Working in NC Editor Mode of a CAM Document in Altium Designer

Created: February 10, 2023 | Updated: February 10, 2023
Applies to Altium Designer versions: 23 and 24

Parent page: Inspecting Fabrication Data with the CAM Editor

Placing Drills

In order for the command of the Place » Drill menu to be available, make sure that you are in the NC Editor, rather than the CAM Editor. Editor selection is carried out from the View menu.

Create Drill(s)

To convert existing circular flashes to drill points, choose the Place » Drill » Create Drill(s) command from the main menus. After launching the command, the cursor will change to a square and you will enter flash-to-drill conversion mode. Conversion is made by performing the following sequence of actions:

  1. Position the cursor over a circular flash that you wish to convert to a drill point, and click.
  2. Continue adding circular flashes in this way to build a selection ready for conversion.

    Clicking away from an object allows you to drag a selection area, for including multiple objects in the selection. Selection is cumulative.
  3. With all required flashes selected, right-click - the selected flashes will be converted to drill points, and new tool entries will be added in the Tool Table dialog, below any existing entries.
  4. Continue to select further circular flashes for conversion to drill points, or right-click, or press Esc, to exit.

Modify Drill(s)

To change the tool associated with selected drill points on the current document, choose the Place » Drill » Modify Drill(s) command from the main menus. After launching the command, the cursor will change to a square and you will enter drill modification mode. Modification is made by performing the following sequence of actions:

  1. Position the cursor over a drill point that you wish to modify, and click.
  2. Continue adding drill points in this way to build a selection ready for modification.
Clicking away from an object allows you to drag a selection area, for including multiple objects in the selection. Selection is cumulative.
  1. With all required drill points selected, right-click - the Select Mill/Drill Tool dialog will appear. Use the dialog to select the new tool that you wish to associate to these selected drill points and click OK - the selected drill points will now use the new tool.
  2. Continue to select further drill points for modification, or right-click, or press Esc, to exit.

Build Drill Layer

To create a drill layer from the Gerber information in the current document, choose the Place » Drill » Build Drill Layer (PTH) command from the main menus. After launching the command, a new layer - drill_template - will be created, and added to the layers list in the CAMtastic panel. All circular flashes in the design will automatically be detected and drill points created for each. These drill points will be visible on the drill_template layer. The original flash objects are not converted to drill points on their individual layers.

  • The Top and Bottom layer types must be assigned in the Layers Table dialog (Tables »  Layers) before a drill layer can be generated.
  • The drill_template layer is automatically assigned the type Drill Top in the Layers Table dialog.

Add Drill to Rout Plunge Point

To add a drill point to the plunge point of a selected rout path in the current document, choose the Place » Drill » Add Drill to Rout Plunge Point command from the main menus. After launching the command, the cursor will change to a small square and you will be prompted to select mill/rout objects that you wish to add a drill point to. Simply position the cursor over each rout path in turn, and click. Once all rout paths have been selected as required, right-click. A drill point will be added to the plunge point of each rout path.

The drill point will use the same drill tool that was used to define the rout path in each case.

Place Drill Point

To place drill points on the current document, use the Place » Drill » Drill Point command from the main menus.

First, ensure that the layer you wish to place drill points on, is the active layer. This is achieved by double-clicking on the layer name in the layers list area of the CAMtastic panel.

After launching the command, the Select Mill/Drill Tool dialog will appear. Choose the tool from the list of available tools. After clicking OK, the selected drill point will appear floating on the cursor. Simply position the cursor at the location in the workspace that you wish to add the drill point to, and click.

Continue placing further drill points, or right-click, or press Esc, to exit.

  • In order to add drill points, tools must already have been defined, otherwise you will get a dialog alerting you to this fact and you will be directed to the Tool Table dialog, from where you can add tool definitions.
  • The fastest way to generate tools is to generate NC Drill files from the PCB design document. These are imported into the CAMtastic Editor, and the tool definitions added to the Tool Table dialog.
  • You can also create new drill points (tools) from existing flashes, using the Create Drill(s) command. The Tool Table dialog will be updated accordingly.

Place Drill Circle (G84)

Drill circles are placed when you wish to drill holes in the board that are larger in diameter than the largest drill tool. To place drill circles on the current document, use the Place » Drill » Drill Circle (G84) command from the main menus.

First, ensure that the layer you wish to place a drill circle on, is the active layer. This is achieved by double-clicking on the layer name in the layers list area of the CAMtastic panel.

