About Engrave

Access:

Ribbon: CAM tab 2D Milling panel Engrave

The Engrave strategy machines along contours with V-shaped chamfered walls.



Geometry selection for an Engrave operation



Toolpath generated for the selected geometry

Tool tab settings



Coolant:

The type of coolant used with the tool.

Spindle speed:

The rotational speed of the spindle.

Surface speed:

The spindle speed expressed as the speed of the tool on the surface.

Ramp spindle speed:

The rotational speed of the spindle when performing ramp movements.

Cutting feedrate:

Feed used in cutting moves.

Feed per tooth:

The cutting feedrate expressed as the feed per tooth.

Lead-in feedrate:

Feed used when leading in to a cutting move.

Lead-out feedrate:

Feed used when leading out from a cutting move.

Ramp feedrate:

Feed used when doing helical ramps into stock.

Plunge feedrate:

Feed used when plunging into stock.

Feed per revolution:

The plunge feedrate expressed as the feed per revolution.

Geometry tab settings



Contour selections

Use the Contour selections button to select the geometry profiles to be engraved. Contiguous geometry is automatically chained. The Engrave strategy follows along the selected contours in the middle such that the chamfer tool touches the selected edges. The tool moves up and down as the width of the area being cut changes.

Tool Orientation

Specifies how the tool orientation is determined using a combination of triad orientation and origin options.

The Orientation drop-down menu provides the following options to set the orientation of the X, Y, and Z triad axes:

The Origin drop-down menu offers the following options for locating the triad origin:

Heights tab settings



Clearance Height

The Clearance height is the first height the tool rapids to on its way to the start of the tool path.



Clearance Height

Clearance height offset:

The Clearance height offset is applied and is relative to the Clearance height selection in the above drop-down list.

Retract Height

Retract height sets the height that the tool moves up to before the next cutting pass. Retract height should be set above the Feed height and Top. Retract height is used together with the subsequent offset to establish the height.



Retract Height

Retract height offset:

Retract height offset is applied and is relative to the Retract height selection in the above drop-down list.

Feed Height

Feed height sets the height that the tool rapids to before changing to the feed/plunge rate to enter the part. Feed height should be set above the Top. A drilling operation uses this height as the initial feed height and the retract peck height. Feed height is used together with the subsequent offset to establish the height.



Feed Height

Feed height offset:

Feed height offset is applied and is relative to the Feed height selection in the above drop-down list.

Top Height

Top height sets the height that describes the top of the cut. Top height should be set above the Bottom. Top height is used together with the subsequent offset to establish the height.



Top Height

Top offset:

Top offset is applied and is relative to the Top height selection in the above drop-down list.

Bottom Height

Bottom height determines the final machining height/depth and the lowest depth that the tool descends into the stock. Bottom height needs to be set below the Top. Bottom height is used together with the subsequent offset to establish the height.



Bottom Height

Bottom offset:

Bottom offset is applied and is relative to the Bottom height selection in the above drop-down list.

Passes tab settings



Tolerance:

The tolerance used when linearizing geometry such as splines and ellipses. The tolerance is taken as the maximum chord distance.



Loose Tolerance .100



Tight Tolerance .001

CNC machine contouring motion is controlled using line G1 and arc G2 G3 commands. To accommodate this, CAM approximates spline and surface toolpaths by linearizing them; creating many short line segments to approximate the desired shape. How accurately the toolpath matches the desired shape depends largely on the number of lines used. More lines result in a toolpath that more closely approximates the nominal shape of the spline or surface.

Data Starving

It is tempting to always use very tight tolerances, but there are trade-offs including longer toolpath calculation times, large G-code files, and very short line moves. The first two are not much of a problem because Inventor HSM calculates very quickly and most modern controls have at least 1MB of RAM. However, short line moves, coupled with high feedrates, may result in a phenomenon known as data starving.

Data starving occurs when the control becomes so overwhelmed with data that it cannot keep up. CNC controls can only process a finite number of lines of code (blocks) per second. That can be as few as 40 blocks/second on older machines and 1,000 blocks/second or more on a newer machine like the Haas Automation control. Short line moves and high feedrates can force the processing rate beyond what the control can handle. When that happens, the machine must pause after each move and wait for the next servo command from the control.

Sharp corner angle:

??

Linking tab settings



High feedrate mode:

Specifies when rapid movements should be output as true rapids (G0) and when they should be output as high feedrate movements (G1).

This parameter is usually set to avoid collisions at rapids on machines which perform "dog-leg" movements at rapid.

High feedrate:

The feedrate to use for rapid movements output as G1 instead of G0.

Keep tool down

When enabled, the strategy avoids retracting when the distance to the next area is below the specified stay-down distance.

Maximum stay-down distance:

Specifies the maximum distance allowed for stay-down moves.



1" Maximum stay-down distance



2" Maximum stay-down distance

Entry positions

Select geometry near the location where you want the tool to enter.

Parent topic: About 2D Milling