How to use Carveco with your CNC machine

1/ Interface Overview

1. Menus, Shortcuts and View selector.
2. Drawing tools 
3. Global display, showing your drawings, toolpath, etc.
4. Project content window that contains the Toolpath menu, opened by clicking on Toolpath on the right. It contains all the CAM interface of the software, including operation programming, toolpath display and simulation management.

We will focus on the Toolpath window as in the context of this tutorial, we’ll import our clamp *.DXF file directly, without drawing it from scratch. 

You can find the file here:

If you wish to learn the basic concepts of CNC milling, we'd suggest you go through our tutorial series first before following this specific tutorial for Carveco.

2/ Creating a new model

Let's start by creating our new project.

Click on New Model and enter the dimensions of your stock in which we will put our clamp, in our case it is 150 x 150 mm.

3/ Importing the design

We can now import the drawing of the clamp

You can find the file here:

Click on the menu Vector > Import,
And select the dxf file of the clamp (link above)

A window opens showing you the details of the dxf file.
Don't change anything here and keep "auto. rejoin vectors" checked.
Then click OK.

The drawing is not imported and Carveco centers it automatically in your file.

One last step : in order to be able to mill the slot at the tip of the clamp, we will draw a rectangle defining the area to be milled halfway through to create that slot (as Carveco does not understand the milling of open paths).

Select the rectangle tool (in the toolbar on the left), 
The parameters for the rectangle creations are shown on the right panel.
Enter values Width 50mm and Height 15mm and click on Create.

We now need to place this rectangle above the slot.
Go back to the Arrow (selection) tool from the toolbar.

Place your mouse above the middle of the top line of the rectangle until a special icon appears (see picture), meaning you're going to move the rectangle with the middle of this line as a reference point.

When the icon has appeared, drag and drop the rectangle downwards, above the line marking the limit of the slot at the tip of the clamp (shown in green here), hold the click until it snaps to the slot's line and the same icon appears again, showing you you are aligning the middle of the rectangle to the middle of the slot.

Your drawing is now ready for the CAM preparation and should look like that :

4/ Toolpaths creation and Tool library

Open the toolpaths menu of the project, in the right of the screen.
The toolpaths menu appears underneath.

We can see in this menu all the tools around CAM :
- Toolpath Operations are menus for general parameters (such as the material, the tool library and setting tabs...)

- 2D and 3D toolpaths to create various types of milling operations

- And a Simulation button to check the toolpaths created

Let's start setting up our material (stock) specifications. 

Click on "Setup Material" and enter the material thicnkess (for us 12mm)
and set the model position in material to bottom (this means our Z0 will be set on the spoiler board, to be sure the cut goes all the way through).

The softwares automatically sets the top and bottom offset.

Now we can start creating the operations :

First we will cut the slot at the tip of the clamp.
Select "Create area clearance" (which is a pocketing operation) in the 2D toolpath menu and select the rectangle we created to tell which area we want to be cleared.

Set the Start depth to zero (this is the top of the stock)
An the Finish depth to 6 mm (we want this slot to be 6mm deep)

We will now need to select a tool for the job.
In Tool List click on "Add" which will open the Tool library.
Navigate to metric tools > for wood > 2D finishing and select the 6mm End Mill.

The native parameters of Carveco for this tool are corresponding to our needs in this case, but just to check the menu, click on Edit and you'll see how you can edit the specifications, feeds and speeds of the tool here. 

You can create and save copies of tools with different parameters in this library if you plan to reuse the parameters often.

Click OK to save the tool and then click select to select it for the pocket operation we were working on.

Choose the "Offset" clearance strategy to have a continuous spiral movement.

Check the Add Ramping Moves box, as it allow an easy entry in the material instead of plunging straight in it (end mills are made to cut while moving, not straight).
You can keep all the default parameters.

You can now give a name to the operation at the bottom.
Then click Calculate Now.

You can now switch to the 3D view (top left of the view) and see the toolpath displayed. You can also use the simulation menu on the right to have a preview of the toolpath result.

Let's program the rest of the operations :
The next operation is also a pocket toolpath for the hole and the groove:

Go back to the 2D view (button at the top left) to see the drawing again, and select the 2 holes by holding shift. This time the Finish depth is 12mm deep (we want to cut all the way through) but all the other settings are the same and the previous tool is automatically selected so no need to open the tool library.

We can see we now have 2 toolpaths in the list of the project on the right.

The last toolpath is the outline of the clamp : 
Go back to the 2D view and to the toolpath menu and create a Profile Toolpath in 2D Toolpaths, and select the outline of the clamp as the reference.

Select Outside of Selected Vector (so that the tool runs outside of the shape)

- Final depth must be 12mm too (the stock thickness) as we want to cut through.
- We will use the same tool.
- Check the box for ramping moves.
- Check the box to Add Bridges :
In order to avoid the clamp to move when the cut is over, this will add some tabs to hold it to the remaining stock. You can set their size, the default 5x2mm is good for a plywood clamp.

If you are not very experienced, adding 4 tabs is recommended for a secure holding of the finished part. Set it to  Auto add bridges, constant number: 4, 
Then click Add to create the bridges. 

You can see their position is maybe not very logical, we want one tab in the center of each side. Click on Edit Bridges (Manual) and slide them to a decent position.

You can now name it and click Calculate Now.

All the toolpath are now done !
Your file is ready to be exported and sent to your machine.

5/ Export your G-Code

A good practice is to simulate your full job before exporting anything to your machine, to see if it all seems like what you expect to be.

We're now ready to export our G-Code file. 

Click on the toolpaths menu and on Save Toolpath

Check that all the 3 toolpaths are "to save..."

Important: In Machine File Format, select LinuxCNC_Arc_MM_TC (.ngc)

And then Save to your usb key, to transfer it to the Mekanika CNC.

6/ Mill your part

We have another tutorial on how to use your Mekanika machine for the first time when you generate your G-Code, that you can find it here and is adapted to any software.