After launching the command, the Select Mill/Drill Tool dialog will appear. Choose the tool you wish to use for drilling the circle from the list of available tools. After clicking OK, you will enter circle placement mode. Placement is made by performing the following sequence of actions:

  1. Position the cursor at the required position and click to define the center point for the circle.
  2. Move the cursor to define the radius of the circle. As you move the cursor, a line appears to visually define the radius. When the radius is the required size, click again to complete placement of the circle.
  3. Continue placing further drill circles or right-click, or press Esc, to exit circle placement mode.
  • In order to add drill circles, tools must already have been defined, otherwise you will get a dialog alerting you to this fact and you will be directed to the Tool Table dialog, from where you can add tool definitions.
  • The fastest way to generate tools is to generate NC Drill files from the PCB design document. These are imported into the CAMtastic Editor, and the tool definitions added to the Tool Table dialog.
  • When a circle is drilled, the drilling machine actually drills overlapping holes around the circumference of the drill circle, in order to create the overall required hole in the board. You will notice when adding a drill circle that a small white circle is visible inside the circumference. This circle represents the size of the hole that will be drilled using the tool that you selected.

Place Drill Slot (G85)

Drill slots are used when you want to drill straight slots in the board. To place drill slots on the current document, use the Place » Drill » Drill Slot (G85) command from the main menus.

First, ensure that the layer you wish to place a drill slot on, is the active layer. This is achieved by double-clicking on the layer name in the layers list area of the CAMtastic panel.

After launching the command, the Select Mill/Drill Tool dialog will appear. Choose the tool you wish to use for drilling the slot from the list of available tools. After clicking OK, you will enter slot placement mode. Placement is made by performing the following sequence of actions:

  1. Position the cursor at the required location in the workspace and click to anchor the starting point for the slot.
  2. Move the cursor and click to place a second point for the slot.
  3. Continue placing further vertices for the slot, clicking to define each new vertex, or right-click, or press Esc, to exit slot placement mode.
  • In order to add drill slots, tools must already have been defined, otherwise you will get a dialog alerting you to this fact and you will be directed to the Tool Table dialog, from where you can add tool definitions.
  • The fastest way to generate tools is to generate NC Drill files from the PCB design document. These are imported into the CAMtastic Editor, and the tool definitions added to the Tool Table dialog.
  • When a slot is drilled, the drilling machine actually drills overlapping holes, from the start point to the end point, in order to create the overall required slot in the board. In fact, multiple passes are often made to achieve the drilled slot. You will notice when adding a drill slot that a small white circle is visible inside the slot. This circle represents the size of the hole that will be drilled using the tool that you selected.

Place Drill Text (M97, M98)

To place horizontal drill text on the current document, use the Place » Drill » Drill Text (M97, M98) command from the main menus.

First, ensure that the layer you wish to place drill text on, is the active layer. This is achieved by double-clicking on the layer name in the layers list area of the CAMtastic panel.

After launching the command, the Select Mill/Drill Tool dialog will appear. Choose the tool you wish to use for drilling the text from the list of available tools. After clicking OK, you will enter text placement mode. Placement is made by performing the following sequence of actions:

  1. Position the cursor at the required location in the workspace and click to determine the insertion point for the text (its lower-left corner).
  2. The Drill Text dialog appears. Use this dialog to enter the text to be drilled, and also to specify the text height and orientation (by default, this command places text horizontally, but you can change orientation to vertical from this dialog). After clicking OK, the drill text will be placed.
  3. Continue placing further drill text or right-click, or press Esc, to exit text placement mode.
  • In order to add drill text, tools must already have been defined, otherwise you will get a dialog alerting you to this fact and you will be directed to the Tool Table dialog, from where you can add tool definitions.
  • The fastest way to generate tools is to generate NC Drill files from the PCB design document. These are imported into the CAMtastic Editor, and the tool definitions added to the Tool Table dialog.
  • Letters of the text are actually drilled in a standard grid dot matrix pattern, with the hole spacing determined in relation to the tool diameter you have specified. You will notice when adding drill text that small white circles are visible inside the lettering. These circles represent the size of the hole that will be drilled using the tool that you selected.

Place Rout Circle Clockwise (G32)

To place rout circles on the current document so that the inside circle will be routed in a clockwise direction, use the Place » Drill » Circle Clockwise (G32) command from the main menus.

First, ensure that the layer you wish to place a rout circle on, is the active layer. This is achieved by double-clicking on the layer name, in the layers list area of the CAMtastic panel.

After launching the command, the Select Mill/Drill Tool dialog will appear. Choose the tool you wish to use for routing the circle from the list of available tools. After clicking OK, the Enter Value dialog will appear. Use this dialog to enter a value for the diameter of the outside circle, in the currently selected workspace units (inches or mm).

