Derby Makers

The heart of Derby's Maker community

vCarve and CNC Router Instructions

What does it do?

It cuts or carves sheet materials to high accuracy according to a program

How do I use it?

The short version:

  • Design the parts using a 2D or 3D design package, depending on preference and requirements. If you’re using 3D you will need to export a 2D version in most cases.
  • Convert the design to the format needed by the machine. At this stage you may change the layout of parts to get the maximum number out of the sheet, select the type of cut and so on.
  • Give the design to someone qualified to drive the machine

To use the machine itself you will need training for the workshop in general, and the machine in particular.

Conversion to machine format

Currently the conversion is done using Vectric VCarve Pro. A trial version is available on the PCs for learning on, but the full version is needed to output the machine data file.

New file

  • Set the dimensions if the material we are going to be cutting in – e.g. 1220mmx2440mm mdf sheet
  • Reference face – Use the bottom face unless you have a good reason not to. It’s easier as you don’t need to measure the thickness and reset the Z axis for each sheet, and safer as there’s less chance of getting the Z wrong and driving the tool deep into the bed.
  • Material Thickness – If using bottom face as reference this can be nominal. If using the top face as reference it MUST be exact, measured on the sheet you’ll be cutting. Get it wrong and you’ll either not cut through the material, or cut too deeply into the bed.
  • XY Datum – set it to bottom left corner.

Import Vectors

  • Import the vectors from your file. (Line thickness doesn’t matter) – dxf, dwg, eps, pdf, some others.
  • ‘Transform’ -> ‘align to material’ as the vectors are often off the page.
  • ‘Edit’ -> ‘Select all open vectors’ – This will Check that the lines are a continuous line. If there is a problem, you can try going to ‘Edit’->’join vectors’. Start with tolerance set to 0.1mm and increase if necessary. Check the join, especially with large tolerances or joining right angles, as it doesn’t always do what you would expect.

Add Fillets (if needed)

In this case fillets are removing extra material from internal corners because a round tool can’t cut a radius smaller than its own radius. This is usually needed when making pieces that slot together.

  • In the ‘Drawing’ tab (on the left side of the window by default) select ‘Edit objects’->’Create fillets’
  • Select the required fillet type.
  • click in the locations where fillets are needed.

Nest parts

This fits the part(s) onto the sheet(s), aiming for minimal wastage. Set the tool and clearance: Tool diameter – depends on tool, but nominal at this stage.

  • Clearance – half the tool diameter is a good rule of thumb.
  • Border gap (from the edge of the part to the edge of the sheet) – 10mm is usually good.

Part nesting options:

  • Tick rotate parts to find best fit. For right angled parts 90 degrees is usuall fine, unless you want to maintain direction of grain, then it should be set to 180 degrees. Different shapes might work better at different angles – e.g. Triangles. Setting to small angles may get more efficient packing but will take longer to run as there ar more possibilities to try.
  • Don’t tick mirror parts to find best fit or the allow parts inside other parts. They sometimes cause unexpected problems.
  • Nest direction – try either option and then preview with number of copies.
  • Individual part properties – set number of copies for each shape.

Tool paths

This tab is on the right hand side of the window by default. Different sorts of operation are available for each path.


This cuts along the edge of the shape.

  • Start depth – usually 0.
  • Cut depth – how deep the cut should be, usually the same as the material thickness. Don’t cut deeper than the material! If using the bottom face as reference it will warn you if you try to do this, but with top face reference there will be NO WARNING!
  • Inside/outside – which side of the line to cut. Usually it will pick the one you want by default.

This clears material within the shape to the specified depth.

  • Set cut depth
  • Clear pocket – selects the method used to remove material. Usually offset is better.

Now Calculate. This will bring up the preview. Reset the preview and then preview the tool path and it will show you how it’s going to cut. Alt and left mouse button allows you to look at that on the 3d view

  • Select tool – set the correct tool (ask Steve), then check the geometry diameter is correct. This can be affected by the type of make or the wearing on the tool.

Cutting parameters – pass depth, step over etc. should be set automatically according to the tool selected. Check this with Steve though.

  • Go back to the tool path view and then click calculate on the bottom left to check.

Use tabs if there are small parts that the vacuum won’t be able to hold to the bed, or they will flying off. ‘Small part’ is anything less than your hand size, or long and thin.

  • Long thin tabs are usually better than short thick ones.
  • 3D tabs are usually better.
  • Use the ‘Edit tabs’ button to set number and spacing of tabs, and to add them.

