To Contour the Part (Tutorial 1)

Next, run a contouring toolpath along the outside of the part.

  1. On the ribbon, click CAM tab 2D Milling panel 2D Contour.

Tool tab

  1. On the Tool tab, click .
    Remember: Tool definitions can be saved in a library or just for the part you work on. In this example, we will save the tools in the part only. You can always copy the tools to a library at a later time, if you wish to re-use them.

    2. Add a new tool with modified dimensions.

  2. Click .

    3. You can use the default tool type and dimensions (an Ø8 mm flat mill) for this tutorial, but increase the flute length to be able to cut the entire height of the part (22 mm).

  3. Click the Cutter tab.
  4. Change Flute length to: 25 mm
    5. Attention: If you decide to execute this toolpath on a machine tool, ensure that the tool number corresponds with the tool position in your tool changer on the machine tool, i.e. that on position 6 you have an 8 mm flat end mill cutter.
  5. Click the OK button to create your new tool.
  6. Click the Select button to select the tool for your operation and close the Tool Library dialog.

Feed & Speed Group

Expand the Feed & Speed group and change the following parameters:

  1. Spindle speed to: 3000 rpm 
  2. Cutting feedrate to: 800 mm/min 
Attention: If you decide to execute this toolpath on a machine tool, you will also need to set the feed & speed parameters according to the material you are using, and the capabilities of your tool and machine.

Geometry tab

  1. Click the Geometry tab. Ensure that the Contour selections button is active so that you can select the outside edge of the part geometry to run the tool around.
  2. Move the mouse over the bottom front edge. When it highlights, click on it. The bottom contour of the part is chain selected automatically.
  3. An arrow then appears near the chained contour indicating the direction of the toolpath. You can reverse the direction of a selected edge by simply clicking the arrow.

  4. Do not close the Operation dialog box if you are satisfied with your selection, as that will end the 2D Contour operation. Instead, simply proceed to the next step of this tutorial.

Heights tab

  1. Click the Heights tab. A preview of the heights is shown.

    2. Preview of heights: The top orange plane represents the Clearance Height. The second olive green plane represents the Retract Height. The green plane represents the Feed Height. The light blue plane is the Top Height. The dark blue plane is the Bottom Height.

    To make sure that the tool gets all the way through the stock, lower the bottom height by 1 mm.

  2. From the Bottom Height drop-down menu, select Model bottom.
  3. Change Bottom offset to: -1.0 mm 

Observe that the preview plane moves in the graphics window.

Tip: Observe that the various heights can also be adjusted using the mini-toolbar. Simply click the heights plane you wish to change and dynamically drag the arrow manipulator to the value you want. You can also enter the value directly in the mini-toolbar text field.

Start the Calculation

  1. Click at the bottom of the Operation dialog box, or right-click in the graphics window and select OK from the marking menu, to automatically start calculating the toolpath.

The toolpath is calculated and shown in the graphics window.



Important: Notice that in the CAM Browser, a new Setup has been created automatically. This is automatically done when creating a new operation before a setup has been created. A setup defines a number of settings used in all the operations contained within the setup. For example, the WCS can be changed in the setup.

Continue to To Machine the Pocket...

Parent topic: Tutorial 1 - 2D Machining