05. Getting Started - Example Project

Cutting a Calibration Pattern

For our quick introduction we are going to us a 2D Profile toolpath strategy to engrave a precisely sized and aligned rectangle, circle and star. This pattern will use all the steps we have outlined in The CNC Workflow. It will also allow us to check that the CNC machine is working correctly using some simple but important features of the design:

• The rectangle, circle & star should not appear warped or distorted.
• The dimensions of the carved shapes should exactly match the design.
• The alignment points of the 3 shapes should not show any discrepancies.
• The star is rotated slightly clock-wise and the carving should match the original orientation of the design with no unexpected reflections in X or Y.

At the end of this guide we will review these checks and suggest some troubleshooting tips if any of them are not as they should be.

Material, Tooling & Hold-Down

The XY dimensions of the design will be 100mm (4") so you will need a piece of material approximately 150mm (6") square or larger.

The precise thickness of material is not too important as the design will simply be carved into its surface at a depth of 1.5mm (1/16"). Any piece that is 3mm (1/8") thick or greater will therefore be fine. An offcut of plywood or mdf board would be ideal.

To avoid any chance of collision with clamps or cutting into a screw, the best starting method to hold down a small piece of material like this is to use double sided tape. Any heavy duty 'carpet' type tape will work, but you may need to experiment to find a brand that secures well, but can also be cleanly removed once the job is complete.

The toolpth will be created based on a V-bit, but the precise tool angles are not important. If you don't have a V-bit tool, then a small (3mm, 1/8" diameter or less) end mill or ball nose tool will also work but the cuts will be the broader so the calibration pattern may be a little bit more difficult to interpret.

To avoid any chance of collision with clamps or cutting into a screw, the best starting method to hold down a small piece of material like this is to use double sided tape.

Create the Job

• Click `Create a new file` to get started.

This opens the `Job Setup` form. All projects start with a job setup. Here is where we consider the physical dimensions of our design. Note that you do not necessarily need to define the whole material block at this point, just that area needed for your design - the design area can be subsequently positioned anywhere on a larger physical material block using the `XY Datum Position`, which your CNC machine will use as its reference starting point.

Like all forms in the software, you should simply work from the top to the bottom of the `Job Setup` form. Forms are typically laid out with the most significant, non-optional or most commonly updated fields at the top. Sensible defaults are provided for most form fields the first time they are accessed (fields will generally remember their previous setting, once you edit them) so initially you can simply ignore any fields you are not sure about. At the bottom of most forms are the buttons to OK (accept), Apply or Cancel any changes you have made.

• The job setup form allows for projects that will be cut from both sides or using a rotary axis, but for now we will simply select `Single Sided`.

We will set the `Job Size` units according to your preference.

Note that your CNC machine controller will be set to expect toolpaths defined in either metric or imperial units and you will need to refer to your CNC manufacturer to determine your particular setting - the Post-Processor you select later will need to match the toolpath to the controller's requirements but this is entirely independent of the units you prefer for designing within the software - everything will be automatically converted, if necessary, when the toolpath file is created.

• Set the width & height of your new job to both be 150mm (6")
• Set the
• Click OK

Design the Calibration Artwork

Your project needs to start with design drawing. On the left-hand side of the screen there are a number of tabbed panels that provide access to various tools to help you to draw your design.

In due course, we will use our design to begin creating toolpaths for our CNC machine. The functions relating to toolpaths and toolpath strategies are located in another panel on the right-hand side of the screen. Initially this panel is hidden. Once our design is largely complete we will switch our focus to the toolpath panel on the right.

This is the typical workflow when creating a CNC project and so the software interface makes this switching of focus easy and intuitive.

For now let's continue to focus on the tools available in left-hand design panel.

The first thing we will do is create a simple 100mm Square, using the Rectangle tool in the Design Panel on the left. Witht he Rectangle tool open, click into the 3D View to place a default rectangle, and in the Edit Boxes on the Right nd Bottom of the rectangle, click into each one and type 100.

