SmartBench - First Project

CAD/CAM - Vectric

Create a new job file

Start by creating a new file by clicking on Create a new file link.

Job type

Select Single Sided, we will only be cutting on one side.

Job size

Specify the minimum dimensions of the stock material you will be using.

Z zero position

We will use “Machine Bed” as Z0 datum for the job. This means we will be registering the initial position of the tool on the surface of the bed, rather than the top surface of the material. For pros and cons on this read here.

XY datum position

Select the bottom left corner of the bounding box. Click here to read about setting your XY datum. 

Modelling resolution and appearance

These settings do not affect the cut path and are used only for preview rendering. Select Standard (fastest) from the drop down to speed up the preview rendering of the cut path. Select Birch in Appearance drop down. 

Draw a rectangle

First we will draw the box which will be used to generate the boundary cut:

Click on Draw Rectangle

Define the parameters for the rectangle:

  • Anchor point: bottom left

  • Bottom left corner X position: 10. This will position the bottom left corner 10mm away from the left edge of the stock.

  • Bottom left corner Y position: 10. This will position the bottom left corner 10mm away from the bottom edge of the stock.

  • Corner type: Radiused External, Radius value 10mm. This will round the corners.

  • Width (X): 580. This will allow clearance of 10mm from the right edge of the minimum size stock.

  • Height (Y): 380. This will allow clearance of 10mm from the top edge of the minimum size stock.

Confirm by clicking on the Create button. The rectangle will appear on the job screen.

Draw mounting holes

Next we will draw some circles to act as the mounting holes:

Click on Draw Circle

Define the parameters for the circles:

  • Center Point: offset from edges by 30mm in all 4 corners

  • Diameter: 7mm

Confirm for every circle by clicking on the Create button. The circles will appear on the job screen:

Draw the text

Next we will draw the text which will be used to generate the engrave toolpath:

Click on Draw Text

Confirm by clicking on Close button. The text will appear on the job screen.

Click on the text, the colour of outlines will change to magenta. Go to Edit > Align Selected Objects > Center In Material

The text will be aligned in the center of the material.

Overview

In order to create a toolpath in Vectric, you need to assign a tool to it. Vectric has a database of tools, where you can store setup information about each of the tools you use in your jobs. Tools can even store material-dependent information.

If you are using the Carbitool range of bits sold by either us or anywhere else, get in touch with us for a tool database you can import in to Vectric to get you started. If you are using tool bits from another manufacturer, or tool bits we do not sell on our website; read below to learn how to add them in to the tool database in Vectric.

Accessing the tool database

This will open the Tool Database window.

Option 1: Accessing through toolpath setup

When setting up a toolpath in Vectric, you will need to select a tool. In this example we will be using Quick Engrave toolpath setup. Click on Select…

Option 2: Accessing through main menu

If you have a file open you can add a new tool by going to Toolpaths > Tool Database in the main menu.

This will only add a new tool to the database without applying the tool to any of the existing cut paths.

Adding a tool to the database

The tool database information window with the list of tools already set up will be displayed. Vectric has some tools already in the database. 

If the tool you require does not exist in the database, you can create a new tool. You can also create a copy of a tool and update its details. 

In this example we will create a new engraving tool.

Select the correct material. In this example we will use Softwood.

Select Imperial or Metric tools depending on what cutter you have. In this example we will create a metric tool.

We will then select the Engraving group to create a tool in this group and click on plus button at the bottom.

In our example we are creating a 6.35mm engraving tool with a side angle of 45 degrees, flat diameter 0 and number of flutes 2. Click on Create Settings.

Material specific settings for the cutter can now be created.

Use the following parameters:

  • Pass depth: 2mm

  • Stepover: 2.54 mm or 40% (not important for the purpose of this tutorial)

  • Clearance pass stepover: same as Stepover in the previous step

  • Spindle speed: 20000 rpm

  • Feed units: mm/min

  • Feed rate 3000 mm/min

  • Plunge rate: 750 mm/min

  • Tool number: 1

Click on Apply and then Select.

You have now set up a new tool, stored it in the Vectric tool database and applied the tool choice to the toolpath.

For the purposes of this tutorial, we have provided nominal feeds and speeds for this type of tool.
However, every tool is different, and you may find different speeds and feeds suit your cutter better.
If you need to optimise, you can click here to learn more about feeds and speeds in general.

Now that we have our tools created, it’s time to assign them to some toolpaths. Toolpaths will be generated based on the features we have already drawn.

For this tutorial we will assume we are using a 6mm flat end cutter and 6.35mm 90° v-groove engraving cutter with feeds and speeds which will work well with SmartBench.

