle Oiler	Sample	Sample