This will create your Rectangle to be 100m x 100mm.

Now press the F9 key on the keyboard, and your Rectangle Vector will now be centered in your work space.

Create our First Toolpaths

Now that our design drawing is complete we are ready to consider what toolpath strategy we should use to cut this shape accurately and efficiently.

The software interface can automatically hide the design tools panel and show the toolpath strategy tools panel using the 'Switch to Toolpath commands' button.

• Click on the 'Switch to Toolpath commands' button at the top of the 'Design' tab.

The toolpaths tab will now open on the right-hand side of the software. Here you will find all the tools relating to the creation, editing and saving of toolpaths.

Selecting the most appropriate toolpath strategy for a particular job is one of the toughest aspects of initially learning how to use your CNC effectively. Over time you will explore the different strategies available within this tab and our extensive tutorials and practical examples will to understand what each is used for.

For now we are going to use just the first strategy availble under the Toolpaths Operations - this is the Profile Toolpath.

Click on the Profile Toolpath button to open the 2D Profile Toolpath form.

Saving and Loading the Project

At this point we should probably save our project. Saving the project document using the File->Save menu, or the Ctrl+S shortcut-keys, is just like saving any other conventional application document (i.e. Microsoft Word etc.) and it will include all of your 2D design elements, 3D models and toolpath strategy settings in a `*.crv` or `*.crv3d` file. This is the file that you can come back to any time at a later date to continue your work or to duplicate as the basis of a new project.

Note that this is *not* the file that your CNC machine will read. Saving Toolpaths (see below) is the indepenendent process by which you specifically save the file from this project that your CNC machine needs. It may be helpful to think of the toolpath saving process as more like creating PDF files *from* your Word document - PDF files aren't typically reloaded or edited but they are ready for 'printing'.

Previewing the Toolpath

Before we begin getting our toolpath files over to our CNC machine there is still a *very* important step for us to do in the software. We can preview exactly how our CNC machine will move and what the material should look like after each toolpath is completed using the Preview Toolpaths command.

Saving Toolpaths - Post Processing

You now need to Post Process your Toolpath to save your toolpath out into a file which your CNC Machine will be able to read.

In this guide we will assume that you have completed the "Machine Configuration" Process either Manually or using one of the existing Online Configurations as seen here.

With that step complete, you just need to now open the "Save Toolpath" form, using the bottom right most icon in the Toolpath Panels icons.

Make sure your machine is currently selected in the Machine

Running Your Toolpath

Every CNC machine and controller is different. At this point you will need to refer to your CNC machine manufacturers instructions for the details of running your toolpath file, but we can provide some generally applicable information about the typical process you should expect.

Secure your material

Your piece of material will need to be secured to the machine's bed. This is typically done by clamping, screwing or gluing your material down (larger or more sophisticated machines may have vacuum hold-down). In the first two cases you must be very careful to avoid cutting into your clamps or screws. As we noted in the Job Setup, the toolpath file does not have to be the same size as the material so the simplest way to avoid clamps and screws is to make sure your job dimensions (and thus your toolpaths) are no larger then the unobstructed area of your material and that it is correctly positioned within this region.

Set your origins (datums)

The movements of all toolpaths are relative to the `XY datum position` you selected when you initially created your job (in our example we set the bottom-left corner, but it can also commonly be the center of your design), these are also often referred to as "origins". Now you must indicate to your CNC machine controller where this datum point is physically located on your material. This process is usually referred to as "setting the XY datum", "setting the XY origin" or "zeroing X & Y".

In effect, setting the XY datum will position where your toolpath will be cut on your material.

You will also need to indicate to your controller how deep into the material your toolpath will cut - the equivalent of positioning your toolpath within the material. This is often known as "setting the Z origin", "setting Z zero" or "zeroing Z".

Again at this point it is important to know what `Z Zero Position` setting you used when you created your Job in the software - in our example we set it to be on the surface of the material, but in some circumstances it is useful to set it to the base of the material block, or your CNC machine's bed.