 

For the purposes of this tutorial, we have provided nominal feeds and speeds based on the suggested tool.
However, every tool is different, and you may find different speeds and feeds suit your cutter better.
If you need to optimise, you can click here if you want to learn more about feeds and speeds in general.

 

When you apply a tool, Vectric will use the feed and speed settings saved in its tool database and apply them to the toolpath.
After applying the tool, you can adjust the toolpath settings without changing the values saved in the database.
You can click here to read about changing toolpath settings.

Engrave the text

Click on the text outline to select it and then click on the Toolpaths tab on the right hand side of the job screen. Select Quick Engraving Toolpath.

Hover the mouse over any button for a tip on what it does

Input the following parameters for Quick Engrave:

  • Select the engraving tool. 

  • Depth of engraving: 0.5mm

  • Type of engraving: Outline

  • Post Processor: YetiTool SmartBench

Click Calculate. Note that a ‘Quick Engrave 1’ toolpath will appear in the list.

The preview of the toolpath will also appear in the 3D View tab at the top of the job screen.

Cutting holes

Switch back to 2D View tab.

Click on every circle while holding Shift key on keyboard to select all of them. Selected circles’ outlines will change to dotted magenta lines. 

Click on Pocket Toolpath.

Use the following parameters for Pocket Toolpath:

  • Start Depth: 0

  • Cut Depth: 12.5mm (assuming we are using 12mm thick material and need to produce a thru hole, this means SmartBench will cut 0.5mm below the bottom surface of the stock)

  • Select 6mm flat end cutter

  • Click on Edit Passes…

After clicking the ‘edit passes’ button we can now define the depths of each pass. There are several ways to do this, but for now we will use equal depth passes. In this example we will use 5 passes to get to the depth of each pass to be less than half of the cutter diameter.

  • Number Of Passes: 5

Click on Set Passes
Click on OK to confirm

Click on Calculate.


When we click on Calculate, we will be warned that this will cut through the thickness of the material. This is correct as we want the holes to be through. Confirm by clicking on OK button. 

Note that a ‘Pocket 1’ toolpath will appear in the list.

The preview of the toolpath will also appear in the 3D View tab at the top of the job screen.

Cutting a contour around the rectangle

Switch back to 2D View tab.

Select the contour of the sign. Click on Profile Toolpath.

Use the following parameters for Profile Toolpath:

  • Start Depth: 0

  • Cut Depth: 12.5mm (assuming we are using 12mm thick material and need to produce a thru contour, we need to instruct SmartBench to cut 0.5mm below the bottom surface of the stock)

Select 6mm flat end cutter

Click on Edit Passes…

After clicking the ‘edit passes’ button we can now define the depths of each pass. There are several ways to do this, but for now we will use equal depth passes. In this example we will use 5 passes to get to the depth of each pass less than half of the cutter diameter.

  • Number Of Passes: 5

Click on Set Passes
Click on OK to confirm

Machine Vectors: Outside, Climb.

We need to keep our job in place once the contour is cut through. To achieve this, we will use tabs, which physically link the part to the remaining stock. Tick Add tabs to toolpath.

Specify the length of tabs to be 10mm and thickness 2mm.

Click on Edit Tabs…

We will use a constant number of 8 tabs and also select the option to avoid corners and curved regions.

Click on Add Tabs and then Close.

Click Calculate. 

Vectric will warn the tool will cut through material. This is correct as we want the contour to be through. Confirm by clicking on OK button.

Contour will appear in the list.

The preview of the toolpath will also appear in the 3D View tab at the top of the job screen.

How to rename toolpaths

We strongly recommend renaming the toolpaths in a way you understand what cutter is used. Right click on a toolpath name and select Rename from the menu.

This will activate the name text. Type a new name and press Enter on the keyboard.

Repeat for all toolpaths to achieve a result like this:

What’s next

The job is now ready to be exported to a job file.

We now need to export the toolpaths created in the previous step to job files.

Click here to learn how to export multiple job files for tool changes (this article will open in a new window).

If you are reading through this as part of the SmartBench First project tutorial, click here to proceed to the next step after you have exported your toolpaths.

Cutting the job on SmartBench

Now we have our job files, we need to transfer them to SmartBench:

  • First Routing Project_1-Engrave.gcode

  • First Routing Project_2-3-6mm Mounting holes and contour.gcode

You can transfer your files via USB or via WiFi using our app, SmartTransfer.

In this project we will use the SmartTransfer app to send our files to SmartBench. 

If you want to use USB you can learn how here.

This article is a quickstart guide for SmartTransfer. 

Click here to go to the full SmartTransfer tutorial if you get stuck at any point.

Download the SmartTransfer installer

If you haven’t already, click here to download and install SmartTransfer.

Sending files with SmartTransfer

When you open the application, it will immediately start scanning for SmartBenches, and will display a list of machines found.  

Click on the “My SmartBench” icon.

The default name for SmartBench is “My SmartBench”. If you have already changed the name of your SmartBench, it will show up under that name instead.

Click here to learn more about setting the name for your SmartBench.

 

Open the Windows File Explorer, and navigate to the folder where you have saved both of your job files. Select both of the job files, and drag and drop them into the SmartTransfer window. 

When you see this screen, you can close SmartTransfer.

The spoilboard acts as a sacrificial layer which protects SmartBench when the cutter breaks through the bottom surface of the stock material. It also increases the support provided by the Lower X Beam.

In this project our spoilboard will be using an 8’ x 4’ sheet of 9mm melamine faced MDF. The material is:

  • Rigid

  • Flat

  • Smooth at the bottom

  • Bigger than stock material

Click here to learn what makes a good spoilboard for routing.

Our stock material will be an offcut sheet of 12mm (~½”) plywood of approximately 650 x 650mm (25.5” x 25.5). The material is:

  • Flat

  • Larger than the job

Click here to learn what makes a good stock material.

In this project we are going to hold the spoilboard down with speed clamps at either end (on the leg plate on the home end and on the wheel tracks at the far end).

We will hold the stock material down with screws that will pass through the stock material, the spoilboard and the sacrificial wooden panels on the Y Bench.

Before we can put the spoilboard or stock material onto SmartBench we need to raise the Upper X Beam to create a space for them to fit. Release the cam-locks on either end to lift the beam.

Place the spoilboard on the Y Bench, sliding it under the Upper X Beam.

Align the spoilboard by measuring off the edge of the Y bench at either end while ensuring that it is over the rollers on the Lower X Beam.

When you are happy with the alignment, clamp the spoilboard in place.

Place the stock material on top of the spoilboard and align it by measuring off the edge of the spoilboard.

When you are happy with the alignment you can screw the stock material down. Make sure you do not place any screws in an area where the cutter will travel through them. The image below shows the zones outside the cut path. (if you are using 650mm x 650mm stock)

When your spoilboard and stock material are fixed, it’s time to position the rollers on the Upper X Beam over the stock material. There are rollers on both sides of the beam and they can slide along the full length.

When the rollers are correctly positioned, you can drop the Upper X Beam onto the stock material and clamp it in place making sure that it is level Check that all the rollers are making contact with the stock material.

Click here to read through the offcut stock holding case.

Fitting a tool incorrectly can cause serious damage to SmartBench. 

Click here if you get stuck at any point, or if you need more information about how to fit a tool correctly. 

 

This article gives a quick overview of which tools we need for the job, and a brief summary of how to load them.

We will now need to fit the cutter used in the first job, which is a 90°, v-groove engraving cutter with a ¼” (6.35mm) shank. We will use a 7-6mm collet.

Click here to learn how to size the collet.

Load the collet into the spindle.

Click here to learn how to fit a collet into the spindle.

Load the cutter into the collet.

Click here to learn how to fit a tool into the collet.

Put the spindle switch into the on position, and orientate the spindle so that the switch is facing towards the home end of the Upper X Beam. Load the spindle into the Z Head from above. 

Adjust the position of the spindle motor to maximise airflow, tighten the clamping bolt, and plug the power and signal cables into the Z Head.

Click here to learn how to fit the spindle into Z Head.

We now need to set the XY datum. 

The longest side of our sign will be along the X axis of the SmartBench. Our datum needs to be at the bottom right corner of the stock material, as shown on the diagram.

A: Stock material

B: Spoilboard

Use the PRO app on the SmartBench console to move the Z Head to the bottom right corner of the stock. 

Press the SET button at the bottom of the screen to set the XY datum.

Click here to learn more about how to set the XY datum.

We also need to set the Z datum. Our job is set up to have the Z datum on the top surface of our spoilboard (bottom surface of the stock material).

Use the PRO app on the SmartBench console to move the X axis so that the Z Head is away from the stock, and sitting above the spoilboard. 

A: Stock material

B: Cutter

C: Spoilboard

We will use the probe plate to auto-set the Z datum. 

Use the manual move buttons to move the Z axis down so the tool tip is close to the top surface of the spoilboard.

Remove the Z probe plate from the back of the Z head, and place it underneath the tool tip. 

In the PRO app on the SmartBench console, press the Z Probe button on the right hand side of the console screen.