Save Files

  • Check the tool path list order. Profiles cutting throught the sheet should happen after operations that don’t go all the way through (usually pockets or engraving.) For paths inside paths it’s usually better to do the inside ones first. Buttons at the top right of the list will move the selected path up/down the list.
  • Save the tool path – this will convert the selected paths to code for the CNC machine and save the file with a .nc extension. Pick the ‘PIRANHA’ postprocessor, then save to a local file NOT direct to the USB stick. The machine will only show 8 character file names.
  • Save the VCarve file – this will store all your paths and settings in case you need to recreate the .nc file, or change the material thickness.
  • Get Steve to check the file.
  • Copy and paste the file to the USB drive. NOTE – the machine is fussy about which USB drives it will accept. No pattern has been identified yet, but some types are known to work. (List of types?)
  • Eject the USB drive properly (otherwise it can corrupt the file)

Machining parts using the data file

This MUST be done by a qualified machine operator.

General safety notes

  • Ear protection: The machine and associated fans are loud, so ear protection should be worn.
  • Eye protection: When cutting bits of waste and insufficiently secured parts may be thrown from the machine. Also, despite guarding, a broken tool may fly out. Because of these risks eye protection should be worn.
  • Machine movement: The gantry and router head can move quickly during operation. Keep clear of the machine during operation.


Install the correct tool if not already installed.

  • The collet diameter and tool shank diameter MUST be the same or the tool will be overly stressed, will not perform properly and may break. If there is slack in the fit then it should NOT be used, even if they are marked as being the same size.
  • Collets and tools should be cleaned before and after use.

Power on/off

There are several stages of switching, some on the wall and some on the machine.

Wall Isolation Switches

These are the red rotary switches on the wall mear the machine. They are used for isolating power from the machine during maintenance, and may be locked in the off position to avoid accidental reconnection. There is one each for the CNC Router and for the dust extractor fan, as marked on the switch.

Wall Power Switches

These are the red and green push button switches on the wall near the isolation switches. They are used for everyday switching of power to the CNC Router and for the dust extractor fan, as marked on the switch.

Switches on machine

There is a row of switches on the controller box near the wall, plus some extras around the machine.

  • Emergency stop – red mushroom shaped switches at various positions around the machine will stop it immediately if pressed. Once pressed they must be twisted to be released.
  • Vacuum pump switch – rotary switch on the controller box. Horizontal for off, vertical for on.
  • Power on switch – push button on the controller box. Push the button to turn the machine on.

Vacuum zone operation

  • The vacuum bed is split into 6 zones. These are turned on and off with valves low down on the end of the machine towards the wall. They are labelled with icons similar to rings on a hob.Horizontal for off, vertical for on. (Check!)
  • For best results use only the zones required to hold the material being cut. Cover unused areas of zones with offcuts, preferably non-porous such as ply.
  • The MDF base boards are porous, but over a few days after being skimmed they will block up, probably due to moisture and/or dust. If having trouble with the vacuum the base boards may need to be skimmed again.


Unless otherwise specified the buttons are on the pendant with the LCD screen. Use a firm puch with these buttons to avoid accidental double presses.

  • Power up the machine. Check the isolation switch is on, press the green button on the wall then the button on the controller box.
  • Press ‘Home’ to initialise the machine.
  • Place the material on the bed where required, and alligned to the bed. If precision is required you should allign to the underlying metal bed, not the sacrificial MDF base boards.
  • Move to the reference position for the file being used, usually the bottom left corner, then press the ‘XY-0′ button to set the origin.
  • Turn on the vacuum to pull the base boards and material down (see above for details)
  • Check, and if necessary set, the Z axis origin as required for the file being used. Usually this will be at the base board in a clear area, but if the file uses the top surface as reference you will need to set it at the top of the material. The correct height can be judged using a piece of paper, or where the spindle just starts turning when the x or y are moved. Remember to close the guard after adjusting!
  • Load the file:
    • plug in the USB drive
    • Press ‘Run/Pause’
    • Pick ‘File’ menu
    • Select the file using up/down buttons to navigate and ‘OK’ to select. Beware of a double press at this point as it will start cutting immediately!
  • Override the various speeds or scale the cutting speed if required. Use ‘Run/Pause’ to select, enter the number, then press ‘OK’. It’s usually a good idea to start slow for a new job.
  • Turn on the extractor fan (green button on the wall)
  • Press ‘OK’ to start cutting. The spindle will take some time to reach full speed, and won’t start unless the vacuum is on.

Suitable materials

Most sheet wood and plastic will probably work. So far it has been used with:

  • MDF
  • Birch ply
  • Polycarbonate
  • Acrylic (Perspex)

Technical details

The machine is a Piranha PJCM1325.

  • Bed size: 1300mm x 2500mm
  • Z-axis: 250mm

G-code is produced using Vectric vCarve Pro, but anything producing suitable g-code is likely to work. Some care may be needed over the exact dialect of code produced though. It is known to accept files starting with ‘$’ and with a ‘:’ for whole-line comments.

Comments are closed.