Because this job was created with the `Z Zero Position` to on the `Material Surface`, you will need to jog your CNC machine so that the tip of the tool is touching the surface of the material and then use its control software to zero the Z position.

Alternatively you may have an automatic Z touch plate or probe to achieve the same result - refer to your CNC manufacturer for instructions on this step.

Note: when wanting to do a test 'air cut' this is your opportunity to back your CNC machine upward in Z to a point in the air where the toolpath's maximum depth will not contact any physical material and set your Z zero 'in the air' instead. Running your toolpath with the Z origin in the air like this is a very useful test of movements of a toolpath if you have any doubts or uncertainties about your setup or toolpath settings before any real cutting.

At this point your CNC machine should be in a state where its position indicators would read X=0, Y=0 & Z=0 when the tip of the tool was at the position you defined when you created your origin job - in our example this would be at the bottom-left corner of the area we will cut and just touching the top surface of the material.

Load your toolpath File

Ready to go?

You should always consider a visual check of at least the initial start point and feedrates of an untested toolpath with an 'air cut' (see note above). Pay particular attention to the movement that will form the first full-depth, full-width cut - as this will be when the tool and CNC machine are under the most stress - to ensure that it looks appropriate for the tool and type of material you are intending to cut.

When you first start using your CNC it is worth considering keeping a simple written checklist at your controller. An example might be:

Have I:

• Run an 'air-cut' to check initial movement?
• Checked the material is firmly secured?
• Checked right type and shape of tool is fitted for this toolpath?
• Set the X,Y origin?
• Set the Z origin?
• Turned the spindle on (if not automatically enabled by your CNC machine's controller)?

OK, time to cut!

Always run any toolpath with untested or unverified tool settings with extra care and caution. When cutting with new tools and or in new materials seek advice from your CNC machine or tool manufacturer about the appropriate feeds and speeds for your machine and tooling.

Check the Calibration Cuts

Troubleshooting

Scale / units

My Design is cutting out much smaller/larger then it designed for.

Double check what distance your machine moves when you manually command the controller to jog from X=0 to X=1

The distance it travels should be exactly 1 Inch or 1mm.

If it moves the 1 Inch then you need to ensure that when you save your toolpaths from Aspire that you use the Inches Post Processor.

Likewise, if it moves 1mm, then use the MM Post Processor instead.

If it moves a different distance, instead of one of these options, then the machine calibration needs to be reviewed with help from the machines supplier.

Double check this on each of the X Y and Z Axis's, and it must move the exact same distance on all Axis.

Backlash

Backlash is a physical issue in the machine where an Axis will move the correct distance for a cut, but then loosness on the Axis motor or screw barings will allow it to slip.

This can build up over time for the machine to graducally become more and more misaligned over the duration of a toolpath. Commonly if you see inaccuracy in cuts only in one direction then it will be backlash issues on that one Axis.

Report the issue to your machiine supplier for advice on how to elliminate backlash in your hardware.

Inverted axis

The most common indicator of an inverted axis is text being mirrored in a single direction. A rarer case can be when the router will raise when it should plunge, resulting in it cutting air, even when Z Zero is correctly set. This can be due to a number of factors, such as:

• Hardware Wiring.
• Controller Setup.
• Post Processor setup.

The Hardware wiring is always the first thing to check in these cases, to ensure that the machines hardware is all connected as intended, and there are no wiring issues. If the positive and negative terminals on a motor are reversed then the motor can go in reverse.

The controller setup is part of the controllers calibration, and if values are reversed here, it can cause the motors to then work in reverse.

Post Processor setup can sometimes require the reversing of an Axis. This will have been required by the machine supplier to fit their machines configuration. The Post Processor should usually not be reversed manually, and is setup to fit the machine suppliers specifications. In rare cases where it is needed to be changed to suit a CNC machines which cannot be corrected with the above points then Editing the Post Processor can help.