SmartBench will automatically detect when the tooltip has touched the Z probe plate, and set the datum. 

Once set, the dust shoe will illuminate green and the Z axis will lift.

Click here to learn more about how to set the Z datum.

In the Console menu, click on the “PRO” App.

Navigate to the file load tab in the PRO app

Press the button with the folder icon in the top left of the screen.

Select “First Routing Project_1-Engrave.gcode”. If you cannot find the file you can toggle the list view to view the full file names using the button in the bottom left of the screen.

Once you have selected the file, press the green tick in the bottom right corner.

Once the job is loaded, SmartBench will ask if you want to check the file. If it is a file that you have run before you can skip this step but since this is the first time you will be running this file we recommend that you do this.

When SmartBench has finished checking the file you can press “Finish”.

At this point you can see a preview of the job file on the console. SmartBench will only display the first 1000 lines of gcode.

Click here to learn more about opening a job file. 

As a final check, let’s just check that our spindle and vacuum are operational by using the buttons on the manual move screen.

Right now we’re ready to go.

Once all preparations are done, we can start our job.

Press the green play button on the far right of the console, and follow the on screen instructions. 

You will be asked if you are using a Stylus or the router, in this instance we are using the router.

When you are asked whether the Z head should raise on a job pause, select “Yes”. 

 Read and accept the safety warning screen.

And finally, press the GO button.  

Click here to learn more about starting a job.

Adjusting feeds and speeds

You may need to make adjustments to your feeds and speeds during the cut depending on certain factors such as your material and the condition of your cutting tools.

You can make live adjustments using the buttons on the file run screen shown below.

SmartBench doesn’t have an automatic tool changing facility. You will need to change the tool manually after the first job has finished, and before starting the next job.

Do not power off the SmartBench at any time in the tool change procedure.

If it is powered off it will lose its current XYZ position and will need to be rehomed. This may lead to inaccuracies in the work due to unavoidable variations in the home position.

Click here to read more about homing procedure.

 

Fitting a tool incorrectly can lead to serious damage to SmartBench. 

Click here if you get stuck at any point, or if you need more information about how to fit a tool correctly. 

 

This article gives a quick overview of which tool we need for the next job, and how to do a tool change.

Loading the next job file

SmartBench will stop, and the console will show a job complete screen when the first job has finished. 

Press anywhere on the console screen to return to the PRO app. 

Go into the file chooser, and load the next job file, “First Routing Project_2-3-6mm Mounting holes and contour.gcode”.

Changing tools

Change to the tool required for the next job file. 

Do not power off the machine and just proceed with the tool change.

 

Click here to learn about fitting a tool.

Unload the spindle motor from the Z Head.

Click here to learn more about how to unload the spindle motor from the Z Head.

Undo the collet nut, and remove the v-groove cutter.

Click here to learn how to fit a cutter into the collet.

Fit the 6mm end mill cutter, and tighten the collet nut.

Load the spindle motor back into the Z Head.

Click here to learn how to fit the spindle into Z Head. 

Set a new Z datum

When the tool change is complete, you need to set the new Z datum.

As we did before, set the Z datum with respect to the spoilboard, using the probe plate and the SmartBench console. 

Click here to read more about setting the Z datum.

Starting the next job

You can now start the next job.

Press the green play button on the far right of the console, and follow the on screen instructions. 

You will be asked if you are using a Stylus or the router, in this instance we are using the router.

When you are asked whether the Z Head should raise on a job pause, select “Yes”. 

Accept the safety screen.

And press GO

Clean the work area

Although the extraction removes the vast majority of chips and dust created during the job, there will be some left. 

Use the console to manually move the Z axis up, and move the X axis away from the work area. Clean the work area with a vacuum cleaner. 

Click here to learn how to manually move the SmartBench axis.

Separate the sign from the stock material

When we created the contour cut toolpath for our sign, it was set up to produce the workholding tabs. These tabs are designed to keep the sign attached to the stock material and prevent it from moving during cutting. 

Now we can break the tabs using a sharp utility knife or a multitool cutter. 

Break the tabs close to the stock material to prevent accidental damage to your job. 

Once the sign is detached from the stock material, use a file and sandpaper to smooth the edge of the sign at the tabs locations.

Remove stock material 

Undo the screws attaching the stock material to the spoilboard and remove the stock material from SmartBench. 

Give your machine a thorough clean with a vacuum cleaner to prepare it for the next job.

Power off SmartBench

If you don’t need to use SmartBench, you can power off the machine.

Click here to learn how to properly shutdown and power off SmartBench.

Click here if you want to learn more about designing your own projects with CAD/CAM software.