After clicking OK, you will be returned to the main design window and prompted to select the position for the center of the circle. Simply move the cursor to the required position and click to effect placement of the rout circle.

Continue placing further rout circles, or right-click, or press Esc, to exit.

  • In order to add rout circles, tools must already have been defined, otherwise you will get a dialog alerting you to this fact, and you will be directed to the Tool Table dialog (Tables » NC Tools), from where you can add tool definitions.
  • The fastest way to generate tools is to generate NC Drill files from the PCB design document. These are imported into the CAMtastic Editor, and the tool definitions added to the Tool Table dialog.

Place Rout Circle Counter-Clockwise (G33)

To place rout circles on the current document so that the inside circle will be routed in a counter-clockwise direction, use the Place » Drill » Circle C-Clockwise (G33) command from the main menus.

First, ensure that the layer you wish to place a rout circle on, is the active layer. This is achieved by double-clicking on the layer name, in the layers list area of the CAMtastic panel.

After launching the command, the Select Mill/Drill Tool dialog will appear. Choose the tool you wish to use for routing the circle from the list of available tools. After clicking OK, the Enter Value dialog will appear. Use this dialog to enter a value for the diameter of the outside circle, in the currently selected workspace units (inches or mm).

After clicking OK, you will be returned to the main design window and prompted to select the position for the center of the circle. Simply move the cursor to the required position and click to effect placement of the rout circle.

Continue placing further rout circles, or right-click, or press Esc, to exit.

  • In order to add rout circles, tools must already have been defined, otherwise you will get a dialog alerting you to this fact, and you will be directed to the Tool Table dialog (Tables » NC Tools), from where you can add tool definitions.
  • The fastest way to generate tools is to generate NC Drill files from the PCB design document. These are imported into the CAMtastic Editor, and the tool definitions added to the Tool Table dialog.

Sorting Drill Holes

Use the following commands to define the order in which the NC Drill machine will drill the holes listed in the drill file:

  • View » Sort/Optimize Options » Automatic – automatically define the order in which the NC Drill machine will drill the holes listed in the drill file, based on the use of a defined scan-box.

    After launching the command, the Enter Value dialog will appear. Use the dialog to enter a value for the scan-box used to automatically sort the order that the drill points will be drilled by the NC Drill machine.

    For example, if there are four sizes of hole on the drill layer (associated with four differently-sized drill tools) and you wish the smallest to be drilled first, set a value in the dialog to be greater than the diameter of the smallest drill tool, but less than that of the next drill size up.

    The order for drilling is then automatically defined as follows:

    1. The scan box covers the drill layer in a left-to-right, bottom-to-top fashion, with the drill points associated to the drill tool of equal size, or less, than the scan-box, being drilled first.
    2. The scan box is then reset to the bottom-left of the layer and scans again, with the drill points associated with the next drill size up being drilled next.
    3. The scanning is repeated for each additional drill size used, until all drill points have been accounted for.
  • View » Sort/Optimize Options » User Select – manually define the order in which the NC Drill machine will drill the holes listed in the drill file. After launching the command, the cursor will change to a small square and you will be prompted to select objects in order to define the sort order. Simply position the cursor over a drill point and click to add it to the selection. Continue adding drill points to the selection, in the order that you wish them to be drilled. When all drill holes have been included as required, right-click to effect the ordering.

    Drill points defined in the manual ordering will be drilled first, followed by any points that were not included in the manual selection, drilled in the order in which they were originally created.

  • View » Sort/Optimize Options » None – clear any drill sort/optimize option that has previously been applied. The NC Drill machine will then drill the holes according to the order in which they were originally created. After launching the command, any previously applied sort order/optimization will be cleared, and the drilling order will be returned to the original order in which the drill points were created.

The order in which the NC Drill machine will actually drill the holes, can be previewed using the Preview Drill/Rout command.

Previewing Drill/Rout

To redraw the information on the current drill layer, at a user-defined speed, so that you can see the order in which the drilling machine will proceed to drill your design, the Tables » Layers Order command from the main menus is used.

First, ensure that you have the drill layer selected as the only visible layer in the main design workspace. After launching the command, the Animate Viewing dialog will appear. Use this dialog to define the redraw speed for the layer. Choose from a predefined range of speed values - the larger the value, the slower the redraw speed.

After clicking OK, the current drill layer will be redrawn using the selected speed. The drill points will be redrawn in the order in which they will be drilled by the actual drilling machine.

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

Contact Us

Contact our corporate or local offices directly.

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
200 characters remaining
You are reporting an issue with the following selected text
and/or image within the active document: